[PCB_FORUM] Re: Retaining nets on free-standing vias
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Thu, 2 Mar 2006 15:19:28 -0600
Gary,
Cadence has attempted to address this issue by adding the "Retain net of
vias" selection however this button does not keep the via from losing
the net name in all cases. I will admit that it is much better than
before but again it is does not guarantee the via will also retain the
net name. If you move the via from the assigned shape, then back again
and then off again the via will lose connection to the intended net. So
it does not permanently assign the net to the via and the via does not
always retain the net name. But again I will admit it is much better
than before.
Tony Cosentino
Tekelec
Tony.cosentino@xxxxxxxxxxx
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Gary MacIndoe
Sent: Thursday, March 02, 2006 3:32 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Retaining nets on free-standing vias
Hey guys/gals,
Cadence has addressed this issue, at least to an extent (when copying
vias).
Go into Edit -> Copy, vias turned on, in the Options tab, then check
"Retain net of vias" box. Then, you copy say a gnd via and drop it down
anywhere not on a trace, it retains the gnd net. You can move it around
all you want, it will still be gnd.
Gary E. MacIndoe
PCB Design Engineer
Advanced Micro Devices
Longmont, Colorado
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Daniel So
Sent: Thursday, March 02, 2006 12:05 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Retaining nets on free-standing vias
Linda
I tried going to www.cdnusers.org, registered and then logged on. I went
to Forums -> Silicon-package-board -> Shared code-Skill. There I saw
discussions but no skill codes. Where did I go wrong?
Daniel
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]
Sent: Thursday, March 02, 2006 10:37 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Retaining nets on free-standing vias
Doug,
We have a PCB SKILL forum on the newly launched Cadence user community
website where you can upload your skill routine for all to see.
you will need to register to post the code.
The site is found at www.cdnusers.org. You can register, wait a bit for
your authorization code, login, then click on the "Forums" tab in the
upper navigation bar.
Linda
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Douglas Stanley
Sent: Thursday, March 02, 2006 10:32 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Retaining nets on free-standing vias
My method doesn't really solve the problem, but it makes it easy to deal
with. I wrote a small SKILL routine that allows you to select any via
and change the via's net.
I works by clicking on a via (single select, window, or temp group) and
then clicking on any shape, pin, or cline. The via then takes on the net
of the shape/pin/cline you selected. Works like a champ. It's 30 lines
of code.
Douglas G. Stanley
Broadcom Corporation
(949) 926-5889
dstanley@xxxxxxxxxxxx
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of
Michael.Catrambone@xxxxxxxxxx
Sent: Thursday, March 02, 2006 9:55 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Retaining nets on free-standing vias
Hello,
I deal with this all the time.. The best way I found to handle it was to
define a small static shape on top of the via with the net name attached
to it. This shape is defined a little larger than the via geometry on
the top side of the PCB and whenever I move the via I make sure to
select the shape as well.
Kind of a pain but it gets me past the problem. Maybe someone else has
a better way of handling this.
Mike
"Daniel So" <danielso@xxxxxxxxxxxxx>@freelists.org on 03/02/2006
11:43:43 AM
Please respond to icu-pcb-forum@xxxxxxxxxxxxx
Sent by: icu-pcb-forum-bounce@xxxxxxxxxxxxx
To: <icu-pcb-forum@xxxxxxxxxxxxx>
cc:
Subject: [PCB_FORUM] Retaining nets on free-standing vias
Hi Everyone
Please excuse me if this is an old subject.
I have thru-hole vias connected to a gnd plane on the top layer. There
is +5v plane on the bottom side of the PCB. There are no clines
connected to the vias so when ever I move the gnd plane, the vias are
now associated to the +5v plane. I now have to move the +5v plane before
moving back the gnd plane if I want to keep these vias associated to
gnd. This is really a bad problem on a multi-layer board with different
planes on different layers and when I have vias that I want to keep
associated to different nets.
Is there any way to keep the vias associated to the original nets
without connecting clines to them? Cadence did not have an answer.
Thanks for any suggestions
Daniel So
email: danielso@xxxxxxxxxxxxx
(See attached file: C.htm)
-----------------------------------------------------------
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 please login at
//www.freelists.org. Our list name is icu-pcb-forum or go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
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 please login at
//www.freelists.org. Our list name is icu-pcb-forum or go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
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 please login at
//www.freelists.org. Our list name is icu-pcb-forum or go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
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 please login at
//www.freelists.org. Our list name is icu-pcb-forum or go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
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 please login at
//www.freelists.org. Our list name is icu-pcb-forum
or go to //www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
Other related posts:
