Stats

  • Locked Locked
  • Replies 15
  • Subscribers 167
  • Views 5807
  • 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

Advice on moving forward. (I believe unit's of measurements caused an issue)

StepscanDarcy

I've posted about this a few weeks back, but work has been hectic, and I haven't had a chance to work with ORCAD since.     Here is what's going on.   I have two boards that have  30 pin connectors, which have become obsolete.   We chose a new one, and I got to work making the changes to the board design.   The first board is complete (but being reviewed by someone for me by the company handling the prototype), but when I went to make the changes to the second board, I ran into major issues.   The second board only had one change to make( board #1 had 5).   This change uses the exact 30 pin connector that was changed on board #1.   

When I replaced the footprint on board 1, it simply replaced the old one and broke several connections related to the pins of the connector.   Some simple routing fixed it up in not much time at all (when I figured out what I was doing).   

I was expecting the second board to be done in one afternoon because it required much less work.   To my surprise , replacing the connector on this board, created havoc.  There are ratsnests EVERYWHERE.   So many connections are broken, that it will take me forever to fix it.  

After doing some digging around, I found a possible cause.   Board #1 used one unit of measurement, and board #2 used another(made by different companies), from an old post I found on the forums.   The fix recommended on this thread didn't work for me at all, so now i'm wondering what my next move should be.


Should I just remake the footprint, using the same units as the board?   Or should I change the units of the board to match the units of the footprint?   Is there an even better option that I haven't considered?   Or have I done something else wrong entirely?

Parents
  • excellon1

    Hi to echo what Robert and Redwire said I think the best solution is to make sure your pcb and schematic agree first, if they do perform a forward annotation from the schematic to the board with the new pcb footprint for that connector. Before you forward annotate you can un place your existing footprint. In capture re generate the netlist and choose the options. Uncheck " Allow etch removal during eco"   Check Place changed components
    never option.

    When you are back in your board place the new footprint.

    FYI it is far better to "Forward Annotate" from the schematic to the board to make changes. Key is to insure both schematic and pcb agree from a netlist perspective.

  • StepscanDarcy
    in reply to excellon1

    So, this is what happened.  

    I started over again today from scratch.   Changed the 'footprint' name in capture, and re-generated the netlist with the options you suggested.   I open the newly generated file in pcb editor, and the DRC errors are still there.   I don't know what's going on.

Reply
  • StepscanDarcy
    in reply to excellon1

    So, this is what happened.  

    I started over again today from scratch.   Changed the 'footprint' name in capture, and re-generated the netlist with the options you suggested.   I open the newly generated file in pcb editor, and the DRC errors are still there.   I don't know what's going on.

Children
  • Robert Finley
    in reply to StepscanDarcy

    Go back to the original board again, force run the DRC process.  See if you have any DRCs on the released data.

    I suspect Allegro deliberately does update DRCs each time a layout is opened to keep people with huge layouts from losing their minds waiting for DRCs they aren't ready for, each time they open a board. 

    Whether the board was released with zero DRCs is a factor of taking the time to create rules and region rules to resolve them.

  • StepscanDarcy
    in reply to Robert Finley

    Hey Robert, thanks for taking the time to help me out here, I appreciate it.  Let me fill you in on the newest info.   So, when I open even the original board (no changes by me) and run a DRC update.   All of the problems I was seeing before are present(maybe even more, there's almost 6000!)   So what does this mean?   Did the original board contain all of these errors?    It's not letting me export a gerber because of these, so how was it done before?   I'm too new at this, I have no idea what to do.

  • Dale Peterson
    in reply to StepscanDarcy

    Without seeing your board and based upon what I'm reading. I can only assume that you have little tiny disconnects everywhere. Not DRC violations unless things shifted around so badly that everything is banging together. Did you try adjusting the design's "Accuracy" settings? If the older footprint had graphics parked out to let say-.0001 and the new database was set at .001 (3 place accuracy). During the part swap out on your new layout. OrCAD would have moved those graphics to a .001 location based upon your settings. Thus the graphics shifted.  Why your design screwed up everywhere is stranged.

    Now, let's say you have only a bunch of tiny de-connect. To speed up re-connecting everything try the following- 1. in the color dialog box select "global visibility'   to off. Then hit ok. 2. while in the route mode, window select all the dis-connected traces then right click and hit "finish". Everything track should connect. The changes if any should be so small that it will be something you can live with. 

    Cheers    

  • StepscanDarcy
    in reply to Dale Peterson

    Hey Dale, 

    While I could be wrong, these are showing up as DRC errors.

    But I really like what you've suggested, and I would like to try it.   Where would I go about finding the accuracy setting?

    What really has me interested is this "finish" button that will autocomplete broken connections.  I don't seem to have this option when I right click.   Is it in all versions?  

    Now here's the funny part, the browser i took the screenshot of, is from the ORIGINAL file(before I made any changes).   They weren't showing up by default, so I didn't even know they were there.   Maybe changes made in newer versions of orcad caused changes?   The good news I guess is that I didn't create these problems(my file only has 5527 errors) , but obviously the board works, because I work with them every day.   How was this file able to be exported with all of these errors?   I can generate art files, but no gerber.

  • steve
    in reply to Dale Peterson

    You can also use Tools - Derive Connectivity to resolve these small unconnects....

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.