Re: gEDA-user: Howto make solder mask extend equal for all pads in layout?
Am Sonntag, den 05.10.2008, 00:09 +0100 schrieb Peter Clifton: On Sat, 2008-10-04 at 10:22 -0400, DJ Delorie wrote: Is there something similar for copper clearing of pads/pins in polygons? Not that I'm aware of. Again, you could write one pretty easily by copying the existing one. changeclearsize(selected,10,mil) Also works for mask, if you select the mask layer before running it. A late response... For mask changeclearsize() seems not to act on distance of mask relief to copper but on total relief size. So changeclearsize(selected,8,mil) will not make the relief 8 mil larger than pad (as desired by me) For copper clearance changeclearsize() works fine. To adjust mask DJ's solution seems to work perfect: DJ Delorie wrote on 4 Oct 2008: There is a MinMaskGap() action to increase the mask gap to vendor minimums. What you can do is this: * Enable the mask layer * Select everything that needs the mask set * Use Ctrl-Shift-K to reduce the mask as much as you can for everything selected * :MinMaskGap(Selected,=8,mil) to increase them all to that amount ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Howto make solder mask extend equal for all pads in layout?
On Sun, 2008-10-05 at 18:33 -0700, Steven Michalske wrote: Not having a good laptop week. May I suggest looking into an Apple laptop, I put loving care into each one I work on :-P You work for Apple? Cool. Yes, Apple laptops are very nice... will certainly take a good look at the Mac Book Air when I bite the bullet and look for a replacement machine. A bit expensive, but nice. With the thin-ness though, I'm woried there just can't be any gap behind the LCD, and that it might make it more vulnerable to being damaged. -- 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: Howto make solder mask extend equal for all pads in layout?
Not having a good laptop week. May I suggest looking into an Apple laptop, I put loving care into each one I work on :-P -- Peter Clifton ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Howto make solder mask extend equal for all pads in layout?
There is a MinMaskGap() action to increase the mask gap to vendor minimums. What you can do is this: * Enable the mask layer * Select everything that needs the mask set * Use Ctrl-Shift-K to reduce the mask as much as you can for everything selected * :MinMaskGap(Selected,=8,mil) to increase them all to that amount If you're adventurous, you could look up the sources for MinMaskGap() and add a SetMaskGap() that does the same thing, but forces it to a specific value. Should be relatively easy. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Howto make solder mask extend equal for all pads in layout?
Am Samstag, den 04.10.2008, 10:07 -0400 schrieb DJ Delorie: There is a MinMaskGap() action to increase the mask gap to vendor minimums. What you can do is this: * Enable the mask layer * Select everything that needs the mask set * Use Ctrl-Shift-K to reduce the mask as much as you can for everything selected * :MinMaskGap(Selected,=8,mil) to increase them all to that amount Great! Is there something similar for copper clearing of pads/pins in polygons? If you're adventurous, you could look up the sources for MinMaskGap() and add a SetMaskGap() that does the same thing, but forces it to a specific value. Should be relatively easy. At least I will create a feature request for sourceforge bugtracker. Thanks Stefan Salewski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Howto make solder mask extend equal for all pads in layout?
Is there something similar for copper clearing of pads/pins in polygons? Not that I'm aware of. Again, you could write one pretty easily by copying the existing one. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Howto make solder mask extend equal for all pads in layout?
On Sat, 2008-10-04 at 10:22 -0400, DJ Delorie wrote: Is there something similar for copper clearing of pads/pins in polygons? Not that I'm aware of. Again, you could write one pretty easily by copying the existing one. changeclearsize(selected,10,mil) Also works for mask, if you select the mask layer before running it. Ah crud... just realised I've got a cat-hair re-assembled into my LCD panel. (Aside from the couple of hot-columns and failed left hand half. Not having a good laptop week. -- 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: Howto make solder mask extend equal for all pads in layout?
changeclearsize(selected,10,mil) I keep forgetting about that, because it reduces the clearance on bigger clearances too, which usually isn't what I want. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
