[PCB_FORUM] Re: Allegro Sub drawing / Via stitch problem
- From: "M.Ponraj" <m.ponraj@xxxxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Tue, 28 Jul 2009 12:20:21 +0530
Hi Diane,
Before import the subdrawing, move all the power plane shapes outside the
board. Then you can pull back them into same location.
Regards
Ponraj.M
----- Original Message -----
From: Dickoff, Diane J
To: icu-pcb-forum@xxxxxxxxxxxxx
Sent: Monday, July 27, 2009 11:27 PM
Subject: [PCB_FORUM] Re: Allegro Sub drawing / Via stitch problem
We have thousands of these vias so that is why I don't like to use a net.
Sometimes when we are doing this, we put a little shape inside the via and copy
both.
Diane.
------------------------------------------------------------------------------
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
Sent: Monday, July 27, 2009 10:33 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Allegro Sub drawing / Via stitch problem
Sounds like a valid request. Anytime you have a via in a shape NOT connected
to a pin / pad by a trace...seems to be able to take on different plane net
names from time to time.
For this problem, I simply route a trace inside the shape from pin to EACH
via.
Regards,
Mark
Dickoff, Diane J wrote:
We have made the request with Cadence in a future release that you can assign
a netname to a via. They have not agreed to it yet but it may appear in a
future release. If the via is assigned a netname then it would keep that name
in export subdrawing. We are asking for it to work with defining B/B vias in a
pattern and then copy the pattern with it keeping the correct net names.
Diane.
------------------------------------------------------------------------------
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
Sent: Monday, July 27, 2009 7:39 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Allegro Sub drawing / Via stitch problem
Hi Ismail,
I did that and the planes retain their net names with no problem. But, the
vias drop their net association.
Thanks for the reply,
Mark
ISMAIL wrote:
Hi Mark,
While Export-Subdrawing, goto the "options" tab in the control panel and
check the "Preserve nets of shapes" is enabled.
Try , hope this helps.
Thanks,
Ismail.
------------------------------------------------------------------------------
From: Mark Salberg <msalberg@xxxxxxxxxxxx>
To: Cadence User Group <icu-pcb-forum@xxxxxxxxxxxxx>
Sent: Monday, 27 July, 2009 6:33:42 PM
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 trace 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
_____________________________________________________________________________
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
-----------------------------------------------------------
------------------------------------------------------------------------------
Yahoo! recommends that you upgrade to the new and safer Internet Explorer 8.
_____________________________________________________________________________
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
_____________________________________________________________________________
_____________________________________________________________________________
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
_____________________________________________________________________________
Other related posts:
