Stats

  • Locked Locked
  • Replies 23
  • Subscribers 165
  • Views 10123
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Maintain "Persistence" of Find after done command is completed while routing.

excellon1

Hi.

When in EtchEdit mode or general edit mode for routing I notice that when routing is finished by selecting "Done" the settings in the find dialog
settings get blown out.

I am trying to maintain the relationship between adding etch with find after the fact. In other words after etch is added to the canvas I want the
find dialog to retain ( Cline Segs, Pins, Nets, Rats T etc ) so that those items are selectable for either info or basic editing after the fact.

Is there any way to accomplish this other than creating a macro for find entities ?.

Basic idea is to have find pre-checked for a given command such as routing etc.

Something like a "IF Done" at the macro level would be helpful too though I do not know if something like that is supported ? , Like execute
the macro, after done is selected as an action then the macro runs the part to check find dialog items.

Thanks Paul. 

  • lcan
    in reply to excellon1

    Hi Paul,

    Exactly.  I was hoping to keep the SKILL commands simple for easy editing by myself and others. PCB Design is my more core competency, not SKILL coding.

    Here is what I use for "Placement mode":

    axlCmdRegister("wtm_PlaceKeyPad" `wtm_pe_MKeyPad)

    procedure( wtm_pe_MKeyPad( )

    axlSetFunckey( "/" "prepopup; pop dyn_option_select 'Selection set@:@Select by Lasso'" t)
    axlSetFunckey( "*" "replay C:/Cadence/SPB_17.2/share/local/pcb/scripts/toggle_rot_sym_orig_increment.scr" t)
    axlSetFunckey( "-" "replay C:/Cadence/SPB_17.2/share/local/pcb/scripts/toggle_abs_sym.scr" t)
    axlSetFunckey( "Home" "prepopup; pop dyn_option_select '@:@Swap components'" t)
    axlSetFunckey( "Up" "iangle 90" t)
    axlSetFunckey( "CUp" "move; ipick_to_gridunit 0 +1" t)
    axlSetFunckey( "Pgup" "prepopup; pop dyn_option_select @:@Rotate" t)
    axlSetFunckey( "Right" "prepopup; pop dyn_option_select '@:@Swap pins'" t)
    axlSetFunckey( "Down" "prepopup; pop mirror" t)
    axlSetFunckey( "SDown" "prepopup; pop dyn_option_select @:@Mirror" t)
    axlSetFunckey( "CDown" "move; ipick_to_gridunit 0 -1" t)
    axlSetFunckey( "Pgdown" "prepopup; pop dyn_option_select @:@Move" t)
    axlSetFunckey( "End" "prepopup; pop dyn_option_select '@:@Show Rats'" t)

    axlSetAlias( "f1" "replay C:/Cadence/SPB_17.2/share/local/pcb/scripts/ff_pins_only.scr")
    axlSetAlias( "f2" "replay C:/Cadence/SPB_17.2/share/local/pcb/scripts/ff_text_only.scr")
    axlSetAlias( "f3" "replay C:/Cadence/SPB_17.2/share/local/pcb/scripts/ff_sym_only.scr")
    axlSetFunckey( "Left" "settoggle CMD f1 f2 f3; $CMD" t)

    axlSetAlias( "t1" "wtm_EtchKeyPad")
    axlSetAlias( "t2" "wtm_PlaceKeyPad")
    axlSetFunckey( "F12" "settoggle CMD t1 t2; $CMD" t)

    ; Set a .5MM grid for working in Placement edit mode.
    grid = axlDBGridGet("TOP")
    grid->name = 'all
    grid->xGrids = 25.000
    grid->yGrids = 25.000
    axlDBGridSet(grid)

    axlShell( "placementedit" )
    axlShellPost( "setwindow form.find; FORM find all_off; FORM find Symbols YES; setwindow pcb; move; setwindow form.mini; FORM mini stretch YES; setwindow pcb; prepopup; pop dyn_option_select 'Options@:@Rotation point@:@Symbol Origin'; prepopup; pop dyn_option_select 'Options@:@Rotation type@:@Incremental'; done")

    ); procedure

    Again, to invoke these I create a new popup on the Main Pulldown menu by putting this in the C:Cadence\SPB_17.2\share\local\pcb\menus\Allegro.men file...

    */
    POPUP "&Application Mode"
    BEGIN
    MENUITEM "Placement Edit", "wtm_PlaceKeyPad"
    MENUITEM "Etch Edit", "wtm_EtchKeyPad"
    END

    Hope you find it useful.  You will notice I use the mini keypad on the right of the keyboard, that's just my historical preference.  Modification to use the main keyboard keys should be a straightforward process.

    Bill

  • steve
    in reply to lcan

    Lots of you are editing the menu file which isn't really recommended anymore - if the menu file changes you won't see the updates. You'd be better off using the skill file to load your menu. Details can be found here:- http://orcad.co.uk/images/PDF/PCB_Editor_customization.pdf Page 2 gives you a sample skill file that builds a user-defined menu, you then use an allegro.ilinit file to auto load this menu when you start the tools.

  • lcan
    in reply to steve

    You are absolutely correct, Steve.  My method of using a manually edited Allegro menu file then placed in the local folder is somewhat stale, while functional.  Perhaps that was why I mentioned SKILL coding was not my core competency. I hope folks find the main functions useful. I will research your suggestion, thanks!

    Bill

  • riklee
    in reply to lcan

    I'd like to add that you should not be storing your scripts (or views, extract files etc) in the Cadence hierarchy. There is a scriptpath variable  that you can set to point to your scripts in a local directory e.g. %home%/pcbenv/scripts

    If you had to reinstall the release you could end up losing all the work you put into making the scripts and any other files that you use.

  • lcan
    in reply to riklee

    Rik, thanks for the ancillary data management tip although I would disagree when the customer installation is multi-user server. Backups are mandatory, regardless of installation type.

    What I hope does not get lost is the original topic, the need for a smoother interface in the PCB Editor. Although much wonderful work has been done to Allegro in the past 12 years, there is still a strong need to overhaul its user interface to capitalize on all the robust functionality the Application Modes offer. It is this area where our users want Cadence support and Engineering to focus. With all this excellent new functionality and analysis, putting it at the PCB Designers/Engineers fingertips is essential. Lets focus a little more on what people are asking for that makes the tool easier to use, like Paul did.

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.