Re: gEDA-user: Clearance in fiducials & blocking solder paste
Hi, Attached is a fiducial example. Enjoy! -- Levente Kovacs http://levente.logonex.eu fidu.fp Description: Binary data ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
The problem with this approach is exactly what started off my quest for the Arc. Namely the autorouter is routing through the keepout space on the fiducials. Oliver __ From: John Luciani To: gEDA user mailing list Sent: Sun, December 5, 2010 9:54:00 AM Subject: Re: gEDA-user: Clearance in fiducials & blocking solder paste Arcs aren't allowed in footprints. You can overlay rectangular pads along an arc if you need to. The footprint I use for fiducials is below. The request from the assembly house was 1mm pad with 3mm clearance. The board that assembled my last board did not mention any problems (and the board worked ;) (* jcl *) Element[0x0 "FIDUCIAL" "" "" 0 0 0 0 0 100 0x0] ( Pad[0 0 0 0 3937 7874 11811 "" "1" 0x0800] Pad[0 0 0 0 3937 7874 11811 "" "1" 0x0880] ) ___ geda-user mailing list [1]geda-u...@moria.seul.org [2]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. mailto:geda-user@moria.seul.org 2. http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
This is in the silkscreen of the footprint. Steve On Sun, Dec 5, 2010 at 10:29 AM, Markus Hitter wrote: > > Am 05.12.2010 um 18:54 schrieb John Luciani: > >> Arcs aren't allowed in footprints. > > D'oh. Neither me nor my copy of PCB knew that so this rectangle with rounded > corners worked fine: > > ElementLine [-46000 -12450 46000 -12450 1000] > ElementLine [-46000 12450 46000 12450 1000] > ElementLine [-5 -8450 -5 8450 1000] > ElementLine [ 5 -8450 5 8450 1000] > ElementArc [-46000 -8450 4000 4000 270 90 1000] > ElementArc [ 46000 -8450 4000 4000 180 90 1000] > ElementArc [-46000 8450 4000 4000 0 90 1000] > ElementArc [ 46000 8450 4000 4000 90 90 1000] > > > Markus > > - - - - - - - - - - - - - - - - - - - > Dipl. Ing. (FH) Markus Hitter > http://www.jump-ing.de/ > > > > > > > > ___ > geda-user mailing list > geda-user@moria.seul.org > http://www.seul.org/cgi-bin/mailman/listinfo/geda-user > ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
Am 05.12.2010 um 18:54 schrieb John Luciani: Arcs aren't allowed in footprints. D'oh. Neither me nor my copy of PCB knew that so this rectangle with rounded corners worked fine: ElementLine [-46000 -12450 46000 -12450 1000] ElementLine [-46000 12450 46000 12450 1000] ElementLine [-5 -8450 -5 8450 1000] ElementLine [ 5 -8450 5 8450 1000] ElementArc [-46000 -8450 4000 4000 270 90 1000] ElementArc [ 46000 -8450 4000 4000 180 90 1000] ElementArc [-46000 8450 4000 4000 0 90 1000] ElementArc [ 46000 8450 4000 4000 90 90 1000] Markus - - - - - - - - - - - - - - - - - - - Dipl. Ing. (FH) Markus Hitter http://www.jump-ing.de/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
On Sun, 5 Dec 2010 12:54:00 -0500 John Luciani wrote: > Arcs aren't allowed in footprints. [...] This begs the question, since arcs can be placed on the silk layer in a footprint, is there a particular reason why PCB couldn't be tweaked to allow them on copper layers? -- "There are some things in life worth obsessing over. Most things aren't, and when you learn that, life improves." http://starbase.globalpc.net/~ezekowitz Vanessa Ezekowitz ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
Arcs aren't allowed in footprints. You can overlay rectangular pads along an arc if you need to. The footprint I use for fiducials is below. The request from the assembly house was 1mm pad with 3mm clearance. The board that assembled my last board did not mention any problems (and the board worked ;) (* jcl *) Element[0x0 "FIDUCIAL" "" "" 0 0 0 0 0 100 0x0] ( Pad[0 0 0 0 3937 7874 11811 "" "1" 0x0800] Pad[0 0 0 0 3937 7874 11811 "" "1" 0x0880] ) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
So I tried adding an Arc statement to my footprint, but I am getting a syntax error on import. Here is a snippet of the pcb file, that was generated from my footprint with an Arc inside it. Element["" "soic-08-d.fp" "U?" "unknown" 0 0 0 0 0 100 ""] ( Pad [-12204 -15000 -12204 -15000 4000 8000 12800 "f1" "" "" ] Arc [-13188 -15000 12800 12800 1000 1000 0 180 "" ] Pad [ 12204 15000 12204 15000 4000 8000 12800 "f2" "" "" ] I am guessing Elements are not allowed Arcs. Is there another way to place an arc into a footprint? Oliver ______ From: DJ Delorie To: gEDA user mailing list Sent: Sat, December 4, 2010 11:53:10 PM Subject: Re: gEDA-user: Clearance in fiducials & blocking solder paste Ringing it with copper certainly would work. PCB doesn't have a generic "keep out" feature yet. ___ geda-user mailing list [1]geda-u...@moria.seul.org [2]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. mailto:geda-user@moria.seul.org 2. http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
Ringing it with copper certainly would work. PCB doesn't have a generic "keep out" feature yet. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
Is there a way to "protect" the fiducial? For example I could attempt to ring it with copper. Oliver __ From: DJ Delorie To: gEDA user mailing list Sent: Sat, December 4, 2010 11:29:28 PM Subject: Re: gEDA-user: Clearance in fiducials & blocking solder paste Two notes: 1. "Clearance" is clearance in polygons, not the line/space rule. 2. Add the "nopaste" flag to the pad. ___ geda-user mailing list [1]geda-u...@moria.seul.org [2]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. mailto:geda-user@moria.seul.org 2. http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Clearance in fiducials & blocking solder paste
Two notes: 1. "Clearance" is clearance in polygons, not the line/space rule. 2. Add the "nopaste" flag to the pad. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Clearance in fiducials & blocking solder paste
I am trying to place down some fiducials with a 40mil round copper center with 88mills of clearance (from the center of the fiducial) and 80 mils of solder mask. I am doing it by using the following command inside my footprint file. Pad [-13188 -15000 -13188 -15000 4000 4800 8000 "f1" "" "" ] Now when I run the autorouter it only respects the clearance I give for the net type, and not for the fiducials. The other problem is when I generate the gerbers for my file, I get solder paste on my fiducials which is not what I want. Is there a good way of doing this in gEDA? Oliver ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
