Tabs causing burn marks

Hi All,

I’m looking for a solution to the burn marks caused by making tabs. It seems like at every tab location, there is a small vertical burn mark from where the end-mill stops and moves up to jump over the tab. The severity varies, but in some instance there is an actual groove and burn line. In this case, it becomes very difficult to remove the artifact without sacrificing the surrounding surface.

If anyone has a way to prevent this please let me know.


The solution is to not create tabs, or to add an allowance to the cutting outline and take that allowance off as a last pass.

Use the double-tape-cyanoacrylate method to hold your part to the table. (Glue such as 2P-10 with activator.)

1 Like

Im not sure if wholly elminating tabs would be neccessary, and completely changing your workflow and hold down method could leave the underlying issue unaddressed to come up in a different nasty way later on. Can we get some more info? Machine set up, type of z-axis, router type, type of material being cut, endmill used, etc.

Edit: feed rate, rpm, and depth of cut would help too


In my experience, this is caused by runout and plunge speeds that are off. It can help to have a roughing pass, then a finish pass/spring pass. The plunge, especially with a small endmill (⅛") can cause a lot of runout, causing a little notch where you don’t want it, and the endmill seems to get particularly hot.


Exactly my point @mikep. I had the exact issue you just described before getting decent collets fot my dewalt. Speaking of, I havent checked lately but does CC still output the “after tab plunge” rate set to the feed rate? Or did that get addressed? I havent cut many tabs lately.

Adjust your feeds and speeds so that this doesn’t happen. One technique:

How big of a tab are you leaving?
Maybe adjust that as well. I usually go 0.1" height by 0.2" length. Barely a hop as the bit goes by but enough to hold the piece in place.


If you’re using Fusion 360 to do your CAM, the tabs option in the 2D contour workflow will let you switch to triangular tabs. These have an angled profile that will keep your endmill from stopping on the contour while it raises the tool to hop over the tab.

1 Like

I’m typically cutting hardwoods like Maple or Walnut with a .25" flat end mill.

50ipm, .06depth with a 2deg ramp.

I’ve always wondered what the triangular tabs were for. I think this could be a great solution. I’m going to try this on my next part and see how it goes.


1 Like

Those triangle tabs are called “3D” tabs in Vectric software.

The key advantage is that the bit keeps moving instead of stopping, changing Z, moving again and changing Z again. Instead of stopping, it is a continuous movement.

1 Like

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.