have you posted this to the DXP forum ?
i hope so !
i am reasonably sure this is not an issue with 99SE as we do this
partial isolation routinely and have not had any problems (i refer to
them as 'cuts' to distinguish from 'splits')
ds
_______________________________________________________________________
Integrated Controls, Inc. Tel: 415-647-0480 EXT 107
2851 21st Street Fax: 415-647-3003
San Francisco, CA 94110 www.integratedcontrolsinc.com
Matt Polak wrote:
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]
____________________________________________________________
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]
