gEDA-user: [pcb] overlapping pin/pad -- won't form thermal
Yet another issue with pad+pin stacks. I created hand-solder pads with a pin slightly smaller than the pad to work around the clearance bug. Now, when I click on those pin+pad stacks with the thermal tool, it does not form a thermal. Anybody else see this, or am I doing something wrong? -dave ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: [pcb] overlapping pin/pad -- won't form thermal
pcb doesn't support thermals on pads. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: [pcb] overlapping pin/pad -- won't form thermal
So then the whole concept of getting an oblong through-hole pad by having a pad overlapping a pin is fundamentally broken? There's a day of my life I'll never have back. Pardon my French, but that is bogus. It's not like oblong through-hole pads are a new idea or anything. PCB needs first class support for oblong through-holes. I see that the thermal flag is actually getting set on the pins. It just doesn't render anything. I presume that the clearance area around the pad is killing off the thermal. I realize I can draw them in by hand by turning of new traces clear polygons. I guess for this design that's what I'll have to do, because regenerating all my footprints, regenerating and re-validating the net list, and re-doing all the routing done so far is just too costly. *grump* I'm surprised John Luciani has never complained about this. -dave DJ Delorie wrote: pcb doesn't support thermals on pads. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: [pcb] overlapping pin/pad -- won't form thermal
PCB needs first class support for oblong through-holes. Yup. I've talked about a multi-pin before; this is a pin with arbitrary shaped copper/soldermask/etc on each layer. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: [pcb] overlapping pin/pad -- won't form thermal
Dave wrote: I realize I can draw them in by hand by turning of new traces clear polygons. I guess for this design that's what I'll have to do, because regenerating all my footprints, regenerating and re-validating the net list, and re-doing all the routing done so far is just too costly. That is how I do it. It upsets me that oblong pads are not supported well as I love them for home made boards. If I was bright enough to write C code I would try change it seems well beyond me at present. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: [pcb] overlapping pin/pad -- won't form thermal
DJ Delorie wrote: PCB needs first class support for oblong through-holes. Yup. I've talked about a multi-pin before; this is a pin with arbitrary shaped copper/soldermask/etc on each layer. Yes, when you get to multi layer boards you often want a different annulus on inner layers. I think it's time to think about an expansion to the footprint grammar to support more sophisticated pins and also more sophisticated paste specs. -dave ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: [pcb] overlapping pin/pad -- won't form thermal
On Mon, 2008-03-10 at 16:16 -0800, Dave N6NZ wrote: DJ Delorie wrote: PCB needs first class support for oblong through-holes. Yup. I've talked about a multi-pin before; this is a pin with arbitrary shaped copper/soldermask/etc on each layer. Yes, when you get to multi layer boards you often want a different annulus on inner layers. I think it's time to think about an expansion to the footprint grammar to support more sophisticated pins and also more sophisticated paste specs. I want it on 2-layer boards too, but this is a different case... I've got power terminals which want 5mm clearance to a ground plane, but I don't really want a thermal with its tendrils extending that far out. -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: [pcb] overlapping pin/pad -- won't form thermal
On Mon, Mar 10, 2008 at 5:16 PM, Dave N6NZ [EMAIL PROTECTED] wrote: DJ Delorie wrote: PCB needs first class support for oblong through-holes. Yup. I've talked about a multi-pin before; this is a pin with arbitrary shaped copper/soldermask/etc on each layer. Yes, when you get to multi layer boards you often want a different annulus on inner layers. I think it's time to think about an expansion to the footprint grammar to support more sophisticated pins and also more sophisticated paste specs. -dave Without piling on too much - Expanding the grammar to support inner layer pad outer layer pad would be great. (Would one geometry definition apply to all inner layers?) - Also consider whatever would allow pins (and vias) with no connection to some layers (maybe supporting blind and buried vias in the process?) - Taking this too the limit, consider a shift to a more heirarchical approach which would allow pad definitions to be included in a footprint by reference rather than direct inclusion. (My ignorance of the data structures now used by PCB may be evident here - I don't know how difficult this would be). Joe T ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
