Home > Community > Forums > PCB Design > How can I utilize netlist & device files to place a self-created PCB package symbol

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: *

 How can I utilize netlist & device files to place a self-created PCB package symbol 

Last post Tue, Nov 20 2012 6:12 PM by AamirZ. 7 replies.
Started by Kennn 02 Jun 2010 03:32 PM. Topic has 7 replies and 3065 views
Page 1 of 1 (8 items)
Sort Posts:
  • Wed, Jun 2 2010 3:32 PM

    • Kennn
    • Not Ranked
    • Joined on Wed, May 5 2010
    • Posts 7
    • Points 140
    How can I utilize netlist & device files to place a self-created PCB package symbol Reply

    I am a new user of Allegro PCB editor of OrCAD 16.2. I want to modify an existed PCB design (*.brd) without schematic.
    My question is how can I utilize netlist & device files to place a self-created PCB package symbol.

    I think I need to add my package symbol to Allegro's library. To make Allegro recognize it's name. Then when I modify
    netlist file with the name, Allegro will link to the *.dra file which I created.

    If my thinking is correct, how can I let Allegro to recognize a new symble.

    thanks

    • Post Points: 35
  • Thu, Jun 3 2010 9:10 PM

    • Ejlersen
    • Top 10 Contributor
    • Joined on Mon, Jul 28 2008
    • Aalborg, Copenhagen
    • Posts 569
    • Points 10,080
    Re: How can I utilize netlist & device files to place a self-created PCB package symbol Reply

    Hi

    I'm not sure that I understand exactly what you want

    Do you want to change the footprint (package symbol) of an existing component on the brd file?

    Do you want to insert a brand new component on the brd without adding it to the schematic? If so, what type of component are we talking about since you don't want to place it on the schematic first for documentation purposes?

    Please let me know and it will be easier to help you.

    Best regards

    Ole

    Best regards Ole
    • Post Points: 35
  • Fri, Jun 4 2010 6:09 AM

    • Rik Lee
    • Top 50 Contributor
    • Joined on Tue, Dec 2 2008
    • HOME, SC
    • Posts 166
    • Points 2,730
    Re: How can I utilize netlist & device files to place a self-created PCB package symbol Reply

    You would first export a netlist with properties using the menu selection

    File >Export >Netlist w/Properties

    Open the netlist in a text editor such as Textpad. Make sure the text editor you are using doesn't inset white spaces as characters.
    Modify the netlist to include the new package in the "$PACKAGES" section. The format you need to follow is:

    ALLEGRO_SYMBOL_NAME ! DEVICE_FILE_NAME ; REFDES1 REFDES2 ... REFDESn

    If there are special characters, such as a hyphen, you need to surround the name with single quotes.

    Sample:

    $PACKAGES
    CAP300 ! 'FCAP-1' ; C1 C2 C3
    DIP14_3 ! '74LS00-2' ; U96
    DIP14_3 ! '74LS74-2' ; U69

    If you want to add nets to the design add them to the "$NETS" section with the following syntax (Again, if special characters are used surround the net name with single quotes)

    netname ; refdes.pin refdes.pin ...refdes.pin

    sample:

    $NETS
    '-MTCAS' ; R1.3
    '-PRE' ; K1.6 R1.8 U69.4 U69.10
    '-S0' ; U69.1 U69.13
    A ; R1.7 U1.13 U69.12

    Save the netlist as a new name.

    If you don't have the device file for the symbol you can create that using "File >Create Device" when in the symbol Editor.

    Open the design you want to modify and import the new netlist using the menu selection

    File >Import >Logic

    Select the "Other" tab
    Browse to the netlist file using the epsilon (...)
    Enable (Check) the "Supersede all logical data" checkbox.
    Select "Import Other"

    You should see the component available in the Place >Manually dialog. If you do not ensure that all of the pads, .psm and device file are in the correct paths; padpath, psmpath and devpath respectively.

    Place and route the component.

    You will need to update a schematic if you want this addition documented for the future.

    Hope this helps,

     Rik

    • Post Points: 20
  • Fri, Jun 4 2010 7:48 AM

    • Kennn
    • Not Ranked
    • Joined on Wed, May 5 2010
    • Posts 7
    • Points 140
    Re: How can I utilize netlist & device files to place a self-created PCB package symbol Reply

    Hi,

    I want to insert a new package on the brd without adding it to the schematic. The reason is that this design was releasing from a company. Their schematic was designed by Viewdraw software and I don't own the software. Accordingly, I decide to modify the PCB by netlist.txt & device file.

    Now I have a problem to add a self-created package symble. I don't know how to add my own symble to the brd after I created it. Is there a specific folder to save the *.dra, and device file, then Allegro can recognize my symble?

    thank you for your kindly response

    Ken   

    • Post Points: 5
  • Fri, Jun 4 2010 8:27 AM

    • Kennn
    • Not Ranked
    • Joined on Wed, May 5 2010
    • Posts 7
    • Points 140
    Re: How can I utilize netlist & device files to place a self-created PCB package symbol Reply

    Hello Rik,

    This is really a detailed response. I followed your indication and success to add an existed symbol. But I do'nt know other ALLEGRO_SYMBOL_NAMEs which not exist on the exported netlist.txt. And I don't know how to sign a self-created symbol to be an ALLEGRO_SYMBOL_NAME.

    Do you know where can I get an ALLEGRO_SYMBOL_NAME list and how to sign my own symbol be a ALLEGRO_SYMBOL_NAME?

    You have mentioned "padpath, psmpath and devpath", so I tried to type each of them to the command line and got error "E- Command not found: padpath". I am not understanding this part, can you explain to me again? 

    I know it spend time to answer questions, but it would be very helpful to me. Thank you very much!

    Ken

    • Post Points: 35
  • Mon, Jun 7 2010 6:09 AM

    • Rik Lee
    • Top 50 Contributor
    • Joined on Tue, Dec 2 2008
    • HOME, SC
    • Posts 166
    • Points 2,730
    Re: How can I utilize netlist & device files to place a self-created PCB package symbol Reply

    Hi Ken,

    The ALLEGRO_SYMBOL_NAME is the name of the symbol that you created or have access to in your library such as a DIP14 or CAP300 which you want to add to your design.

    The psmpath, padpath, and devpath are the paths to your library parts.

     ~Rik

    • Post Points: 5
  • Tue, Nov 20 2012 6:09 PM

    • AamirZ
    • Not Ranked
    • Joined on Sun, Oct 14 2012
    • Posts 15
    • Points 240
    Re: How can I utilize netlist & device files to place a self-created PCB package symbol Reply

    Hi Ken

    "padpath, psmpath and devpath" are not run through command line. These are settings follow the process SETUP>USER PREFERANCES> in categories select PATH>LIBRARY and set the paths.

     Aamirz 

    • Post Points: 5
  • Tue, Nov 20 2012 6:12 PM

    • AamirZ
    • Not Ranked
    • Joined on Sun, Oct 14 2012
    • Posts 15
    • Points 240
    Re: How can I utilize netlist & device files to place a self-created PCB package symbol Reply
    Hi Ole

    Want to change D2PAK footprint with TO263-3 on Orcad/Allegro PCB Editor

    I have a PCB *.BRD file. No schematic no netlist. On board 03 D2PAK footprint placed U28, U29, U30. I want to replace a only U29 footprint D2PAK with To263-3. Any body know the procedure to replace the footprint without schematic and netlist.

    Thanks and regards

    Aamir
    • Post Points: 5
Page 1 of 1 (8 items)
Sort Posts:
Started by Kennn at 02 Jun 2010 03:32 PM. Topic has 7 replies.