Allegro Design Entry HDL console window

Syntax

Attribute point

Description

This command accesses the Attribute dialog box for adding, modifying, or deleting properties on a drawing. To use the command, type ATTRIBUTE, point to the desired object, and click the left mouse button. The editor brings up a form containing all the properties attached to the selected object.

Procedures

	Adding Properties
	Displaying and Modifying Property Attributes

Making an Attribute File

Auto

Syntax

AUto {PAth | Dots | Undot | PRoperty group_name prop_name prop_value . . }

Description

This command performs the global addition or deletion of certain objects to or from a drawing.

	PATH automatically assigns unique PATH numbers to bodies on a drawing that do not already have a PATH property. (Some special editor bodies and bodies labeled with a COMMENT property are not assigned PATH properties.) The path property is in the form 'PATH = In', where n is a unique integer.
	DOTS places a dot at each wire connection on the current drawing. Open dots are the default value. To specify filled dots, type SET DOTS_FILLED before entering AUTO DOTS.

UNDOT removes all dots from the drawing except those at the intersection of four wires.

PROPERTY will add user properties onto groups of components. GROUP_NAME is either a single letter identifying a group or a mouse click specifying the nearest group. Any number of property name-value pairs may be specified after the group, and the names and values may be separated by spaces, an equal sign, or a new line. Using this option will cause the entered properties to be automatically annotated onto the components within the group.

See also the SET DOTS_FILLED and SET DOTS_OPEN commands.

Auto Commands

Using the auto dot command

You can use the auto dot command to place dots on a complex circuit. The auto dot option with the set command automatically places dots on a drawing as you are creating it (set autodot on). Automatic dotting places dots at all intersections with an odd number of wires.

1.	When set autodot is off, type

show connections

This command places asterisks temporarily on the drawing to highlight each connection point.

2.	Check the drawing to make sure that no connections have been made by mistake.
3.	Use the refresh command to remove the asterisks from the screen.

Type

auto dot

All the junctions are automatically dotted.

Using the auto undot command

To remove the dots of the same size as the present dot size settings at intersections in a drawing type

auto undot

Note: You cannot use the auto dot and auto undot commands separated by a semi colon (;) on the same line in the console window. The following usage results in an error:

auto dot; autoundot

Using the auto allundot command

To remove all the dots at the intersections in a drawing type

auto allundot

Changing Dot Size

	If you change the size of a dot, the change is not reflected on filled dots in the schematic, however, when you plot the schematic, the change in size gets reflected.
	Change in size is also not reflected in dots that existed previously, it appears only in the dots that you add after changing the size. So, if you want to make all the dots of the same size, first use autoundot to remove the dots within the size specified in logic dot radius, or autoallundot to remove all dots regardless of size. Then add the dots again using auto dot.

Using the auto netprop command

Use this command to apply an attribute list to a set of wires. To attach the specified property on all wires in a group, type

auto netprop <group_name> <property_name> = <property_value>

Using the auto path command

If the SET command option AUTOPATH is on, the PATH property is automatically added to a part when it is added to a drawing. If set autopath is off, you can use the auto path command to assign PATH properties to symbols on a drawing that do not already have a PATH property.

Using the auto property command

To attach properties to symbols in a group, type

auto property <group_name> <property_name> = <property_value>

Using the autoroute command

The set command option autoroute on activates automatic routing after moving an object in the direct mode. The set autoroute option can be turned on or off.

Backannotate

Syntax

Backannotate {annotation file | <cr>}

Description

This command annotates designs with physical information from the Packager. The editor reads the specified schematic annotation file produced by the Packager. The file includes physical information such as location designators, pin numbers, physical net names on the design, and user-defined properties, if any.

The annotated properties added by the editor are soft properties. Soft property names begin with a dollar sign (for example, $LOCATION) and are not written into the connectivity file. This allows Packager to reassign physical information each time the design is repackaged.

You can move and delete soft properties, or you can change a soft property into a hard property by using the PROPERTY command and adding a property with the same property name without the dollar sign.

To generate a backannotation file, use the following directive when running the Packager:

output backannotation;

By default, this directive is set.

To process the backannotation file generated by the Packager (pstback.dat), type either of the commands BACKANNOTATE PSTBACK.DAT or BACKANNOTATE <cr>. BACKANNOTATE <cr> brings up the File Browser form. The user can then select the name of the backannotation file from the form. The editor reads the file, edits each named drawing in turn, adds the appropriate physical information, and writes the drawing. Backannotation aborts if any errors are detected during the process.

Do not run backannotation if any other user who has write permissions is working on the design. Running backannotation when another user is working on the design results in incomplete backannotation.

Limitations of Backannotation

1.	Sizeable parts having property SIZE > 1 are not backannotated.
2.	Net properties are backannotated only if they have existing placeholders.

3.	Properties on buses are not backannotated unless they exist on individual bits of the bus.

See also the SET command options that control property visibility and pin number placement.

Badd

Syntax

BADd { [block_name] point1 point2 } . . .

Description

This command can be used to create and add blocks. The block is a rectangle between point1 and point2. If you omit block_name, Design Entry HDL automatically names the block (the name will be "BLOCK" followed by an integer). If you do enter a block_name, and a symbol for that part already exists, you will be thrown into the add command.

Example

To add a new block CACHE to the design:

1.	Type badd CACHE in the console window.
2.	Click the design window and drag to form a rectangle.

Note: The cursor shape changes to a + sign.

3.	Click the design window again to end the drawing.

Related Commands

Add
Bpadd
Bpdelete
Bprename
Bpmove
Brename
Broute
Bstretch
Bwire

Bpadd

Syntax

BPAdd {pin_name :mode point}...

Description

Add or rename pins on blocks. bpadd adds pins to blocks with a user-specified name. It is useful if you want to define the interface pins of a block before you connect up your blocks. mode specifies whether the block pin is an input pin, an output pin, or an inout pin, and can take values input, output, inout, respectively. You can change the mode of the pin while you are placing it on the block. pin_name is the name of the pin that will be created. Point is where the pin is created.

Related Commands

Badd
Bpdelete
Bprename
Bpmove
Brename
Broute
Bstretch
Bwire

Bindview

Syntax

Bindview point1 point2

Description

This command makes a drawing that is visible in one viewport visible in another viewport also. Any changes you make to one copy of the drawing also appear on the other copy.

Point1 selects the drawing to make visible. Point2 specifies the new viewport where the drawing should appear.

When you use BINDVIEW, the drawing name is not added to the drawing stack in the second viewport. If you issue a command, such as SHOW or RETURN, the bound drawing does not appear in the list. When you EDIT or RETURN to a drawing in the bound viewport, the binding is removed. Use BINDVIEW again to re-bind the drawing.

Bpdelete

Syntax

BPDelete {point}...

Description

This command deletes pins on blocks. You can choose the pins to be deleted by pointing to them with the mouse.

Example

To delete a pin, type bpdelete in the console window and select the pin using the left mouse button.

Related Commands

Badd
Bpadd
Bprename
Bpmove
Brename
Broute
Bstretch
Bwire

Bpmove

Syntax

BPMove {point1 point2}...

Description

This command moves a pin from point1 on a block to point2.

Example

To move a pin from point1 on a block to point2:

1.	Type bpmove in the console window.
2.	Click to select the pin to be moved (point1).

3.	Click to place the pin on the block (point2).

If you try to undo this operation, some hanging properties may remain on the schematic. This is because the bpmove command actually moves a pin and its properties on the symbol while the undo command operates only on the schematic.

To remove these hanging properties, perform the following steps:

1.	setsticky_on
2.	get

3.	setsticky_off

Related Commands

Badd
Bpadd
Bpdelete
Bprename
Brename
Broute
Bstretch
Bwire

Bprename

Syntax

BPRename {pin_name point}...

Description

This command renames pins on blocks. In this command, pin_name is the new name of the pin and point is location of the pin.

Example

To rename a pin named PRESET to CLOCK, type bprename CLOCK in the console window and click PRESET.

Related Commands

Badd
Bpadd
Bpdelete
Bpmove
Brename
Broute
Bstretch
Bwire

Brename

Syntax

BREname {[block_name] point1}...

Description

This command renames blocks. This is useful if you allowed the system to generate default names for your blocks and want to rename them. It does not remove old blocks from the disk. It does, however, remove the old block from the memory if you are not actually viewing it. So if the old block had not been saved to disk, it will have been removed. If the old block had been saved to the disk, Design Entry HDL generates the following message:

You might want to remove <old_block_name> with the remove command.

If you do not need the old block any longer, you can remove it from the disk by using the remove command, for example remove <old_block_name>.

This command is also useful if you want to create a block similar to one you already have. You can copy the block (with the COPY command) and rename the copy of the block. The original block will be unaffected.

Example

To rename a block named CACHE to MEMORY, type brename MEMORY in the console window and click CACHE.

Related Commands

Badd
Bpadd
Bpdelete
Bpmove
Bprename
Broute
Bstretch
Bwire
Copy
Remove

Broute

Syntax

BROUte {[signal_name] point1 point2}...

Description

This command routes a signal named signal_name between point1 and point2. If the signal_name is a bus name, create a heavy wire.

Related Commands

Badd
Bpadd
Bpdelete
Bpmove
Bprename
Brename
Bstretch
Bwire
Route
Wire

Browse

Syntax

Browse {<libname> | <cr>}

Description

This command accesses the COMPONENT BROWSER dialog box. It lets you scan through all libraries and active directories. You can also access the COMPONENT BROWSER with the ADD command.

BROWSE <libname> sets the library field to the given library name and resets the selection list to that library. The default is the design library.

Example

To display the COMPONENT BROWSER dialog box, type browse in the console window and press Enter.

To display the COMPONENT BROWSER dialog box with the library set to standard, type browse standard in the console window and press Enter.

Bstretch

Syntax

BStretch {point1 point2} . . .

Description

This command resizes blocks. Select the side or corner of the block you want to stretch with point1. Then select where it stretches to with point2. Pins will move with the side they are attached to. Pins pointing to the left or right will only move horizontally. Pins pointing to the top or bottom only move vertically. You may not shrink a block so much that its pins or its origin fall outside it.

Wires attached to the instance of the block being stretched will be attached to new pin locations. However, they are not re-routed. If a new wire stub is not straight, use the SPLIT and DELETE commands to straighten it.

Example

To resize a block, type bstretch in the console window and select the side or corner of the block you want to stretch. Drag to the point you want to resize the block. Click again to end the block.

Related Commands

Badd
Bpadd
Bpdelete
Bpmove
Bprename
Brename
Broute
Bwire
Delete
Split

Bubble

Syntax

BUBble point...

Description

This command toggles the state of a pin between bubbled and unbubbled. Bodies must be defined with bubbleable pins to permit this conversion. If the pins are established as part of a bubble group, the BUBBLE command can be used to convert the symbol from one form to another.

The BUBBLED property is automatically attached to bubbled pins to indicate that only low-asserted signals may be connected to them. The BUBBLED property should never be entered, assigned, or attached by the user.

You can also specify the coordinates of the pin in the console window instead of pointing to the pin in the design window. This is true for all console commands that require pointing to an object in the design window.

For example, a NOT symbol is defined with both the BUBBLED and BUBBLE_GROUP properties attached:

BUBBLED=(B)

BUBBLE_GROUP=(A|B)

Because BUBBLED is equal to (B), pin 'B' is bubbled when the part is initially added to a drawing. If you type BUBBLE and point to either pin A or B, the attached BUBBLE_GROUP property specifies that pin A is now the bubbled pin and pin B the unbubbled pin.

Example

To toggle the state of a pin, type bubble in the console window and click the pin in the design window.

To make two pins as part of the same bubble-group such that the BUBBLE command can be applied to the pins, you must ensure the following:

1.	Both the pins must have a wire stub and a bubble attached to them, similar to the symbol of LS04 in the lstll library.
2.	BUBBLE_GROUP property must be attached to the component symbol with the value containing all pin names in the bubble group. For example, BUBBLE_GROUP = (A<7..0> \| B<7..0>).

3.	The pin that you want to make bubbled by default, should be specified with a BUBBLED property on the component. For example, BUBBLED = B<7..0>

Note: If the BUBBLED property is not specified, pins A and B appear as unbubbled on instantiation. When you run the BUBBLE command, both the pins will appear as bubbled. However, if the BUBBLED property has been specified only for pin B, then it will appear as bubbled by default, and pin A will appear as unbubbled. When you run the BUBBLE command again the A will appear as bubbled and B as unbubbled. Thus, the BUBBLE command acts as a toggle for changing the bubbled state of a pin.

Busname

Syntax

BUSName bus_name point point

Description

This command places single-bit vectored signal and pin names on a drawing. For example, the bus name A<7..0:2> results in the signal names A<7>, A<5>, A<3>, and A<1>.

To use the BUSNAME command, first place separate wires or pins (use the COPY command). Next, enter the bus name in Design Entry HDL signal syntax (for example, DATA<15..0>\I). Then, select two points. Design Entry HDL will find all the wires you have crossed and add the properties to those wires.

For examples, if you issue the following command:

busname a<20..0:2>\I

then pick two points, such that you have crossed over three wires, the crossed wires will be named as a<20>\I, a<18>\I and a<16>\I respectively, then you can select another two points and the wires crossed will be named a<14>\I and a<14>\I and so on.

If the first thing you do after entering the BUSNAME command is to enter a point, the editor uses the most recently entered signal name. This is useful if you place the first two signal names incorrectly. If the attachment lines show that the names are not connected to the appropriate signals, use UNDO to delete the incorrect attachments, then type BUSNAME and click on the drawing area. You can then reposition the first two names.

Related Commands

Signame
Bustap

Bustap

Syntax

BUSTap bus_tap_value point point...

Description

This command fills in the value of the BN (bit number) properties on bus taps in drawings.

The bus_tap_value should be in the Design Entry HDL signal syntax with the first number as the start tap value, the second number as the end tap value, and the third number the increment. For example, a bus_tap_value of 7..0:2 results in BN values of <7>, <5>, <3>, and <1>, with <7> being placed on the tap closest to the first point, <1> on the tap closest to the second point, and <5> and <3> on the taps in-between.

The third number is optional. If no third number is specified, for example, 7..0, an increment of 1 is assumed. The second number is also optional, and if not specified, for example `7', all taps pointed to will have a BN value of the first number.

Bwire

Syntax

Bwire {[signal_name] point point } . . .

Description

The bwire command adds a net between point/component/block and a block. When the net is added, a pin also gets attached at the connection point in the block.

See also the WIRE, BROUTE, ROUTE commands, and the SET and SHOW commands to change default wiring behavior.

Example

To create a net AB and a pin AB on a block in the design:

1.	Type bwire AB in the console window.
2.	Start at some point and end on a block in the design.

A net named AB and a pin on the selected block named AB are created.

Related Commands

Broute
Route
Set
Show
Wire

Change

Syntax

Change {group_name | point}...

Description

This command modifies selected lines of text in place. The selected text items are highlighted, and the cursor is placed on the first text item. In case of notes, the cursor is placed before the character you click.

For properties, if both the name and the value is visible, the cursor is placed after the = character. If only the name or the value is visible, the cursor is placed at the beginning. After changing one line of text, the user can move over to the next text item by typing <cr>. The changes made to the line of text are then committed. The changes made to each line of text can be undone using the UNDO command.

Example

Type change and click a note in the design window. The cursor is placed before the character you clicked in the note. If you clicked the beginning of the note, the cursor is placed before the first character of the note.

The following commands are useful for editing text:

<BackSpace>	Deletes the previous character
<Delete>	Deletes the current character
Ctl<k>	Deletes to the end-of-line
Ctl<e>	Brings up the selected text items in an editor
<-	Moves backward
->	Moves forward

Check

Syntax

CHEck <cr>

Description

This command checks for connectivity problems and general errors on the current drawing. An option exists to allow the user to turn the check on or off. Design Entry HDL performs the following checks on the schematic:

Duplicate components in the same location

set option: CHECK_PARts_at_same_loc <ON/OFF>

To correct the error, use the split console command and separate overlapping elements. For more information on the split console command, see Split .

Pins attached to more than two wire segments (this may not be an error, but is an error if a wire inadvertently shorts the pins on a device)

set option: CHECK_TWo_wires_at_pins <ON/OFF>

Wires connected to only one pin and not named (NC wires)

set option: CHECK_Unconn_wires <ON/OFF>

Nets that are named but not connected to any pins

set option: CHECK_SIGNAMES <ON/OFF>

Wires that come close to but do not contact pins

set option: CHECK_PIN_near_wire_endpt <ON/OFF>

Missing TITLE and/or ABBREV properties

set option: CHECK_TItle_abbrev <ON/OFF>

Bodies that are placeholders

set option: CHECK_Body_place_holders <ON/OFF>

Pins located at the origin (0,0) in BODY drawings

set option: CHECK_PINS_at_origin <ON/OFF>

Multiple dots at the same location

set option: CHECK_Arcs_at_same_loc <ON/OFF>

To correct the error, use the split console command and separate overlapping elements. For more information on the split console command, see Split .

Hard properties with the? value (placeholders)

set option: CHECK_Prop_place_holders <ON/OFF>

Wires connecting the pins of a two-pin body

set option: CHECK_Shorted_pin <ON/OFF>

Wire segments hidden by parts of a body

set option: CHECK_Hidden_wires <ON/OFF>

To correct the error, use the split command and separate overlapping elements.

Pin properties which are no longer attached to pins.

set option: CHECK_Missing_pins <ON/OFF>

To correct the error, reattach properties to new pins, delete properties or replace part.

Inconsistent section properties

set option: CHECK_Pack_sec_type_props <ON/OFF>

To correct the error, resection the part.

Signame properties defined within a symbol (body).

set option: CHECK_SIGNAME_in_body <ON/OFF>

To correct the error, remove signame properties from the body files.

	Duplicate PATH properties
	Wires overlapping a body

Check for legal HDL net names (hdl_direct on only)

set option: CHECK_Net_names_hdl_ok <ON/OFF>

Check for legal HDL port names (hdl_direct on only)

set option: CHECK_Port_names_hdl_ok <ON/OFF>

Check for legal HDL symbol names (hdl_direct on only)

set option: CHECK_Symbol_names_hdl_ok <ON/OFF>

Run checks automatically when writing drawings.

set option: CHECK_On_write <ON/OFF>

CHECK lists each detected error. After you run the CHECK command, you can use the ERROR command to locate each error on the drawing.

Related Commands

Circle

Syntax

Circle point point

Description

This command adds circles to a drawing. To place a circle on the drawing, enter the CIRCLE command and select a point as the center of the circle. To size the circle dynamically, drag the mouse and then click again to place the circle on the drawing.

Circles and arcs are rarely necessary on logic designs but are commonly used for creating symbol drawings.

Related Commands

Arc

Copy

To make multiple properties of an object

Syntax

COPy {[count][REPEAT][ALL] source_point destination_point | [count][REPEAT][ALL] group_name destination_point | property_point destination_point attach_point }

Description

This command copies objects, properties, and groups in the current drawing or between viewports.

COUNT indicates the number of copies to place on the drawing. To make multiple copies, type COPY and enter a number to specify the number of copies to make. Move the cursor to the object or group to be copied and click to select an object or the center button to select a group. Click to place the copies at grid points or the right button to place copies at the vertex nearest the cursor. After you place the first copy, the remaining copies are automatically added to the drawing. The second copy is offset from the first copy by the same distance as the first copy is from the original. You can use this feature to copy single items and groups.

SOURCE_POINT is the object to copy, PROPERTY_POINT is the property to copy, and DESTINATION_POINT is the position point for the new copy. When you copy a property, ATTACH_POINT attaches the property to an object (symbol, pin, rewire).

To copy an object (such as a symbol or a wire), type COPY, position the cursor on the object, and press the appropriate button. The left button picks up a copy of the object at the grid point nearest the cursor. The right button picks up a copy of the object at the vertex nearest the cursor. (The vertex of the copy snaps to the cursor.) This is useful for copying component bodies and wires. Click to place the copy on the grid point nearest the cursor or the right button to attach the copy to the nearest vertex (useful for attaching copies of wires at new locations).

To copy a group, use the GROUP or SELECT command to define a group, then type COPY. Move the cursor to the group to be copied and click the center button to select the nearest group. You can also type the single-letter GROUP_NAME and press <cr>. Click to place the copy.

To copy properties, type COPY, and click to select the property to copy. Move the cursor to the location for the copy and click. A flexible line is drawn from the property to the cursor. Move the cursor to the object where the property is to be attached and click. You can attach the property to a part, wire, pin, or signal name.

You cannot copy default symbol properties, soft properties, PIN_NUMBER properties, or properties generated by the SECTION, PINSWAP, and BACKANNOTATE commands. User-added properties are included in copies of parts. Signal names are not copied. Wire properties are not included when you copy a wire. If a default symbol property on a symbol was changed, the copy of the symbol contains the changed value.

There are two options to the COPY command. COPY ALL will copy section properties, soft properties, pin properties, wire properties, and properties attached to other properties. This option is especially useful if you are copying a section of logic from one drawing to another. If you want to place a copy of something in several unrelated places, try using the COPY REPEAT option. This option causes the copy command to reselect the objects you originally selected after you have placed a given instance. The REPEAT and ALL options may be used together.

Groups of properties are not copied. When applicable, properties attached to objects are copied with the group.

Procedures

	To copy an object
	To copy an object and its properties

Dehighlight

Syntax

DEHighlight [ Net | PArt | PIn | Any ] pt

DEHighlight [ Net | PArt | PIn | Any ] object_name

Description

Net, Part and Pin are used to specify the object type you want to unhighlight. You may use Any if you want all selected objects to be unhighlighted. This is also the default argument if you do not specify any object type

pt	To pick a component to be unhighlighted, point to the object and press the left button. Select a group by pointing to the required group and pressing the middle button.
object_name	If you would prefer typing in the name of the object, you may do so by using the second version of this command.

For nets, the object name is the signal name of the net, for example, FOO.

For parts, the object name is the value of the PATH property attached to the component, for example, 7P.

For pins, the object name is the value of the PATH property attached to that component to which the pin belongs, followed by a period ("."), followed by the name of the pin, for example, 7P.A<SIZE-1..0>.

Wildcards such as * and ? may be used in specifying the object name,

For example, FOO*, 7*P, 7P.A*.

The Dehighlight command is used to unhighlight an already highlighted object throughout the system.

Related Commands

Highlight
Unhighlight

Delete

Syntax

DELete {point | group_name}...

Description

This command removes objects from a drawing. To delete an object, point to any part of the object and press the left button. To delete a group, use the center button or type in the single-letter group_name. DELETE removes the object or group nearest to the cursor.

You cannot delete default properties on bodies and pin number properties generated by the PINSWAP command.

The UNDO command lets you retrieve groups or objects deleted by mistake.

Example

To delete an object:

1.	Type delete in the console window.
2.	Point to an object in the design window and press the left button.

Procedures

	Deleting an object
	Deleting a group

Related Commands

Undo

Diagram

Syntax

DIAgram [<library>]cell[.type][.version][.page]

Description

This command works like the File – Save As menu option in Design Entry HDL. You can use an existing drawing as a pattern for a new drawing or save a copy of a drawing by a different name before making changes to it.

	<LIBRARY> is the name of the library where the drawing resides. The library name must be enclosed in angle brackets. If no library is specified, the current library is the default.
	CELL is the new name of the drawing. The current drawing name is taken by default. For example, if the Design Entry HDL title bar displays ATM.SCH.1.2, the current drawing name is ATM.

	TYPE is the drawing type. The drawing type can be SCH (schematic), SYM (symbol). If no drawing type is specified, the current drawing type is used. For example, if the Design Entry HDL title bar displays ATM.SCH.1.2, the current drawing type is SCH.
	VERSION is the version number of the drawing type. For example, if the Design Entry HDL title bar displays ATM.SCH.1.2, the version number of the drawing type SCH is 1. If no version number is specified, the default value 1 is used.

PAGE is the page number for the drawing. For example, if the Design Entry HDL title bar displays ATM.SCH.1.2, the page number of the current drawing is 2. If no page number is specified, the default value 1 is used.

To rename a drawing, edit the drawing to be changed, type DIAGRAM and the new name of the drawing. Type WRITE to save a copy of the drawing by its new name.

For example, to use the drawing SHIFTER.SCH.1.1 as a pattern for a new drawing named NEWSHIFTER.SCH.1.1, use the commands:

EDIT SHIFTER.SCH.1.1

DIAGRAM NEWSHIFTER

WRITE

The NEWSHIFTER.SCH.1.1 drawing is saved to disk.

Directory

Syntax

DIRectory {[<directory>][name][.[type][.[vers][.[page]]]] |<cr>}

Description

This command lists the names and contents of directories in the current directory list in the order that the directories are searched with the current working directory displayed first.

DIRECTORY <cr> accesses the DIRECTORY BROWSER form. The DIRECTORY BROWSER form shows the current library or directory. Any items listed in the left section of the form are from the current directory or library. To list the contents of a different directory or library, select the Current Dir/Lib field and type the directory or library name. The directory form can be turned off by typing in SET DIRFORM OFF.

<DIRECTORY> is the directory name whose contents you want to list. The name must be enclosed in angle brackets. If no directory is specified, the current directory is taken by default. NAME is the drawing to be listed. Unless you specify the drawing type, the version number, and the page number, the DIRECTORY command displays only the drawing name. You can also list drawings by type, versions, or pages.

You can use wildcards in all fields of the directory and drawing names. An asterisk matches any string. A question mark matches any single character.

Some command examples are

DIR	Lists all drawing names in the current directory
DIR <*>	Lists all active directories (but no drawing names)
DIR <time>*	Lists all drawing names (parts) in the TIME library
DIR <>	Lists all drawing names in all active directories and libraries
DIR ls*	Lists real file name and directory type for current directory.
DIR .	Lists all drawings.

Related Commands

IGnore
Library

Display

Displaying properties on objects in a group

Syntax

DISplay { Name | Value | Both | Invisible | Default | scale_factor | Center_justified | Left_justified | Right_justified | Heavy | Thin | Pattern <pattern_number> | Filled | Open }{ point . . . | group_name . . . }

Description

This command changes the way objects or groups are displayed on a drawing. Any change made with the DISPLAY command remains in effect until another DISPLAY command is used to change it again.

To change the display of a single object, use the left mouse button. To change the display of a group, use the middle mouse button or type in the single-letter group name.

Groups can contain any type of object. Group names, options, and point entries can be included in any order and in any combination, except that the first argument MUST be a command option.

The command options are described below:

	NAME, VALUE, BOTH, and INVISIBLE determine the way properties are displayed on the drawing. Although a property consists of a name and value pair, usually only the value is displayed when a property is added to a drawing. These options allow you to display the name alone, the value alone, both, or neither.
	DEFAULT and SCALE_FACTOR determine the size of text displayed on the drawing.

		DEFAULT displays text on the drawing using the default text size specified in the Text tab of the Design Entry HDL Options dialog box. For example, if the default text size is 0.082 inches, the size of the selected text on the drawing will be set to 0.082 inches.
		You specify a scale_factor to enlarge or reduce the size of the text on the drawing. For example, if the default text size specified in the Text tab of the Design Entry HDL Options dialog box is 0.082 inches, the DISPLAY 2 command will enlarge the size of the selected text to 0.164 inches.

Note: To display the size of a string, type SHOW SIZE and point to the string. Use SET SIZE to alter the default size of added text.

A text string added to a drawing is defined by a vertex at the lower left corner of the string. To change the justification, use DISPLAY CENTER_JUSTIFIED, DISPLAY RIGHT_JUSTIFIED, or DISPLAY LEFT_JUSTIFIED.

HEAVY, THIN, and PATTERN change the way an existing wire appears on a drawing. Heavy makes the wire thicker making it look like a bus. Thin returns a heavy wire to the default wire thickness. Pattern changes a wire to one of six patterned lines. Pattern 1 is a filled line (the default); patterns 2-6 are a variety of dotted and dashed lines. In a LOGIC drawing, the entire net changes. In a SYMBOL or DOC drawing, only the wire segment specified by the cursor changes.

	FILLED and OPEN change the display of dots already added to a design.
	Open dots scale when the ZOOM or SCALE command is used; filled dots do not. The SET DOTS_FILLED command adds dots to the drawing filled by default.

Procedures

	Displaying properties on objects
	Resizing text

Dot

Syntax

Dot point...

Description

This command adds dots to drawings to indicate connection points. Dots are used in logic drawings to indicate that lines crossing one another are connected. By default, lines crossing are not connected unless dotted. Wires joining at a 'tee' are connected, even without a dot. Dots are used in symbol drawings to indicate pin connection points.

Dots can be filled or open. By default, all added dots are open. To change to filled dots, type SET DOTS_FILLED. To fill an open dot, type DISPLAY FILLED and point to the dot.

AUTO DOTS places a dot at all connection points in a logic drawing. AUTO UNDOT automatically removes all dots except those at the intersections of four wires.

AUTO UNDOT removes all existing dots in the drawing.

Example

To indicate a connection point on a wire, type dot in the console window and click on the wire where you want the connection point.

Echo

Syntax

Echo message

Description

This command displays messages in the console window. Use this command to show messages during the execution of a script for tracking its progress and debugging.

Example

echo 50% script completed

Edit

Syntax

Edit {[<directory>][drawing][.[type][.[version][.[page]]]]|<cr> | point}

Description

This command displays an existing drawing to be edited or creates a new drawing.

EDIT <cr> accesses the View Open form that allows you to open an existing drawing for editing. The View Open form can be turned off by typing SET EDITFORM OFF.

To edit a drawing directly from the command line, type EDIT and the drawing name. <DIRECTORY> is the directory where the editor is to search for the drawing. If not specified, each directory in the list is searched until a drawing by that name is found. The directory name must be enclosed in angle brackets. DRAWING is the name of the drawing to edit. If the specified drawing is found, it is displayed on the screen. If it is not found, the system creates a new drawing by that name in the current library when you write the drawing.

The default value for both version and page is 1. Page specifications for symbol drawings are ignored, but each symbol can have multiple versions. Other drawing types can also have multiple versions and pages.

You can edit a second drawing without writing the current drawing. EDIT saves the first drawing, along with any changes, in a temporary file before bringing in the new drawing. If you edit the first drawing again, EDIT displays the modified version from temporary storage. The SHOW HISTORY command lists all drawings that have been edited during the current session and states whether they have been modified.

The EDIT command also allows you to examine the drawings associated with symbols on the screen. By default, the SYMBOL.CSS file of a hierarchical symbol is edited when you select the symbol from the current drawing. For example, to edit the logic associated with a SUBTRACTOR symbol in the current drawing, type EDIT and point to the symbol with the left button. The current drawing is placed in temporary storage, and the drawing SUBTRACTOR.SYM.1.1 is displayed for editing.

Procedures

	Navigating the drawing hierarchy
	Opening a drawing

	Creating a design page
	Displaying pages in a multi-page drawing

Related Commands

Get
Return
Gotosheet

Error

Syntax

Error <cr>

Description

This command locates and displays each error detected by the CHECK command. It draws a blinking highlighted rectangle at the location of the error and displays a message describing the error.

Exclude

Syntax

EXClude [group_name|Mpoint|DEFault][option...][selection ...| group_name]

where option is:

BOdies | WIres | PRoperties | NEts | Connections

and selection is:

Lpoint | Ctrl+Rpoint | Mpoint

Description

This command removes items or groups from the current group.

	If the first argument is a single-letter group name, the group will become the current group. Alternatively, click the middle mouse button on a highlighted group to make it the current group. If a group is not specified, or the word default is provided, the most recently created group will remain the current group.
	To remove individual objects, click the left mouse button or press Ctrl and click the right mouse button.

	To remove previously-defined groups, click the middle mouse button on a highlighted group or enter the single-letter group name.
	Option flags allow the user to remove types of objects in a group. Options are applied to the objects in the initial current group.

Specifying BODIES, WIRES, or PROPERTIES removes all occurrences of the specified type from the current group. NETS is the same as WIRES. Specifying CONNECTIONS removes all symbol pins (but not the symbol origins) from the current group.

Example

Exclude A ne

This command excludes all nets in group A from the group.

Related Commands

Find
Group
Include
Select

Exit

Syntax

EXIt <cr>

Description

This commands terminates an editing session. The editor displays a message if there are unwritten changes to any drawings in the current editing session and asks you if you really want to quit. You must answer Y or YES to exit. Any other response aborts the command.

The QUIT command is the same as the EXIT command.

Related Commands

Quit

Filenote

Syntax

FILenote {file_name point| <cr>}

Description

This command includes a named text file in a drawing at the specified point. POINT is the position in the drawing to add the text. When the file is added, each line in the file is converted into a note that can be individually moved, copied, deleted, or changed. Empty lines in the file are ignored. To include a blank line in the note, type a space on the line in the file.

FILENOTE <cr> brings up a file browser. Select the file and click the position on the drawing where you want to place the note.

Find

Syntax

FINd pattern

Description

This command searches the current drawing and places all objects that match a specified pattern into a group. A pattern can match symbol names, notes, property names, property values, or signal names. You can search for properties by specifying both name and value separated by an equal sign.

Wildcards are allowed in a pattern. An asterisk matches any number of characters, and a question mark matches any single character. FIND is not case-sensitive.

All items found with the command are placed in a list. You can step through the list items using the NEXT command. This command places a blinking highlighted rectangle around each item on the display so that it can be changed or deleted.

By using the SET NEXTgroup command before the FINd command, you can add the results of the FINd operation to the specified group. Commands to do this are:

SET NEXTgroup <groupname>

FINd pattern

Examples

To find all ls04 components on a drawing and add them in group A, run the following console commands:

set nextgroup A

find ls04

To find all objects on a drawing that start with the letter mem and add them in group A, run the following console commands:

set nextgroup A

find mem*

	Suppose you have 5 instances of ls04 with property LOCATION = U1 on a page. To change LOCATION property of all these instances to U8, perform the following steps:
	a.	Type the console command:

find LOCATION = U1

Type the console command:

change A

Right-click on the canvas and select Editor from the pop-up menu.

The text editor opens.

	d.	Change the value of LOCATION property to U8 for all the objects.
	e.	Choose File – Save and save the file.

Related Commands

Group
Exclude
Include
Select
Set

Get

Syntax

Get { [<directory>][drawing][.[type][.[version][.[page]]]] }

Description

This command replaces the current copy of a drawing with the version stored on the disk. The fresh copy of the drawing replaces any previously read (and perhaps modified) version in the editor. GET is useful while editing a drawing if you want to discard the current work and go back to an earlier version.

Note: All modifications to the current drawing are lost when you use the Get command.

Example

To discard changes to your current drawing:

1.	Type get in the console window and press Enter.

A Design Entry-HDL message box appears asking you to confirm if you really want to get the drawing from the disk.

2.	In the Design Entry-HDL message box, click Yes.

Related Commands

Edit

_globalModify

Syntax

_globalModify

Description

Opens the Component Change tabbed page of the Global Modification window. Use this page to replace a component with a new component across a design.

_globalChange

Syntax

_globalChange

Description

Opens the Property Change tabbed page of the Global Modification window. Use this page to change properties of components, pins, and nets across a design.

_globalDelete

Syntax

_globalDelete

Description

Opens the Property Delete tabbed page of the Global Modification window. Use this page to delete properties of components, pins, and nets across a design.

Gotosheet

Syntax

GOtosheet N

where N is the page number in a hierarchical design.

Description

This command allows you to go to a specific page in a hierarchical design.

This allows you to easily refer to a page in Design Entry HDL against a plotted page or a cross-reference report.

	When you plot a schematic page, the page number of the schematic page is plotted if you have added the custom text variables for page numbers on the schematic page.
	When you perform cross-referencing on a design, the cross-reference reports display the schematic page numbers.

Enter the page number displayed on the plotted page or the cross-reference report to go to the page in Design Entry HDL.

Related Commands

Grid

Syntax

GRId {<cr>|[ON][OFf][Dots][Lines] [grid_size grid_multiple]}

Description

This command alters the grid display. A grid helps you place objects and ensure wire alignment and pin connections. The GRID command options can be used to turn the grid on or off, change the display to solid lines (the default) or dotted lines, and alter the default spacing. GRID <cr> toggles the grid on and off or you can specify ON or OFF. The current values of the grid spacing are displayed on the status line at the bottom of the screen.

Grid_size specifies the separation of the grid lines. Grid_multiple indicates how many lines of the grid are skipped before the next line is displayed. The default value for LOGIC drawings is 5 (2 for SYMBOL drawings). You can specify a positive integer to change the default grid multiple. Specify 1 to display every line, 2 to display every other line, and so on. Be aware that if you change the grid size, objects that were previously on a grid location may now be off-grid and wires may not be connected even if they appear so. (This is why you should use the right mouse button to connect wires to pins and other vertices.)

See also the SET command to change the default editor values.

Related Commands

Group

Syntax

GROup [group_name|DEFault][type...] {selection...| group_name | ALL}

where type is:

BOdies | PRoperties | NOtes | WIres | DOts.

and selection is:

{Lpoint Lpoint...Ctrl+Rpoint} | Ctrl+Rpoint | Mpoint

Description

This command allows the user to draw a polygon to specify the boundaries of a group. The group is defined as a collection of objects.

	If the first argument is a single-letter group name, that group will become the current group. If a group name is not specified, or DEFault is specified, a single-letter group name will be automatically assigned to the group that is created.
	The group selection can be restricted to a specified type or set of types by providing one or more of the type arguments.

For example, the command group A bodies properties includes only the components and properties among the objects you have selected for grouping in group A, even though there are notes, wires or dots among the objects you have selected for grouping.

	You can use the mouse to draw a polygon around the objects to be grouped. Click the left mouse button to start the line or to change the direction of the line. Complete the polygon by pressing Ctrl+right mouse button when the cursor is near the starting point. You can draw additional polygons to include other objects in the group.
	Press Ctrl and click the right mouse button to include individual objects in the group.

	Click the middle mouse button on another highlighted group to include its contents in the current group.
	Use the name of a previously created group to include its contents in the current group.

For example, the command group C A includes the contents of group A in group C.

Use ALL to select all objects in the current drawing.

For example, the command group A bodies all includes all the components in the current drawing in group A.

The console window displays the group name and the number of bodies, properties, notes, dots, and wires in the group.

Related Commands

Auto
Find
Include
Exclude
Select

HIEr_write

Syntax

HIEr_write

Description

This command writes the hierarchical blocks in a schematic starting from the level of hierarchy from which it is executed. For every block, the hier_write command writes all the page and netlisting files. It then generates marker files for every block in the schematic in the temp/hierwrite directory of the design.

The hier_write command is different from the write command as write command saves only the current page while hier_write saves all the pages in the hierarchy.

Highlight

Syntax

HIGhlight [Net | PArt | PIn | Any] pt

HIGhlight [Net | PArt | PIn | Any] object_name

Net, Part and Pin are used to specify the object type you want to highlight. You may use Any if you want all selected objects to be highlighted. This is also the default argument if you do not specify any object type.

pt	To pick a component to be highlighted, point to the object and press the left mouse button. Select a group by pointing to the desired group and pressing the middle mouse button.
object_name	If you prefer typing in the name of the object, you may do so by using the second version of this command.

For nets, the object name is the signal name of the net, for example, FOO.

For parts, the object name is the value of the PATH property attached to the component, for example, 7P.

For pins, the object name is the value of the PATH property attached to the component to which the pin belongs, followed by a period ("."), followed by the name of the pin, for example, 7P.A<SIZE-1..0>.

Wild cards such as "*" and "?" may be used in specifying the object name, for example, FOO*, 7*P, 7P.A*.

Description

The Highlight command is used to select objects in one tool and for operations by other tools in the system. For example, you could type in the open command in the simulator and then use the highlight net command in Design Entry HDL, to open a particular signal. Highlight is also used to allow the user to co-relate the same nets, parts and pins in the system. Thus, you could have your PCB layout tool and Design Entry HDL up at the same time and use the highlight part command in Design Entry HDL to highlight the component in both Design Entry HDL and the PCB layout tool.

If an object is already highlighted and you pick the object in the highlight pt version of the command, the object gets unhighlighted in the system. Thus, if you have selected a whole set of nets to open in the simulator, you could just double-click on the nets you want to select in Design Entry HDL and the net will be selected, but will not be left highlighted. However, if you type in the name of the object, it will be highlighted, even if it was already highlighted.

Related Commands

Dehighlight
Unhighlight

HMirror

Syntax

HMirror point

Description

This command is used to create a mirrored version of a selected symbol about horizontal axis (x-axis). To create a mirrored version of a symbol, type hmirror in the console window and select the symbol with the left mouse button.

Related Commands

Mirror

HPlot

Syntax

hplot [worklib/<schematic_name>/sch_1/module_order.dat]

Description

This command plots the hierarchical blocks in a schematic starting from the level of hierarchy from which it is executed. On UNIX, hplot reads the .cpm file of the design to determine whether it has to use Windows plotting or HPF plotting. You can set the Plotting Facility Windows or HPF) on UNIX using the Plotting tab in the Design Entry HDL Options dialog box.

In hierarchy mode, hplot plots a hierarchical block only once even if the block has multiple occurrences in a design. In occurrence edit mode, hplot plots all the occurrences of a hierarchical block in a design.

If you run the hplot command without any argument, it prints all the blocks in the schematic by reading the pc.db file of the schematic. If you specify the path of the module_order.dat file while executing the hplot command, hplot plots the blocks in accordance with the order specified in the file.

IGnore

Syntax

IGnore {directory_name | library_name | * | <cr> }

Description

This command causes a specified library and all its symbols to be deleted from the active search list. IGNORE <cr> ignores the design library. IGNORE * ignores all the project libraries in the current search list.

The IGNORE command prompts you to confirm that a library is to be removed from the search list. Click Yes to ignore the library. If the current drawing contains a part from the ignored library, that part is deleted from the screen and either turned into a placeholder or replaced if there is a part by the same name in another active library.

Example

To delete the lsttl library from the active search list:

1.	Type ignore lsttl in the console window.
2.	In the Design Entry-HDL confirmation window, click Yes.

imginsert

Syntax

imginsert [{filename} (starting coordinates)]

Description

Inserts an image into the schematic canvas. This command launches the Open dialog box from where you can select the image that you want to paste.

You can also insert an image at a pre-defined location from the command line.

Example

imginsert c:/abc.bmp (1000, 1200)

This command places the bitmap file, abc.bmp, at the specified location on the schematic.

imgstretch

Syntax

imgstretch [(starting coordinates) (ending coordinates)]

Description

Stretches a selected image horizontally or vertically on the schematic. You can also specify the starting and ending coordinates for stretching the image.

Example

imgstretch (1000, 1200) (1500, 2500)

imgcapture

Syntax

imgcapture [(starting coordinates) (ending coordinates)]

Description

This command captures screen shots of a selected part on a schematic. When you capture an image, it is copied to the clipboard from where it can be pasted into any graphics editor or a graphics-aware text editor such as Microsoft Word.

Example

imgcapture (1000, 1200) (1500, 2500)

where (1000, 1200) represent the starting coordinates and (1500, 2500) represent the ending coordinates.

Include

Syntax

INClude [group_name|Mpoint|DEFault][option...][selection ...| group_name]

where option is:

BOdies | WIres | PRoperties | NEts | Connections

and selection is:

Ctrl+Rpoint | Mpoint

Description

This command adds items or groups in the current group.

	If the first argument is a single-letter group name, the group will become the current group. Alternatively, click the middle mouse button on a highlighted group to make it the current group. If a group is not specified, or the word default is provided, the most recently created group will remain the current group.
	To add individual objects, click the left mouse button or press Ctrl and click the right mouse button.

	To add previously-defined groups, click the middle mouse button on a highlighted group or enter the single-letter group name.
	Option flags allow the user to include types of objects in a group. Options are applied to the objects in the initial current group and to any additions made to the current group by the include command.

		BODIES or WIRES include all bodies or wires that have properties already in the current group.
		PROPERTIES include all properties attached to objects already in the related group.

		NETS include all nets of wires attached to bodies or wires already in the related group.
		CONNECTIONS include all the objects connected to the pins of any symbol already in the chosen group.

Example

Include A pr

This command includes properties of all objects in group A to the group.

Related Commands

Exclude
Find
Group
Select

Library

Syntax

LIbrary {library_name | <cr> }

Description

This command adds the specified library to the search list.

LIBRARY <cr> accesses the Search Stack form that allows you to add or delete libraries in the active search list. The Search Stack form can be turned off by entering the command SET LIBFORM OFF.

To add a library directly, enter the LIBRARY command and the library_name value directly on the command line. The last library added to the list is searched after any previously specified directories are examined.

Related Commands

Loadstrokes

Syntax

LOADStrokes {strokes_file | <cr>}

Description

This command loads a user-defined strokes_file. Strokes are user-defined line drawings you create with the mouse. You can customize command entry in the editor by using strokes.

When you access the editor, a set of default strokes is initially read from the file <your_install_dir>/tools/fet/concept/concept.strokes. You can specify a file containing your own strokes by issuing the LOADSTROKES command at the keyboard or including the command in the START_CONCEPTHDL section of your .cpm file.

To draw a stroke, press and hold the right mouse button and drag to form the required stroke. If the stroke you enter does not match an existing stroke, an error message is produced. If you produce a valid stroke, the related command is executed.

Strokes must be entered in the same direction as they were created. This allows you to have two strokes that look the same but that are bound to different commands. For example, you may have two different strokes that both appear as diagonal lines but are bound to different commands. The difference is that one stroke is drawn from upper left to lower right, and the other is drawn from lower left to upper right. When you use the editor to view strokes, a cross signifies the starting point of the stroke.

To create your own strokes_file, or edit an existing strokes_file, you use the Stroke Editor. This system utility is used to create strokes for many applications.

LOADSTROKES <cr> brings up the File Browser form. You can then select the strokes_file from the form.

Related Commands

Strokefile

Mirror

Syntax

MIrror point

Description

This command is used to create a mirrored version of a selected symbol. If editing a symbol drawing, this command will not mirror all lines and arcs in the drawing about the Y axis. Justified text is shifted from left to right or right to left in the mirrored version. No other rotation is done.

