Can anybody tell me exactly what this is talking about? I don’t have anything in my drill file specifying a hole as small as the one DRC is failing on. Also when I preview in ViewMate, it informs me I have a zero length trace and gives it’s coordinates. There is nothing but a solid line outlining a component on my top silkscren layer where it’s pointing to and I cant find a zero-length anything there. Here’s the DRC error I’m getting. Anybody?
There were errors in the Top Layer File. Please address them and resubmit
After playing around and resubmitting each layer one at a time, I have found out I get this error for both the Top and Bottom Copper Layers, so it doesn’t seem to be a drill problem. By the way, I’m using Ultiboard for my design. Does anybody know of some way to find out what my “Aperture 24” is in Ultiboard?
open up your gerber file with a text editor. look for a line that looks somethinglike this:
%ADD24R,0.00390X0.0520*%
or perhaps
%ADD24C,0.0039
That’s the apperture defintion
then scroll down unitl you find a line lke:
D24*
the line following that contains coordinates where that apperture is used. It might look like this:
X010597Y007685D02*
note the x and y coords. (1.0597, 0.7685) in this case.
Look at those cordinates in your cad program. if it’s not obvious, you’ll need to get a gerber viewer (I use viewmate, its free). open the gerber with the gerber viewer and move the cursor to those coordinates. what ever is there is the offending item.
there’s like, a bunch of coordinates under the line that says
G54D24*
and some of them appear to be negative even though my origin is located at the same place (bottom left) on everything. would deleting this entire D24 section in the gerber file cause it to not work at all?
also, an aperture is like a hole, correct? the problem isn’t on my drill layer, only the top and bottom copper layers
no, an aperture is a shape that can be drawn with. it has nothing to do with drills. think of it as a “brush shape”. The aperture is too small (<8 mil).
you could try deleting it but it’s anyone’s guess what that will mean for your board. Figure out where the aperture is used (look at the gerber for the offending layer, like I said). It should become obvious.
Because gerber format doesn’t have a lot of drawing shapes (apertures), some of them have to be simulated with lots of little lines. that could be your problem. Also, some times text is drawn with narrow lines. got text on copper layers?
well see, theres like almost a hundred coordinates with this particular aperture. i deleted everything in that section and viewed the gerber again. looks identical, so i think imma go ahead and send it out modified
Well, after going round and round with this “Aperture too thin” problem, I finaly came across the problem…at least in my case. I have a very small SMD device whose pads are .2mm wide, which comes out to 7.874 mils…a tad too thin for the Sparkfun check. I changed the pad size to exactly 8 mils, and it has now at least passed the first hurdle of the “Aperture too thin” problem. So, if you find yourself going in and thinking you’ve changed everything (deleting ground planes, manually routing “suspected” wires, moving parts, etc.) make sure your SMD pads are not the problem. Maybe this helps someone…maybe not
