[PCB_FORUM] Re: Allegro Sub drawing / Via stitch problem
- From: "Andrew Noonan (annoonan)" <annoonan@xxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Wed, 29 Jul 2009 10:29:34 -0700
Having faced this same issue in a recent design, I went the more
quantifiable route. I've created a simple custom report, selecting Net
Name, and Net Via Count, as my two items to report on. One report for
the pre-clipped in board, one for the post-.
Compare these reports side-by-side in a spreadsheet, add a simple
formula to compare row counts, and highlight any row that does not have
equal vias. At least you can then examine those nets and make an
evaluation.
Andrew
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Craig Lewis
Sent: Wednesday, July 29, 2009 8:34 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Allegro Sub drawing / Via stitch problem
Chris,
That's a slick trick. That will find "all" floating objects.
Thanks,
Craig
cmward@xxxxxxxxxx wrote:
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
-----------------------------------------------------------
----------------------------------------------------------- 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:
