[PCB_FORUM] Re: Retaining nets on free-standing vias
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Thu, 2 Mar 2006 15:52:33 -0600
All,
I called Cadence about that a long time ago and was told that is a
function/feature that many designers actually demanded. At first, it was
annoying but after awhile, I simply laid down my planes last. This is
where dynamic shapes are really handy.
Cheers,
Ron Scott C.I.D.+
Texas Instruments
Storage Products Group
Tel: 214.567.4715
Cell: 972.816.7978
rg-scott@xxxxxx
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Gary MacIndoe
Sent: Thursday, March 02, 2006 15:43
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Retaining nets on free-standing vias
Les,
I'm on 15.5, but I think it first appeared on 15.2.
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 Les Wong
Sent: Thursday, March 02, 2006 1:48 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Retaining nets on free-standing vias
Gary:
Is that Allegro 15.5 ?
Les
--- Gary MacIndoe <gary.macindoe@xxxxxxx> wrote:
>
> 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
>
=== message truncated ===
-----------------------------------------------------------
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:
