Cadence Breadcrumbs
CommunityForums PCB Design Capture CIS Equivalent to Altium's "Smart Paste" functionality in OrCAD...

Equivalent to Altium's "Smart Paste" functionality in OrCAD or Capture CIS?

There's two things I really miss from using Altium, one is the excellent find/replace and the other Smart Paste. I haven't been able to find a way to do Smart Paste, and it makes schematics extremely tedious. I've spent the last hour and a half looking for some kind of tcl/tk script that does even any part of the functionality of Atlium's Smart Paste, but I can't find anything. 

What I want is, for example, the ability to copy a bunch of net Aliases, and automatically generate offpage connectors or ports with the same names. There are some tricks to speed up this process that I've been able to find, but they're all just hacks around what Altium has offered for years. 

Where are all the community tcl/tk scripts? Someone must have written something like this before? Why isn't Cadence adding this kind of functionality? 

  • there have a tools named EDAisWARE_CoolEditBox-1_0 for free. you could use it.


    Thank you so much.  Exactly what I needed.  Only problem is I can't figure out how it's supposed to be installed.   I have 16.6, 17.2, and 17.4 installed.

    The installer isn't adding something to C:\Cadence\SPB_17.4\tools\capture\tclscripts\capAutoLoad, which I am familiar with.

  • If memory serves me correctly this is installed either in your %HOME%\cdssetup\tclscripts folder (which would then work for any version or %HOME%\cdssetup\OrCAD_Capture\version\tclscripts for a specific version. It may also go into %HOME%\MarketPlaceSkillApps so you'll have to check your installation.

  • I found some answers to my questions, so I'm going to post them here so they're searchable for future users...

    (SMART PASTE) - to answer my request for an equivalent for Altium's Smart Paste, the EDAisWare CoolEditBox collection of scripts is by far the closest thing I've found. It's very close to as powerful, though not as nicely implemented. EDAis seems to be the Israeli Cadence support partner. There is an old youtube video from EDAis which shows the functionality - ParsysEDA also has a video which highlights the CoolEditBox - Note that these are both quite old. I was able to download the script installation package from the OrCAD Marketplace, but it didn't install correctly, and when I re-organized the files to use the \capAutoLoad\ folder, the scripts were calling an old DLL which apparently isn't used anymore. The scripts did work, but I found an even better solution...

    I emailed EDAis support - - , and was given a file with updated scripts which don't have any of the DLL loading issues. I simply placed this folder (unzipped) directly into C:\Allegro\cdssetup\OrCAD_Capture\, and everything worked great. I'd highly suggest sending them an email asking for the latest CoolEditBox package. I would share the .zip here directly, but I'm not sure about the licensing, so I suggest emailing them directly. They were very helpful. 

    (FIND AND REPLACE) - I've been trying to find an equivalent to Altium's functionality with Find and Replace text the closest I've found so far is that there is a TCL script included in the Cadence install called capDesignUtil.tcl. This script can be found at C:\Cadence\<VERSION>\tools\capture\tclscripts\capDB\capDesignUtil.tcl, and it doesn't appear to be auto-loaded via the \capAutoLoad\ folder, so it needs to be invoked manually or added to the \capAutoLoad\ folder. The capDesignUtil.tcl script has some good commenting and examples in it, along with quite a few helpful functions that allow for searching, replacing, and limiting of scope to particular objects like Aliases or Ports, as well as limiting scope to page or project. It also seems to allow for regex wildcards, which the build-in Find/Replace doesn't allow for (terrible). There is an excellent youtube video which shows the usage here - The video is old, but a helpful comment points out that the example in the video can be updated like:

    source C:/Cadence/<VERSION>/tools/capture/tclscripts/capDB/capDesignUtil.tcl

    capDesignUtil::replaceAlias {ADDR_(.*)} {A\1}

    The generic format for this command is "capDesignUtil::replaceAlias {regex to find} {regex to replace}". Again, if you look in the capDesignUtil.tcl script directly, there are more examples in the comments as well as other functions (procs). 

    Also super important to note that you'll need to be really careful using this, as the UNDO functionality is limited. You don't want to accidentally find/replace in your entire project when you just mean to limit scope to a single schematic page!

  • Thank you very much.   EDAis does amazing things in Tcl.  Beats having to read the Tcl API for Orcad docs.

    If you find my SKILL utility over in the skill board, I ran into a problem with   capDesignUtil::replaceAlias

    It seems to do random things if the two strings are of different lengths.