• State
  • Locked Locked
  • Replies 4 replies
  • Subscribers 81 subscribers
  • Views 1074 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

DIM100 connector footprints

ENVER CANDAN
Prodigy 60 points

Other Parts Discussed in Thread: CONTROLSUITE

Hi,

I am trying to come up with an easy way to add DIM100 connector for my controlCARD to my circuit board. I use Cadence and Allegro for schematic and PCB design. I went through control suite's hardware starter modules, there is schematic file in orcad. there is also a footprint name assigned to the model in the schematic but this footprint file does not exist anywhere in controlSuite.

In control suite it says "Simply copy and paste the schematic into a design and import the PADS or GERBER drawing into a PCB and the DIM100 or DIM168 connector for the controlCARD is designed onto your board." however it is not that easy for me. I try to import pads to allegro, it generates this error.

Expected VALID_LAYER N, where N <= 2 (Total route layers)!!! on line 12310

Line 12310: VALID_LAYER 3
ERROR: Finished with errors.

Even though this operation import pads to a board, when I will try to generate netlist for my design in ORCAD schematic, it will say missing footprint for the connector model schematic file that TI provided in control suite.

I feel like it must be a really easy procedure but I couldn't figure it out. Any suggestions?

  • 0
    TI__Guru 57255 points

    Enver,

    I just tried this process and ran into the same issue.

    If you delete out VALID_LAYER 3 through 64 (lines 12310 through 12371) in the .asc file you can get rid of the importing errors.  After this, Allegro will be able to import in the PADS file and everything should work fine.

    For convenience, I've attached the .brd file that I received when I went through the process.


    Thank you,
    Brett

    TEX016_DIM100HSMr1_0_Copy.brd
  • 0 in reply to Brett Larimore
    Prodigy 60 points

    Hi Brett, thanks for your reply.

    Deleting out lines worked well but the file you sent doesn't address my footprint problem.
    I mean in the schematic file, footprint section for controlcard is assigned to a file but this file doesn't exist anywhere.
    And the file that you attached is .brd. Since it is not footprint when I try to create netlist from the schematic it generates missing footprint error.

    Do you have any suggestion for that?

    Enver

  • 0 in reply to ENVER CANDAN
    TI__Guru 57255 points

    Enver,

    Unfortunately, I am only partially aware of how the Cadence system works.  What I say below should be possible (and is possible in Mentor's suite), but the steps may be a bit different for Cadence.

    Can you somehow export the DIMM100 footprint in the brd file into a Cadence decal/footprint?  I would think you'd then be able to assign this new decal to the DIMM100 schematic symbol.

    Hopefully this helps.


    Thank you,
    Brett

  • 0 in reply to Brett Larimore
    Prodigy 60 points

    I figured out how to do this. After, connector board is imported to Allegro, go File - Export - Libraries;

    Then select package symbols and directory, click export.