gEDA-user: Is this type of footprint possible?
Hello all, I want to use a component with the attached footprint. Is it possible to make a footprint with an arc inside? Any help appreciated. Regards, Robert attachment: Wurth-elektronik-744043120.jpg ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Is this type of footprint possible?
my...@iae.nl wrote: Hello all, I want to use a component with the attached footprint. Is it possible to make a footprint with an arc inside? I'm not sure about the exact drawing method you show, but it is possible to make an arc path that matches your concave edge, and add rectangular or polygonal areas to overlap it and make the approximate shape. The approximation I suggest will have rounded corners at the ends of the concave edge. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Is this type of footprint possible?
On Mon, 2010-03-29 at 09:16 -0500, John Griessen wrote: but it is possible to make an arc path that matches your concave edge, But currently we have no true arcs in footprint definition, so we have to approximate the arcs in the footprint file with multiple line elements. Or maybe we may draw the arc in the final pcb layout, when the position of the footprint is fix and will not change. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Is this type of footprint possible?
On Mon, 29 Mar 2010 11:29:34 +0200, myken-kVLBEChPVFc wrote: Is it possible to make a footprint with an arc inside? Not with real arcs, but arbitrarily close. The pads of footprints can be composed of multiple straight tracks. If they all get the same number, pcb considers them to be part of the same pad. The GUI of pcb provides no easy way to draw such complex shapes. The best bet is to draw the footprint with a vector drawing application like inkscape, save as postscript and convert to pcb with ps2edit. See the wiki for more detailed instruction: http://geda.seul.org/wiki/geda:pcb_tips#what_is_the_best_way_to_do_weird_footprints Hope, this helps, ---)kaimartin(--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Is this type of footprint possible?
I want to use a component with the attached footprint. Is it possible to make a footprint with an arc inside? Practically I would approximate the land pattern by creating a pad with three parts, i.e. a pad for each side and then a long rectangular pad across the top to connect them. Make them rectangular pads which stay outside of the 1.80mm diameter. It is unlikely that the small amount of pad area lost will make a difference IMO. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Is this type of footprint possible?
Thanks, I will try this approach, although the simplicity of Duncan's solution also appeals to me, but I don't know if I get into trouble with manufacturing (placement) tolerances using such a simple footprint. Any way, thanks for your reply. Regards, Robert. On Mon, 2010-03-29 at 18:04 +, Kai-Martin Knaak wrote: On Mon, 29 Mar 2010 11:29:34 +0200, myken-kVLBEChPVFc wrote: Is it possible to make a footprint with an arc inside? Not with real arcs, but arbitrarily close. The pads of footprints can be composed of multiple straight tracks. If they all get the same number, pcb considers them to be part of the same pad. The GUI of pcb provides no easy way to draw such complex shapes. The best bet is to draw the footprint with a vector drawing application like inkscape, save as postscript and convert to pcb with ps2edit. See the wiki for more detailed instruction: http://geda.seul.org/wiki/geda:pcb_tips#what_is_the_best_way_to_do_weird_footprints Hope, this helps, ---)kaimartin(--- ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
