Several months ago, I made a few 0.1" to 0.05" [AVR ISP adapters. I made 0.05" footprints (20mil drill, 24mill diameter on 0.05" pitch) myself in my own Eagle library. I ordered the boards and the footprints worked; the 0.05" headers fit into the holes perfectly.
Fast forward to today. I used that same symbol/footprint for 3 new boards ([1, [2, [3) I ordered from BatchPCB. When I got my boards back, the drill holes for the header are too small and the headers won’t fit into them. I went back into Eagle and verified that I had used the same symbol/footprint as before. I also measured the holes of my AVR ISP boards in Eagle and verified they match the sizes in Eagle on my new boards. I can’t view this issue inside gerbv since it does not show drill holes.
I also noticed that on my AVR ISP boards, the via holes are 24mills (0.609mm) in Eagle. This is about the size of my header holes (20mil), so a single pin of my header (20mil/0.5mm) can fit into the via holes, albeit tightly. I used the same via size on my new boards (24mills/0.609mm), but they are visibly smaller and the header pin won’t fit into the vias on any of my new boards. I have always used the sfe_gerb274x.cam file when generating gerber files that get submitted to BatchPCB.
While it’s still possible I did something wrong, I’m leaning towards something happening during the panelization process or at goldphoenix. If it’s my mistake, I’ll gladly resubmit my boards with the problem fixed. I just need to know what to fix so I don’t waste another $50 on an order that has the wrong drill holes. I need to completely understand what happened so I can get confidence back that what I design in Eagle will come back from BatchPCB with the proper dimensions.
Is anyone else having any problems with panel 735? Anyone have any other debug ideas? I sent an email to BatchPCB support last week, but I haven’t heard anything back.
yzf600:
I can’t view this issue inside gerbv since it does not show drill holes.
I think gerbv does show the drill holes. I usually set the colour to the background colour (usually black) and move the drill hole gerber file to the top of the list so it displays over the top of the others.
Greg Erskine:
I usually set the colour to the background colour (usually black) and move the drill hole gerber file to the top of the list so it displays over the top of the others.
Thanks for that info. I see my drill holes now in gerbv.
I was able to get a SAMTEC generated Eagle lbr file for the 0.05" headers. Their footprints for these headers are 24 mil drill, 39 diameter @ 0.05" spacing. My footprints were 20mil drill, 24 diameter (yes I know, pretty crappy footprint design). When viewed in the layout window, both footprints have diameters 20mil larger than what was specified in the footprint. How come the samtec footprint is 24drill/39dia, but when place into my layout, the footprint changes to 24drill/44diameter? The resulting footprint has 6mil spacing between via rings (DRC violation). After experimenting a ton in Eagle, it turns out the diameter of the via rings can be overridden by the “restring” tab of DRC window. The [SparkFun.dru file as the minimum set to 10mil. This 10mil is actually the width between the drill hole and the ring edge, so x2 to get the full diameter. 10x2=20. This explains why the resulting diameters in the layout window were always different than the footprints. I can now use the official SAMTEC footprint in my designs if I just decrease the Sparkfun pad restring values from 10mil to 9mil. I’ll assume this is kosher to do since min trace widths are 8mil. I believe SparkFun had 10mil instead of the minimum 8mil because in one of their tutorials, they said it’s better to make the rings slightly larger in case the drill hole isn’t perfectly centered on the via pad.
Without being able to measure the holes on the real physical boards, I think I have a story of what happened. I believe a 20mil drilled hole, once plated with solder, ends up being smaller than 20mil. Since my header pins are 20mil (measured with my digital caliper), they don’t fit. I think somehow I got lucky with my AVR isp boards and the drill sizes got bumped up to 22 or 24 mil somehow.
Turns out I was able to still solder the headers to the boards. I just have SMT headers now . Since the holes are plated through, it actually keeps the headers from pulling the pads off the pcb like a normal smt header would tend to do. Going forward, I’ve switched to using the SAMTEC provided footprints, with the 9mil restring pad value.](http://www.sparkfun.com/tutorial/Eagle-DFM/SparkFun.dru)
. Since the holes are plated through, it actually keeps the headers from pulling the pads off the pcb like a normal smt header would tend to do. Going forward, I’ve switched to using the SAMTEC provided footprints, with the 9mil restring pad value.](