The MIrror command should be used with caution, especially with bodies with unmarked pins, such as merge bodies. Reversing the bits causes subtle, hard-to-find errors in the design.

See SET LEFT/RIGHT and DISPLAY LEFT/RIGHT for justifying text, and the ROTATE, SPIN, and VERSION commands.

Example

To create a mirrored version of a symbol, type mirror in the console window and select the symbol with the left mouse button.

Related Commands

Display
Rotate
Set
Spin
Version

Modify

Syntax

MODify point

Description

This command modifies a selected part. Design Entry HDL displays the Physical Part Filter dialog box that lists all parts satisfying the selection criteria based on the properties attached to the selected component.

If the user selects a primitive from the popup, the package type corresponding to the primitive is used to seed the PACK_TYPE property in the .ptf file.

The old part is modified, the properties on the old part is now a union of the properties that existed on the old part and the properties on the new part. If the old part and the new part have the same property name but different property values,

- if multiple properties with this name can be legally attached, a new property identical to the one on the new part is attached to the old part

- otherwise, the value of the property on the old part is modified with the value of the property on the new part.

All error messages are displayed in the Design Entry HDL console window.

Example

1.	To modify a part, type modify in the console window.
2.	Click the part you want to modify in the design window.

The Physical Part Filter window appears.

3.	Select the new part in the Physical Part Filter window.
4.	Click Close.

The old part is replaced with the new part you selected in Step 3.

Procedures

	Modifying an object
	Modifying components in a group

Move

Syntax

MOVe {source_point destination_point|group_name destination_point}

Description

This command moves objects from one position to another in the current drawing or between drawings in different viewports. MOVE operates on groups or individual objects. Source_point is the object to move. Group_name is the name of a group to move. Destination_point is the new position of the group or object. Properties (excluding PATH properties) attached to objects are moved with objects. Properties can also be moved independent of objects. To undo the effect of moving objects from one viewport to another viewport, an undo command must be entered in each viewport.

To move a single object, type MOVE and position the cursor on the object to move. Press the left button to pick up the object that is nearest to the cursor (regardless of the grid setting) or the right button to pick up an object's vertex nearest the cursor. A vertex is defined as a symbol origin, symbol pin, a wire end, or a note origin. The right button is useful for moving bodies or off-grid objects. Move the object to its new location and press the left button to place the object on the grid point nearest the cursor or the right button to attach the object to the nearest vertex. Note that when using the right button for the source_point, any visible object is selected. The right button as a destination_point only considers symbol pins, symbol origins or wire ends as attachment points.

To move an object from off-grid to on-grid, type Move in the console window and press Enter. Keeping the CTRL key pressed, right-click on an off-grid component. The component will attach to your mouse pointer. To place the symbol on grid, (left-) click on the canvas. The symbol is placed at the closest grid point.

To move a defined group, specify the name of the group or press the center button to select the group to move.

MOVE preserves electrical connectivity when there are electrical connections (wires) leading to moved objects or groups. You can automatically re-route a wired part you have moved to another area of your design. You can move the part into place with the wires connected directly or orthogonally, or without wires as follows:

The first click of the middle button (while dragging) changes the shape of the wire from orthogonal to direct.

The second click of the middle button detaches the part from any wires and allows you to move the part freely.

The third click of the middle button re-attaches the wires and lets you drag the object the usual way until you place the object with the left button.

The wires are automatically re-routed only when you place the part with the wires connected directly (non-orthogonally) and the SET option AUTOROUTE is on (SET AUTOROUTE ON).

To move a whole wire and any attached object around the screen, select the middle of the wire. To lengthen a wire, select the outer third of the wire. When a wire is attached between two objects, you can move the wire and one object independently of the other object by selecting the wire nearest the object you want to move.

Procedures

	Moving text, wires, or an unwired component
	Moving a wired component

	Moving multiple objects
	Moving a group

Next

Syntax

NExt <cr>

Description

This command displays the items located by the FIND command. The NEXT command traverses the list of items found by the FIND command and draws a blinking highlighted rectangle around the item. You can perform an operation on the object and then issue the NEXT command to proceed to the next item. You can step through the list only once.

NEXT cannot be used after the CHECK command. Use ERROR after the CHECK command.

Related Commands

Note

Syntax

Note text_line... point...

Description

This command adds text strings to a drawing. Notes are text strings that appear on the drawing but do not affect the evaluation of the drawing. They are used to document a drawing. There are two ways to add notes to a drawing:

	Specify the points on the drawing where the notes are to be located and then type in the text. Press <cr> after each note to position each note on the drawing. As long as there are points remaining, the editor interprets entered text as notes to the drawing.
	Type in each line of text first and press <cr>. (You can enter several strings before placing them.) Then use the cursor and the left button to indicate where each note is to appear on the drawing.

Place quotes around notes beginning with an opening parenthesis. Notes within quotes are not interpreted as commands.

Related Commands

Filenote

Page commands

You can renumber the pages of a design through the _Page and Page commands:

_PAGE commands

	_PAGEInsert
	_PAGEDelete

	_PAGECompress
	_PAGEMove

_PAGEInsert

Inserts pages before or between existing or non-existing pages in a schematic. All subsequent pages are renumbered automatically and you need not worry about renumbering them manually. The maximum number of pages that you can insert in a single command is 250.

_PAGEInsert <Number_of_pages> <Location> [-nosave] [-noconfirm]

Number_of_pages	Indicates the number of pages to insert. The valid range is 1 - 250. This parameter must always precede the Location parameter.
Location	Indicates the location from where you want to insert the page(s). Pages are always inserted before the current page at the target location. To add pages at the end of the schematic, you would specify Location as one greater than the last page number. If you specify Location as more than one greater than the last page number, a page gap is created between the current last page and the first of the newly inserted pages. See Inserting Pages at the End of a Schematic .
-nosave	Keeps the newly inserted pages from being saved. Use this parameter to create page gaps in a schematic. This parameter can be placed anywhere in the argument list.
-noconfirm	Bypasses the message prompting you to confirm before executing the command. If you choose Cancel, the command is terminated. This parameter can be placed anywhere in the argument list.

Note: : Existing gaps in page numbers do not affect the _PAGEInsert command. If you insert a new page at a location where there is already a page gap, the command adds an additional page and the size of the page gap is unchanged.

Examples

The following examples of the _PAGEInsert command are explained in the context of different scenarios:

	Inserting Pages between Two Pages
	Inserting Pages at the End of a Schematic

	Inserting a Page Gap between Two Pages
	Inserting Pages Beyond the End of the Schematic

Inserting Pages between Two Pages

Initial page sequence: 1-10

_PAGEInsert 5 4

This command will insert 5 pages before page 4. The current page 4 will become page 9. All the pages will be saved and the corresponding Page* files will be created under the sch_1 directory. Finally, a message will display a summary of the newly inserted pages.

New page sequence: 1-15

Inserting Pages at the End of a Schematic

Initial page sequence: 1-15

_PAGEInsert 5 16

This command will add 5 pages starting from page 16. All the pages will be saved and the corresponding Page* files will be created under the sch_1 directory.

New page sequence: 1-20

Inserting a Page Gap between Two Pages

Initial page sequence: 1-3, 6-10, 12-15

_PAGEInsert 3 8 -nosave

This command will:

	Move pages, page 8 onwards, by three places to accommodate the new pages. As a result, the existing page 8 will become page 11.
	Insert a three-page gap - 8,9,10.

If you click the Next Page or Previous Page buttons to move to other pages, you will be prompted to save page 8. If you choose to save this page, the correspondingPage8.*files will be created and the page number count will increase by one.

New page sequence: 1-3, 6-8, 11-13, 15-18

However, if you choose not to save page 8, the result of the _PAGEInsert command would be a 3 page gap in the schematic at the point of insert.

New page sequence: 1-3, 6-7, 11-13, 15-18

Inserting Pages Beyond the End of the Schematic

Initial page sequence: 1-3, 6-10, 12-15

The -nosave option is of no value for this case as everything beyond the end of the schematic module is already blank.

_PAGEInsert 2 25 -noconfirm

This command will insert 2 pages starting from page 25. There will be a 9 page gap between pages 15 and 25. The confirmation message will be suppressed and the pages will be inserted without prompting you for confirmation

New page sequence: 1-3, 6-10, 12-15, 25-26

_PAGEDelete

You delete existent or non existent pages from a schematic by using the _PAGEDelete command. Unlike the existing PAGE DELete command, which leaves a page gap when you delete a page, the _PAGEDelete command does not create any page gaps, by default. As a result, the subsequent pages are automatically adjusted to reflect the new page sequence.

Syntax

_PAGEDelete <List_of_Pages> [-retain] [-noconfirm]

List_of_Pages	Indicates the pages to delete. You can specify an explicit number or a range of numbers. For example, 1,2,3,5-7, is a valid range. Spaces are not allowed between page numbers.
-retain	Retains the physical page numbers of the pages affected by the deletion. This parameter can be placed anywhere in the argument list.
-noconfirm	Bypasses the message prompting you to confirm before executing the command. If you choose Cancel, the command is terminated. This parameter can be placed anywhere in the argument list.

Note: The _PAGEDelete command can be used to remove specific page gaps. To remove all page gaps, use the _PAGECompress command.

Examples

The following examples of the _PAGEDelete command are explained in the context of different scenarios.

	Deleting Existing Pages
	Deleting Non-existent Pages

	Deleting Non-existent Pages out of Page Range
	Deleting Pages to Retain Physical Page Numbers of the Pages Following the Page(s) Being Deleted

Deleting Existing Pages

Initial page sequence: 1-15

_PAGEDelete 6-8

This command will delete pages 6, 7, and 8. The physical page numbers of all the pages following page 8 will be moved in by 3.

New page sequence: 1-12

Deleting Non-existent Pages

Initial page sequence: 1-3, 6-10, 12-15

_PAGEDelete 4 -noconfirm

If you try to delete a non existent page, the _PAGEDelete command will reduce the page gap between pages 3 and 6 by 1. Consequently, the pages after page 4 will move in by 1. The confirmation message will be suppressed and the pages will be deleted without prompting you for confirmation.

New page sequence: 1-3, 5-9, 11-14

Deleting Non-existent Pages out of Page Range

Initial page sequence: 1-3, 6-10, 12-15

_PAGEDelete 48

If you try to delete a non existent page, which is out of the page range of the schematic, it will result in an error:

Result: Command cannot be executed

Deleting Pages to Retain Physical Page Numbers of the Pages Following the Page(s) Being Deleted

Initial page sequence: 1-15

_PAGEDelete 6-8 -retain

This command will delete pages 6, 7, and 8. However, the physical page numbers of all the pages following page 8 will be retained. A gap of three pages will be created between pages 5 and 9.

New page sequence: 1-5, 9-15

_PAGECompress

You remove all the page gaps in a schematic by using the _PAGECompress command.

Syntax

_PAGECompress

Note: The _PAGECompress command does not accept any arguments.

Example

Initial page sequence: 1 4-5 10-13 15-17

_PAGECompress

New page sequence: 1-10

_PAGEMove

You move a sequence of pages to existent or non-existent locations in a schematic by using the _PAGEMove command. Unlike the existing PAGEMove command, which moves pages only at non existent locations, the _PAGEMove command allows page movement to existing pages of a schematic. Also, unlike the existing PAGEMove command, which allows only a single page move at a time, the _PAGEMove command allows you to move multiple pages, simultaneously. In addition, you can move non-contiguous pages to contiguous locations.

The _PAGEMove command works as a drag-and-drop functionality in a GUI, and does not create any page gap for the moved pages. As a result, the total page count remains the same. However, gaps existing in page numbers before the move command is executed are retained.

Syntax

_PAGEMove <List_of_Pages> <Before_Page > [-noconfirm]

List_of_Pages	Indicates the pages to move. This parameter must come before the Before_Pageparameter.
Before_Page	Indicates a location in the schematic where the pages will be moved. For example, if you specify 5 as Before_Page, the moved pages will precede the current page 5. To move pages to the end, specify a number, which is one greater than the last physical page.
-noconfirm	Bypasses the message prompting you to confirm before executing the command. If you choose Cancel, the command is terminated. This parameter can be placed anywhere in the argument list.

Examples

The following examples of the _PAGEMove command are explained in the context of different scenarios:

	Moving a Page before an Existing Page
	Moving a Set of Pages outside the Current Range of Pages

	Moving Non-contiguous Pages to Contiguous Locations
	Moving a Set of Pages to a Location which Falls within the Range of the Pages to be Moved

Moving a Page before an Existing Page

Consider a Team Design scenario where you have a team of three designers A, B, and C, working on a design. Each designer owns different sections of the design:

	Designer A is writing the CPU logic in pages 1-10
	Designer B is writing the CONTROL logic in pages 11-20

Designer C is writing the MEMORY logic in pages 21-30

After integrating the design, as a Team Lead, you realize that a part of the CPU logic created in pages 4-8 should be moved after the CONTROL logic between pages 14 and 15. You decide to move pages 4-8 by executing the following command:

_PAGEMove 4-8 15

This command:

1.	Moves pages 15-30 out 5 pages to make space for the 5 pages being moved.
2.	Moves pages 4-8 to the blank slots created in step 1

3.	Removes the 5 page gap (4-8) created in step 2 by moving all pages in by 5.

Moving a Set of Pages outside the Current Range of Pages

Initial page sequence: 1-3, 6-10, 12-15

_PAGEMove 6-9 17

This command will move pages 6-9 before the non-existent page 17 inserting pages backwards from page 16. Therefore, initial page 9 will be moved to page 16, the initial page 8 will be moved to page 15, and so on and so forth. All existing page gaps are maintained, but the page gaps created in the process of the move command are closed.

New page sequence: 1-3, 6, 8-11, 13-16

Moving Non-contiguous Pages to Contiguous Locations

Initial page sequence: 1-3, 6-10, 12-15

_PAGEMove 3,7,9 15 -noconfirm

This command will move pages 3, 7, and 9 before page 15. Pages 3, 7, and 9 will move to Pages 12, 13, and 14, respectively, and the other pages will be adjusted accordingly. The confirmation message will be suppressed and the pages will be moved without prompting you for confirmation.

New page sequence: 1-2, 5-7, 9-15

Moving a Set of Pages to a Location which Falls within the Range of the Pages to be Moved

Initial page sequence: 1-3, 6-10, 12-15

_PAGEMove 6-9 7

This command will result in an error as the target move location is within the range of the pages to be moved. A warning message is displayed and no action is taken.

Page

	page move
	page swap

	page delete
	page reset

page forcereset

page move

page move <@lib.cell(view)> X Y

Moves existing page X to a non-existing page Y.

Note: You cannot move a page to a page that already exists.

page swap

page swap <@lib.cell(view)> X Y

Swaps existing pages X and Y.

page delete

page delete <@lib.cell(view)> X

Deletes an existing page X.

Note: The move, swap, and delete commands cannot be executed on pages if:

	the page is currently being edited.
	the page is being edited, and changes in the page have not been saved.

Note: You need not save or repackage the design after you run the move or swap command. This is because the canonical names in the design do not change after you run the move and swap commands. If you run the delete command, you must save and repackage the design.

page reset

page reset X

Sets the existing page number to X.

This command sets the logical page number of the currently open page to X. X is a logical page number. When this command is run, Design Entry HDL first checks the existence of the logical page number X in the physical page files.This command is executed only if the logical page X does not exist in any of the physical page files.

page forcereset

page forcereset X

This command sets the logical page number of the currently open page to X. This command is the same as the pagereset command except for the fact that Design Entry HDL does not check for the existence of the logical page number X in any of the physical page files before setting the logical page number X to the currently open page.

You should keep the following points in mind while executing the page reset and page forcereset commands:

1.	To commit the change made by the pageforcereset or pagereset command, you have to save the page.To reflect this status, a * is shown on the Design Entry HDL title bar. If you want to de-commit the change made by any of these commands, do not save the page because you cannot undo the command.
2.	If two different physical pages have the same logical page number, and you try to save the design, Design Entry HDL displays an error message stating that the physical pages have the same logical page number. The message prompts you to use the page forcereset command and then save the schematic to resolve the page conflict.

You can then use the pageforcereset command to change the logical page numbers.

3.	Running the pageforcereset and pagereset commands makes the occurrence properties of objects, which are on renumbered pages, unusable. A message box appears informing you that the page reset command might make the opf properties for objects on the page unusable. You get the following error message:
4.	While cross-probing or globally locating objects, canonical names are shown with the logical page numbers. For example, the canonical name @top_lib.top.(sch_1):page2_i5 displayed in the Global Find dialog box means that the component that has the PATH=i5 property is located in the logical page 2 in the sch_1 view of the cell top in the library named top_lib.

Paint

Syntax

PAInt {color_name{point|group_name}|DEFault{point|group_name}} <cr>

Description

This command assigns selected colors to specified groups or objects. You can also enter the color_name on the PAINT command line, point to an object and press the left button. Select a group by entering the group_name or by pointing to the required group and pressing the center button.

PAINT DEFAULT paints objects or specified groups in their preset default colors. Use the SET COLOR commands (interactively or in the startup file) to establish default colors for the objects in your drawings. On a monochrome display, use the SHOW COLOR command to see what color an object is currently painted.

There are 16 available colors

	AQUA
	GREEN

	PINK
	SKYBLUE

	BLUE
	MONO

	PURPLE
	VIOLET

	BROWN
	ORANGE

	RED
	WHITE

	GRAY
	PEACH

	SALMON
	YELLOW

Procedures

	Specifying color of an object
	Specifying color for a group use

Pastespecial

Syntax

pastespecial [(starting coordinates) (ending coordinates)]

Description

Displays the Paste Special dialog box. Use this dialog box to specify whether you want to:

	Paste copied schematic parts on to the target schematic directly
	Change the signal names of the schematic before pasting them on the target location

Pause

Syntax

PAUse

Description

This command temporarily interrupts the editor until you press a key. PAUSE is useful in demos and scripts.

Pinnames

Syntax

PINNames point

Description

This command adds a PIN NAMES symbol to a schematic drawing that defines the functional circuitry of a symbol drawing. This is used in hierarchical design and in library development.

The PIN NAMES symbol is added to an unused area of the schematic drawing. Design Entry HDL automatically attaches the names of the pins on the corresponding symbol drawing to the PIN NAMES symbol in the schematic drawing, and appends a \I suffix (scope = interface) to each signal name. The signal names can then be reattached to signals in the schematic drawing. The use of the PIN NAMES symbol eliminates the need to retype the signal names and reduces the chances of mislabeling signal names or omitting the interface scope (\I) signal property.

Pinswap

Syntax

PINSwap {point1 point2 | pin_number point }

Description

This command swaps the pin number defined to be in the same pin group. This command can only be used after initial pin number assignment using the SECTION command. Also, pin swapping can only occur between pins that have been defined in the library as swappable. For example, it may be legal to swap the two input pins of a NAND gate, but not the input and output pins of the gate.

There are two ways to swap pins:

	Type PINSWAP and point to the two pins to be swapped.
	Type PINSWAP, type in a new pin number, and then point to an existing pin. The selected pin is swapped with the pin having the pin number you specified.

The properties attached by the PINSWAP command cannot be changed, they can only be deleted and moved. Once pins on a part have been swapped, the part cannot be resectioned using the SECTION command.

The PINSWAP command also swaps sections within HAS_FIXED_SIZE parts.

Related Commands

Backannotate
Section

Plot

Syntax

Plot

Plots the currently opened drawing

Plot cache

Plots all pages of the schematic named cache.

Plot cache.sym.1.1

Plots the symbol view of cache

Plot cache.sym.1.2

Plots page 2 schematic of cache

Plot cache.sch.1.*

Plots all pages of version 1

Note: To plot custom variables, you must open the design before running plot commands. Plot commands cannot evaluate the custom variables for unopened designs.

PPTAdd

Syntax

PPTAdd {"path"[",path"];}

Description

When using component selection in the physical mode, PPTADD provides the search path to locate the ppt files to be used.

The list of paths are pushed on to a stack. The last one specified is the first one searched.

This command replaces the SET PPTPATH option.

Related Commands

Add
PPTDelete

PPTDelete

Syntax

PPTDelete {"path"[",path"];}

Description

The PPTDelete command is used to remove paths to part table files used in the physical component selection. The command, however, does not affect the stack order.

Related Commands

Add
PPTAdd

PPTEcho

Syntax

PPTEcho

Description

When using the component selection in physical mode, PPTECHO lists the search path which will be used to locate the ppt files.

Related Commands

Property

Syntax

Property {attach_point location_point name_and_value | name_and_value attach_point location_point | attach_point name_and_value location_point}

Description

This command attaches a property name and a value to a specified vertex of an object. Properties allow you to associate information with selected objects on a drawing. The information is passed to other design programs for processing and analysis. A property consists of a name-value pair that is attached to an object (a symbol, pin, wire, or signal name). Operations on groups are not performed using the property command. Instead, use AUTO PROPERTY.

A property name can be any string of alphanumeric characters and underscores, provided that the first character is an alphabetic character. A property name cannot contain any spaces or punctuation marks except the underscore.

A property value can be any string of text up to 255 characters, including spaces and punctuation marks.

There are two ways to assign properties.

Type PROPERTY <cr>.

Select the objects where properties are to be attached. Use the left button for objects. Select as many objects as the number of properties you want to attach. Type the name and value of the property, separated by a space or an equal sign. Press <cr> after each property entry. The properties are attached to the selected objects in the same order as the initial selection.

Type PROPERTY <cr>.

Type the name and value of the property, separated by a space or an equal sign. Press <cr> after each property entry. Then specify the location on the drawing where the text of the property value should appear. Select as many objects as the number of properties you entered. The properties are attached to the objects you select in the same order as the initial property entries.

Each property attached to a given object, except the SIG_NAME property must have a unique name. If a newly entered property has the same name as a property currently attached to that object, the new property value replaces the old property value.

When a property is added to a drawing, only the property value appears. The SHOW PROPERTIES command temporarily displays the names and values of all properties on a drawing. The DISPLAY command changes the permanent display of property name and value pairs. The SET PROP_DISPLAY command controls the default display of added properties.

Quit

Syntax

QUIt <cr>

Description

This command terminates an editing session. The editor displays a message if there are unwritten changes to any drawings in the current editing session and asks you if you really want to quit. You must answer Y or YES to quit. Any other response aborts the command.

The EXIT command is the same as the QUIT command.

Related Commands

Exit

Reattach

Syntax

REAttach text_point attach_point

Description

This command reattaches properties (including signal names) from one object to another. For example, you can use the REATTACH command to attach a property from the input pin to the output pin of a device.

To reattach a property, type REATTACH and select the property. A line is drawn from the property to the current cursor position. Specify the new attach_point for the property. Use the MOVE command to position the property at its new attachment point.

Recover

Syntax

RECover <recover_log_file>

Description

This command is used for recovering drawings that were being edited when Design Entry HDL or your system crashed.

Every time you start Design Entry HDL, a temporary directory is created in the <project_directory>/temp directory. By default, xxnedtmp is the name of the temporary directory. If the xxnedtmp directory already exists, a xxnedtmp1 directory is created. If these two directories already exist, xxnedtmp2 is created, and so on. An undo log file for each drawing is stored in this directory. The name of the undo log file for the first drawing edited is undo1.log. The second drawing's undo log file is undo2.log, and so on.

