Home > Community > Forums > PCB Design > Symbols & Padstacks

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Symbols & Padstacks 

Last post Thu, May 2 2013 1:45 PM by gveitch. 5 replies.
Started by gveitch 02 May 2013 09:01 AM. Topic has 5 replies and 912 views
Page 1 of 1 (6 items)
Sort Posts:
  • Thu, May 2 2013 9:01 AM

    • gveitch
    • Not Ranked
    • Joined on Thu, May 2 2013
    • Burling, Ontario
    • Posts 5
    • Points 85
    Symbols & Padstacks Reply

     Hello,

    I have a general question here.  Say I am given a Symbol (.dra & .psm) to use in my design. 

    I do not have the padstack used within this symbol (.pad).  Am I still able to open the .dra file in PCB Editor?

    Can I use the symbol in Allegro?  Can I pull the padstack file out of the symbol file somehow?

    Im asking because I have a symbol that I can open fine by itself in PCB Editor.  However, when I import it from Capture to Allegro in my design, it barks at me because it can't find the related padstack file.

    Thank you in advance.

    Filed under:
    • Post Points: 20
  • Thu, May 2 2013 9:22 AM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,413
    • Points 24,115
    Re: Symbols & Padstacks Reply
    You do need to have the PAD file, as you have found but it is cached in the DRA file. Open the DRA file and File>Export>Libraries, check all the boxes and Export to get the details exported to the current working directory. Check that your PSMPATH and PADPATH settings are set to pickup the files when the Logic (netlist) is loaded.
    • Post Points: 20
  • Thu, May 2 2013 11:49 AM

    • gveitch
    • Not Ranked
    • Joined on Thu, May 2 2013
    • Burling, Ontario
    • Posts 5
    • Points 85
    Re: Symbols & Padstacks Reply

     Thanks!  I am using PCB Editor 16.3.

    I don't have 'Libraries' under File>Export

    Only: 

    DXF, IDF, Sub-Drawing, IPF, Techfile, Parameters, Save desing to 16.01, save design to 16.2

    Where else would I find this?

    • Post Points: 35
  • Thu, May 2 2013 12:02 PM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,413
    • Points 24,115
    Re: Symbols & Padstacks Answer Reply
    The version would have been a help at the outset! Open the DRA file, Tools>Padstack>Modify Design Padstack, pick a Padstack in Options, Edit button, in the Pad Designer, File>Save As, the name will be filled in and the directory should be the current working directory. Repeat as necessary for the Design Padstacks.
    • Post Points: 5
  • Thu, May 2 2013 12:46 PM

    • mcatramb91
    • Top 75 Contributor
    • Joined on Thu, Jan 3 2013
    • Chelmsford, MA
    • Posts 101
    • Points 4,995
    Re: Symbols & Padstacks Answer Reply

    If you don't see it in the menu, I would run the batch command "dump_libraries" from a DOS command prompt.

    Type system on the Allegro command line to get to a DOS command prompt quickly then type the following:

    dump_libraries <symbol.dra>

    This will not only dump the Padstacks used in the symbol but also any related Shape Symbols that may be used in the Padstacks as well.

    Hope this helps,
    Mike Catrambone

    • Post Points: 20
  • Thu, May 2 2013 1:45 PM

    • gveitch
    • Not Ranked
    • Joined on Thu, May 2 2013
    • Burling, Ontario
    • Posts 5
    • Points 85
    Re: Symbols & Padstacks Reply

    Thank you both!

     Both methods work.  My bad not mentioning the version originally, did not realize how different they are.

    • Post Points: 5
Page 1 of 1 (6 items)
Sort Posts:
Started by gveitch at 02 May 2013 09:01 AM. Topic has 5 replies.