I’ve been fiddling with a layout for an evening now trying to get the DRC bot to accept it. It has a MLF32 footprint on topside that the DRC bot really dislikes.
At first the footprint had too narrow clearances, but I fixed that. In fact, I made sure there was extra clearance. 9.6 mils to be exact.
Pads are 10 mils with 9.685 mil spacing. The footprint is still flagged as in violation???
The interesting thing is that traces leading from the pads are NOT flagged… They are 10mils wide and are spaced 9.685 mils apart just like the pads. In fact they have been drawn so as to always originate from the center of the pads.
Designs passes DRC in Eagle with clearance of 9.685 mils and minimum width of 10mils.
KreAture:
I’ve been fiddling with a layout for an evening now trying to get the DRC bot to accept it. It has a MLF32 footprint on topside that the DRC bot really dislikes.
At first the footprint had too narrow clearances, but I fixed that. In fact, I made sure there was extra clearance. 9.6 mils to be exact.
Pads are 10 mils with 9.685 mil spacing. The footprint is still flagged as in violation???
The interesting thing is that traces leading from the pads are NOT flagged… They are 10mils wide and are spaced 9.685 mils apart just like the pads. In fact they have been drawn so as to always originate from the center of the pads.
Designs passes DRC in Eagle with clearance of 9.685 mils and minimum width of 10mils.
Look at the Gerber files with a Gerber viewer such as GCPrevue. Have the viewer show the outlines of the traces, instead of showing solid traces. EAGLE may have screwed up and drawn the SMD pads as narrow traces, instead of as rectangles. This happened to me when I modified a BRD file I got from the web. I ended up doing the board from scratch. :x
Ahh yes, the drawn pads issue. We get this a lot, simply email us (support at batchpcb.com) and we can manually pass your design if that is the only issue. The problem comes from the lack of intelligence in the bot, it simply sees that a too-narrow trace is present. It does not know that the trace is really making up part of a pad. Until we get a better DRC bot, the only other way besides emailing us to pass it is to have your layout program not draw those pads with traces. That may involve editing the part library though.
I checked the library when I got the error the first time.
Then I changed the pads created with the SMD command like all the other pads on my design. I changed the pads to be only 10 mils so that there would be more than enough clearance, but I don’t see why it should use drawn pads.
I have double checked the footprint in a gerber viewer and indeed somehow for that single footprint Eagle has decided to draw it using lots of lines instead of just it’s correct outlines.
Going to fix that now and see if that solves it for good.
KreAture, thanks for posting the follow up. I have had that problem in the past with a part/footprint I created for an ATtiny24. Now that I know what caused it, I can fix it before I order another board.
Was going to point out the rounded pads, but you guys figured that out already.
Re EAGLE creating pads as a set of narrow traces - This used to be a problem on EAGLE v5.0 and earlier when rotating a component by 45 deg. v5.1 and up has improved on this by implementing the pad as a rotated polygon instead, which means such designs now pass the bot - at least in my experience.
Out of curiosity KreAture, which version of EAGLE are you using? Also, what was the roundness setting? I’ve not used it but from the drawings in datasheets, rounding the pads would seem like a better match for the leads.
I haven’t had time to upgrade all my comps yet so this one actually runns 4.16.r1 !
What I really dislike is how Eagle is not easily set up automatically for shared libraries. (I have 3 computers.)
I’d also like it for Eagle to install to “Program files/Eagle CAD” and not have any version-specific data in the path. That way it can keep the libraries whenever I uppgrade. I really hate it when I need to update due to libraries.
