Stats

  • Locked Locked
  • Replies 4
  • Subscribers 166
  • Views 14218
  • 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

Traces constantly becoming disconnected from pads for unknown reason.

wdecook

Using Orcad PCB Designer 16.6

When routing a board, I keep finding that several traces become disconnected from the pins they are routed to. It looks like the trace connects to each pin, the trace and pins both have the same net and are on the same layer, but a ratsnest is shown and the trace does not move if the symbol is moved.

This is an ongoing thing. Just when I think I'm done routing, I check the design status and there are hundreds more disconnected nets. Sure enough, traces that have already been routed have become disconnected. 

I had a theory that this may be related to using place replicate, but it now seems to be happening to traces that are not associated with a place replicate group. 

Does anybody know why this is happening and how to stop it?

  • When you are routing (so in the Route - Connect command) make sure that you have Pins, Vias etc enabled in the Find Filter, also make sure that you have Snap to connect point enabled in the Options menu.
  • When routing, pins and vias are selected and snap to connect point is enabled. The problem is not the initial routing. The problem is that traces that were initially successfully routed (meaning the ratsnest goes away, the trace is on the same net as pins, and the trace stretches and moves with a symbol it is connected to) become unrouted sometime later. The trace does not go away, it is just no longer connected to the pads (meaning that there is now a ratsnest again and the trace does not move with a symbol). The trace does still have the correct net and appears to be over the pin, however. This is happening to hundreds of connections over and over again.
  • Have you been changing the design units after routing ? If so if you are not allowing enough decimal places then sometimes the "rounding" of mils to mm can occur and you may have some small connections to make. If this is the case you can run Tools - Derive Connectivity, check both boxes and click on OK which should resolve these connections. "Ideally" pick a design unit and stick with it. If this is not the case then I recommend contacting Cadence Online support / Channel Partner so they can investigate this further.
  • Thanks Steve. I've found that the source of this problem was related to place replicate and version control. When a place replicate module was made by one person on one computer, but not checked into version control, the sub-circuits based off of this module would become disconnected when the board file is opened on another machine that didn't have the proper .mdd file. I feared that I would have to go back through and disband all of the groups and manually delete all connect lines and vias in the problem areas, then reapply the place replicate module definitions. Your tip about Tool->Derive Connectivity saved my day. That's what I needed. Thank you.
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.