Dennis Saputelli wrote:
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]
Me too - SOP on 4 layer boards. Never seen this behavior, Graham Brown
____________________________________________________________
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]
