Hey Protel'ers,
Just a heads-up on things, DXP but may apply to 99SE as well... A couple months ago I had posted about a really nasty problem we had where a set of Gerbers we sent out for fabrication was randomly missing some via-plane connections on the Gerber set, but NOT in the actual Protel CAD design. Obviously this caused a bit of consernation, since suddenly it seemed that Protel was randomly dropping connection spokes on the export without any explanation or repeatability. I think I have figured out what was going on, and so for anyone using split-planes in designs, you may want to read the following --
The only drops that we had were (I believe) a couple on the connection to the ground plane. In this design, we had done a "partially split" ground plane - instead of making absolutely isolated sections, we used knockout traces to 'partially isolate' particular areas of interest (to help constrain ground-noise w/o the pain of total splits) but still leave decent connecting-gaps under busses and things to allow all signals that referenced the ground plane to flow uninterrupted, as well as flow of the actual ground reference to the entire board..
This seemed to work very well in our design, but Protel seems to get slightly cranky whenever you start manually placing primatives on the plane layers. Once it sees a trace on a plane, even a trace that doesn't necessarly cut the plane entirely but just slices into part of it, Protel immediately starts treating the plane as if it were a total split-plane... Sort of.... *Normally* in a full-isolated split-plane design you would have two (or more) seperate, distinct nets. Without this total isolation, however, Protel often gets confused, and starts to think there's multiple sets of the same nets, even when there's not.
I started to notice when editing that occasionally certain vias that connect to the ground plane would suddenly be thinking they were connected another 'phantom' GND net, and thus the connecting spokes would disappear entirely. Doing a double-click on the ground plane (in Single Layer View Mode) to regenerate it always fixed this problem entirely and made all of the vias happy once again. For indeterminant reasons, vias would float in and out of these 'phantom' net disconnections throughout the working process. We made gratuitous use of the "Associate Free Pads Through Connected Copper" feature during layout due to excessive pad-swaps on an FPGA, and I wouldn't be surprised if this might have contributed to the mix.
Just before doing my Gerber exports for the most recent board this was happening on, though, I did the "regenerate" trick on both of my planes, and saved immediately afterwards, and did the export from that current working set of data. The boards came back and are up and running on the bench without any problems, and taking a look at the Gerbers that were generated, this seems to have solved the mysterious inconsistency problem. It also explains why it was entirely possible for the Gerbers to be exported, fabbed, and then looking at CAD data a couple weeks later, have it be inconsisten with the previous export. At least in my mind, I can call this one solved and put to bed.
So in any case, a word of the wise to those of you who are using split-planes in your designs. Always always ALWAYS do a final "regenerate" on your split-plane layers as the last thing you do before exporting your Gerbers, or you may have some difficult problems to track down after fabrication!
Thanks again to everyone who offered suggestions on this the first time around! I hope my bad experience can save some of you future headaches.
Regards, -- Matt ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
