Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
Exchange ideas, news, technical information, and best practices.
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.
It's not all about the technlogy. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
I would like to use Orcad Capture TCL scripting. Before the 1st hotfix of 16.3 the command window in Capture echoed all of the operations performed during the editing session. Also .captcl session script log file was available as it is written in the manual. Since 1st and till the 7th hotfix neither command window echo nor .captcl session script log fileare available, and this was my ultimate source of examples.
What can be done to get both features back? (Apart from uninstalling all of the hotfixes.)
BTW, I use Win7/64 and tried to run Capture as administrator, if this info may help.
I think the logging option was turned off to increase performance.
If I remember correct you can turn it on again
1. View->Toolbar->Command Window
2. In the command window write "SetOptionBool Journaling TRUE"
Try this out and let me know if it works out for you (NB: You'll probably have a line with that option set to FALSE in your Capture.ini file.)
In reply to Ejlersen:
Thank You very much, Your suggestion works. The capture.ini configuration option is called just "Journaling". After all, it would be good to see all this described in manual.
We are trying to turn off the Input arrows on the schematic that is new with OrCAD 16.3. We have tried the command with no success:
SetOptionBool DrawPinArrows Off
We get back the following message:
SetOptionBool <Option> < TRUE | FALSE | ON | OFF | 1 | 0 >. Option can be one of: RotateInstPropInContext ViewerShowPinInfo FlushImmediate Journaling
It appears this is not a valid command.
In reply to PCBLady:
I think that the option may only have been enabled after applying a hotfix, if you are running a base release, this setting may have no effect. As an alternative, try the Capture.ini file, usually alongside Capture.exe in the installation, close Capture before attacking this, there will be a "DrawPinArrows" entry in there, in the Preferences section, True is the default value, set the text value to False, save the changed file, restart Capture and see if that makes any difference, if not, you may need an update (hotfix) applied.
In reply to oldmouldy:
Well.....that certainly fixed it after updating with the latest hotfix.
Thanks for the tip!
I am trying to get into Tcl/Tk - and it's not going so smoothly!
Is there anybody still hooked up to this Forum?
In reply to Geoff:
I'm trying to write some scripts as well, but it takes lots of time since there is lack of documentation. Is anyone aware of some document describing database access functions? I have a specific question, for example: I need to select some wires then access and modify flat nets properties. How do I get to flat net properties whet the object I select is a wire? (I'm managed to get from wire object to net object, but how can I get to the flat net?)
All the best,
In reply to Azef:
You can look at the document in <installation>\tools\capture\tclscripts\OrCAD_Capture_TclTk_Extensions.pdf for examples and description. You can also look at samples in <installation>\tools\capture\tclscripts directory.
If you are selecting wire on schematic - see GetSelectedObjects command examples in the document.
Flatnets are calculated by Capture schematic on runtime. Flatnets do not have properties in OrCAD Database. The properties of Flatnets are propogated from the net occurrences. To access the properties at any object see section "3.2.24 Iterate over all effective properties of any object".
Looking at the XML version of the design is one of the best ways to see the structure of the database of your design and to understand which object's property you need to modify to get the desired result. From the TCL command line execute the following command
XMATIC_DSN2XML <DSNFilename> <outputXmlName>
The above command will create an XML output file that shows all the database objects in the design and their relationships.
The document I have mentioned above has examples of TCL iterators that allow you access to any objects in a design. The Effective property examples in the document show you how to modify properties.
If you need further help - you can send your questions to firstname.lastname@example.org
In reply to paragc:
Thank You for the information.
I used GetSelectedObjects and was able to iterate properties of the wire and then - net, but was unable to get from net level further. From XML export You suggested, I understood that what I need is NetOccurence instead of Flatnet, but I still got a question: how can I get to NetOccurence from NetScalar (or Net)?
Hi,In the OrCAD_Capture_TclTk_Extensions.pdf, if we search for GetNetOccurrence we find the following:GetNetOccurrence(pNet, status) : returns DboNetOccurrenceParameters:pNet: DboSchematicNet *status: DboState &The function is of DboInstOccurrence (which is Schematic occurrence) which takes schematic net. So for a wire net, we need to get the schematic net and using it we can get the net occurrence from the schematic occurrence. Following are the commands:# Get the wire objectset lWire [GetSelectedObjects] set lStatus [DboState]# Get the Wire Netset wireNet [$lWire GetNet $lStatus] #Get the Schematic Net for the wire Netset lSchNet [$wireNet GetSchematicNet]# Get the schematic occurrence set schOcc [GetInstanceOccurrence] # Get the Net occurrence from the # schematic occurrence for a given schematic netset lNetOcc [$schOcc GetNetOccurrence $lSchNet $lStatus]Thanks
In reply to Kuenga606:
I tried the above example on a sample schematic I had and what I got back confuses me. I have a net that has the netname "test2" selected and I followed the commands from Kuenga606 and what I got as a response to lNetOcc was "_203f310a_p_DboNetOccurrence". I assume this is what they call in the TCL/TK Extensions App note a "CString". I tried running the command
puts [DboTclHelper_sGetConstCharPtr $lNetOcc]
and I get back the following
[ 1]No matching function for overloaded 'DboTclHelper_sGetConstCharPtr'
What does this mean? How do I see the actual netname "String"?
In reply to rob22:
lNetOcc is the object of class 'class DboNetOccurrence '. This object understands the API listed under 'class DboNetOccurrence' in the PDF 'OrCAD_Capture_TclTk_Extensions.pdf'. To get the name from the object we need to use the following API:
GetNetName(name) : returns DboStateParameters:name: CString &
set lCStrObj [DboTclHelper_sMakeCString]
$lNetOcc GetNetName $lCStrObj
puts [DboTclHelper_sGetConstCharPtr $lCStrObj]
To get the flatnet name we need to do the following:
set lFlatNetObj [$lNetOcc GetFlatNet $lStatus]
$lFlatNetObj GetName $lCStrObj
puts [DboTclHelper_sGetConstCharPtr $lCStrObj]
I am trying to iterate over libaries in CIS and tryng make copy part from existing library to new library with new name. I have difficulites to try proper commands for it.
To access libary I used these commands:
#to access sessionset lSession $::DboSession_s_pDboSession set lStatus [DboState]DboSession -this $lSession# to access existing libraryset lLibraryPath [DboTclHelper_sMakeCString C:/Cadence/tcl/DISCRETES.OLB]set lLib [DboSession_GetLibAndSchematics $lSession $lLibraryPath $lStatus]# the iterate via to wanted package...set pkgNameIter [$lLib NewPackageNamesIter $lStatus]set pPkgName [DboTclHelper_sMakeCString]set lStatus [$pkgNameIter NextName $pPkgName]# create new libraryset newLib [$lSession CreateLib [DboTclHelper_sMakeCString "C:/Cadence/tcl/test.OLB"] $lStatus]
DEADLOCK here... I have no exact imagination of data // commands model and I am unable to copy the part under new name.
I will appreaciate some guide how to copy part from one olb file to another
Many thanks in advance.
Typing the above command by itself did not work for me, so I contacted Cadence. See below for their response:
Please run the following two
commands in the TCL shell-
This should then enable the
display of journaling commands n the TCL shell.
Running both the commands worked for me.
I`m trying to get the objects which are connecting by a wire I select,
so I iterate all thing in a page and try to find if there are matching netname with the selecting wire,but it is Inefficient.
How can I do with another better way?