Submitting gerbers generated by EAGLE 4.16 to the DRC bot, they are failed due to a too-small aperture in the top copper file. The board adheres to the 8/8/20 rules and passes all the EAGLE DRCs. On further inspection, the culprit is some of the SMD footprints have very small roundings (roundness=5) on the corners of the pads. The gerber generator creates these by defining some ridiculously small aperture to run around the square pad and create the (unnecessary) rounded corners.
Is there a way to correct this behavior (force un-rounded pads) for now and the future, short of hand-editing hundreds of footprints in the library to set roundness=0, or hand-editing hundreds of future Gerbers to change the unwanted apertures? (SMD pad roundings are already set all 0s under the EAGLE layout editor DRC → Shapes tab, to no effect.)](http://tim.cexx.org/images/eagle_rounded_smd.gif)
If you’re referring to the one under DRC → Shapes… that is already set to all 0s, and having no effect (the “roundness” values in the libraries are superceding it).
My current settings there are: Roundness:
Min: 0mil
%: 0
Max: 0mil
But the pads get rounded anyway.
For now I have just hacked around inside the library (changed roundness to “0” for all pads on parts that appear in this specific board) and gotten past this error, but I still would like to know how to fix this once and for all. Maybe even an “I know what I’m doing” checkbox to bypass erroneous DRC bot errors (IIRC, Gold Phoenix will take the rounded pads / small apertures without complaint, so long as the actual resulting copper obeys 8/8 rules)
Now getting past that, my next issue is EAGLE generates a 0mil “line” around holes (it shows even on copper layers!), which is causing failure on the 2nd-level DRC bot (drc2 “at” sparkfun.com). Any ideas how to fix this too?
There is another setting to change the shapes or lands…it is something like use the shape in the library or always be square or round…it is a drop down box.
As for the 0 mil line…I have no idea what would be causing that…I’ve never had that problem.
I know this is not much help…but given my current situation…it is the best i can do until I get my design computer back running…which will be after tomorrow. (card comes tomorrow)
Don’t know how that one slipped past the goalie. Dimension layer was turned off for copper layers, but the one non-plated hole on the board (again part of a footprint in Someone Else’s Library™) was creating the 0mil circle on the copper layers all the same. A hard delete of all the gerbers (this is on a network share folder), reboot and regenerate them all with the [SFE-Special.cam job, and the bogus 0mil apertures are gone!
I ran into another small glitch, but I think it deals only with one specific library part - the drills for the through-hole pads should be .020", but end up as .0197 in the gerber (roundoff problems?). For now I’ve “fixed” this in the gerber directly, but it should be easy enough to fix for real assuming this is the only part affected.
First BatchPCB order accepted (all DRCs pass) this morning All this after my formerly favorite board house (rhymes with “PCB Slab Distress”) wastes my time for three days accusing me of “multiple layouts” (the one time I have a single board legitimately split into high- and low-voltage sections) and refuses to make the board. Can’t wait for this one to arrive!](http://www.sparkfun.com/tutorial/PCB/SFE-Special.cam)
I ran into the problem described in the original post today, and decided to post this to save someone else the time I spent troubleshooting! Turns out I had several problems, so it was an iterative process with the DRC bot since it bails on the first one it finds.
First problem was some Linear Technology parts with DFN packages, which I used as a starting point for newer LT parts that didn’t exist. The pads had rounded corners. Changing “roundness” to zero on these pads removed the error.
Second (major) problem was due to my using a wire width of 0.1mm on the polygons I had created for the ground plane. I figured the border could be any width since the overall polygon is what matters. However, the wire width does show up in the Gerber files and needs to be wider than 8 mils to pass DRC.
Unfortunately there’s really no good way to figure out what part or trace is causing the problem in the aperture table. I isolated the parts by putting them on a new board with no traces. To figure out the polygon wire width problem I had to import the Gerber files into GC-Prevue, find the offending aperture entry, and bumped it up to something ridiculous (ie: from .009 to 1.0), which made it very obvious what trace or region was the culprit.
Add another vote for fixing the bug that causes the DRC bot to report “Error - Aperture too thin” on packages with rounded pads, or at least providing a more-meaningful error message. Just lost about 2 hours on this one. :evil:
Lead-free solder paste doesn’t spread as well during reflow, so it may leave the corners of rectangular pads exposed. Pretty much any RoHS-equipped board house can deal with rounded pads, so it shouldn’t be considered an error by the DRC bot, as far as I know.
(IIRC, Gold Phoenix will take the rounded pads / small apertures without complaint, so long as the actual resulting copper obeys 8/8 rules)
All this after my formerly favorite board house (rhymes with “PCB Slab Distress”) wastes my time for three days accusing me of “multiple layouts” (the one time I have a single board legitimately split into high- and low-voltage sections) and refuses to make the board. Can’t wait for this one to arrive!](