I'm using Eagle, flatcam and a CNC laser machine. My problem is when I'm trying to export my board, all my pads are filled ! It means, when my board will be engraved (chimical method), I will not find any holes in the middle of the pad to use for drilling (manual)

Eagle board:

enter image description here

Flatcam preview:

enter image description here

Do you know where I can change this to have "open pads" ? It's an eagle parameter ? flatcam parameter ?

Thanks for your advice, I'm a newbee

  • \$\begingroup\$ Not quite sure why you can not drill through the copper... \$\endgroup\$ – PlasmaHH Apr 28 '16 at 13:27
  • 1
    \$\begingroup\$ @PlasmaHH: I think its not a problem of drilling through the copper. I think he'd like a "target" on the pad while manually drilling the holes. \$\endgroup\$ – JRE Apr 28 '16 at 13:30
  • \$\begingroup\$ Yes, it would self-centre the drill for him. \$\endgroup\$ – Transistor Apr 28 '16 at 14:07
  • \$\begingroup\$ can you post a screenshot of the holes on the gerber files? If they are filled its an eagle issue, if they are opened then its a flatcam issue. \$\endgroup\$ – Wesley Lee Apr 28 '16 at 14:35
  • \$\begingroup\$ @WesleyLee they are filled in the gerbers - it's by design as otherwise it would cause issues in commercial fabrication. \$\endgroup\$ – Tom Carpenter Apr 28 '16 at 14:39

Unfortunately there is no way to do this directly. The Eagle CAM processor specifically fills in hole areas with copper so that if there is any misalignment in the drilling stage of manufacture you don't end up with gaps in the copper next to the hole which could cause problems in the through-hole plating step and during assembly.

I understand for home assembly it would be a useful feature to create self-aligned holes, but there are no options in the CAM processor to do it. Even the DXF export ULP has the same behaviour (fills holes).

You can do it by printing the design to a PDF showing only the copper layer. This does result in the holes showing up as unfilled. However this is only useful for home chemical etching using say the toner-transfer method. I don't think there is a way to import the PDF into Freecad for milling.

You can get creative in eagle and redesign all your pads to be made of polygons shaped with a hole in the middle and a much smaller pad off to one side, however this would be far more trouble than its worth and would likely be a DRC nightmare.

| improve this answer | |
  • \$\begingroup\$ Huum, ok I see. So, I probably have to play with the EXELLON file to merge the drill info... \$\endgroup\$ – maxic31 Apr 28 '16 at 14:49

Since I don't use Eagle or Flatcam, I'm going to make an oddball suggestion for a solution that will work regardless of the software you used to generate the gerber and excellon files.

  1. Download Gerbv and install it. Or, for Linux users, install gEda since Gerbv is part of that package.
  2. Open the gerber file for the bottom side of your PCB in Gerbv
  3. Open the excellon (drill) file in Gerbv.
  4. Check that the gerbers and excellon data line up (drill holes on the pads and not floating off in space somewhere.)
  5. Set the color of the drill layer to white and make it the top layer.
  6. Set the color of the gerber layer to be black. All of your traces will appear to be gone. Don't panic. They are just black lines on a black background.
  7. Export the resulting file as an SVG. The black background doesn't get exported, so the resulting svg has a transparent background with black traces and white drill holes.
  8. Use any SVG viewer/editor to display the final file. I used Inkscape
  9. Print the SVG and use the printout as your mask (photoresist or laser toner transfer) for etching the PCB.

This is pretty much universal, so long as Gerbv can understand your gerber and excellon files.

Gerbv couldn't read some files from I got from Maxim, so there are exceptions.

| improve this answer | |

Check out LineGrinder instead. Works with your Gerber files directly.

It's excellent software and I've used it successfully to do what you're trying to achieve. It can not only use your Excellon drill file to mark drill locations, but can even reference pin holes for flipping if you are trying to do double sided.

| improve this answer | |
  • \$\begingroup\$ Looks to be the same type of software as Flatcam. Both produce GCode. Can either produce something suitable to be used as a mask for chemical etching? \$\endgroup\$ – JRE Apr 28 '16 at 16:10
  • \$\begingroup\$ Flatcam is already putting out suitable GCode (whether CNC isolation routed or chemical etched irrelevant in this case), except that Flatcam is not leaving a hole to route (or etch) away for the drill marks, and LineGrinder will do this no problem, it's just a setting in the tool to use your drill file to mark pilot holes. So, yes, this will produce a suitable mask for the OP. \$\endgroup\$ – Joel Wigton Apr 28 '16 at 16:13
  • \$\begingroup\$ @maxic31 So did you give this a try? \$\endgroup\$ – Joel Wigton May 1 '16 at 23:01

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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