gEDA-user: Jumpers on single layer PCBs
Presently I use a second layer (such as a jumper layer) to draw on jumpers for single layer FR4 PCBs, however this is cumbersome; and it doesn't support zero ohm SMT resistors. Does PCB have any support for adding jumper components, where the pins would essentially be shorted (the same net) but physically separate? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Jumpers on single layer PCBs
Does PCB have any support for adding jumper components, where the pins would essentially be shorted (the same net) but physically separate? Not really. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Jumpers on single layer PCBs
Oh. Thanks anyway. Any hack-ish way to add this in? (Because I'd like each jumper to have a refdes and BOM entry if possible.) On 31 May 2011 21:44, DJ Delorie [1]d...@delorie.com wrote: Does PCB have any support for adding jumper components, where the pins would essentially be shorted (the same net) but physically separate? Not really. ___ geda-user mailing list [2]geda-user@moria.seul.org [3]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. mailto:d...@delorie.com 2. mailto:geda-user@moria.seul.org 3. 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: Jumpers on single layer PCBs
Oh. Thanks anyway. Any hack-ish way to add this in? (Because I'd like each jumper to have a refdes and BOM entry if possible.) Put them in the schematics :-) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Jumpers on single layer PCBs
On Tue, 31 May 2011 21:59:04 +0100 Thomas Oldbury toldb...@gmail.com wrote: Oh. Thanks anyway. Any hack-ish way to add this in? (Because I'd like each jumper to have a refdes and BOM entry if possible.) What I'd do is define a copper layer. Draw your jumpers on the that layer. Don't send the layer data to the fab house. Make sure you have mask openings on vias. Solder jumpers in the vias. I recommend using double sided boards. Levente -- Levente Kovacs http://levente.logonex.eu ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Jumpers on single layer PCBs
On Tue, May 31, 2011 at 2:09 PM, Levente Kovacs leventel...@gmail.com wrote: On Tue, 31 May 2011 21:59:04 +0100 Thomas Oldbury toldb...@gmail.com wrote: Oh. Thanks anyway. Any hack-ish way to add this in? (Because I'd like each jumper to have a refdes and BOM entry if possible.) What I'd do is define a copper layer. Draw your jumpers on the that layer. Don't send the layer data to the fab house. Make sure you have mask openings on vias. Solder jumpers in the vias. I recommend using double sided boards. I was just writing an email recommending that. If you want a BOM of jumper wires, you could make a script that takes all the traces on the jumper wire layer and spits out a list by length and location. Bonus points if it collates jumper wires of the same length and provides a count. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Jumpers on single layer PCBs
Double sided boards are great, but not so great when the product is supposed to cost only $3/each, after an MSP430, mains power supply, heatsink, triac etc. On 31 May 2011 22:09, Levente Kovacs [1]leventel...@gmail.com wrote: On Tue, 31 May 2011 21:59:04 +0100 Thomas Oldbury [2]toldb...@gmail.com wrote: Oh. Thanks anyway. Any hack-ish way to add this in? (Because I'd like each jumper to have a refdes and BOM entry if possible.) What I'd do is define a copper layer. Draw your jumpers on the that layer. Don't send the layer data to the fab house. Make sure you have mask openings on vias. Solder jumpers in the vias. I recommend using double sided boards. Levente -- Levente Kovacs [3]http://levente.logonex.eu ___ geda-user mailing list [4]geda-user@moria.seul.org [5]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. mailto:leventel...@gmail.com 2. mailto:toldb...@gmail.com 3. http://levente.logonex.eu/ 4. mailto:geda-user@moria.seul.org 5. 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: Jumpers on single layer PCBs
On Wed, Jun 1, 2011 at 6:59 AM, Thomas Oldbury toldb...@gmail.com wrote: Oh. Thanks anyway. Any hack-ish way to add this in? (Because I'd like each jumper to have a refdes and BOM entry if possible.) The hack I use for solder jumpers is to make a footprint that is open circuit, and bridge where needed with copper text. DRC ignores text, even when it is on copper layers. So placing a '-' character or a '|' character on copper with a suitably large font provides an electrical connection without upsetting DRC. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Jumpers on single layer PCBs
Can you still get single sided FR2? On May 31, 2011, at 2:26 PM, Thomas Oldbury toldb...@gmail.com wrote: Double sided boards are great, but not so great when the product is supposed to cost only $3/each, after an MSP430, mains power supply, heatsink, triac etc. On 31 May 2011 22:09, Levente Kovacs [1]leventel...@gmail.com wrote: On Tue, 31 May 2011 21:59:04 +0100 Thomas Oldbury [2]toldb...@gmail.com wrote: Oh. Thanks anyway. Any hack-ish way to add this in? (Because I'd like each jumper to have a refdes and BOM entry if possible.) What I'd do is define a copper layer. Draw your jumpers on the that layer. Don't send the layer data to the fab house. Make sure you have mask openings on vias. Solder jumpers in the vias. I recommend using double sided boards. Levente -- Levente Kovacs [3]http://levente.logonex.eu ___ geda-user mailing list [4]geda-user@moria.seul.org [5]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. mailto:leventel...@gmail.com 2. mailto:toldb...@gmail.com 3. http://levente.logonex.eu/ 4. mailto:geda-user@moria.seul.org 5. 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 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Jumpers on single layer PCBs
On 05/31/2011 04:26 PM, Thomas Oldbury wrote: Double sided boards are great, but not so great when the product is supposed to cost only $3/each, after an MSP430, mains power supply, heatsink, triac etc. You seem to have BOM'd out on that product... ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Jumpers on single layer PCBs
On 05/31/2011 04:26 PM, Thomas Oldbury wrote: Double sided boards are great, but not so great when the product is supposed to cost only $3/each What you really want is the high volume technique of using carbon conductive ink traces and insulating layers silk screened on and single copper FR4 or FR2 or composite paper/glass boards with no drilling, just punch press tooling for holes. But then you have to order by the panel full and pay some setup charges for any change once the punch press tool is made. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
