[PCB_FORUM] Re: Allegro Sub drawing / Via stitch problem
- From: <cmward@xxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Wed, 29 Jul 2009 08:05:11 -0600
Another way to find them is to highlight all nets in Black, only your vias that
are “not on a net” will remain
Thanks,
Chris
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Craig Lewis
Sent: Wednesday, July 29, 2009 6:38 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Allegro Sub drawing / Via stitch problem
The cleanest way would be to write a short SKILL utility to find all vias on a
dummy net inside that shape. The next easiest would be to select all via in the
shape and do a Show Element on them, save the file to your favorite text editor
and search for "not on a net."
Craig
Mark Salberg wrote:
No, I just routed a trace (inside the shape) from a pin to the vias to force
it...Then just export / import to 0,0.
Anyone know how to search for these "floating" vias? Danging via does not work.
Would like to locate any instances I may have missed.
Thanks,
Mark
cadman10@xxxxxxxxxxx wrote:
Hello Mark,
Normaly this happens becouse when the vias do not have a net association they
inherit the net name of the first shape they find,B Have you tried to disable
the dynamic shapes on the board first , then import your subdrawing, then
enable the dynamic shapes and force your imported shape to update first
good luck
cadman
On Jul 27, 2009, Mark Salberg <msalberg@xxxxxxxxxxxx>
<mailto:msalberg@xxxxxxxxxxxx> wrote:
Not quite that easy Jean,
Actually stitching to many different power supplies on 8 different
layers.
Just want to keep the import the same as the export.
Importing clip all at once by 0,0 origin.
Jean Bratton wrote:
IF< /u> all of your stitching vias are to GND, then you can move all of
your non-GND positive planes off-board before reading in the clip. Then the
unconnected vias will get associated with GND, and then you can move the other
planes back on the board.
Jean Bratton
Senior PCB Designer
Freedom CAD Services, Inc.
Office: 603-864-1349
Email: jean.bratton@xxxxxxxxxxxxxx
Visit us at http://www.freedomcad.com
-----Origi nal Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
Sent: Monday, July 27, 2009 9:04 AM
To: Cadence User Group
Subject: [PCB_FORUM] Allegro Sub drawing / Via stitch problem
Hello all,
When Exporting a Sub-Drawing I found that any vias in a shape used for
stitching...connected to a shape, but has no traces to a pin...looses
connectivity and sometimes connect to a different plane after import
sub-drawing.
The only way I have found to fix it is to ALSO route a t race from a
pin
to the via to force the connection.
Is there a way to locate any occurrences of this prior to exporting a
Sub-Drawing?
Thought maybe dangling wire reporting as dangling via...but a Dangling
via is defined a a via with only one connection from a pin. These vias
simply dropped in a shape for thermal reasons do not get flagged.
Any thoughts as to how to find them in a design?
Thanks,
Mark
_____________________________________________________________________________
S canned by IBM Email Security Management Services powered by
MessageLabs. For more information please visit http://www.ers.ibm.com
_____________________________________________________________________________
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by
MessageLabs. For more information please visit http://www.ers.ibm.com
_____________________________________________________________________________
_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by
MessageLabs. For more information please visit http://www.ers.ibm.com
<http://%0A%20/www.ers.ibm.com>
_____________________________________________________________________________
----------------------------------------------------------- To
subscribe/unsubscribe: Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe To view the archives of this list go
to //www.freelists.org/archives/icu-pcb-forum/ Problems or Questions: Send
an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by MessageLabs. For
more information please visit http://www.ers.ibm.com
_____________________________________________________________________________
_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by MessageLabs. For
more information please visit http://www.ers.ibm.com
_____________________________________________________________________________
----------------------------------------------------------- To
subscribe/unsubscribe: Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe To view the archives of this list go
to //www.freelists.org/archives/icu-pcb-forum/ Problems or Questions: Send
an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
Other related posts:
