Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
I have designed an land pattern for a micro USB connector. The connector have 2 x 0.9mm drill holes under it.
The problem is the clearance distance around these holes being to big and overlaps the soldering pads for the very same connector.
These holes are just plain holes, I don't need the same clearance rules as for traces. Is there a way to override the automatic clearance and set them manually?
---- EDIT ---
As you can see, the hole clearance overlaps the pad on the top layer (red).
Yes, this is done in the DRC settings. One of the parameters sets how far traces must be from board edges, which includes the edges of unconnected holes. I don't remember the exact setting name, but run "drc", look thru the settings, and you should be able to spot it.
You are saying you looked in the DRC but didn't find it. It's actually quite obvious and one of only two setting under the "Distance" tab:
I got the answer in the Element 14 forum for EAGLE. It isn't possible to just change a few rules, it is all dimension borders or none being affected. This is the answer I got:
The copper clearance from holes and the edge of your board is set in the DRC. (DRC>Distance>Copper/Dimension)You can reduce this to zero and the copper will fill right up to the lines marked in the Dimension layer. Then you need to check and address the issues that arise from this. The copper will be allowed right to the edge of the board which is not good practice so place a tRestrict bRestrict wires here to constrain the pour. The second thing you need to check is the solder stop top and bottom around the hole and the board edges. Milling and plain hole drilling is the last stage and keeping solder stop away from the cutter prevents chipping. HTH Warren
-- Viewed / responded via the newsgroup at news.cadsoft.de
Although, I didn't want zero distance, just a smaller distance. Anyway the procedure is still necessary if the distance becomes to short for the manufacturing process.