I'm new to PCB, how to create isolation slots or air gaps in PCB using eagle CAD.


  • \$\begingroup\$ I don't know what you think a "isolation slot" or "air gap" means in this context. \$\endgroup\$ Commented Jan 20, 2016 at 12:11
  • 3
    \$\begingroup\$ @Olin: Why do you think he might mean anything other than the standard definitiion? \$\endgroup\$
    – Dave Tweed
    Commented Jan 20, 2016 at 13:26

2 Answers 2


EDIT: I saw you were not talking about spark gaps but rather about air gaps. Well this can be done simply with the milling layer. Nevertheless I leave the answer as it is if that's acceptable.

If you are looking into sending your data directly in EAGLE file format then the following should work:

  • With the top layer (1) you can draw copper.
  • With the tStop layer (29) you can remove the solder mask on certain areas.
  • With tRestrict (41) you can prevent the flood of copper if you are using a polygon pour.
  • With milling (46) you can specify which areas need to be milled.

If you are going to use GERBER-Files (highly recommend doing it) then you can be pretty much flexible and use any layer. However, due increase risk of miss interpretation by others I suggest not using any layer but the layers I mentioned above.

Hope this helps.

Picture for an example:

enter image description here

Bonus tip: I suggest creating directly a part of the spark gap because it will later make routing a lot easier for you.

Caution: Always make sure your manufacturer can actually handle your PCB requirements! For example mine can only handle millings down to 0.8mm so be sure you know your limits.

  • \$\begingroup\$ Just because you put something in a layer, that doesn't mean that the manufacturers defaults will use it that way, or that your job files are set to correctly use them (if you're making Gerbers) \$\endgroup\$ Commented Jan 20, 2016 at 14:14
  • \$\begingroup\$ I'm aware of that and that's exactly why I don't recommend sending EAGLE files to a manufacturer. When using Gerbers it is also clear that you have to define which file is which layer but that was not asked here. \$\endgroup\$
    – Marco
    Commented Jan 20, 2016 at 14:27
  • \$\begingroup\$ I just gave him general advice because that's how the layers should be used for according to EAGLE. \$\endgroup\$
    – Marco
    Commented Jan 20, 2016 at 14:34

I don't think this is specific to Eagle, but generally if you want milled isolation slots you will specify that on a mechanical layer, the same as the outline routing or V-grooves.

Typically (check your PCB manufacturer's instructions) slots that touch copper will be plated by default and if they don't touch copper they'll be unplated by default but you should be able to change that with a call-out on the mechanical layer.

The center of the drawn contours should be the edge of the milled slot- in other words the width of the lines you draw will not be used in any way.

Note that the manufacturer has a choice of tools to use to do the milling. Inside corners will, by necessity, have a non-zero radius (equal to the radius of the milling tool), so even if you draw the corners sharp they will end up with some internal radius. You can ask for a specific tool radius but they'll probably use what they want. For example, if they use a 1mm diameter routing tool you'll end up with 0.5mm radius on internal corners (and, of course, your minimum slot width will be 1mm). Larger tools will cut faster, wear slower and be less prone to breakage, so they are going to tend to prefer larger radii. If you design the slots with rounded internal corners with radii equal to half the slot width you should not have any unpleasant surprises on that account. In practice that may mean making them a bit longer than you would otherwise make them.


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.