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 -----------------------------------------------------------