Note: The temporary directory (for example, ./xxnedtmp) and all of its files are deleted if Design Entry HDL terminates normally.

An example illustrating the use of the recover command is:

RECOVER temp/xxnedtmp1/undo2.log

The recovered drawing is given a unique name (for example RECOVER1.SCH.1.1) and is only saved in the memory (not on disk). You should use the diagram command to change the drawing name and use write command to write the drawing out to the disk.

Related Commands

Diagram
Write

Redo

Syntax

REDo <cr>

Description

This command reverses the last UNDO command. The system keeps a list of operations performed during the current editing session in a log file. The UNDO and REDO commands perform their functions according to this log file.

Remove

Syntax

REMove [<directory>][name][.[type][.[version][.[page]]]]

Description

Deletes a drawing from a design directory. REMOVE allows only one argument at a time. Repeat the procedure to delete additional drawings. If no directory is given, REMOVE searches for the specified drawing in the currently active design directory.

To delete a drawing, type REMOVE and the name of the drawing to be deleted, and press <cr>. The editor displays the names of the files to be deleted and asks you if you really want to remove the files. You must answer Y or YES to remove them. Any other response aborts the command. The directory entries are deleted, and the files are purged.

Wildcards are allowed in drawing_name. A question mark matches any single character, and an asterisk matches any number of characters. If only the drawing_name is specified, REMOVE deletes all drawing types (SYMBOL, LOGIC, SIM, and so on), versions, pages, and files (ASCII, binary, dependency, and connectivity) of the specified drawing in the directory.

Replace

Syntax

REPlace {symbol_name point | symbol_name <cr> group_name}

Description

This command substitutes one part for another. The default version of the symbol is 1. Specify the version number to replace another version of a symbol.

There are several ways to use the REPLACE command.

	Type the name of the replacement part. Then use the cursor to point to the symbol or bodies to be replaced.
	Use the FIND command to group all the occurrences of a symbol to be replaced. Then, use the group_name option with the REPLACE command to globally change all the occurrences of the symbol. A message displays the number of bodies that are replaced.

Pin properties are reattached if a pin name on the new part is the same as a pin name on the first part. If the pin names do not match, the pin property becomes a symbol property.

All properties are retained except those generated by the BACKANNOTATE, SECTION, and PINSWAP commands. Unnamed signal names attached to the symbol are deleted. All default properties that have a value of ? receive the value of the property with the same name on the replaced symbol (if one exists). Wire connections to the original part are retained only if the pins are in the same location. The rotation of the original symbol is preserved when the symbol is replaced.

Procedures

	Replacing a component
	Replacing components of a group

Return

Syntax

RETurn <cr>

Description

This command returns to the previously edited drawing. If the current drawing is modified but not written, the system saves a copy of the drawing before returning to the previous drawing.

The SHOW HISTORY command lists the drawings that you edited during the current session.

The SHOW RETURN command lists the drawings that the RETURN command will return to in the order that they will be accessed.

Rotate

Syntax

ROTate point

Description

This command rotates a symbol or text string by 90 degrees, with mirrors at 180 and 270 degrees. When a symbol is rotated, all notes and properties are also rotated and translated. You can then act on the properties independently.

To rotate a symbol or text string, type ROTATE and then point to the object to rotate. Each time you press the button, the part rotates 90 degrees. In the 90 -degree rotation, symbol notes are rotated 90 degrees to the left in their original justification.

Rotating some parts 180 degrees reverses the order of the pins. This can cause subtle errors in your designs if pins become incorrectly wired. To avoid this, a 180-degree rotation of a part becomes a mirror of a 0-degree rotation (about the Y axis). A 270-degree rotation of a part is a mirror of a 90-degree rotation (about the X axis). To get the other two rotations and the other two mirrors, use the MIRROR command to create another version of the device.

See SET and DISPLAY for justifying text.

Related Commands

Add
Display
Mirror
Set
Spin

Route

Syntax

ROUTE point point

Description

This command draws a wire connecting two selected points. The ROUTE command connects two points by drawing a series of orthogonal line segments between them. If it cannot determine a route, it draws a diagonal line directly between the two points. ROUTE will not run a wire through any existing objects or vertices.

To select the nearest pin or wire vertex for a ROUTE point, use the right button to select the point. Use any other button to select the nearest grid point.

Related Commands

Broute
Bwire
Wire

s2l

Syntax

s2l design

Description

This command runs the s2l (short2long) command on the current design. To update only the current page, type

s2l

The s2l command should be run on designs that have been upreved from SCALD to Design Entry HDL having property names that exceed 16 characters.

Before you run this command, you should execute the following two commands:

uprev design

uprev_write

In SCALD designs, property names in Design Entry had a limit of 16 characters. For a property name that has more than 16 characters, Design Entry HDL assigns a new property name with a shortened version and the original property name (over 16 characters) as its value. The original value, which has more than 16 characters, is entered by the user in <your_install_dir>/tools/fet/pxl/allegroprp.dat.

When Packager-XL is run on the SCALD design, it replaces the shortened property name with the original property name after finding it in allegroprp.dat.

For example, the property ELECTRICAL_CONSTRAINT_SET is shortened to ELECTRICAL_CONST by Design Entry HDL. Design Entry HDL also assigns ELECTRICAL_CONSTRAINT_SET as the value for the ELECTRICAL_CONST property. When Packager-XL is run on the design, it converts ELECTRICAL_CONST to ELECTRICAL_CONSTRAINT_SET and passes the design to Allegro.

In HDL, Packager-XL does not perform this conversion. Instead, this functionality of Packager-XL is handled by the s2l command entered in the Design Entry HDL console command window.

The character limit for a property name in Design Entry HDL is now 31.

Scale

Syntax

SCAle {point1 point2 drawing_name | drawing_name point1 point2}

Description

This command smashes a drawing and includes it in the current drawing. Point1 and point2 indicate the size of the rectangle where the smashed drawing will be placed. Drawing_name is the name of the drawing to smash. All bodies are turned into wires, arcs, and text. SCALE is useful for creating documentation drawings and new bodies.

When a drawing is smashed, all connectivity information is lost. The drawing can no longer be interpreted by the Compiler.

Related Commands

Script

Syntax

SCRipt { file_name | <cr> }

Description

This command performs the commands listed in the specified text file. Script files let you change the default editor behavior. SCRIPT allows you to operate in the batch mode using the same syntax as if you typed in the command. You can use the mouse to enter points, or you can specify the X-Y coordinates in the script file.

The syntax for specifying the points is:

(X Y)

where X and Y can range from +16000 to -16000.

For example, the command vpdelete (0,0) will delete the viewport that has the coordinates (0,0).

You can configure a script to accept input during execution by including user input tokens in a script. User input tokens must be placed at the beginning of a new line. When the editor sees a user input token in a script, it highlights a menu button with the name of the editor command being executed. There are two user input tokens:

	$< When the editor encounters this token in a script, it prints from the token to the end of the text line as a prompt in the message window, and then waits for one item of input. The input can be a typed line, a function key press, a mouse action, or a Ctrl+C. You cannot use a <cr> as a response to a user input request.
	$; This token also prints from the token to the end of the text line as a prompt and awaits input. This token accepts and interprets inputs until you enter a semicolon. If this token is included, the editor follows the prompt with the message "Type ; when done with user input.”

To abort a script, press Ctrl+C. To abort at a user input token prompt, type a semicolon.

SCRIPT <cr> brings up the File Browser. The user can then select the names of the script file from the form.

The SCRIPT command will not recognize GED commands that begin with the word "FORCE" (such as FORCEPROP, FORCEADD, FORCEBUB, FORCENOTE, and FORCEQUIT).

Related Commands

IGnore
Library
Set
Use

Searchstack

Syntax

SEArchstack <cr>

Description

Accesses the SEARCHSTACK BROWSER form. This form lists the libraries and directories that are currently accessed through the USE or LIBRARY commands.

BROWSE opens or updates the DIRECTORY BROWSER form that lists the contents of a library or directory.

USE places the active directory at the top of the search list and makes it your current working directory. There is no limit to the number of directories and libraries that can be in use at one time.

IGNORE deletes the specified directory or library from the active search list. When you select a directory or library to ignore, the editor prompts you to be sure you want to ignore it. Move the cursor to the message window, type Y or N, and press <cr>. The specified directory or library is removed from the search stack.

LIBRARY accesses the AVAILABLE LIBRARIES form that lists all the available libraries. From AVAILABLE LIBRARIES, you can select any number of libraries to add to the active search list. As you select libraries, the library names appear in the SEARCHSTACK BROWSER form.

Section

Syntax

SECtion [pin_number]point

Description

This command displays different pin numbers for different sections of a symbol. The SECTION command lets you assign physical part sections to selected logical parts. As you step through the different sections of a symbol, the pin numbers of each section are displayed on the drawing. Sectioning a part automatically assigns path properties to the drawing.

If the logical part selected can be assigned to a section, the pin numbers for the section are displayed on the drawing. If the same part is selected again, the next section is selected and the new pin numbers are displayed. This makes it possible to step through all the different possible sections by pointing to the same part.

To assign a specific section directly, enter a pin_number that uniquely defines the section and then point to the part. This avoids having to step through each section individually.

To remove section information from a part, use the REPLACE command to replace the sectioned symbol with a new copy of the part.

You can section only parts with SIZE = 1 or HAS_FIXED_SIZE characteristics. To assign sections to a HAS_FIXED_SIZE part, point to the pin of the section to be assigned. To swap sections within a HAS_FIXED_SIZE part, use the PINSWAP command.

Example

To assign a specific section to an LS00 component, type section 11 in the console window and click the component in the design window.

Note: You can click the component again to change the section.

Related Commands

Backannotate
Pinswap
Set

Select

Syntax

SELect [group_name | DEFault][type...]{selection...| group_name |ALL}

where type is:

BOdies | PRoperties | NOtes | WIres | DOts

and selection is:

{Lpoint Lpoint} | Ctrl+Rpoint | Mpoint

Description

Provides a stretchable rectangle to specify the boundaries of a group. The group is defined as a collection of objects.

	If the first argument is a single-letter group name, that group will become the current group. If a group name is not specified, or DEFault is specified, a single-letter group name will be automatically assigned to the group that is created.
	The selection can be restricted to a specified type or set of types by providing one or more type arguments.

For example, the command select A bodies properties includes only the components and properties among the objects you have selected for grouping in group A, even though there are notes, wires or dots among the objects you have selected for grouping.

	You can click the left mouse button, drag the mouse to define the opposite corners of a stretchable rectangle which contains the objects to include in the group, and click again. You can draw additional rectangles to include other objects in the group.
	Press Ctrl+right mouse button to include individual objects in the group.

	Click the middle mouse button on another highlighted group to include its contents in the current group.
	Use the name of a previously created group to include its contents in the current group.

For example, the command select C A includes the contents of group A in group C.

Use ALL to select all objects in the current drawing.

For example, the command select A bodies all includes all the components in the current drawing in group A.

The console window displays the group name and the number of bodies, properties, notes, dots, and wires in the group.

Related Commands

Auto
Find
Group
Include
Exclude

Set

Syntax

SET {option | <cr>}

Description

This command establishes the default options for Design Entry HDL editor and overrides the project (.cpm) setting. The SET commands can be issued during an editing session or placed in the START_CONCEPTHDL section of your .cpm file.

Note: The SET commands in Design Entry HDL are temporary commands valid for the current session only.

SET <cr> accesses the Design Entry HDL Options dialog box. You can then use this dialog box to set different options. You can close the Design Entry HDL Options dialog box by typing SET SETFORM OFF in the Console Command window.

The SET command options listed below are grouped by the tabs they belong to in the Design Entry HDL Options dialog box. Related options (usually opposites) are listed together and are separated by a slash. The default is shown first. For example, in the save_workspace command option, ‘on’ is the default setting.

Most of the command options are Boolean in nature that can either be ‘on’ or ‘off’. The table below provides a single example of setting a Boolean option (save_workspace). The other Boolean options are set in a similar way. For all command options that are not Boolean, an example is provided in the following table. In addition, a single example is provided for command options that are similar, for example, changing the default color of objects, such as dot and wire.

SET Command Options	Description

General
save_workspace [on/off]	Saves window and toolbar settings when you exit Design Entry HDL. Example: set save_workspace on
click_to_type [on/off]	Activates a window when you click in it. Otherwise, a window is activated when you move the cursor into it.
autopan [on/off]	Enables panning behavior that lets you move the window over the drawing, rather than move the drawing inside the window.
rmb [on/off]	Changes the behavior of the right mouse button (RMB). If the option is turned off: Clicking right displays the context (pop-up) menu Pressing Ctrl+RMB causes a command-dependent action. If the option is turned on, this functionality is reversed, where clicking right causes a command-dependent action and pressing Ctrl+RMB displays the context menu.
multiformat_vectors [on/off]	Allows multiple-format signal names in the design. When you select this option: (), <>, and [ are considered special characters that designate a vectored signal. They cannot be used anywhere else in the signal name. The parentheses must be matched correctly and must contain either an integer or a parameter. Colon (:), comma (,) and ampersand (&) are considered special characters that represent concatenation. They cannot be used anywhere else in the signal name. When this option is not selected, ( ) and [ are considered legal characters that have no special meaning and can be used in signal names. They do not designate vectored signals. Only < > can be used to designate vectored signals. Comma (, ) and ampersand (&) are considered legal characters that have no special meaning and can be used in signal names. They do not represent concatenation. Only a colon (:) represents concatenation.
lmb [on/off]	Changes the behavior of the select and drag mouse operation and for running commands with strokes. If the option is turned off: Select an object on the schematic and drag the mouse to move the object. Press the left mouse button and drag the mouse to select multiple objects on the schematic. To exclude components, properties or wires from the selected objects, click the right mouse button and choose Exclude to exclude components, properties or wires from the selected objects. You can now click on one of the selected objects and drag the mouse to move all the selected objects. Press Ctrl or SHIFT and hold down the left mouse button to run commands with strokes. If the option is turned on: Press Ctrl, select an object on the schematic and drag the mouse to move the object. Press Ctrl or SHIFT, hold down the left mouse button and drag the mouse to select multiple objects on the schematic. To exclude components, properties or wires from the selected objects, click the right mouse button and choose Exclude to exclude components, properties or wires from the selected objects. You can now press Ctrl, click on one of the selected objects and drag the mouse to move all the selected objects. Hold down the left mouse button to run commands with strokes.
addform [on/off]	Opens the Add Component dialog box when you enter the add command in the console window and then press Return.
catform [on/off]	Displays the Category View tab by default when you open the Add Component dialog box or when you enter the add command in the console window and then press Return.
editform [on/off]	Activates the View Open dialog box when you enter the edit command in the console window and then press Return.
libform [on/off]	Activates the Search Stack dialog box when you enter the lib command in the console window and then press Return. If off, the current search stack is displayed.
ppt_browser [on/off]	Automatically opens the Physical Part Filter dialog box when you open the Add Component dialog box or when you enter the add command in the console window and then press Return.
preselect [on/off]	Activates the pre-select mode for Design Entry HDL menus.
default_page_border_name <name>	Specifies the name of the page border. Example: set default_page_border_name A SIZE PAGE
default_page_border_version <version>	Specifies the version of the page border symbol. Example: set default_page_border_version 1

Paths
ppt_optionset_path<path>	Specifies the path to the PPT Option Set file that you want Design Entry HDL to use by default. This file stores the default display settings for physical properties in the schematic and in the Physical Part Filter dialog box. Example: set ppt_optionset_path C:\MyDocs
attributes_dir <location of attribute files>	Sets the path for the location of attribute files, e.g. the default allegro_net.att is located at $CDS_INST_DIR/tools/fet/concept/attributes. Example: set attributes_dir $CDS_INST_DIR/tools/fet/concept/attributes
CAT_path <location of the directory that contains the category files>	Specifies the directory that contains the category (.cat) files used to organize components by category. The component categories are displayed in the Category View tab of the Add Component dialog box. The Add Component dialog box also loads the category files located in the libraries that you use in your project.

Graphics
MOVE_Orthog/MOVE_Direct	Draws wires that you move as Orthogonal or Direct.
ORthog_wire/DIrect_wire	Draws wires that you add as Orthogonal or Direct.
AUTORoute <ON/OFF>	Automatically routes a wire around objects when you move a component in the drawing.
AUTOHeavy <ON/OFF>	Automatically thickens a wire when you attach a bus signal name to it.
tap_add_signal [on/off]	Automatically inserts the specified tap symbol, bits, and wire names of bus taps when you use the tap command.
tap_body <symbol>	Specifies the tap symbol to be used in a schematic. Example: set tap_body tap
AUTODot <ON/OFF>	Automatically displays dots at wire connections.
DOTS_Filled/DOTS_Open	Adds open or filled dots at wire connections.
BOdy_dot_radius<integer>	Adjusts the diameter of dots at wire connections in symbol drawings. Example: set Body_dot_radius 25
LOgic_dot_radius<integer>	Adjusts the diameter of dots at wire connections in schematic drawings. Example: set Logic_dot_radius 25

Text
CAPSLOCK_OFF/CAPSLOCK_ON	Displays text as all caps.
SIZe <real>	Specifies the size of text (property name, property value, signal name, URL, or note) in the plotted schematic. The default value is 0.082 inches. Example: set size 1.000
CEnter_justified/LEft_justified/RIght_justified	Justifies text Left, Center, or Right.
user_editor <editor>	Specifies the text editor that Design Entry HDL displays for certain functions. Example: set user_editor wordpad
PIn_size <real>	Adjusts the size of the pin number displayed on the schematic to be larger or smaller. The unit is in inches. The pin number size is not related to Text Size you specify in this dialog box. Example: set pin_size 1.000
PRop_display<display_type>	Controls the way properties are displayed-Invisible, Name only, Value only, or Both name and value. Example: set prop_display Invisible
ROtate <ON/OFF>	Automatically rotates pin numbers that are attached to vertical pins.
STICKY_OFF/STICKY_ON	Deletes a default property from a schematic when the property has been deleted from a symbol drawing.
AUTOPath <ON/OFF>	Automatically attaches a PATH property to an added part.
pinprop_vis [on/off]	Controls the visibility of symbol pin properties when the symbol/component is instantiated on the schematic. Invisible does not display the symbol pin properties. Defined by Component makes pin properties visible or not depending on how property visibility is defined on the symbol. Example: Let us say that the symbol PQR.SYM.1.1 has the property NO_SWAP_PIN = TRUE attached to a pin on it. If the visibility for this property is set to Name in the symbol pin, and you select Defined by Component in Design Entry HDL, NO_SWAP_PIN will be visible on component PQR after it is instantiated on a schematic in Design Entry HDL. If you select Invisible, NO_SWAP_PIN will not be visible on the schematic, but will be visible in the symbol.

Color
COLOR_Arc <color>	Changes the default arc color. Example: set color_arc peach
COLOR_Dot <color>	Changes the default dot color.
COLOR_Wire <color>	Changes the default wire color.
COLOR_Note <color>	Changes the default note color.
COLOR_Property<color>	Changes the default property color.
color_body <color>	Changes the default body color.
occ_color <color>	Changes the default occurrence property color.
BACKground_color<color>	Change the default color for the drawing area. Example: set background_color red

Grid
DECimal/FRactional/Metric	Defines the grid type.
default_grid [on/off]	Displays or hides the grid.
default_grid [line/dot]	Displays the grid as Dots or dashed Lines.
default_grid <size> <mult>	Adjusts the grid size to be smaller or larger and displays every nth grid line to define where objects can be placed so that pins do not fall off-grid. This ensures the correct connectivity of wires and symbols. Example: set default_grid 0.150 6
default_body_grid [on/off]	Displays or hides the grid.
default_body_grid [line/dot]	Displays the grid as Dots or dashed Lines.
default_body_grid <size> <mult>	Adjusts the grid size to be smaller or larger and displays every nth grid line to define where objects can be placed so that pins do not fall off-grid. This ensures the correct connectivity of wires and symbols.
default_doc_grid [on/off]	Displays or hides the grid.
default_doc_grid [line/dot]	Displays the grid as Dots or dashed Lines.
default_doc_grid <size> <mult>	Adjusts the grid size to be smaller or larger and displays every nth grid line to define where objects can be placed so that pins do not fall off-grid. This ensures the correct connectivity of wires and symbols.

Plotting
wplot_thin_width	Specifies the width of lines used to draw thin wires, boundaries of components, and text on schematics. By default, the single line width is 1.
wplot_thick_width	Specifies the width of lines used to draw buses and thick wires on schematics. By default, the double line width is 10.
WPLOT_ADJust	Specifies the percentage by which to increase or decrease the size of the drawing. Design Entry HDL then plots the drawing on one or more papers of the specified size. For example, if you have a drawing with Cadence A size page border, the percentage specified is 100, and the paper size selected is A4. The Cadence A size page border is bigger in size than A4. So, the schematic is plotted on more than one A4 paper.
WPLOT_FIT_to_page	Adjusts the size of the drawing so that it fits into one page of the specified paper size. For example, you may have a drawing with Cadence A size page border, and the paper size selected is A4. Even though the Cadence A size page border is bigger in size than A4, the schematic is plotted so that it fits on one A4 paper.
Wplot_screen	Plots the portion of the schematic that is displayed on the screen.
Wplot_sheet	Plots an entire page.
WPLOT_PLOTTER	Sets the plotter to the name specified.

Output
AScii/NOAscii	Saves an ASCII representation of the logic.
BInary/NOBinary	Saves a binary representation of the logic.
CONFirm_write <ON/OFF>	Provides confirmation about saving the drawing.
DEPendency/NODependency	Saves an ASCII file with dependency information.

Check
CHECK_On_write <ON/OFF>	Runs a check whenever you save a design. Errors are recorded in cp.mkr and netlister.mkr.
CHECK_Missing_pins<ON/OFF>	Checks for pin properties that are no longer attached to pins.
CHECK_Unconn_wires<ON/OFF>	Checks for unnamed wires connected to only one pin (NC wires) and for named nets not connected to any pins.
CHECK_SHorted_pin<ON/OFF>	Checks for two pins on one component that are connected to the same wire, i.e. two pins shorted together.
CHECK_PARts_at_same_loc <ON/OFF>	Checks for overlaid components.
CHECK_Hidden_wires<ON/OFF>	Checks for wire segments hidden by portions of components.
CHECK_PIN_near_wire_endpt <ON/OFF>	Checks for wires that do not quite contact pins.
CHECK_Arcs_at_same_loc <ON/OFF>	Checks for overlaid arcs.
CHECK_PINS_at_origin<ON/OFF>	Checks for pins at the origin (0,0) in symbol drawings.
CHECK_TWo_wires_at_pins <ON/OFF>	Checks for wires overlapping a component at the pin.
CHECK_SIGNAMES <ON/OFF>	Checks for multiple names attached to the same signal.
CHECK_SIGNAME_in_body <ON/OFF>	Checks for the SIG_NAME property on a pin in a symbol file.
CHECK_Body_place_holders <ON/OFF>	Checks for placeholder components that appear due to changes in the related library.
CHECK_PRop_place_holders <ON/OFF>	Checks for placeholder properties that appear due to changes in the related library.
CHECK_PACk_sec_type_props<ON/OFF>	Checks for multiple SEC-type properties on an instance.

set NEXTgroup

This command sets the name of the group you want to create with the Find command.

If a group with the same name exists, this command resets the group and allows you to create a new group with the same name. For example, suppose that group A contains 2 properties. If you run the following console commands on a schematic that has two instances of the ls04 component, the new group A will contain 2 bodies:

set nextgroup A

find ls04

set HDL_Direct

This command sets options for the write console command. When you save a drawing, the write command is executed that writes the drawing onto the disk.

When the HDL_Direct option is on/off, the write command writes/does not write the following files in the sch_1 view of the schematic:

		verilog.v
		vhdl.vhd

		hdldirect.dat
		viewprps.prp

*.sir

Note: The hier_write and uprev_write console commands are not affected by the HDL_Direct option. These commands always write all the files onto the disk.

set sticky_on and set sticky_off

When you place a component on the schematic, the properties specified on the symbol for the component become the default properties for the instance of the component. You cannot delete the default properties for the instance.

If you delete a property or modify the property name on the symbol, the property may still be present on the instance of the component as a default property. These are called dangling properties. Design Entry HDL displays the following error message when it finds dangling properties on the schematic:

The default property <property> [with value <value>] is no longer on the body <symbol_name>. To turn the deleted default properties into non-default properties type SET STICKY_ON;GET;SET STICKY_OFF.

Note: The dangling properties will not be visible on the schematic or in the Attributes dialog box.

If you want the dangling properties to be converted to non-default properties, run the following console commands in the following order:

set sticky_on

get

set sticky_off

The dangling properties become visible on the schematic or in the Attributes dialog box. The non-default properties are applicable only to the instance of the component in the schematic. You can delete the non-default properties on the component.

	If you want to delete the dangling properties, do the following:
	a.	Run the set sticky_off console command.

Run the write console command or choose File – Save to save the schematic.

Show

Syntax

SHow {option |<cr>}

Description

This command temporarily displays objects or information on classes of objects. The temporary information is erased when you redraw the screen.

To see all the SHOW options, type SHOW <cr> in the console window. The available SHOW options are displayed in the console window. The various SHOW options are described in the table below.

Attachments

Displays a line between visible properties and the property owner

COLor pt

Displays the color of the selected object

The color is displayed in the Design Entry HDL console window and as ticker text in the status bar.

COOrdinate pt

Gives the editor the location of the specified point in coordinates

DISTance pt pt

Displays the distance between two selected points.

	Clicking the left mouse button at two grid points displays the distance between the two grid points.
	Clicking the middle mouse button (in a three button mouse) or Ctrl+left mouse button at two points on the screen displays the distance between the two screen points.

The distance is displayed in the Design Entry HDL console window and as ticker text in the status bar.

Group pt

Highlights the group and lists the group name and contents. You can also specify the group by name.

History

Lists all drawings read in during the editor session

Keys

Lists the command string assigned to each function key

Modified

Lists drawings in all viewports that were modified but not saved during the editor session

Net pt

Highlights the selected net and displays the net name. You can also specify the net by name.

The net name is displayed in the Design Entry HDL console window and as ticker text in the status bar.

Origins

Displays an asterisk at each object origin (including text) on display

PIns

Displays an asterisk at each pin on display

PRoperties

Displays the names and values of all properties on the display (including any invisible properties)

PWd

Displays the name of the current project directory

The current directory is displayed in the Design Entry HDL console window and as ticker text in the status bar.

RELease

Lists the date and number of the current version of the editor

RETurn

Lists all the drawings that the editor can return to, in the order of return

Size pt

Displays the size of the selected text string (property name, property value, URL, signal name, note) in inches.

The text size is displayed in the Design Entry HDL console window and as ticker text in the status bar.

VECtors pt

Displays the pin names of the selected symbol

Example

To display the color of an object, type show color and click the object in the design window. The color of the selected object is displayed in the console window.

Signame

Syntax

SIGname {point signal_name | signal_name point }...

Description

This command attaches signal names to wires or pins. There are two ways to attach a signal name.

	Type SIGNAME and point to the location for each signal name. A rectangular box appears at each location. Type the text for the signal name and press <cr>.
	Type SIGNAME and enter one or more signal names. Specify the points to place the signal names on the drawing. The signal name is attached to the wire or pin that is closest to the specified point.

Signal names are handled internally as properties. For example, attaching a signal called BUS ENABLE to a wire is equivalent to attaching a property SIG_NAME=BUS ENABLE, to that wire.

When editing a SYMBOL drawing, signal names are known as PIN_NAME properties. They can be attached only to pin connections.

Related Commands

Smash

Syntax

Smash {point | group_name}...

Description

This command breaks a symbol into individual wires, arcs, and notes. Any properties attached to the symbol are deleted. The SMASH command works on individual bodies and on groups.

The SMASH command is useful for creating library symbol drawings. For example, once a 2-input AND gate exists, N-input AND gates can be made by using the following commands:

edit N AND.body

add 2 AND <pt>

smash <pt>

Attach the N inputs and write the drawing. Because 2 AND is no longer a symbol, the editor writes the drawing instead of producing an error message as it does when a symbol is added to a symbol drawing.

Procedures

	Smashing a component
	Breaking up components in a group

Related Commands

Filenote
Scale

Spin

Syntax

SPIn point...

Description

This command changes the orientation of text strings and components. Spins are in 90-degree increments (0, 90, 180, and 270). When you spin a symbol, all notes and properties are also spun and translated. You can then act on the properties independently.

The SPIN command does a true rotation of the symbol, as opposed to the ROTATE command, which mirrors for 180 and 270 degrees. Use SPIN with care; allowing 180-degree rotations of devices may reverse the order of the pins (for example, in mergers). This can cause subtle errors in a design.

Related Commands

Mirror
Rotate
Set
Version

Split

Syntax

SPLit point point...

Description

This command splits a single wire into two wires or separates two or more objects that are placed at the same location. The currently selected item blinks so you know what you have selected.

To split a single wire into two wires, type SPLIT and select a point along the wire with the mouse. If you want to separate the end of a wire from some objects, point near the end of the wire. If you want to break a wire into two attached segments, point near the middle of the wire. This creates a bend in the wire at the selected location. Select and position the appropriate section of the wire.

To disconnect two or more items at the same location, type SPLIT and select a location. One of the objects at that location is attached to the cursor and can be moved on the screen. Select the original location again to separate the second object. Continue to select objects until the correct item is attached to the cursor. You can cycle through the objects repeatedly. Move the object to its new location and click the mouse to place the object.

Strokefile

Syntax

Strokefile {strokes_file | <cr>}

Description

This command loads a user-defined custom strokes_file. Strokes are user-defined line drawings you create with the mouse. You can customize command entry in the editor by using strokes.

When you access the editor, a set of default strokes is initially read from the file <your_install_dir>/tools/fet/concept/concept.strokes.

You can specify a file containing your own strokes by issuing the STROKEFILE command at the keyboard or by including the command in your START_CONCEPTHDL section of your .cpm file.

To use a stroke, press and hold the left or center mouse button and draw the required stroke. If the stroke you enter does not match an existing stroke, an error message is generated. If you draw a valid stroke, the related command is executed.

STROKEFILE <cr> brings up the Browser. You can then select the strokes_file from the form.

Related Commands

Loadstrokes

Swap

Syntax

Swap point1 point2...

Description

This command swaps two properties or two notes. Only two notes or two properties can be swapped, not a note and a property. Default properties and those generated by the PINSWAP, SECTION, and BACKANNOTATE commands cannot be swapped.

System

Syntax

System {operating_system_command | <cr> }

Description

This command accesses the operating system. To execute a particular system command, enter it on the same line as the SYSTEM command. Without an argument, the editor provides an interactive shell. You are connected to the operating system and can run any operating system commands.

To exit from the operating system and return to the editor, type Ctrl-D or Exit on UNIX-based systems and EXIT on Windows-based systems.

Tap

Syntax

TAp bus_tap_value point point...

Description

This command taps a bit or a set of bits from a bus and wires them to a pin. The bus_tap_value is the bit or set of bits you want to tap off the bus. You can enter any number of bus_tap_value(s) before you start selecting points. There are two modes of this command. In mode 1, you first select the pin you want to tap to and then the bus to tap from. In mode 2, you first choose the bus and then choose the pin.

Mode 1:

1.	Enter one or more bus_tap_values -- such as 3..0, 5, 2 etc. separated by CARRIAGE_RETURNs. If you do not enter a bus_tap_value, a question mark is used for the tap bits.
2.	Choose the pin you want the tap to go to. Use any mouse button. Now, you have a wire attached to the mouse.

If you click at a point with the left mouse button (and the point is not too close to a bus, you will get a kink at the point you clicked and you can keep drawing your wire. If you choose a point very close to a bus, or you use the middle or left mouse buttons, the command will find the closest bus, and draw a wire from your last point to the bus. It also adds a tap symbol, called "CTAP" by default, between your bus and the wire. The BN property on the tap symbol will be given the appropriate value. If the set option TAP_ADD_SIGNAL is ON, a signal name will be attached to the wire, specifying the bus name the tap has gone to and the bits tapped assuming that the bus you tap from has a vectored name.

The next signal name you entered will be used for the next tap (i.e. go back to step 1 or 2).

Mode 2:

1.	Enter one or more tap names -- such as 3..0, 5, 2 etc. separated by Carriage Returns If you do not enter a tap name, a question mark will be used for the tap bits.
2.	Choose the bus you want the tap from. Use any mouse button.

Now, you have a wire attached to the mouse. If you click at a point with the left mouse button (and the point is not too close to a pin, you will get a kink at the point you clicked and you can keep drawing your wire. If you choose a point very close to a pin, or you use the middle or right mouse buttons, the command will find the closest pin, and draw a wire from your last point to the pin. It will also add a tap symbol called "CTAP" by default, between the bus you chose and the first wire segment. It will give the BN property on the pin of the CTAP symbol the bits you specified. It will add the signal name to the wire you are adding if you so desire (specify your choice with the set variable TAP_ADD_SIGNAL).

Note: In this mode, you can terminate the tap wire, by clicking at the same point twice, (with the YELLOW (left) mouse button) after the tap symbol has been added. This is useful if you haven't yet added the component you want the tapped wire to go to, or you want the tapped wire to go to another wire etc.

4.	The next signal name you entered, will be used for the next tap (i.e. go back to step 1 or 2).

Advanced User Section

Restrictions: The tap command works with very specific kinds of tap bodies.

Rules for creating a tap symbol are

The tap symbol should

	Have exactly two pins.
	One pin MUST be at the origin of the symbol.

	This pin may NOT have a BN property attached to it.
	The second pin MUST be located on the positive x axis i.e. its coordinates should be (x, 0), where x > 0.

	The second pin MUST be on a grid point.
	The second pin MUST have a BN property.

It is recommended that the first pin have a \NAC \NWC on it and the second pin have a \NAC.

As a default the tap symbol CTAP from the standard library is used. If you want to change the tap symbol, use the command

set TAP_BODY <yourtapname>

For example,

set TAP_BODY ktap

Related Commands

Bustap

Textsize

Syntax

textsize <size in inches> <group name>

to change text size of properties in a group.

textsize <size in inches> Click on property

to change text size of a property.

textsize <size in inches> Click on note

to change the text size of a note.

You can specify a text size that has up to three decimal places. The minimum text size that you can specify is 0.008 inches and the maximum is 1.740 inches. The text size you specify should be a multiple of 0.002 inches.

Note: The above commands change the size of text in the plot.

Procedures

	Setting text size of a property or a note
	Changing size of text in a group

Undo

Syntax

UNDo <cr>

Description

This command undoes the operation of the previous drawing command. The editor keeps a list of operations performed during the current editing session. Repeated applications of UNDO reverses the effects of events according to this list.

You can undo past a write to the beginning of a session if you edit a single drawing, write it, and then continue to edit the original drawing. If you edit a second drawing immediately after writing the first, and then return to the first drawing, you cannot undo past the point where you accessed the second drawing.

UNDO only affects the current drawing. For example, to undo the move command used to transfer an object from one drawing to another, type UNDO in the destination drawing to remove the object, and then type UNDO in the original drawing to replace the object.

Note: If you have performed an operation relating to the addition of a component, which has a property whose value exceeds 256 characters, and want to reverse the operation, the UNDO command will not work.

Related Commands

Redo

Unhighlight

Syntax

UNHighlight [ Net | PArt | PIn | Any ] pt

UNHighlight [ Net | PArt | PIn | Any ] object_name

Net, Part, and Pin are used to specify the object type you want to unhighlight. You may use Any if you want all selected objects to be unhighlighted. This is also the default argument if you do not specify any object type.

There are two ways to select an object:

To pick a component to be unhighlighted, point to the object and press the left button. Select a group by pointing to the required group and pressing the middle button.

object_name

If you prefer typing in the name of the object, you may use the second version of this command.

For nets, the object name is the signal name of the net, for example, FOO.

For parts, the object name is the value of the PATH property attached to that part or component, for example, 7P.

For pins, the object name is the value of the PATH property attached to that part or component to which the pin belongs, followed by a period ("."), followed by the name of the pin, for example, 7P.A<SIZE-1..0>.

Wildcards such as * and ? may be used in specifying the object name,

for example, FOO*, 7*P, 7P.A*.

Description

The Unhighlight command is used to unhighlight an already highlighted object throughout the system.

Related Commands

Highlight
Dehighlight

Unix

Syntax

UNIx {operating_system_command | <cr> }

Description

This command accesses the Unix operating system. To execute a particular system command, enter it on the same line as the UNIX command. Without an argument, the editor provides an interactive shell. You are connected to the Unix operating system and can run any operating system commands.

To exit from the operating system and return to the editor, press Ctrl-D or type Exit on UNIX-based systems.

On Windows-based systems, the unix command opens up the command prompt. To know more about accessing the operating system from Windows-based system, refer to the System command help.

Example

To execute a particular Unix command, for example ls:

1.	Type unix ls in the console window and press Enter.

The files and folders in the project directory are listed.

2.	To exit from the operating system and return to the editor, press Ctrl-D or type Exit.

Updatesheetvars

Syntax

updatesheetvars

Description

This command updates the custom text variables for page numbers on all pages in a design.

Use

Syntax

Use {library_name | <cr>}

Description

This command specifies a working library. Library_name refers to the name of the library you want to use. If the library is not in the current directory, include the pathname.

USE places the specified library at the top of the active search list, and it becomes your current working library. If the library has been previously specified, it is moved to the top of the library search stack.

There is no limit to the number of libraries that can be in use at one time.

USE <cr> brings up the file browser form. The user can then select a library_name from the form.

Related Commands

Directory
IGnore
Library

Vectorize

Syntax

VECtorize

Description

Note: This command works only on Solaris.

This command creates a file named vector.dat, which contains a vector plot format version of the current drawing. This file can be used to transmit files to other machines or drive a pen plotter (with the aid of a format conversion program).

Version

Syntax

VERsion {point | group_name}...

Description

This command selects an alternate version of a symbol. Some bodies are created with different symbolic representations. For example, the NAND gate is equivalent to an INVERT-OR gate by DeMorgan's Theorem. A NOR gate is equivalent to an INVERT-AND gate. All versions of a symbol refer to the same logic drawing.

To step from one representation of a symbol to another, type VERSION and point to a symbol. The editor determines the current version of the symbol and displays the next version in the sequence. Continue pressing the mouse button to cycle through all the symbol versions. After the last version of the sequence is displayed, the first version is redisplayed.

You can use the FIND command to group all occurrences of a specified symbol, and then issue the VERSION command with the group_name option to globally change the drawing. The center button changes the version of the bodies in the group closest to the cursor.

The separate versions of a symbol must all make reference to the same logic drawing. Using a different version of a symbol has no influence on the logic drawing defining it.

Procedures

	Versioning a component
	Versioning components of a group

Related Commands

Add
Replace
Rotate

Vpadd

Syntax

VPAdd <cr>

Description

This command creates a new viewport. Viewports let you look at different views of the same drawing or open different drawings at the same time. You can zoom the windows independently to focus on different sections of the design, use the WIRE and ROUTE commands to connect points between viewports, and use the new viewport as a global view of the original design.

When you create a viewport, the current drawing is copied to the new viewport and fit to the size of the window. Any operations you perform in either window appear on both copies of the drawing.

Select the active viewport by placing the cursor within the viewport. If the SET command option CLICK_TO_TYPE is ON, click the left mouse button within the window in order to make the window active.

To edit a different drawing, make sure the cursor is in the correct viewport and use the EDIT command to access the new drawing. When you edit different designs simultaneously, you can use the COPY and MOVE commands to share information between the drawings.

No matter which viewport is active, all commands and system responses appear in the message window of viewport1 (the main viewport). The message window is not considered a part of viewport1. If you move the cursor from one viewport into the message window of viewport1, the system still considers the viewport you were in as the active viewport. To activate viewport1, make sure the cursor enters the graphic window area of the viewport.

To move a viewport, place the cursor in the title bar of the viewport, press and hold the left mouse button, and move the viewport to the new location. To resize a viewport, place the cursor in a corner of the viewport, press and hold the left mouse button, and resize the viewport.

Vpdelete

Syntax

VPDelete point...

Description

This command deletes an existing viewport. VPDELETE remains active until you enter a semicolon or select another command.

To delete a viewport, click the left mouse button in the viewport. Any drawings that are active in the viewport are not saved but are noted as being modified drawings. Use the SHOW MODIFIED command to list drawings that have been changed but not written. To save the modified drawings, edit the drawing in another viewport and issue the WRITE command.

Related Commands

Vpadd

Window

http://support.cadence.com/wps/mypoc/cos?uri=deeplinkmin:DocumentViewer;src=pubs;q=/conref/conref16.3/conrefIX.html

Syntax

WINdow {; | Down | Fit | In | Left | Out | Previous | point;|point point; | point point point |Right | scale_factor |Up}...

Description

This command changes the view of the current drawing. WINDOW can use up to three arguments. If there are fewer than three arguments, terminate the command with a semicolon.

The command options are

WINDOW	Redraws the image without changing the center or scale. This refreshes the screen and clears all messages.
DOWN	Repositions the center of the screen down below the drawing (moves the drawing up on the screen).
FIT	Fits the drawing to the entire screen.
IN	Enlarges the size of the drawing on the screen.
LEFT	Repositions the center of the screen to the left of the drawing (moves the drawing right on the screen).
OUT	Reduces the size of the drawing on the screen.
PREVIOUS	Switches from the current window scale and positions to the previous window scale and position.
Pt ;	Pans the drawing and makes the point the center of a new screen display of the drawing. The scaling of the drawing remains the same. Use the right button to enter the single point.
Pt pt ;	Defines a rectangle with the specified points at opposite corners. The rectangle expands to fill the screen, providing a close-up view of the specified portion of the drawing.
Pt pt pt:	Changes the size of the drawing depending on the ratio between the points. The first point defines the new center of the drawing, and the display becomes either larger or smaller, depending on the other points. The drawing is redisplayed with the first point at the center. If the distance between the first point and the third point is greater than the distance between the first point and the second point, the items appear larger; if the distance is smaller, items appear smaller.
RIGHT	Repositions the center of the screen to the right of the drawing (move the drawing left on the screen).
Scale_factor	Enlarges or reduces the drawing by the specified factor. The center of the window remains the same.
UP	Repositions the center of the screen above the drawing (move the drawing down on the screen).

Related Commands

Wire

Syntax

WIRe {[signal_name] point point}...

Description

This command adds wires to a drawing. The wire begins at the first point specified and runs to the second. Specify additional points to draw a wire with more segments. To snap the wire to the nearest vertex, press the right button.

To end a wire at a pin, dot, or other wire, press the left button.

To end a wire in a free space, press the left button twice at the final point.

Because schematics almost exclusively use orthogonal wires, the default wire mode is orthogonal (bent). Once the wire is started and the cursor changes direction, the attached wire remains orthogonal, whether the cursor is moved horizontally, vertically, or diagonally. To bend a wire, press the left button. Press the center button to change the orientation of the bend. If you press the center button a second time, the wire becomes diagonal. A third press returns the wire to the first orthogonal position.

If you enter a signal_name, the wire will be given that signal name.

See the BWIRE, BROUTE, ROUTE commands. See also the SET and SHOW commands to change default wiring behavior.

Related Commands

Write

Syntax

WRite [<directory>][drawing_name][.[type][.[version][.[page]]]] | <cr>

Description

This command writes the current drawing onto the disk. WRITE always asks for confirmation to write a drawing, even if no errors exist in the drawing. This is a safety feature to prevent unintentional writes. <DIRECTORY> is the directory where the drawing resides. If no directory is given, the drawing is written to the directory from which it was retrieved. If you write a newly-created drawing without giving a directory name, the drawing is written to the current directory. If only a directory name is given, the drawing is written into the specified directory. This is useful when copying drawings between directories.

DRAWING_NAME is the name of the drawing to write. If no drawing_name is specified (WRITE <cr>), the drawing is written to the file name shown on the status line at the top of the display. If no drawing type, version number, or page number are specified, the default is SCH.1.1.

If you enter a drawing name and a drawing with that name already exists in a directory, a warning message is displayed. Type YES to overwrite the existing drawing with the new drawing. Type NO to cancel the write.

Related Commands

Zoom

Syntax

Zoom{;| Down |Fit |In | Left | Out | Previous | point; | point point; | point point point | Right | scale_factor | Up }...

Description

This command reduces and enlarges portions of the drawing on the screen. ZOOM can use up to three arguments. If there are fewer than three arguments, terminate the command with a semicolon. The command options are:

ZOOM	Redraws the image without changing the center or scale. This refreshes the screen and clears all messages.
FIT	Fits the drawing to the entire screen.
LEFT	Repositions the center of the screen to the left of the drawing (moves the drawing right on the screen).
PREVIOUS	Switches from the current window scale and position to the previous window scale and position.
Pt pt	Defines a rectangle with the specified points at opposite corners. The rectangle expands to fill the screen, providing a close view of the specified portion of the drawing.
RIGHT	Repositions the center of the screen to the right of the drawing (moves the drawing left on the screen).
U	Repositions the center of the screen up above the drawing (moves the drawing down on the screen).
Scale_factor	Enlarges or reduces the drawing by the specified amount. The center of the window remains the same.
Pt pt	Changes the size of the drawing depending on the ratio between the points. The first point defines the new center of the drawing, and the display becomes either larger or smaller, depending on the other points. The drawing is redisplayed with the first point at the center. If the distance between the first point and the third point is greater than the distance between the first point and the second point, the items appear larger. If the distance is smaller, items appear smaller.
Pt	Pans the drawing and make that point the center of a new screen display of the drawing. The scaling of the drawing remains the same. Use the right button to enter the single point.
OUT	Reduces the size of the drawing on the screen.
IN	Enlarges the size of the drawing on the screen.
DOWN	Repositions the center of the screen down below the drawing (moves the drawing up on the screen).

Procedures

	Zooming in and out of a drawing
	Panning the drawing

Related Commands

Window

Reply

Jerry GenPart over 15 years ago

Hi Alastair,

You can go to - http://support.cadence.com

and select this document:

Look in the Index for the “console commands” and you’ll see them all listed. You can click the links to

get a complete description of the commands.

Below is the complete list from the link above –

Jerry

Allegro Design Entry HDL Reference Guide

Product Version 16.3 December 2009

Console Command Reference

Add

Syntax

ADd [component_name][.view][.version] [point] [point...] | <cr>

ADD <cr> accesses the Component Browser dialog box. You can use this dialog box to add components to the drawing. The Component Browser dialog box can be turned off by typing in SET ADDFORM OFF.

Use the REPLACE command to substitute one component for another.

Dialog Boxes

Add Component-Library View

Add Component-Category View

Related Commands

Arc

Syntax

ARc point1 point2 { point3 | ; }

Description

This command creates arcs, usually on symbols. The two points define the ends of the arc. The curvature of the arc is controlled dynamically by dragging the mouse after you place the second point.

Click to place the arc at the nearest screen pixel. Click the center button to place the arc at the nearest grid intersection (useful when building accurate semicircles or matching mirrored arcs).

Typing a semi-colon after placing the second point will create a circle.

Related Commands

Circle

Assign

Syntax

Assign function_key "quoted-string"

Description

For example,

ASSIGN F2 "zoom fit"

ASSIGN <shift>F2 "zoom in"

ASSIGN <cntrl>F2 "zoom out"

Function key names correspond as closely as possible with the text printed on the keyboard. The function keys for the various systems are:

IBM: F6-F10, F12, 4-9, page up/down, the directional arrows

Sun: F1-F9, R4-R12

SHOW KEYS lists the current function key assignments. ECHO <key press> displays the key name or the assignment.

Attribute

Syntax

Attribute point

Description

Procedures

	Adding Properties
	Displaying and Modifying Property Attributes

Making an Attribute File

Auto

Syntax

AUto {PAth | Dots | Undot | PRoperty group_name prop_name prop_value . . }

Description

This command performs the global addition or deletion of certain objects to or from a drawing.

	PATH automatically assigns unique PATH numbers to bodies on a drawing that do not already have a PATH property. (Some special editor bodies and bodies labeled with a COMMENT property are not assigned PATH properties.) The path property is in the form 'PATH = In', where n is a unique integer.
	DOTS places a dot at each wire connection on the current drawing. Open dots are the default value. To specify filled dots, type SET DOTS_FILLED before entering AUTO DOTS.

UNDOT removes all dots from the drawing except those at the intersection of four wires.

See also the SET DOTS_FILLED and SET DOTS_OPEN commands.

Auto Commands

Using the auto dot command

1.	When set autodot is off, type

show connections

This command places asterisks temporarily on the drawing to highlight each connection point.

2.	Check the drawing to make sure that no connections have been made by mistake.
3.	Use the refresh command to remove the asterisks from the screen.

Type

auto dot

All the junctions are automatically dotted.

Using the auto undot command

To remove the dots of the same size as the present dot size settings at intersections in a drawing type

auto undot

Note: You cannot use the auto dot and auto undot commands separated by a semi colon (;) on the same line in the console window. The following usage results in an error:

auto dot; autoundot

Using the auto allundot command

To remove all the dots at the intersections in a drawing type

auto allundot

Changing Dot Size

	If you change the size of a dot, the change is not reflected on filled dots in the schematic, however, when you plot the schematic, the change in size gets reflected.
	Change in size is also not reflected in dots that existed previously, it appears only in the dots that you add after changing the size. So, if you want to make all the dots of the same size, first use autoundot to remove the dots within the size specified in logic dot radius, or autoallundot to remove all dots regardless of size. Then add the dots again using auto dot.

Using the auto netprop command

Use this command to apply an attribute list to a set of wires. To attach the specified property on all wires in a group, type

auto netprop <group_name> <property_name> = <property_value>

Using the auto path command

Using the auto property command

To attach properties to symbols in a group, type

auto property <group_name> <property_name> = <property_value>

Using the autoroute command

The set command option autoroute on activates automatic routing after moving an object in the direct mode. The set autoroute option can be turned on or off.

Backannotate

Syntax

Backannotate {annotation file | <cr>}

Description

To generate a backannotation file, use the following directive when running the Packager:

output backannotation;

By default, this directive is set.

Limitations of Backannotation

1.	Sizeable parts having property SIZE > 1 are not backannotated.
2.	Net properties are backannotated only if they have existing placeholders.

3.	Properties on buses are not backannotated unless they exist on individual bits of the bus.

See also the SET command options that control property visibility and pin number placement.

Badd

Syntax

BADd { [block_name] point1 point2 } . . .

Description

Example

To add a new block CACHE to the design:

1.	Type badd CACHE in the console window.
2.	Click the design window and drag to form a rectangle.

Note: The cursor shape changes to a + sign.

3.	Click the design window again to end the drawing.

Related Commands

Add
Bpadd
Bpdelete
Bprename
Bpmove
Brename
Broute
Bstretch
Bwire

Bpadd

Syntax

BPAdd {pin_name :mode point}...

Description

Related Commands

Badd
Bpdelete
Bprename
Bpmove
Brename
Broute
Bstretch
Bwire

Bindview

Syntax

Bindview point1 point2

Description

This command makes a drawing that is visible in one viewport visible in another viewport also. Any changes you make to one copy of the drawing also appear on the other copy.

Point1 selects the drawing to make visible. Point2 specifies the new viewport where the drawing should appear.

Bpdelete

Syntax

BPDelete {point}...

Description

This command deletes pins on blocks. You can choose the pins to be deleted by pointing to them with the mouse.

Example

To delete a pin, type bpdelete in the console window and select the pin using the left mouse button.

Related Commands

Badd
Bpadd
Bprename
Bpmove
Brename
Broute
Bstretch
Bwire

Bpmove

Syntax

BPMove {point1 point2}...

Description

This command moves a pin from point1 on a block to point2.

Example

To move a pin from point1 on a block to point2:

1.	Type bpmove in the console window.
2.	Click to select the pin to be moved (point1).

3.	Click to place the pin on the block (point2).

To remove these hanging properties, perform the following steps:

1.	setsticky_on
2.	get

3.	setsticky_off

Related Commands

Badd
Bpadd
Bpdelete
Bprename
Brename
Broute
Bstretch
Bwire

Bprename

Syntax

BPRename {pin_name point}...

Description

This command renames pins on blocks. In this command, pin_name is the new name of the pin and point is location of the pin.

Example

To rename a pin named PRESET to CLOCK, type bprename CLOCK in the console window and click PRESET.

Related Commands

Badd
Bpadd
Bpdelete
Bpmove
Brename
Broute
Bstretch
Bwire

Brename

Syntax

BREname {[block_name] point1}...

Description

You might want to remove <old_block_name> with the remove command.

If you do not need the old block any longer, you can remove it from the disk by using the remove command, for example remove <old_block_name>.

Example

To rename a block named CACHE to MEMORY, type brename MEMORY in the console window and click CACHE.

Related Commands

Badd
Bpadd
Bpdelete
Bpmove
Bprename
Broute
Bstretch
Bwire
Copy
Remove

Broute

Syntax

BROUte {[signal_name] point1 point2}...

Description

This command routes a signal named signal_name between point1 and point2. If the signal_name is a bus name, create a heavy wire.

Related Commands

Badd
Bpadd
Bpdelete
Bpmove
Bprename
Brename
Bstretch
Bwire
Route
Wire

Browse

Syntax

Browse {<libname> | <cr>}

Description

This command accesses the COMPONENT BROWSER dialog box. It lets you scan through all libraries and active directories. You can also access the COMPONENT BROWSER with the ADD command.

BROWSE <libname> sets the library field to the given library name and resets the selection list to that library. The default is the design library.

Example

To display the COMPONENT BROWSER dialog box, type browse in the console window and press Enter.

To display the COMPONENT BROWSER dialog box with the library set to standard, type browse standard in the console window and press Enter.

Bstretch

Syntax

BStretch {point1 point2} . . .

Description

Example

To resize a block, type bstretch in the console window and select the side or corner of the block you want to stretch. Drag to the point you want to resize the block. Click again to end the block.

Related Commands

Badd
Bpadd
Bpdelete
Bpmove
Bprename
Brename
Broute
Bwire
Delete
Split

Bubble

Syntax

BUBble point...

Description

For example, a NOT symbol is defined with both the BUBBLED and BUBBLE_GROUP properties attached:

BUBBLED=(B)

BUBBLE_GROUP=(A|B)

Example

To toggle the state of a pin, type bubble in the console window and click the pin in the design window.

To make two pins as part of the same bubble-group such that the BUBBLE command can be applied to the pins, you must ensure the following:

1.	Both the pins must have a wire stub and a bubble attached to them, similar to the symbol of LS04 in the lstll library.
2.	BUBBLE_GROUP property must be attached to the component symbol with the value containing all pin names in the bubble group. For example, BUBBLE_GROUP = (A<7..0> \| B<7..0>).

3.	The pin that you want to make bubbled by default, should be specified with a BUBBLED property on the component. For example, BUBBLED = B<7..0>

Busname

Syntax

BUSName bus_name point point

Description

This command places single-bit vectored signal and pin names on a drawing. For example, the bus name A<7..0:2> results in the signal names A<7>, A<5>, A<3>, and A<1>.

For examples, if you issue the following command:

busname a<20..0:2>\I

Related Commands

Signame
Bustap

Bustap

Syntax

BUSTap bus_tap_value point point...

Description

This command fills in the value of the BN (bit number) properties on bus taps in drawings.

Bwire

Syntax

Bwire {[signal_name] point point } . . .

Description

The bwire command adds a net between point/component/block and a block. When the net is added, a pin also gets attached at the connection point in the block.

See also the WIRE, BROUTE, ROUTE commands, and the SET and SHOW commands to change default wiring behavior.

Example

To create a net AB and a pin AB on a block in the design:

1.	Type bwire AB in the console window.
2.	Start at some point and end on a block in the design.

A net named AB and a pin on the selected block named AB are created.

Related Commands

Broute
Route
Set
Show
Wire

Change

Syntax

Change {group_name | point}...

Description

Example

The following commands are useful for editing text:

<BackSpace>	Deletes the previous character
<Delete>	Deletes the current character
Ctl<k>	Deletes to the end-of-line
Ctl<e>	Brings up the selected text items in an editor
<-	Moves backward
->	Moves forward

Check

Syntax

CHEck <cr>

Description

Duplicate components in the same location

set option: CHECK_PARts_at_same_loc <ON/OFF>

To correct the error, use the split console command and separate overlapping elements. For more information on the split console command, see Split .

Pins attached to more than two wire segments (this may not be an error, but is an error if a wire inadvertently shorts the pins on a device)

set option: CHECK_TWo_wires_at_pins <ON/OFF>

Wires connected to only one pin and not named (NC wires)

set option: CHECK_Unconn_wires <ON/OFF>

Nets that are named but not connected to any pins

set option: CHECK_SIGNAMES <ON/OFF>

Wires that come close to but do not contact pins

set option: CHECK_PIN_near_wire_endpt <ON/OFF>

Missing TITLE and/or ABBREV properties

set option: CHECK_TItle_abbrev <ON/OFF>

Bodies that are placeholders

set option: CHECK_Body_place_holders <ON/OFF>

Pins located at the origin (0,0) in BODY drawings

set option: CHECK_PINS_at_origin <ON/OFF>

Multiple dots at the same location

set option: CHECK_Arcs_at_same_loc <ON/OFF>

To correct the error, use the split console command and separate overlapping elements. For more information on the split console command, see Split .

Hard properties with the? value (placeholders)

set option: CHECK_Prop_place_holders <ON/OFF>

Wires connecting the pins of a two-pin body

set option: CHECK_Shorted_pin <ON/OFF>

Wire segments hidden by parts of a body

set option: CHECK_Hidden_wires <ON/OFF>

To correct the error, use the split command and separate overlapping elements.

Pin properties which are no longer attached to pins.

set option: CHECK_Missing_pins <ON/OFF>

To correct the error, reattach properties to new pins, delete properties or replace part.

Inconsistent section properties

set option: CHECK_Pack_sec_type_props <ON/OFF>

To correct the error, resection the part.

Signame properties defined within a symbol (body).

set option: CHECK_SIGNAME_in_body <ON/OFF>

To correct the error, remove signame properties from the body files.

	Duplicate PATH properties
	Wires overlapping a body

Check for legal HDL net names (hdl_direct on only)

set option: CHECK_Net_names_hdl_ok <ON/OFF>

Check for legal HDL port names (hdl_direct on only)

set option: CHECK_Port_names_hdl_ok <ON/OFF>

Check for legal HDL symbol names (hdl_direct on only)

set option: CHECK_Symbol_names_hdl_ok <ON/OFF>

Run checks automatically when writing drawings.

set option: CHECK_On_write <ON/OFF>

CHECK lists each detected error. After you run the CHECK command, you can use the ERROR command to locate each error on the drawing.

Related Commands

Circle

Syntax

Circle point point

Description

Circles and arcs are rarely necessary on logic designs but are commonly used for creating symbol drawings.

Related Commands

Arc

Copy

To make multiple properties of an object

Syntax

COPy {[count][REPEAT][ALL] source_point destination_point | [count][REPEAT][ALL] group_name destination_point | property_point destination_point attach_point }

Description

This command copies objects, properties, and groups in the current drawing or between viewports.

Groups of properties are not copied. When applicable, properties attached to objects are copied with the group.

Procedures

	To copy an object
	To copy an object and its properties

Dehighlight

Syntax

DEHighlight [ Net | PArt | PIn | Any ] pt

DEHighlight [ Net | PArt | PIn | Any ] object_name

Description

pt	To pick a component to be unhighlighted, point to the object and press the left button. Select a group by pointing to the required group and pressing the middle button.
object_name	If you would prefer typing in the name of the object, you may do so by using the second version of this command.

For nets, the object name is the signal name of the net, for example, FOO.

For parts, the object name is the value of the PATH property attached to the component, for example, 7P.

Wildcards such as * and ? may be used in specifying the object name,

For example, FOO*, 7*P, 7P.A*.

The Dehighlight command is used to unhighlight an already highlighted object throughout the system.

Related Commands

Highlight
Unhighlight

Delete

Syntax

DELete {point | group_name}...

Description

You cannot delete default properties on bodies and pin number properties generated by the PINSWAP command.

The UNDO command lets you retrieve groups or objects deleted by mistake.

Example

To delete an object:

1.	Type delete in the console window.
2.	Point to an object in the design window and press the left button.

Procedures

	Deleting an object
	Deleting a group

Related Commands

Undo

Diagram

Syntax

DIAgram [<library>]cell[.type][.version][.page]

Description

	<LIBRARY> is the name of the library where the drawing resides. The library name must be enclosed in angle brackets. If no library is specified, the current library is the default.
	CELL is the new name of the drawing. The current drawing name is taken by default. For example, if the Design Entry HDL title bar displays ATM.SCH.1.2, the current drawing name is ATM.

	TYPE is the drawing type. The drawing type can be SCH (schematic), SYM (symbol). If no drawing type is specified, the current drawing type is used. For example, if the Design Entry HDL title bar displays ATM.SCH.1.2, the current drawing type is SCH.
	VERSION is the version number of the drawing type. For example, if the Design Entry HDL title bar displays ATM.SCH.1.2, the version number of the drawing type SCH is 1. If no version number is specified, the default value 1 is used.

To rename a drawing, edit the drawing to be changed, type DIAGRAM and the new name of the drawing. Type WRITE to save a copy of the drawing by its new name.

For example, to use the drawing SHIFTER.SCH.1.1 as a pattern for a new drawing named NEWSHIFTER.SCH.1.1, use the commands:

EDIT SHIFTER.SCH.1.1

DIAGRAM NEWSHIFTER

WRITE

The NEWSHIFTER.SCH.1.1 drawing is saved to disk.

Directory

Syntax

DIRectory {[<directory>][name][.[type][.[vers][.[page]]]] |<cr>}

Description

This command lists the names and contents of directories in the current directory list in the order that the directories are searched with the current working directory displayed first.

You can use wildcards in all fields of the directory and drawing names. An asterisk matches any string. A question mark matches any single character.

Some command examples are

DIR	Lists all drawing names in the current directory
DIR <*>	Lists all active directories (but no drawing names)
DIR <time>*	Lists all drawing names (parts) in the TIME library
DIR <>	Lists all drawing names in all active directories and libraries
DIR ls*	Lists real file name and directory type for current directory.
DIR .	Lists all drawings.

Related Commands

IGnore
Library

Display

Displaying properties on objects in a group

Syntax

Description

This command changes the way objects or groups are displayed on a drawing. Any change made with the DISPLAY command remains in effect until another DISPLAY command is used to change it again.

To change the display of a single object, use the left mouse button. To change the display of a group, use the middle mouse button or type in the single-letter group name.

Groups can contain any type of object. Group names, options, and point entries can be included in any order and in any combination, except that the first argument MUST be a command option.

The command options are described below:

	NAME, VALUE, BOTH, and INVISIBLE determine the way properties are displayed on the drawing. Although a property consists of a name and value pair, usually only the value is displayed when a property is added to a drawing. These options allow you to display the name alone, the value alone, both, or neither.
	DEFAULT and SCALE_FACTOR determine the size of text displayed on the drawing.

		DEFAULT displays text on the drawing using the default text size specified in the Text tab of the Design Entry HDL Options dialog box. For example, if the default text size is 0.082 inches, the size of the selected text on the drawing will be set to 0.082 inches.
		You specify a scale_factor to enlarge or reduce the size of the text on the drawing. For example, if the default text size specified in the Text tab of the Design Entry HDL Options dialog box is 0.082 inches, the DISPLAY 2 command will enlarge the size of the selected text to 0.164 inches.

Note: To display the size of a string, type SHOW SIZE and point to the string. Use SET SIZE to alter the default size of added text.

	FILLED and OPEN change the display of dots already added to a design.
	Open dots scale when the ZOOM or SCALE command is used; filled dots do not. The SET DOTS_FILLED command adds dots to the drawing filled by default.

Procedures

	Displaying properties on objects
	Resizing text

Dot

Syntax

Dot point...

Description

Dots can be filled or open. By default, all added dots are open. To change to filled dots, type SET DOTS_FILLED. To fill an open dot, type DISPLAY FILLED and point to the dot.

AUTO DOTS places a dot at all connection points in a logic drawing. AUTO UNDOT automatically removes all dots except those at the intersections of four wires.

AUTO UNDOT removes all existing dots in the drawing.

Example

To indicate a connection point on a wire, type dot in the console window and click on the wire where you want the connection point.

Echo

Syntax

Echo message

Description

This command displays messages in the console window. Use this command to show messages during the execution of a script for tracking its progress and debugging.

Example

echo 50% script completed

Edit

Syntax

Edit {[<directory>][drawing][.[type][.[version][.[page]]]]|<cr> | point}

Description

This command displays an existing drawing to be edited or creates a new drawing.

EDIT <cr> accesses the View Open form that allows you to open an existing drawing for editing. The View Open form can be turned off by typing SET EDITFORM OFF.

Procedures

	Navigating the drawing hierarchy
	Opening a drawing

	Creating a design page
	Displaying pages in a multi-page drawing

Related Commands

Get
Return
Gotosheet

Error

Syntax

Error <cr>

Description

This command locates and displays each error detected by the CHECK command. It draws a blinking highlighted rectangle at the location of the error and displays a message describing the error.

Exclude

Syntax

EXClude [group_name|Mpoint|DEFault][option...][selection ...| group_name]

where option is:

BOdies | WIres | PRoperties | NEts | Connections

and selection is:

Lpoint | Ctrl+Rpoint | Mpoint

Description

This command removes items or groups from the current group.

	If the first argument is a single-letter group name, the group will become the current group. Alternatively, click the middle mouse button on a highlighted group to make it the current group. If a group is not specified, or the word default is provided, the most recently created group will remain the current group.
	To remove individual objects, click the left mouse button or press Ctrl and click the right mouse button.

	To remove previously-defined groups, click the middle mouse button on a highlighted group or enter the single-letter group name.
	Option flags allow the user to remove types of objects in a group. Options are applied to the objects in the initial current group.

Example

Exclude A ne

This command excludes all nets in group A from the group.

Related Commands

Find
Group
Include
Select

Exit

Syntax

EXIt <cr>

Description

The QUIT command is the same as the EXIT command.

Related Commands

Quit

Filenote

Syntax

FILenote {file_name point| <cr>}

Description

FILENOTE <cr> brings up a file browser. Select the file and click the position on the drawing where you want to place the note.

Find

Syntax

FINd pattern

Description

Wildcards are allowed in a pattern. An asterisk matches any number of characters, and a question mark matches any single character. FIND is not case-sensitive.

By using the SET NEXTgroup command before the FINd command, you can add the results of the FINd operation to the specified group. Commands to do this are:

SET NEXTgroup <groupname>

FINd pattern

Examples

To find all ls04 components on a drawing and add them in group A, run the following console commands:

set nextgroup A

find ls04

To find all objects on a drawing that start with the letter mem and add them in group A, run the following console commands:

set nextgroup A

find mem*

	Suppose you have 5 instances of ls04 with property LOCATION = U1 on a page. To change LOCATION property of all these instances to U8, perform the following steps:
	a.	Type the console command:

find LOCATION = U1

Type the console command:

change A

Right-click on the canvas and select Editor from the pop-up menu.

The text editor opens.

	d.	Change the value of LOCATION property to U8 for all the objects.
	e.	Choose File – Save and save the file.

Related Commands

Group
Exclude
Include
Select
Set

Get

Syntax

Get { [<directory>][drawing][.[type][.[version][.[page]]]] }

Description

Note: All modifications to the current drawing are lost when you use the Get command.

Example

To discard changes to your current drawing:

1.	Type get in the console window and press Enter.

A Design Entry-HDL message box appears asking you to confirm if you really want to get the drawing from the disk.

2.	In the Design Entry-HDL message box, click Yes.

Related Commands

Edit

_globalModify

Syntax

_globalModify

Description

Opens the Component Change tabbed page of the Global Modification window. Use this page to replace a component with a new component across a design.

_globalChange

Syntax

_globalChange

Description

Opens the Property Change tabbed page of the Global Modification window. Use this page to change properties of components, pins, and nets across a design.

_globalDelete

Syntax

_globalDelete

Description

Opens the Property Delete tabbed page of the Global Modification window. Use this page to delete properties of components, pins, and nets across a design.

Gotosheet

Syntax

GOtosheet N

where N is the page number in a hierarchical design.

Description

This command allows you to go to a specific page in a hierarchical design.

This allows you to easily refer to a page in Design Entry HDL against a plotted page or a cross-reference report.

	When you plot a schematic page, the page number of the schematic page is plotted if you have added the custom text variables for page numbers on the schematic page.
	When you perform cross-referencing on a design, the cross-reference reports display the schematic page numbers.

Enter the page number displayed on the plotted page or the cross-reference report to go to the page in Design Entry HDL.

Related Commands

Grid

Syntax

GRId {<cr>|[ON][OFf][Dots][Lines] [grid_size grid_multiple]}

Description

See also the SET command to change the default editor values.

Related Commands

Group

Syntax

GROup [group_name|DEFault][type...] {selection...| group_name | ALL}

where type is:

BOdies | PRoperties | NOtes | WIres | DOts.

and selection is:

{Lpoint Lpoint...Ctrl+Rpoint} | Ctrl+Rpoint | Mpoint

Description

This command allows the user to draw a polygon to specify the boundaries of a group. The group is defined as a collection of objects.

	If the first argument is a single-letter group name, that group will become the current group. If a group name is not specified, or DEFault is specified, a single-letter group name will be automatically assigned to the group that is created.
	The group selection can be restricted to a specified type or set of types by providing one or more of the type arguments.

	You can use the mouse to draw a polygon around the objects to be grouped. Click the left mouse button to start the line or to change the direction of the line. Complete the polygon by pressing Ctrl+right mouse button when the cursor is near the starting point. You can draw additional polygons to include other objects in the group.
	Press Ctrl and click the right mouse button to include individual objects in the group.

	Click the middle mouse button on another highlighted group to include its contents in the current group.
	Use the name of a previously created group to include its contents in the current group.

For example, the command group C A includes the contents of group A in group C.

Use ALL to select all objects in the current drawing.

For example, the command group A bodies all includes all the components in the current drawing in group A.

The console window displays the group name and the number of bodies, properties, notes, dots, and wires in the group.

Related Commands

Auto
Find
Include
Exclude
Select

HIEr_write

Syntax

HIEr_write

Description

The hier_write command is different from the write command as write command saves only the current page while hier_write saves all the pages in the hierarchy.

Highlight

Syntax

HIGhlight [Net | PArt | PIn | Any] pt

HIGhlight [Net | PArt | PIn | Any] object_name

pt	To pick a component to be highlighted, point to the object and press the left mouse button. Select a group by pointing to the desired group and pressing the middle mouse button.
object_name	If you prefer typing in the name of the object, you may do so by using the second version of this command.

For nets, the object name is the signal name of the net, for example, FOO.

For parts, the object name is the value of the PATH property attached to the component, for example, 7P.

Wild cards such as "*" and "?" may be used in specifying the object name, for example, FOO*, 7*P, 7P.A*.

Description

Related Commands

Dehighlight
Unhighlight

HMirror

Syntax

HMirror point

Description

Related Commands

Mirror

HPlot

Syntax

hplot [worklib/<schematic_name>/sch_1/module_order.dat]

Description

IGnore

Syntax

IGnore {directory_name | library_name | * | <cr> }

Description

Example

To delete the lsttl library from the active search list:

1.	Type ignore lsttl in the console window.
2.	In the Design Entry-HDL confirmation window, click Yes.

imginsert

Syntax

imginsert [{filename} (starting coordinates)]

Description

Inserts an image into the schematic canvas. This command launches the Open dialog box from where you can select the image that you want to paste.

You can also insert an image at a pre-defined location from the command line.

Example

imginsert c:/abc.bmp (1000, 1200)

This command places the bitmap file, abc.bmp, at the specified location on the schematic.

imgstretch

Syntax

imgstretch [(starting coordinates) (ending coordinates)]

Description

Stretches a selected image horizontally or vertically on the schematic. You can also specify the starting and ending coordinates for stretching the image.

Example

imgstretch (1000, 1200) (1500, 2500)

imgcapture

Syntax

imgcapture [(starting coordinates) (ending coordinates)]

Description

Example

imgcapture (1000, 1200) (1500, 2500)

where (1000, 1200) represent the starting coordinates and (1500, 2500) represent the ending coordinates.

Include

Syntax

INClude [group_name|Mpoint|DEFault][option...][selection ...| group_name]

where option is:

BOdies | WIres | PRoperties | NEts | Connections

and selection is:

Ctrl+Rpoint | Mpoint

Description

This command adds items or groups in the current group.

	If the first argument is a single-letter group name, the group will become the current group. Alternatively, click the middle mouse button on a highlighted group to make it the current group. If a group is not specified, or the word default is provided, the most recently created group will remain the current group.
	To add individual objects, click the left mouse button or press Ctrl and click the right mouse button.

	To add previously-defined groups, click the middle mouse button on a highlighted group or enter the single-letter group name.
	Option flags allow the user to include types of objects in a group. Options are applied to the objects in the initial current group and to any additions made to the current group by the include command.

		BODIES or WIRES include all bodies or wires that have properties already in the current group.
		PROPERTIES include all properties attached to objects already in the related group.

		NETS include all nets of wires attached to bodies or wires already in the related group.
		CONNECTIONS include all the objects connected to the pins of any symbol already in the chosen group.

Example

Include A pr

This command includes properties of all objects in group A to the group.

Related Commands

Exclude
Find
Group
Select

Library

Syntax

LIbrary {library_name | <cr> }

Description

This command adds the specified library to the search list.

LIBRARY <cr> accesses the Search Stack form that allows you to add or delete libraries in the active search list. The Search Stack form can be turned off by entering the command SET LIBFORM OFF.

Related Commands

Loadstrokes

Syntax

LOADStrokes {strokes_file | <cr>}

Description

This command loads a user-defined strokes_file. Strokes are user-defined line drawings you create with the mouse. You can customize command entry in the editor by using strokes.

To create your own strokes_file, or edit an existing strokes_file, you use the Stroke Editor. This system utility is used to create strokes for many applications.

LOADSTROKES <cr> brings up the File Browser form. You can then select the strokes_file from the form.

Related Commands

Strokefile

Mirror

Syntax

MIrror point

Description

The MIrror command should be used with caution, especially with bodies with unmarked pins, such as merge bodies. Reversing the bits causes subtle, hard-to-find errors in the design.

See SET LEFT/RIGHT and DISPLAY LEFT/RIGHT for justifying text, and the ROTATE, SPIN, and VERSION commands.

Example

To create a mirrored version of a symbol, type mirror in the console window and select the symbol with the left mouse button.

Related Commands

Display
Rotate
Set
Spin
Version

Modify

Syntax

MODify point

Description

If the user selects a primitive from the popup, the package type corresponding to the primitive is used to seed the PACK_TYPE property in the .ptf file.

- if multiple properties with this name can be legally attached, a new property identical to the one on the new part is attached to the old part

- otherwise, the value of the property on the old part is modified with the value of the property on the new part.

All error messages are displayed in the Design Entry HDL console window.

Example

1.	To modify a part, type modify in the console window.
2.	Click the part you want to modify in the design window.

The Physical Part Filter window appears.

3.	Select the new part in the Physical Part Filter window.
4.	Click Close.

The old part is replaced with the new part you selected in Step 3.

Procedures

	Modifying an object
	Modifying components in a group

Move

Syntax

MOVe {source_point destination_point|group_name destination_point}

Description

To move a defined group, specify the name of the group or press the center button to select the group to move.

The first click of the middle button (while dragging) changes the shape of the wire from orthogonal to direct.

The second click of the middle button detaches the part from any wires and allows you to move the part freely.

The third click of the middle button re-attaches the wires and lets you drag the object the usual way until you place the object with the left button.

The wires are automatically re-routed only when you place the part with the wires connected directly (non-orthogonally) and the SET option AUTOROUTE is on (SET AUTOROUTE ON).

Procedures

	Moving text, wires, or an unwired component
	Moving a wired component

	Moving multiple objects
	Moving a group

Next

Syntax

NExt <cr>

Description

NEXT cannot be used after the CHECK command. Use ERROR after the CHECK command.

Related Commands

Note

Syntax

Note text_line... point...

Description

	Specify the points on the drawing where the notes are to be located and then type in the text. Press <cr> after each note to position each note on the drawing. As long as there are points remaining, the editor interprets entered text as notes to the drawing.
	Type in each line of text first and press <cr>. (You can enter several strings before placing them.) Then use the cursor and the left button to indicate where each note is to appear on the drawing.

Place quotes around notes beginning with an opening parenthesis. Notes within quotes are not interpreted as commands.

Related Commands

Filenote

Page commands

You can renumber the pages of a design through the _Page and Page commands:

_PAGE commands

	_PAGEInsert
	_PAGEDelete

	_PAGECompress
	_PAGEMove

_PAGEInsert

_PAGEInsert <Number_of_pages> <Location> [-nosave] [-noconfirm]

Number_of_pages	Indicates the number of pages to insert. The valid range is 1 - 250. This parameter must always precede the Location parameter.
Location	Indicates the location from where you want to insert the page(s). Pages are always inserted before the current page at the target location. To add pages at the end of the schematic, you would specify Location as one greater than the last page number. If you specify Location as more than one greater than the last page number, a page gap is created between the current last page and the first of the newly inserted pages. See Inserting Pages at the End of a Schematic .
-nosave	Keeps the newly inserted pages from being saved. Use this parameter to create page gaps in a schematic. This parameter can be placed anywhere in the argument list.
-noconfirm	Bypasses the message prompting you to confirm before executing the command. If you choose Cancel, the command is terminated. This parameter can be placed anywhere in the argument list.

Examples

The following examples of the _PAGEInsert command are explained in the context of different scenarios:

	Inserting Pages between Two Pages
	Inserting Pages at the End of a Schematic

	Inserting a Page Gap between Two Pages
	Inserting Pages Beyond the End of the Schematic

Inserting Pages between Two Pages

Initial page sequence: 1-10

_PAGEInsert 5 4

New page sequence: 1-15

Inserting Pages at the End of a Schematic

Initial page sequence: 1-15

_PAGEInsert 5 16

This command will add 5 pages starting from page 16. All the pages will be saved and the corresponding Page* files will be created under the sch_1 directory.

New page sequence: 1-20

Inserting a Page Gap between Two Pages

Initial page sequence: 1-3, 6-10, 12-15

_PAGEInsert 3 8 -nosave

This command will:

	Move pages, page 8 onwards, by three places to accommodate the new pages. As a result, the existing page 8 will become page 11.
	Insert a three-page gap - 8,9,10.

New page sequence: 1-3, 6-8, 11-13, 15-18

However, if you choose not to save page 8, the result of the _PAGEInsert command would be a 3 page gap in the schematic at the point of insert.

New page sequence: 1-3, 6-7, 11-13, 15-18

Inserting Pages Beyond the End of the Schematic

Initial page sequence: 1-3, 6-10, 12-15

The -nosave option is of no value for this case as everything beyond the end of the schematic module is already blank.

_PAGEInsert 2 25 -noconfirm

New page sequence: 1-3, 6-10, 12-15, 25-26

_PAGEDelete

Syntax

_PAGEDelete <List_of_Pages> [-retain] [-noconfirm]

List_of_Pages	Indicates the pages to delete. You can specify an explicit number or a range of numbers. For example, 1,2,3,5-7, is a valid range. Spaces are not allowed between page numbers.
-retain	Retains the physical page numbers of the pages affected by the deletion. This parameter can be placed anywhere in the argument list.
-noconfirm	Bypasses the message prompting you to confirm before executing the command. If you choose Cancel, the command is terminated. This parameter can be placed anywhere in the argument list.

Note: The _PAGEDelete command can be used to remove specific page gaps. To remove all page gaps, use the _PAGECompress command.

Examples

The following examples of the _PAGEDelete command are explained in the context of different scenarios.

	Deleting Existing Pages
	Deleting Non-existent Pages

	Deleting Non-existent Pages out of Page Range
	Deleting Pages to Retain Physical Page Numbers of the Pages Following the Page(s) Being Deleted

Deleting Existing Pages

Initial page sequence: 1-15

_PAGEDelete 6-8

This command will delete pages 6, 7, and 8. The physical page numbers of all the pages following page 8 will be moved in by 3.

New page sequence: 1-12

Deleting Non-existent Pages

Initial page sequence: 1-3, 6-10, 12-15

_PAGEDelete 4 -noconfirm

New page sequence: 1-3, 5-9, 11-14

Deleting Non-existent Pages out of Page Range

Initial page sequence: 1-3, 6-10, 12-15

_PAGEDelete 48

If you try to delete a non existent page, which is out of the page range of the schematic, it will result in an error:

Result: Command cannot be executed

Deleting Pages to Retain Physical Page Numbers of the Pages Following the Page(s) Being Deleted

Initial page sequence: 1-15

_PAGEDelete 6-8 -retain

This command will delete pages 6, 7, and 8. However, the physical page numbers of all the pages following page 8 will be retained. A gap of three pages will be created between pages 5 and 9.

New page sequence: 1-5, 9-15

_PAGECompress

You remove all the page gaps in a schematic by using the _PAGECompress command.

Syntax

_PAGECompress

Note: The _PAGECompress command does not accept any arguments.

Example

Initial page sequence: 1 4-5 10-13 15-17

_PAGECompress

New page sequence: 1-10

_PAGEMove

Syntax

_PAGEMove <List_of_Pages> <Before_Page > [-noconfirm]

List_of_Pages	Indicates the pages to move. This parameter must come before the Before_Pageparameter.
Before_Page	Indicates a location in the schematic where the pages will be moved. For example, if you specify 5 as Before_Page, the moved pages will precede the current page 5. To move pages to the end, specify a number, which is one greater than the last physical page.
-noconfirm	Bypasses the message prompting you to confirm before executing the command. If you choose Cancel, the command is terminated. This parameter can be placed anywhere in the argument list.

Examples

The following examples of the _PAGEMove command are explained in the context of different scenarios:

	Moving a Page before an Existing Page
	Moving a Set of Pages outside the Current Range of Pages

	Moving Non-contiguous Pages to Contiguous Locations
	Moving a Set of Pages to a Location which Falls within the Range of the Pages to be Moved

Moving a Page before an Existing Page

Consider a Team Design scenario where you have a team of three designers A, B, and C, working on a design. Each designer owns different sections of the design:

	Designer A is writing the CPU logic in pages 1-10
	Designer B is writing the CONTROL logic in pages 11-20

Designer C is writing the MEMORY logic in pages 21-30

_PAGEMove 4-8 15

This command:

1.	Moves pages 15-30 out 5 pages to make space for the 5 pages being moved.
2.	Moves pages 4-8 to the blank slots created in step 1

3.	Removes the 5 page gap (4-8) created in step 2 by moving all pages in by 5.

Moving a Set of Pages outside the Current Range of Pages

Initial page sequence: 1-3, 6-10, 12-15

_PAGEMove 6-9 17

New page sequence: 1-3, 6, 8-11, 13-16

Moving Non-contiguous Pages to Contiguous Locations

Initial page sequence: 1-3, 6-10, 12-15

_PAGEMove 3,7,9 15 -noconfirm

New page sequence: 1-2, 5-7, 9-15

Moving a Set of Pages to a Location which Falls within the Range of the Pages to be Moved

Initial page sequence: 1-3, 6-10, 12-15

_PAGEMove 6-9 7

This command will result in an error as the target move location is within the range of the pages to be moved. A warning message is displayed and no action is taken.

Page

	page move
	page swap

	page delete
	page reset

page forcereset

page move

page move <@lib.cell(view)> X Y

Moves existing page X to a non-existing page Y.

Note: You cannot move a page to a page that already exists.

page swap

page swap <@lib.cell(view)> X Y

Swaps existing pages X and Y.

page delete

page delete <@lib.cell(view)> X

Deletes an existing page X.

Note: The move, swap, and delete commands cannot be executed on pages if:

	the page is currently being edited.
	the page is being edited, and changes in the page have not been saved.

page reset

page reset X

Sets the existing page number to X.

page forcereset

page forcereset X

You should keep the following points in mind while executing the page reset and page forcereset commands:

1.	To commit the change made by the pageforcereset or pagereset command, you have to save the page.To reflect this status, a * is shown on the Design Entry HDL title bar. If you want to de-commit the change made by any of these commands, do not save the page because you cannot undo the command.
2.	If two different physical pages have the same logical page number, and you try to save the design, Design Entry HDL displays an error message stating that the physical pages have the same logical page number. The message prompts you to use the page forcereset command and then save the schematic to resolve the page conflict.

You can then use the pageforcereset command to change the logical page numbers.

3.	Running the pageforcereset and pagereset commands makes the occurrence properties of objects, which are on renumbered pages, unusable. A message box appears informing you that the page reset command might make the opf properties for objects on the page unusable. You get the following error message:
4.	While cross-probing or globally locating objects, canonical names are shown with the logical page numbers. For example, the canonical name @top_lib.top.(sch_1):page2_i5 displayed in the Global Find dialog box means that the component that has the PATH=i5 property is located in the logical page 2 in the sch_1 view of the cell top in the library named top_lib.

Paint

Syntax

PAInt {color_name{point|group_name}|DEFault{point|group_name}} <cr>

Description

There are 16 available colors

	AQUA
	GREEN

	PINK
	SKYBLUE

	BLUE
	MONO

	PURPLE
	VIOLET

	BROWN
	ORANGE

	RED
	WHITE

	GRAY
	PEACH

	SALMON
	YELLOW

Procedures

	Specifying color of an object
	Specifying color for a group use

Pastespecial

Syntax

pastespecial [(starting coordinates) (ending coordinates)]

Description

Displays the Paste Special dialog box. Use this dialog box to specify whether you want to:

	Paste copied schematic parts on to the target schematic directly
	Change the signal names of the schematic before pasting them on the target location

Pause

Syntax

PAUse

Description

This command temporarily interrupts the editor until you press a key. PAUSE is useful in demos and scripts.

Pinnames

Syntax

PINNames point

Description

This command adds a PIN NAMES symbol to a schematic drawing that defines the functional circuitry of a symbol drawing. This is used in hierarchical design and in library development.

Pinswap

Syntax

PINSwap {point1 point2 | pin_number point }

Description

There are two ways to swap pins:

	Type PINSWAP and point to the two pins to be swapped.
	Type PINSWAP, type in a new pin number, and then point to an existing pin. The selected pin is swapped with the pin having the pin number you specified.

The properties attached by the PINSWAP command cannot be changed, they can only be deleted and moved. Once pins on a part have been swapped, the part cannot be resectioned using the SECTION command.

The PINSWAP command also swaps sections within HAS_FIXED_SIZE parts.

Related Commands

Backannotate
Section

Plot

Syntax

Plot

Plots the currently opened drawing

Plot cache

Plots all pages of the schematic named cache.

Plot cache.sym.1.1

Plots the symbol view of cache

Plot cache.sym.1.2

Plots page 2 schematic of cache

Plot cache.sch.1.*

Plots all pages of version 1

Note: To plot custom variables, you must open the design before running plot commands. Plot commands cannot evaluate the custom variables for unopened designs.

PPTAdd

Syntax

PPTAdd {"path"[",path"];}

Description

When using component selection in the physical mode, PPTADD provides the search path to locate the ppt files to be used.

The list of paths are pushed on to a stack. The last one specified is the first one searched.

This command replaces the SET PPTPATH option.

Related Commands

Add
PPTDelete

PPTDelete

Syntax

PPTDelete {"path"[",path"];}

Description

The PPTDelete command is used to remove paths to part table files used in the physical component selection. The command, however, does not affect the stack order.

Related Commands

Add
PPTAdd

PPTEcho

Syntax

PPTEcho

Description

When using the component selection in physical mode, PPTECHO lists the search path which will be used to locate the ppt files.

Related Commands

Property

Syntax

Property {attach_point location_point name_and_value | name_and_value attach_point location_point | attach_point name_and_value location_point}

Description

A property value can be any string of text up to 255 characters, including spaces and punctuation marks.

There are two ways to assign properties.

Type PROPERTY <cr>.

Quit

Syntax

QUIt <cr>

Description

The EXIT command is the same as the QUIT command.

Related Commands

Exit

Reattach

Syntax

REAttach text_point attach_point

Description

Recover

Syntax

RECover <recover_log_file>

Description

This command is used for recovering drawings that were being edited when Design Entry HDL or your system crashed.

Note: The temporary directory (for example, ./xxnedtmp) and all of its files are deleted if Design Entry HDL terminates normally.

An example illustrating the use of the recover command is:

RECOVER temp/xxnedtmp1/undo2.log

Related Commands

Diagram
Write

Redo

Syntax

REDo <cr>

Description

Remove

Syntax

REMove [<directory>][name][.[type][.[version][.[page]]]]

Description

Replace

Syntax

REPlace {symbol_name point | symbol_name <cr> group_name}

Description

This command substitutes one part for another. The default version of the symbol is 1. Specify the version number to replace another version of a symbol.

There are several ways to use the REPLACE command.

	Type the name of the replacement part. Then use the cursor to point to the symbol or bodies to be replaced.
	Use the FIND command to group all the occurrences of a symbol to be replaced. Then, use the group_name option with the REPLACE command to globally change all the occurrences of the symbol. A message displays the number of bodies that are replaced.

Pin properties are reattached if a pin name on the new part is the same as a pin name on the first part. If the pin names do not match, the pin property becomes a symbol property.

Procedures

	Replacing a component
	Replacing components of a group

Return

Syntax

RETurn <cr>

Description

This command returns to the previously edited drawing. If the current drawing is modified but not written, the system saves a copy of the drawing before returning to the previous drawing.

The SHOW HISTORY command lists the drawings that you edited during the current session.

The SHOW RETURN command lists the drawings that the RETURN command will return to in the order that they will be accessed.

Rotate

Syntax

ROTate point

Description

See SET and DISPLAY for justifying text.

Related Commands

Add
Display
Mirror
Set
Spin

Route

Syntax

ROUTE point point

Description

To select the nearest pin or wire vertex for a ROUTE point, use the right button to select the point. Use any other button to select the nearest grid point.

Related Commands

Broute
Bwire
Wire

s2l

Syntax

s2l design

Description

This command runs the s2l (short2long) command on the current design. To update only the current page, type

s2l

The s2l command should be run on designs that have been upreved from SCALD to Design Entry HDL having property names that exceed 16 characters.

Before you run this command, you should execute the following two commands:

uprev design

uprev_write

When Packager-XL is run on the SCALD design, it replaces the shortened property name with the original property name after finding it in allegroprp.dat.

In HDL, Packager-XL does not perform this conversion. Instead, this functionality of Packager-XL is handled by the s2l command entered in the Design Entry HDL console command window.

The character limit for a property name in Design Entry HDL is now 31.

Scale

Syntax

SCAle {point1 point2 drawing_name | drawing_name point1 point2}

Description

When a drawing is smashed, all connectivity information is lost. The drawing can no longer be interpreted by the Compiler.

Related Commands

Script

Syntax

SCRipt { file_name | <cr> }

Description

The syntax for specifying the points is:

(X Y)

where X and Y can range from +16000 to -16000.

For example, the command vpdelete (0,0) will delete the viewport that has the coordinates (0,0).

	$< When the editor encounters this token in a script, it prints from the token to the end of the text line as a prompt in the message window, and then waits for one item of input. The input can be a typed line, a function key press, a mouse action, or a Ctrl+C. You cannot use a <cr> as a response to a user input request.
	$; This token also prints from the token to the end of the text line as a prompt and awaits input. This token accepts and interprets inputs until you enter a semicolon. If this token is included, the editor follows the prompt with the message "Type ; when done with user input.”

To abort a script, press Ctrl+C. To abort at a user input token prompt, type a semicolon.

SCRIPT <cr> brings up the File Browser. The user can then select the names of the script file from the form.

The SCRIPT command will not recognize GED commands that begin with the word "FORCE" (such as FORCEPROP, FORCEADD, FORCEBUB, FORCENOTE, and FORCEQUIT).

Related Commands

IGnore
Library
Set
Use

Searchstack

Syntax

SEArchstack <cr>

Description

Accesses the SEARCHSTACK BROWSER form. This form lists the libraries and directories that are currently accessed through the USE or LIBRARY commands.

BROWSE opens or updates the DIRECTORY BROWSER form that lists the contents of a library or directory.

USE places the active directory at the top of the search list and makes it your current working directory. There is no limit to the number of directories and libraries that can be in use at one time.

Section

Syntax

SECtion [pin_number]point

Description

To assign a specific section directly, enter a pin_number that uniquely defines the section and then point to the part. This avoids having to step through each section individually.

To remove section information from a part, use the REPLACE command to replace the sectioned symbol with a new copy of the part.

Example

To assign a specific section to an LS00 component, type section 11 in the console window and click the component in the design window.

Note: You can click the component again to change the section.

Related Commands

Backannotate
Pinswap
Set

Select

Syntax

SELect [group_name | DEFault][type...]{selection...| group_name |ALL}

where type is:

BOdies | PRoperties | NOtes | WIres | DOts

and selection is:

{Lpoint Lpoint} | Ctrl+Rpoint | Mpoint

Description

Provides a stretchable rectangle to specify the boundaries of a group. The group is defined as a collection of objects.

	If the first argument is a single-letter group name, that group will become the current group. If a group name is not specified, or DEFault is specified, a single-letter group name will be automatically assigned to the group that is created.
	The selection can be restricted to a specified type or set of types by providing one or more type arguments.

	You can click the left mouse button, drag the mouse to define the opposite corners of a stretchable rectangle which contains the objects to include in the group, and click again. You can draw additional rectangles to include other objects in the group.
	Press Ctrl+right mouse button to include individual objects in the group.

	Click the middle mouse button on another highlighted group to include its contents in the current group.
	Use the name of a previously created group to include its contents in the current group.

For example, the command select C A includes the contents of group A in group C.

Use ALL to select all objects in the current drawing.

For example, the command select A bodies all includes all the components in the current drawing in group A.

The console window displays the group name and the number of bodies, properties, notes, dots, and wires in the group.

Related Commands

Auto
Find
Group
Include
Exclude

Set

Syntax

SET {option | <cr>}

Description

Note: The SET commands in Design Entry HDL are temporary commands valid for the current session only.

SET Command Options	Description

General
save_workspace [on/off]	Saves window and toolbar settings when you exit Design Entry HDL. Example: set save_workspace on
click_to_type [on/off]	Activates a window when you click in it. Otherwise, a window is activated when you move the cursor into it.
autopan [on/off]	Enables panning behavior that lets you move the window over the drawing, rather than move the drawing inside the window.
rmb [on/off]	Changes the behavior of the right mouse button (RMB). If the option is turned off: Clicking right displays the context (pop-up) menu Pressing Ctrl+RMB causes a command-dependent action. If the option is turned on, this functionality is reversed, where clicking right causes a command-dependent action and pressing Ctrl+RMB displays the context menu.
multiformat_vectors [on/off]	Allows multiple-format signal names in the design. When you select this option: (), <>, and [ are considered special characters that designate a vectored signal. They cannot be used anywhere else in the signal name. The parentheses must be matched correctly and must contain either an integer or a parameter. Colon (:), comma (,) and ampersand (&) are considered special characters that represent concatenation. They cannot be used anywhere else in the signal name. When this option is not selected, ( ) and [ are considered legal characters that have no special meaning and can be used in signal names. They do not designate vectored signals. Only < > can be used to designate vectored signals. Comma (, ) and ampersand (&) are considered legal characters that have no special meaning and can be used in signal names. They do not represent concatenation. Only a colon (:) represents concatenation.
lmb [on/off]	Changes the behavior of the select and drag mouse operation and for running commands with strokes. If the option is turned off: Select an object on the schematic and drag the mouse to move the object. Press the left mouse button and drag the mouse to select multiple objects on the schematic. To exclude components, properties or wires from the selected objects, click the right mouse button and choose Exclude to exclude components, properties or wires from the selected objects. You can now click on one of the selected objects and drag the mouse to move all the selected objects. Press Ctrl or SHIFT and hold down the left mouse button to run commands with strokes. If the option is turned on: Press Ctrl, select an object on the schematic and drag the mouse to move the object. Press Ctrl or SHIFT, hold down the left mouse button and drag the mouse to select multiple objects on the schematic. To exclude components, properties or wires from the selected objects, click the right mouse button and choose Exclude to exclude components, properties or wires from the selected objects. You can now press Ctrl, click on one of the selected objects and drag the mouse to move all the selected objects. Hold down the left mouse button to run commands with strokes.
addform [on/off]	Opens the Add Component dialog box when you enter the add command in the console window and then press Return.
catform [on/off]	Displays the Category View tab by default when you open the Add Component dialog box or when you enter the add command in the console window and then press Return.
editform [on/off]	Activates the View Open dialog box when you enter the edit command in the console window and then press Return.
libform [on/off]	Activates the Search Stack dialog box when you enter the lib command in the console window and then press Return. If off, the current search stack is displayed.
ppt_browser [on/off]	Automatically opens the Physical Part Filter dialog box when you open the Add Component dialog box or when you enter the add command in the console window and then press Return.
preselect [on/off]	Activates the pre-select mode for Design Entry HDL menus.
default_page_border_name <name>	Specifies the name of the page border. Example: set default_page_border_name A SIZE PAGE
default_page_border_version <version>	Specifies the version of the page border symbol. Example: set default_page_border_version 1

Paths
ppt_optionset_path<path>	Specifies the path to the PPT Option Set file that you want Design Entry HDL to use by default. This file stores the default display settings for physical properties in the schematic and in the Physical Part Filter dialog box. Example: set ppt_optionset_path C:\MyDocs
attributes_dir <location of attribute files>	Sets the path for the location of attribute files, e.g. the default allegro_net.att is located at $CDS_INST_DIR/tools/fet/concept/attributes. Example: set attributes_dir $CDS_INST_DIR/tools/fet/concept/attributes
CAT_path <location of the directory that contains the category files>	Specifies the directory that contains the category (.cat) files used to organize components by category. The component categories are displayed in the Category View tab of the Add Component dialog box. The Add Component dialog box also loads the category files located in the libraries that you use in your project.

Graphics
MOVE_Orthog/MOVE_Direct	Draws wires that you move as Orthogonal or Direct.
ORthog_wire/DIrect_wire	Draws wires that you add as Orthogonal or Direct.
AUTORoute <ON/OFF>	Automatically routes a wire around objects when you move a component in the drawing.
AUTOHeavy <ON/OFF>	Automatically thickens a wire when you attach a bus signal name to it.
tap_add_signal [on/off]	Automatically inserts the specified tap symbol, bits, and wire names of bus taps when you use the tap command.
tap_body <symbol>	Specifies the tap symbol to be used in a schematic. Example: set tap_body tap
AUTODot <ON/OFF>	Automatically displays dots at wire connections.
DOTS_Filled/DOTS_Open	Adds open or filled dots at wire connections.
BOdy_dot_radius<integer>	Adjusts the diameter of dots at wire connections in symbol drawings. Example: set Body_dot_radius 25
LOgic_dot_radius<integer>	Adjusts the diameter of dots at wire connections in schematic drawings. Example: set Logic_dot_radius 25

Text
CAPSLOCK_OFF/CAPSLOCK_ON	Displays text as all caps.
SIZe <real>	Specifies the size of text (property name, property value, signal name, URL, or note) in the plotted schematic. The default value is 0.082 inches. Example: set size 1.000
CEnter_justified/LEft_justified/RIght_justified	Justifies text Left, Center, or Right.
user_editor <editor>	Specifies the text editor that Design Entry HDL displays for certain functions. Example: set user_editor wordpad
PIn_size <real>	Adjusts the size of the pin number displayed on the schematic to be larger or smaller. The unit is in inches. The pin number size is not related to Text Size you specify in this dialog box. Example: set pin_size 1.000
PRop_display<display_type>	Controls the way properties are displayed-Invisible, Name only, Value only, or Both name and value. Example: set prop_display Invisible
ROtate <ON/OFF>	Automatically rotates pin numbers that are attached to vertical pins.
STICKY_OFF/STICKY_ON	Deletes a default property from a schematic when the property has been deleted from a symbol drawing.
AUTOPath <ON/OFF>	Automatically attaches a PATH property to an added part.
pinprop_vis [on/off]	Controls the visibility of symbol pin properties when the symbol/component is instantiated on the schematic. Invisible does not display the symbol pin properties. Defined by Component makes pin properties visible or not depending on how property visibility is defined on the symbol. Example: Let us say that the symbol PQR.SYM.1.1 has the property NO_SWAP_PIN = TRUE attached to a pin on it. If the visibility for this property is set to Name in the symbol pin, and you select Defined by Component in Design Entry HDL, NO_SWAP_PIN will be visible on component PQR after it is instantiated on a schematic in Design Entry HDL. If you select Invisible, NO_SWAP_PIN will not be visible on the schematic, but will be visible in the symbol.

Color
COLOR_Arc <color>	Changes the default arc color. Example: set color_arc peach
COLOR_Dot <color>	Changes the default dot color.
COLOR_Wire <color>	Changes the default wire color.
COLOR_Note <color>	Changes the default note color.
COLOR_Property<color>	Changes the default property color.
color_body <color>	Changes the default body color.
occ_color <color>	Changes the default occurrence property color.
BACKground_color<color>	Change the default color for the drawing area. Example: set background_color red

Grid
DECimal/FRactional/Metric	Defines the grid type.
default_grid [on/off]	Displays or hides the grid.
default_grid [line/dot]	Displays the grid as Dots or dashed Lines.
default_grid <size> <mult>	Adjusts the grid size to be smaller or larger and displays every nth grid line to define where objects can be placed so that pins do not fall off-grid. This ensures the correct connectivity of wires and symbols. Example: set default_grid 0.150 6
default_body_grid [on/off]	Displays or hides the grid.
default_body_grid [line/dot]	Displays the grid as Dots or dashed Lines.
default_body_grid <size> <mult>	Adjusts the grid size to be smaller or larger and displays every nth grid line to define where objects can be placed so that pins do not fall off-grid. This ensures the correct connectivity of wires and symbols.
default_doc_grid [on/off]	Displays or hides the grid.
default_doc_grid [line/dot]	Displays the grid as Dots or dashed Lines.
default_doc_grid <size> <mult>	Adjusts the grid size to be smaller or larger and displays every nth grid line to define where objects can be placed so that pins do not fall off-grid. This ensures the correct connectivity of wires and symbols.

Plotting
wplot_thin_width	Specifies the width of lines used to draw thin wires, boundaries of components, and text on schematics. By default, the single line width is 1.
wplot_thick_width	Specifies the width of lines used to draw buses and thick wires on schematics. By default, the double line width is 10.
WPLOT_ADJust	Specifies the percentage by which to increase or decrease the size of the drawing. Design Entry HDL then plots the drawing on one or more papers of the specified size. For example, if you have a drawing with Cadence A size page border, the percentage specified is 100, and the paper size selected is A4. The Cadence A size page border is bigger in size than A4. So, the schematic is plotted on more than one A4 paper.
WPLOT_FIT_to_page	Adjusts the size of the drawing so that it fits into one page of the specified paper size. For example, you may have a drawing with Cadence A size page border, and the paper size selected is A4. Even though the Cadence A size page border is bigger in size than A4, the schematic is plotted so that it fits on one A4 paper.
Wplot_screen	Plots the portion of the schematic that is displayed on the screen.
Wplot_sheet	Plots an entire page.
WPLOT_PLOTTER	Sets the plotter to the name specified.

Output
AScii/NOAscii	Saves an ASCII representation of the logic.
BInary/NOBinary	Saves a binary representation of the logic.
CONFirm_write <ON/OFF>	Provides confirmation about saving the drawing.
DEPendency/NODependency	Saves an ASCII file with dependency information.

Check
CHECK_On_write <ON/OFF>	Runs a check whenever you save a design. Errors are recorded in cp.mkr and netlister.mkr.
CHECK_Missing_pins<ON/OFF>	Checks for pin properties that are no longer attached to pins.
CHECK_Unconn_wires<ON/OFF>	Checks for unnamed wires connected to only one pin (NC wires) and for named nets not connected to any pins.
CHECK_SHorted_pin<ON/OFF>	Checks for two pins on one component that are connected to the same wire, i.e. two pins shorted together.
CHECK_PARts_at_same_loc <ON/OFF>	Checks for overlaid components.
CHECK_Hidden_wires<ON/OFF>	Checks for wire segments hidden by portions of components.
CHECK_PIN_near_wire_endpt <ON/OFF>	Checks for wires that do not quite contact pins.
CHECK_Arcs_at_same_loc <ON/OFF>	Checks for overlaid arcs.
CHECK_PINS_at_origin<ON/OFF>	Checks for pins at the origin (0,0) in symbol drawings.
CHECK_TWo_wires_at_pins <ON/OFF>	Checks for wires overlapping a component at the pin.
CHECK_SIGNAMES <ON/OFF>	Checks for multiple names attached to the same signal.
CHECK_SIGNAME_in_body <ON/OFF>	Checks for the SIG_NAME property on a pin in a symbol file.
CHECK_Body_place_holders <ON/OFF>	Checks for placeholder components that appear due to changes in the related library.
CHECK_PRop_place_holders <ON/OFF>	Checks for placeholder properties that appear due to changes in the related library.
CHECK_PACk_sec_type_props<ON/OFF>	Checks for multiple SEC-type properties on an instance.

set NEXTgroup

This command sets the name of the group you want to create with the Find command.

set nextgroup A

find ls04

set HDL_Direct

This command sets options for the write console command. When you save a drawing, the write command is executed that writes the drawing onto the disk.

When the HDL_Direct option is on/off, the write command writes/does not write the following files in the sch_1 view of the schematic:

		verilog.v
		vhdl.vhd

		hdldirect.dat
		viewprps.prp

*.sir

Note: The hier_write and uprev_write console commands are not affected by the HDL_Direct option. These commands always write all the files onto the disk.

set sticky_on and set sticky_off

The default property <property> [with value <value>] is no longer on the body <symbol_name>. To turn the deleted default properties into non-default properties type SET STICKY_ON;GET;SET STICKY_OFF.

Note: The dangling properties will not be visible on the schematic or in the Attributes dialog box.

If you want the dangling properties to be converted to non-default properties, run the following console commands in the following order:

set sticky_on

get

set sticky_off

	If you want to delete the dangling properties, do the following:
	a.	Run the set sticky_off console command.

Run the write console command or choose File – Save to save the schematic.

Show

Syntax

SHow {option |<cr>}

Description

This command temporarily displays objects or information on classes of objects. The temporary information is erased when you redraw the screen.

To see all the SHOW options, type SHOW <cr> in the console window. The available SHOW options are displayed in the console window. The various SHOW options are described in the table below.

Attachments

Displays a line between visible properties and the property owner

COLor pt

Displays the color of the selected object

The color is displayed in the Design Entry HDL console window and as ticker text in the status bar.

COOrdinate pt

Gives the editor the location of the specified point in coordinates

DISTance pt pt

Displays the distance between two selected points.

	Clicking the left mouse button at two grid points displays the distance between the two grid points.
	Clicking the middle mouse button (in a three button mouse) or Ctrl+left mouse button at two points on the screen displays the distance between the two screen points.

The distance is displayed in the Design Entry HDL console window and as ticker text in the status bar.

Group pt

Highlights the group and lists the group name and contents. You can also specify the group by name.

History

Lists all drawings read in during the editor session

Keys

Lists the command string assigned to each function key

Modified

Lists drawings in all viewports that were modified but not saved during the editor session

Net pt

Highlights the selected net and displays the net name. You can also specify the net by name.

The net name is displayed in the Design Entry HDL console window and as ticker text in the status bar.

Origins

Displays an asterisk at each object origin (including text) on display

PIns

Displays an asterisk at each pin on display

PRoperties

Displays the names and values of all properties on the display (including any invisible properties)

PWd

Displays the name of the current project directory

The current directory is displayed in the Design Entry HDL console window and as ticker text in the status bar.

RELease

Lists the date and number of the current version of the editor

RETurn

Lists all the drawings that the editor can return to, in the order of return

Size pt

Displays the size of the selected text string (property name, property value, URL, signal name, note) in inches.

The text size is displayed in the Design Entry HDL console window and as ticker text in the status bar.

VECtors pt

Displays the pin names of the selected symbol

Example

To display the color of an object, type show color and click the object in the design window. The color of the selected object is displayed in the console window.

Signame

Syntax

SIGname {point signal_name | signal_name point }...

Description

This command attaches signal names to wires or pins. There are two ways to attach a signal name.

	Type SIGNAME and point to the location for each signal name. A rectangular box appears at each location. Type the text for the signal name and press <cr>.
	Type SIGNAME and enter one or more signal names. Specify the points to place the signal names on the drawing. The signal name is attached to the wire or pin that is closest to the specified point.

Signal names are handled internally as properties. For example, attaching a signal called BUS ENABLE to a wire is equivalent to attaching a property SIG_NAME=BUS ENABLE, to that wire.

When editing a SYMBOL drawing, signal names are known as PIN_NAME properties. They can be attached only to pin connections.

Related Commands

Smash

Syntax

Smash {point | group_name}...

Description

This command breaks a symbol into individual wires, arcs, and notes. Any properties attached to the symbol are deleted. The SMASH command works on individual bodies and on groups.

The SMASH command is useful for creating library symbol drawings. For example, once a 2-input AND gate exists, N-input AND gates can be made by using the following commands:

edit N AND.body

add 2 AND <pt>

smash <pt>

Procedures

	Smashing a component
	Breaking up components in a group

Related Commands

Filenote
Scale

Spin

Syntax

SPIn point...

Description

Related Commands

Mirror
Rotate
Set
Version

Split

Syntax

SPLit point point...

Description

This command splits a single wire into two wires or separates two or more objects that are placed at the same location. The currently selected item blinks so you know what you have selected.

Strokefile

Syntax

Strokefile {strokes_file | <cr>}

Description

This command loads a user-defined custom strokes_file. Strokes are user-defined line drawings you create with the mouse. You can customize command entry in the editor by using strokes.

When you access the editor, a set of default strokes is initially read from the file <your_install_dir>/tools/fet/concept/concept.strokes.

You can specify a file containing your own strokes by issuing the STROKEFILE command at the keyboard or by including the command in your START_CONCEPTHDL section of your .cpm file.

STROKEFILE <cr> brings up the Browser. You can then select the strokes_file from the form.

Related Commands

Loadstrokes

Swap

Syntax

Swap point1 point2...

Description

System

Syntax

System {operating_system_command | <cr> }

Description

To exit from the operating system and return to the editor, type Ctrl-D or Exit on UNIX-based systems and EXIT on Windows-based systems.

Tap

Syntax

TAp bus_tap_value point point...

Description

Mode 1:

1.	Enter one or more bus_tap_values -- such as 3..0, 5, 2 etc. separated by CARRIAGE_RETURNs. If you do not enter a bus_tap_value, a question mark is used for the tap bits.
2.	Choose the pin you want the tap to go to. Use any mouse button. Now, you have a wire attached to the mouse.

The next signal name you entered will be used for the next tap (i.e. go back to step 1 or 2).

Mode 2:

1.	Enter one or more tap names -- such as 3..0, 5, 2 etc. separated by Carriage Returns If you do not enter a tap name, a question mark will be used for the tap bits.
2.	Choose the bus you want the tap from. Use any mouse button.

4.	The next signal name you entered, will be used for the next tap (i.e. go back to step 1 or 2).

Advanced User Section

Restrictions: The tap command works with very specific kinds of tap bodies.

Rules for creating a tap symbol are

The tap symbol should

	Have exactly two pins.
	One pin MUST be at the origin of the symbol.

	This pin may NOT have a BN property attached to it.
	The second pin MUST be located on the positive x axis i.e. its coordinates should be (x, 0), where x > 0.

	The second pin MUST be on a grid point.
	The second pin MUST have a BN property.

It is recommended that the first pin have a \NAC \NWC on it and the second pin have a \NAC.

As a default the tap symbol CTAP from the standard library is used. If you want to change the tap symbol, use the command

set TAP_BODY <yourtapname>

For example,

set TAP_BODY ktap

Related Commands

Bustap

Textsize

Syntax

textsize <size in inches> <group name>

to change text size of properties in a group.

textsize <size in inches> Click on property

to change text size of a property.

textsize <size in inches> Click on note

to change the text size of a note.

Note: The above commands change the size of text in the plot.

Procedures

	Setting text size of a property or a note
	Changing size of text in a group

Undo

Syntax

UNDo <cr>

Description

Related Commands

Redo

Unhighlight

Syntax

UNHighlight [ Net | PArt | PIn | Any ] pt

UNHighlight [ Net | PArt | PIn | Any ] object_name

There are two ways to select an object:

To pick a component to be unhighlighted, point to the object and press the left button. Select a group by pointing to the required group and pressing the middle button.

object_name

If you prefer typing in the name of the object, you may use the second version of this command.

For nets, the object name is the signal name of the net, for example, FOO.

For parts, the object name is the value of the PATH property attached to that part or component, for example, 7P.

Wildcards such as * and ? may be used in specifying the object name,

for example, FOO*, 7*P, 7P.A*.

Description

The Unhighlight command is used to unhighlight an already highlighted object throughout the system.

Related Commands

Highlight
Dehighlight

Unix

Syntax

UNIx {operating_system_command | <cr> }

Description

To exit from the operating system and return to the editor, press Ctrl-D or type Exit on UNIX-based systems.

On Windows-based systems, the unix command opens up the command prompt. To know more about accessing the operating system from Windows-based system, refer to the System command help.

Example

To execute a particular Unix command, for example ls:

1.	Type unix ls in the console window and press Enter.

The files and folders in the project directory are listed.

2.	To exit from the operating system and return to the editor, press Ctrl-D or type Exit.

Updatesheetvars

Syntax

updatesheetvars

Description

This command updates the custom text variables for page numbers on all pages in a design.

Use

Syntax

Use {library_name | <cr>}

Description

This command specifies a working library. Library_name refers to the name of the library you want to use. If the library is not in the current directory, include the pathname.

There is no limit to the number of libraries that can be in use at one time.

USE <cr> brings up the file browser form. The user can then select a library_name from the form.

Related Commands

Directory
IGnore
Library

Vectorize

Syntax

VECtorize

Description

Note: This command works only on Solaris.

Version

Syntax

VERsion {point | group_name}...

Description

The separate versions of a symbol must all make reference to the same logic drawing. Using a different version of a symbol has no influence on the logic drawing defining it.

Procedures

	Versioning a component
	Versioning components of a group

Related Commands

Add
Replace
Rotate

Vpadd

Syntax

VPAdd <cr>

Description

When you create a viewport, the current drawing is copied to the new viewport and fit to the size of the window. Any operations you perform in either window appear on both copies of the drawing.

Select the active viewport by placing the cursor within the viewport. If the SET command option CLICK_TO_TYPE is ON, click the left mouse button within the window in order to make the window active.

Vpdelete

Syntax

VPDelete point...

Description

This command deletes an existing viewport. VPDELETE remains active until you enter a semicolon or select another command.

Related Commands

Vpadd

Window