I can't use the "pour over same net" option. I have several dedicated GND returns ...
btw, this is with P99SE SP6. -- Dean Carpenter deano at areyes com 94TT :) ----- Original Message ----- From: "Dave Sanders" <[EMAIL PROTECTED]> To: "Protel EDA Discussion List" <[email protected]> Sent: Wednesday, March 09, 2005 12:13 AM Subject: RE: [PEDA] Weird - via won't join GND polygons > Although I'm sure I've somehow managed to relief connect vias in the past, > having a quick play with it now it seems that particular rule (polygon > connect style) doesn't seem to work for vias, even though you can specify > vias directly in the rule builder. Not sure if it is a bug or not, but I > guess it is understandable since you don't solder to them anyway, so they > don't need reliefs, just direct connects. > > To get the direct connect, use the tick box "pour over same net" in the > polygon dialog box. > > Ta, > Dave > > > -----Original Message----- > From: [EMAIL PROTECTED] > [mailto:[EMAIL PROTECTED] Behalf Of Nukien > Sent: Wednesday, 9 March 2005 4:28 p.m. > To: Protel EDA Discussion List > Subject: Re: [PEDA] Weird - via won't join GND polygons > > > Weird. Not working here. > > I have polygons on top and bottom layers, both on GND net. I drop a via on > a blank spot, and it picks up the GND net just fine. I can verify that in > the properties for the via. > > I then redo the polygons, they rebuild, but the via is isolated. But it > still has the GND net associated with it, and there's a rats-nest line > leading to the nearest pad on the GND net. If I select the via, the whole > GND net is highlighted as you would expect. Even weirder, DRC doesn't flag > a Broken Net error ... > > The polygons have correctly attached to all the GND pads on the various > components, just not the via. The polys are definitely good - they're > providing connectivity all over the place for GND. > > Dropping round pads with the same dimensions works fine. > > What the <bleep> ? > > PS - what's the "Minimum primitive size - Length" box for in the polygon > properties dialog ? I've never messed with it - I think it's always set to > 2mil. > > -- > Dean Carpenter > deano at areyes com > 94TT :) > ----- Original Message ----- > From: "Dennis Saputelli" <[EMAIL PROTECTED]> > To: "Protel EDA Discussion List" <[email protected]> > Sent: Tuesday, March 08, 2005 6:56 PM > Subject: Re: [PEDA] Weird - via won't join GND polygons > > > > vias connect fine to pours > > > > i do it all the time > > touch or place the via on a grounded pin or pad, then drag onto pour > > > > if you place them initially directly on the pour sometimes they pick up > > the ground net and sometimes they don't > > > > sometimes just wiggle them on the pour and they pick it up > > > > not as much of a bother as it sounds > > > > and/or select them and global edit the net name to 'selected same' > > > > nothing wrong with your named free pads method though, we do that > > sometimes too > > > > ds > > > > > > _______________________________________________________________________ > > Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 > > 2851 21st Street Fax: 415-647-3003 > > San Francisco, CA 94110 www.integratedcontrolsinc.com > > > > > > Bruce Walter wrote: > > > Vias don't connect. Convert them all to free pads. Give them all the > same > > > designator (98, 99, etc.), then you can make unique rules for connect > style > > > (solid, etc.). > > > > > > TQFP - probably clearance rules. The space between the pins, along with > the > > > track width of the polygon lines and/or the clearance rule won't allow a > > > connect. Adjust the settings, or draw a trace to a (similar) free pad. > > > > > > -----Original Message----- > > > From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] > On > > > Behalf Of Nukien > > > Sent: Saturday, March 05, 2005 9:02 PM > > > To: Protel EDA Discussion List > > > Subject: [PEDA] Weird - via won't join GND polygons > > > > > > Well, this is weird. I have GND polygons on top and bottom layers of a > > > 2-layer board. Very standard. To fulfill connectivity, I drop vias > > > (35/28mil) around to join the two planes, and as expected, they pick up > GND > > > as their net. Then dbl-click the planes, select each one, and have it > > > rebuild. > > > > > > The vias are isolated. > > > > > > They're definitely in the GND net. So are the planes. The Polygon > Connect > > > Style rule is set to Relief-Connect, using 90deg 30mil tracks. > > > > > > I know this is something simple, but it's eluding me ... > > > > > > Hrm - just noticed, the GND pins on the TQFP chips aren't joining the > GND > > > planes either. The GND side of the decoupling 0805 caps are joining > just > > > find though. Ah, got that one figured out - the relief traces are too > big - > > > changed it from 30mil to 20mil, and now they join. > > > > > > But the via are still isolated. > > > > > > -- > > > Dean Carpenter > > > deano at areyes com > > > 94TT :) > > > > > > ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
