2
\$\begingroup\$

I made a custom footprint for an 8 pin TSSOP IC, using custom padstacks and creating a new package (no wizard). Each of the four pins on a side are 0.3mm wide and 0.5mm apart (BSC). In the .dra file everything looks right. However, when I add the components into a .brd file, the pins have a couple issues. On both sides, the two middle pins are 0.6mm away from the corner pins, and only 0.4mm away from each other. Not only are these the wrong distances, it also doesn't add up to the correct total distance from corner pin to corner pin (1.6mm instead of 1.5mm). The pins are also only 0.2mm wide instead of 0.3mm. Any idea what could be causing this? I know there are a bunch of options/settings that could contribute but I don't know what they are (fairly new OrCAD user). Image with blue pinsis .dra, red pins is .brd enter image description here enter image description here

\$\endgroup\$
11
  • 1
    \$\begingroup\$ Screenshots with labelled dimensions would really help. \$\endgroup\$
    – DKNguyen
    Jan 7 at 16:05
  • 1
    \$\begingroup\$ How are you measuring anyways? With the measurement tool? Or manually with the grid which may or may not be set to the same spacing between files? \$\endgroup\$
    – DKNguyen
    Jan 7 at 16:09
  • 1
    \$\begingroup\$ That's weird. What happens if you place the footprint on a fresh board? Or what do you see in the footprint file when you export it from your board file? \$\endgroup\$
    – DKNguyen
    Jan 7 at 16:33
  • 1
    \$\begingroup\$ @InBedded16 Weird. Does it happen if you just make a new footprint from scratch? Either with or without the wizard? Maybe it's just corrupt. Or worse, software bug. \$\endgroup\$
    – DKNguyen
    Jan 8 at 0:31
  • 1
    \$\begingroup\$ @DKNguyen yeah I just made a completely new footprint using the wizard this time and the same issue is persisting. Footprint looks fine, .brd file looks off. Not great. Probably time to set up tech support meeting. Thanks for your help! \$\endgroup\$
    – InBedded16
    Jan 10 at 23:32

2 Answers 2

3
\$\begingroup\$

The .brd file has its own copy of all footprints and padstacks from the first moment they were used. If it did not, then every time you moved the .brd file you would need to move every other file with it too, even footprints and padstacks in other directories. And someone mucking with a component or padstack for use in design could destroy its use in a previously existing design.

Similarly, footprint files also contain their own copy of the padstacks they are using which also need to be refreshed.

You need to refresh the footprint and/or padstacks in the .brd file if you ever want the .brd file to take on any changes.

For footprints, Place>Update Symbols

For padstacks which appear directly in the .brd file (and not those that appear through a symbol. Things like vias.) you go Tool>Padstack>Refresh.

It might vary a bit from version to version, so basically look in the menus that you normally use to place components or where you handle padstacks.

For that matter, you can also export all padstacks and footprints used in a .brd file with File>Export>Libraries

EDIT:

I just noticed you are talking about a new footprint. If the footprint had never been used before, then either the the units being used for either your footprint or .brd file are not what you think they are. Or the datums for various things like padstacks aren't what you think they are.

I always use move x, move y, move x y, move ix, move iy, and move ix iy commands for placement.

If it's anything else I would need to see the file. I've always used a wizard though but often need to modify things afterwards for weird irregular footprints.

\$\endgroup\$
1
  • \$\begingroup\$ Thanks for the input. I have refreshed both the padstack and the mechanical symbol several times and nothing changes. I don't think it is the units because the footprint is off in relation to itself not the rest of the board, if that makes sense. Would it be helpful to upload screenshots of the two instances? Can't upload the whole file. \$\endgroup\$
    – InBedded16
    Jan 7 at 16:05
2
\$\begingroup\$

General info (aiming for clarity, not perfect accuracy), feel free to correct me if I made dumbnesses.

Orcad uses DRA files to generate a "symbol" (footprint) file (PSM). This PSM file is what is ACTUALLY used in your board design. The filename of the PSM (without the extension) must match the value of the "PCB Footprint" field in your schematic.

SO, if your "PCB Footprint" == "smr0805", then orcad will look for a file called smr0805.psm, and copy that in to your design.

If you reference a PADSTACK in your SYMBOL drawing, orcad will look for a .PAD file of the same name, and copy that in to your design.

For both the SYMBOL and PADSTACK, orcad will search in directories you tell it to in the respective design feature paths setting.

Things to check:

  1. Ensure your DRA file has generated a PSM file. This should happen automatically, but you can ensure it happened.
    Create PSM file

  2. Ensure Orcad has the PATHs of both your PSM and PAD files that you are creating.
    PSM and PAD path entry box

  3. Orcad will use the FIRST file it finds, from top to bottom. So, ensure your paths are ordered "correctly". In my case, my directories are ordered so that the find priority is: project, company library, orcad standard library, downloads.
    Path entry dialog

  4. as DKNguyen said, ensure all your pads and symbols are up to date.

\$\endgroup\$
1
  • \$\begingroup\$ Hey thanks for laying all that out. When I make edits on the SYMBOL or the PAD I see those reflected in the .brd file so it is definitely finding the correct files. \$\endgroup\$
    – InBedded16
    Jan 7 at 22:37

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.