gEDA-user: How to connect pads to anything?
Hello all, yesterday I tried to replace a number of 2-pin jumpers (footprint JUMPER2) with solder jumpers. gschem2pcb does it's duty, removes the old footprints and provides the new ones. The rats nest is drawn correctly. However if I try to connect these new footprints with anything, the connection is simply ignored. Optimize the rats nest and the yellow lines don't vanish, the number of missing connections is kept. The autorouter doesn't do anything, als everything else is connected. Instead I even get DRC errors stating the track and the pad are too close *sigh* After googling and reading the pcb handbook for the better part of a day I'm stuck. Whatever I try, pads can't be connected to anything. Not on the solder side, not on the top side, not to vias. What's the secret? The most simple footprint I tried looks that: Element[ Solder Jumper on the solder side JUMPER_SOLDER 10 10 -5000 5000 0 100 ] ( Pad[2200 -1500 2200 1500 3600 3200 2000 1 1 square] Pad[-2200 -1500 -2200 1500 3600 3200 2000 2 2 square] ElementLine [ ... ) I'm using the software packaged with Ubuntu 10.04 on AMD64, which appears to be version 20091103. BTW., the reason I started using gEDA is to develop electronics for another open source project, RepRap. See http://reprap.org/wiki/Generation_7_Electronics . Thanks, Markus ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
Markus Hitter: ... Whatever I try, pads can't be connected to anything. Not on the solder side, not on the top side, not to vias. The footprint pads might be on the component side. What's the secret? The most simple footprint I tried looks that: Element[ Solder Jumper on the solder side JUMPER_SOLDER 10 10 -5000 5000 0 100 ] ( Pad[2200 -1500 2200 1500 3600 3200 2000 1 1 square] Pad[-2200 -1500 -2200 1500 3600 3200 2000 2 2 square] ElementLine [ ... ) If your traces are on the solder side, try to add onsolder after square, like Pad[2200 -1500 2200 1500 3600 3200 2000 1 1 square,onsolder] There is also under Edit-Move to current Layer M, but I haven't been able to move a footprint to the solder layer with that. Regards, /Karl Hammar - Aspö Data Lilla Aspö 148 S-742 94 Östhammar Sweden +46 173 140 57 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
On Sun, 2010-10-17 at 15:35 +0200, Karl Hammar wrote: There is also under Edit-Move to current Layer M, but I haven't been able to move a footprint to the solder layer with that. Of course you can not move it to inner layers, so Move to current Layer makes not much sense. Hoover mouse over footprint and press key b -- this is for lesstif, but may work for gtk too. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
On Sun, 2010-10-17 at 15:47 +0200, Stefan Salewski wrote: For replacing footprints there is a special mode which allows you to replace single footprints -- sorry can not remember currently. It is Load element data to paste buffer, and now SHIFT LEFT MOUSE CLICK over old elements. That will replace the footprint, but you still may have to rotate it. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
Markus Hitter wrote: Instead I even get DRC errors stating the track and the pad are too close *sigh* Maybe your design rules are prohibiting making the connection? You could try disabling the auto enforce drc clearance - look under the settings menu selections. If that works out, you may have to change your design rules (menu File-Preferences-Sizes-DesignRuleChecking). Otherwise, change the spacing on your solder jumper. I see that you have the pads about 8.1 mils apart - that's pretty close. Check your design rules. gene ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
ElementLine [ ... is that a typo? The line is incomplete. I deleted, and then loaded the part onto a layout, which worked out. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
Am 17.10.2010 um 15:47 schrieb Stefan Salewski: On Sun, 2010-10-17 at 14:50 +0200, Markus Hitter wrote: Hello all, yesterday I tried to replace a number of 2-pin jumpers (footprint JUMPER2) with solder jumpers. Of course, this should work fine, it does for me. gsch2pcb removes the old footprints, but for my 2009 snapshot it has not put the new ones, you have to do something like load element data to buffer to insert the new ones, and you may have to load the new netlist again. And you have to watch for the orientation of the new footprints, you may have to rotate them 180 degree. And press O key to update ratsnest. Did you make your layout with the autorouter? I have done all manually, so I am not sure if the autorouter needs special care when exchanging footprints. For replacing footprints there is a special mode which allows you to replace single footprints -- sorry can not remember currently. Thanks for the quick answer, Karl, Stefan. All what you suggest works fine already. The new pads appear, I route mostly manually and I can flip the pad The problem is, an overlap between a pad and a track isn't recognized as a connection. I'll try to show this with a screenshot, the rats nest is freshly optimized: inline: Bildschirmfoto.png Markus ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
If you are willing, send the .pcb file over. I can take a closer look. gene ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
On Sun, 2010-10-17 at 16:20 +0200, Markus Hitter wrote: The problem is, an overlap between a pad and a track isn't recognized as a connection. That would make sense if your dark red traces are on an inner layer. As gene glick wrote, you may send a board for investigation. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
Am 17.10.2010 um 16:17 schrieb gene glick: ElementLine [ ... is that a typo? It's an intentional cut to keep the message short. There are further ElementLines. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
Am 17.10.2010 um 16:25 schrieb gene glick: If you are willing, send the .pcb file over. I can take a closer look. That would be greatly appreciated! Schematics and the board with the 2-pin jumpers are on Github, it's the Gen7Board.xxx: http://github.com/Traumflug/Generation_7_Electronics I've attached here my current version of the solder jumper, it's a bit different from what you see on the screenshot. JUMPER_SOLDER.fp Description: Binary data The jumpers I want to replace are J1 ... J12, placed horizontally in the upper half. Markus ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
On Sun, 2010-10-17 at 16:54 +0200, Markus Hitter wrote: Am 17.10.2010 um 16:25 schrieb gene glick: If you are willing, send the .pcb file over. I can take a closer look. That would be greatly appreciated! Schematics and the board with the 2-pin jumpers are on Github, it's the Gen7Board.xxx: http://github.com/Traumflug/Generation_7_Electronics I've attached here my current version of the solder jumper, it's a bit different from what you see on the screenshot. My initial guess: Your traces are not in the top and bottom groups, so it are inner layers. That works for true trough-hole parts, but you tried to replace with smd parts. Currently I an testing lesstif hid for gentoo, so all looks very strange to me, but my guess may be correct. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
On Sun, 2010-10-17 at 17:20 +0200, Stefan Salewski wrote: My initial guess: Your traces are not in the top and bottom groups, so Use the layers dialog, and make it similar as tut1.pcb for two layer layout. solder x GND-solder x VCC-solder x comonent x GND-component x Vcc-component x unused unused (bottom) x (top) x I set up layers stack when I start a new layout, but I think it will work if you change it now. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: How to connect pads to anything?
Am 17.10.2010 um 17:44 schrieb Stefan Salewski: solder x GND-solder x VCC-solder x comonent x GND-component x Vcc-component x unused unused (bottom) x (top) x I set up layers stack when I start a new layout, but I think it will work if you change it now. Heck, adopting the last two lines of the scheme above worked like a charme. Thanks a lot for the help everybody! 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: How to connect pads to anything?
Stefan Salewski m...@ssalewski.de writes: What I wanted to say was: Move to current Layer makes not much sense for footprints, because we can have inner layers, it does make sense, sometimes ... but we can not move footprints to that layers. ... pity -- Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
