I'm trying to create a plated cutout in eagle for a DC barrel jack connector (https://www.sparkfun.com/datasheets/Prototyping/Barrel-Connector-PJ-202A.pdf) for a 4 layer board to be fabed by oshpark. I've followed the general guidelines provided by eagle:

In the package I used a long pad with a drill size equal to the shortest dimension of the desired rectangle. I then drew a rectangle of the desired cut out on the middle layers and milling layer.

The trouble is that oshpark doesn't use the milling layer -- they want all holes on the dimension layer so I am forced to copy the rectangle onto the dimension layer too. The DRC for oshpark also dictates a 15 mil spacing between copper and dimension. What this means is that I'm left with a pad that's unconnected on the inner layers because the dimension layer +15 mil spacing is too far away from the pad on the inner layer.

enter image description here

Obviously it would be nice to have that connected. I played with the restring of pads and can of course increase that so there's contact as shown here:

enter image description here

The problem is that now every pad now has this property, which isn't desirable. Is there anyway to either change the shape of inner layer pads selectively or selectively change the restring value for a package? Alternatively is there anyway to accomplish what I'm trying to do in another way?

  • \$\begingroup\$ Why don't you generate the gerbers instead of sending off design files? That way you can do things in whichever layer(s) suits you. \$\endgroup\$ Commented Nov 7, 2013 at 2:36
  • \$\begingroup\$ Interesting. And then edit the gerbers? As it stands if I generate the gerbers the gerbers will reflect the design as is. \$\endgroup\$
    – Doov
    Commented Nov 7, 2013 at 3:43
  • 1
    \$\begingroup\$ You use another layer that does not interfere with your routing (like the milling layer). Then you generate that particular gerber from both dimension and milling layers. No need to edit the gerbers. \$\endgroup\$ Commented Nov 7, 2013 at 4:00
  • \$\begingroup\$ If you post as an answer I'm happy to give you the credit. \$\endgroup\$
    – Doov
    Commented Nov 7, 2013 at 4:06

2 Answers 2


Instead of sending off the design files, generate the gerbers yourself (which is what most pcb manufacturers accept anyway).

Use layers that do not interfere with your routing (like the milling layer), and generate that particular gerber file using both the dimension and the milling layer.


From your screenshots it appears you have created an internal cut-out (I think). Therefore you won't be able to do what you want with OSHPark. On their support website it states that they do not support plated cut-outs:

All internal cutouts will be unplated, and must be 0.1 inches (2.54mm / 100 mil) wide.

The link above is worth a look as it suggests some work-arounds.

When I include these types of jack connectors in my EAGLE projects, I use plated through holes for the legs which are quite a bit bigger than the actual legs - as shown in the picture towards the end of the page linked above.

Also, in addition to apalopohapa's answer (I do not have enough rep to comment on his answer), OSHPark provide the CAM job file for generating your own gerber files; refer to this page: http://support.oshpark.com/support/solutions/articles/106997-cam-job-for-eagle-cad

  • \$\begingroup\$ Yeah that's what the site says, but when I emailed them they said it would work. I've actually spun a board with an HDMI connector (similar situation), but didn't have a need to connect the shell of the connector and they came back as intended. I've also done the large plated through hole, but it's just really clunky and takes up a lot of board space. I know that oshpark can process the .brd, but if you have large polygons etc their server crashes and tosses the job. My board is ~4"x4" with polygons on all 4 layers -- the oshpark processing engine breaks every time I try to upload it. \$\endgroup\$
    – Doov
    Commented Nov 7, 2013 at 18:14
  • \$\begingroup\$ BTW another reason I like generating my own gerbers is that I can use whatever font I want in eagle whereas if I use the oshpark gerber generators then I'm limited to vector font. \$\endgroup\$
    – Doov
    Commented Nov 7, 2013 at 18:18
  • \$\begingroup\$ That's interesting, didn't know that they would actually allow it. Have never encountered the large polygon issue with their website before though, have always just uploaded a Gerbers ZIP. The CAM job in the link above makes that very straightforward (although you might want to turn on additional layers in the top and bottom silkscreen menus). \$\endgroup\$
    – user31299
    Commented Nov 8, 2013 at 21:43

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.