Stats

  • Locked Locked
  • Replies 4
  • Subscribers 166
  • Views 18908
  • 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

Getting libraries and footprints from a PCB Editor file for use in the original OrCAD Capture file.

ColdBoondock

 I'm quite new to OrCAD and all the software packages, and so have a very low understanding of things while I'm trying to learn.

 My problem is that I have an exisiting Capture file that I would like to update, add parts to, and export to the PCB Editor. The capture file has several issues when trying to make a netlist because the file I was given refers to places on disks and in memory that I don't have access to. I have the original PCB file made from the original Capture file and have been trying to work backwards to get the information needed for Capture (footprints & libraries).

 I used File>Export Libraies in the PCB Editor which dumped the libraries and left them in a directory. These files have.txt .dra .pad .psn and .fsm extensions. I've done some searching to see how some of these files are used in storing the physical information about the parts they describe, but I'm sure I don't understand it completely yet. 

 Ultimately, my question is how, if it's possible, do I use those .dra et. al files to allow Capture to understand the components in the schematic so that it can make a usable netlist to export to the Editor.

 The exact error I'm getting is that, for a good number of parts, the associated files are "not found in PSMPATH or must be "dbdoctor"ed".

  I apologize in advance for my simplistic level of understanding and thank you for taking the time to try to help me.

  • Dhamodharann
    What ever you had done is been correct. You can use the converted .dra file use it for capture directly.Before that you have to assign the paths for the footprint library.Open pcb editor-----> setup---> user preference editor---->paths--->library----> padpath---->C:\CADENCE\SPB_16.5\SHARE\PCB\PCB_LIB\SYMBOLS\ psm path.----->C:\CADENCE\SPB_16.5\SHARE\PCB\PCB_LIB\SYMBOLS\ . After that apply. save it,then update the net list. With this you wont get any warnings. Before updating check schematic symbols pin numbers and footprint pin numbers are get correctly matched.In case any mismatch means the error will be occured. Thanks & Regards.. Dhamodharan
  • ColdBoondock

     Thank you for the quick response.

     When I first netlist and export the Capture file to the Editor, I get a blank canvas. If I export the netlist out of the Editor I get a text file showing the components that should be there, which would mean that the netlist at least exists and is getting exported.

     I added the directory where the exported library files are saved to the list of directories in the paths for the padpath and the psmpath.  I resaved the design but am unsure of how to refresh/update the netlist. Possibly something simple that I just haven't found yet?

     I tried re-netlisting and re-exporting the design from Capture to see if having the updated preferences would let it make the right connections, but I get the same result.

     

    Edit: This seems to have drastically reduced the number of those  PSMPATH/dbdoctor warnings it was generating. Now It just seems to be missing data for a couple of headers, diodes, and inductors. Is there a reason why exporting the libraries would not have output the data for these types of items? Would there be some way to specifically export the data for those specific components, assuming I can find them in the Editor File? If there is, I'd suspect I could add those files to the directories in the paths and it would work properly.

     Edit 2: I was able to recover the footprint files from a number of other places in memory and disks and place them in the directory added to the paths. It seems to like it now. Thank you very much! Regards.

  • steve

    You will see a blank canvas when you first import the netlist. Parst aren't dumped on the canvas. Have a look at Place - Manually and you should see a list of parts that you can click on and bring in either one by one or by clicking the part in the schematic (or drawing a window areound). If you want you can use Place - Quickplace and then place based on property or schematic page but you'll need a Board Outline first so you can place around the edges of the PCB. You can also get a list if you use the Setup - Application Mode - Placement Edit then look at the fold out Options menu on the right hand side. There are videos showing all this plus more on youtube. Look for channel parsyseda.

  • ColdBoondock

    Thank you, Steve, that's helpful! I'll be looking into that.

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.