Re: gEDA-user: Funny pad rotation
On 3/23/10, DJ Delorie d...@delorie.com wrote: Looks like a fundamental design issue. We use the X layer to draw lines, which includes pads, but with the tiny offsets in the x,y points, we end up passing two points to the X layer that have the same coordinates, so it draws a zero-angle line. If you zoom in far enough, eventually rotates the pad on the screen. To get this right, we'd have to somehow calculate when X is going to do the wrong thing based on our scaling, and draw those lines as polygons instead, so that we can do the math with more precision. I thought it was a very well-known feature; it was reported in 2007 (http://sourceforge.net/tracker/?func=detailaid=1800872group_id=73743atid=538811); I support a patch for rectifying it here: http://repo.or.cz/w/geda-pcb/dti.git/shortlog/refs/heads/ineiev-dspdances.squashed Cheers, Ineiev ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Funny pad rotation
On Thu, 2010-03-25 at 06:34 +, Ineiev wrote: On 3/23/10, DJ Delorie d...@delorie.com wrote: Looks like a fundamental design issue. We use the X layer to draw lines, which includes pads, but with the tiny offsets in the x,y points, we end up passing two points to the X layer that have the same coordinates, so it draws a zero-angle line. If you zoom in far enough, eventually rotates the pad on the screen. To get this right, we'd have to somehow calculate when X is going to do the wrong thing based on our scaling, and draw those lines as polygons instead, so that we can do the math with more precision. I thought it was a very well-known feature; it was reported in 2007 (http://sourceforge.net/tracker/?func=detailaid=1800872group_id=73743atid=538811); I support a patch for rectifying it here: http://repo.or.cz/w/geda-pcb/dti.git/shortlog/refs/heads/ineiev-dspdances.squashed Patch looks good, but I'm not sure it is necessary to pass 5 vertices (manually closing the polygon). I think it would be fair to assume the polygon is closed, and this is what (at least the GTK HID) does - so it would be more appropriate to pass 4 vertices. I note that (guessing from the context when viewing the patch), the thindraw is manually drawn line by line done in DrawPadLowLevel, so there is no worry that the gdk_draw_polygon (used in the HID-fill_polygon) call, does not appear to close the shape if it were called to draw a non-filled polygon. -- 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!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Funny pad rotation
Hi, On 3/25/10, Peter Clifton pc...@cam.ac.uk wrote: Patch looks good, but I'm not sure it is necessary to pass 5 vertices (manually closing the polygon). Quite right, thank you; I've updated it in repo.or.cz: http://repo.or.cz/w/geda-pcb/dti.git/shortlog/refs/heads/ineiev-dspdances.squashed Regards, Ineiev ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Funny pad rotation
I thought it was a very well-known feature; it was reported in 2007 ([1]http://sourceforge.net/tracker/?func=detailaid=1800872group_id =73743atid=538811); Yes, but that bug report came with a request explicitly asking that it not be fixed! References 1. http://sourceforge.net/tracker/?func=detailaid=1800872group_id=73743atid=538811 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Funny pad rotation
Yes, but that bug report came with a request explicitly asking that it not be fixed! Okay, yes it's amusing, but is there really a justifiable reason *not* to fix it? It's *not* expected behavior. It looks and feels and acts like a bug. I wasted quite a bit of time before thinking to ask the list for help. And, if I hadn't checked my gerbers carefully, I would have wasted several hundred or thousand dollars as well. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Funny pad rotation
I'm having an issue exporting my board from PCB as a gerber. Please take a look at this screenshot: http://flickr.com/gp/oskay/L98vvn The pads look normal-- square to the page --in PCB, but are rotated strangely when I export as gerber. The footprint, as it appears in my PCB document is: Element[ gullwing_opto IRD201 unknown 325000 262500 -7000 -17500 0 100 ] ( Pad[-6703 -1 -6700 1 4000 2000 5000 1 square] Pad[6700 1 6703 -1 4000 2000 5000 2 square] ElementLine [-3000 -8900 -3000 -6900 700] ElementLine [-3000 8900 -3000 6900 700] ElementLine [6700 -7900 6700 -4400 700] ElementLine [6700 7900 6700 4400 700] ElementLine [-6700 -7900 -6700 -4400 700] ElementLine [-6700 7900 -6700 4400 700] ElementLine [-6700 -7900 6700 -7900 700] ElementLine [-6700 7900 6700 7900 700] ElementArc [-3000 0 4000 4000 45 270 700] ) Is this a known bug? Any workaround? Thanks! -Windell ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Funny pad rotation
On Tue, Mar 23, 2010 at 3:09 PM, Windell H. Oskay wind...@oskay.net wrote: I'm having an issue exporting my board from PCB as a gerber. Please take a look at this screenshot: http://flickr.com/gp/oskay/L98vvn The pads look normal-- square to the page --in PCB, but are rotated strangely when I export as gerber. The footprint, as it appears in my PCB document is: Element[ gullwing_opto IRD201 unknown 325000 262500 -7000 -17500 0 100 ] ( Pad[-6703 -1 -6700 1 4000 2000 5000 1 square] Pad[6700 1 6703 -1 4000 2000 5000 2 square] ElementLine [-3000 -8900 -3000 -6900 700] ElementLine [-3000 8900 -3000 6900 700] ElementLine [6700 -7900 6700 -4400 700] ElementLine [6700 7900 6700 4400 700] ElementLine [-6700 -7900 -6700 -4400 700] ElementLine [-6700 7900 -6700 4400 700] ElementLine [-6700 -7900 6700 -7900 700] ElementLine [-6700 7900 6700 7900 700] ElementArc [-3000 0 4000 4000 45 270 700] ) Is this a known bug? Any workaround? Are the pads exactly square? (sorry about my laziness to do the math). Try making them slightly rectangular. That worked for me for going the other way: I found it impossible to rotate a perfectly square pad 45 degrees. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Funny pad rotation
That's really wierd. The exports are correct, the GUI is wrong - your footprint really does have oddly rotated pads: Pad[-6703 -1 -6700 1 ... That's a dX of 3 and a dY of 2. If you enable thindraw (the | key) it shows the correctly rotated outlines. Debugging... ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Funny pad rotation
On Mar 23, 2010, at 1:19 PM, DJ Delorie wrote: That's really wierd. The exports are correct, the GUI is wrong - your footprint really does have oddly rotated pads: Pad[-6703 -1 -6700 1 ... That's a dX of 3 and a dY of 2. If you enable thindraw (the | key) it shows the correctly rotated outlines. Debugging... Wow-- yes-- you're right. It sure shows up in thindraw mode. Thanks! -Windell ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Funny pad rotation
Looks like a fundamental design issue. We use the X layer to draw lines, which includes pads, but with the tiny offsets in the x,y points, we end up passing two points to the X layer that have the same coordinates, so it draws a zero-angle line. If you zoom in far enough, eventually rotates the pad on the screen. To get this right, we'd have to somehow calculate when X is going to do the wrong thing based on our scaling, and draw those lines as polygons instead, so that we can do the math with more precision. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
