Optimizing toolpaths for detailed pocket cuts

How To
1

Forgive me if this has been covered before, but I couldn’t find anything with the logical (to me) search terms.

I’m curious about optimizing toolpaths. For instance, assume you want to create a pocket cut for a sans serif font. Given the size of the project you can use a 1/8" bit for most of the cut. However, there are certain letters that don’t cut cleanly.

The obvious solutions to me are:

  1. Choose a smaller bit
  2. Use two toolpath operations - the first to cut out the bulk of the pocket with a larger bit, and then a second to get the details with a smaller bit.

Option 1 has it’s drawbacks - long cut time, higher potential to wear out/break a bit

Option 2, if optimized should be more efficient, but the second toolpath ultimately goes over the area that’s already been cut, when it only needs to hit the parts, typically around the edges of the pocket, to finalize the shape. My issue is that I’m not sure how to structure option 2 for optimal cut time. One hypothesis: have toolpath 1 as a pocket cut with a larger bit, and then for toolpath 2 use a smaller bit and a contour cut with the inside offset? However, this doesn’t yield clean results.

Screenshot 2025-10-24 at 4.23.52 PM
Screenshot 2025-10-24 at 4.23.52 PM3024×1964 493 KB

You can see here that the “n” and “r” have material left where the curve and straight sections meet. The corners aren’t square either.

I’m sure this same concept is applicable in many different contexts, but letter carving is one of the first that came up for me.

Edit as I write this - I found this thread: Should large pockets with details be cut with two bits? - #5 by mhotchin

It mentions the pocket + contour approach, but will that still yield rounded corners? Is an additional path with a vee bit necessary?

For context - I’m purely in the design phase - not using CC Pro (yet) - and trying to get a handle on how these things all work before jumping in and getting a machine and all the bells and whistles.

Thanks for your patience!

2

A tool needs to be ~10% smaller than the narrowest region in a pocket.

For a work-around see:

3

Will, thanks for the response. I can follow what you’re doing there, but I don’t understand the why.

  • What purpose does adding the geometry at the narrowest point serve? Would this need to be repeated for each letter with a narrow point? I would assume so.
  • How did you determine what the offset measurement should be?
4

The measurement at the narrowest point in all of the geometry is needed — once one gets that, that measurement (a bit less than the circle which fits at that narrowest position) is used for a single inset operation.

5

Ah! OK. That makes more sense. I assumed there was some sort of relationship there, but wasn’t sure exactly what it was. Many thanks for the clarification.

6

Hi Jason, I like Will’s solution as all is in one nice toolpath.
I use the following technique to create rest pocketing in carbide create as follows.

  1. Save your file as a different name so you have your original tucked away. This process will remove a lot of the text.
  2. On your renamed file look at your simulation and identify where your tool has not been able to pocket the shape. Go back to your design and draw a shape that overlaps the regions you have identified.
    sqaures inserted
    sqaures inserted541×368 19.9 KB
  3. Select one letter and the shape you drew .Use your Boolean tools (intersection) to remove all but the area that was not pocketed. Do the same to the other letters.
    squares after boolean
    squares after boolean519×403 11.9 KB
  4. Select the 2 shapes, create a pocket toolpath with the same depth as your original toolpath but with a small end mill (1mm).
  5. Run the toolpath - job done.
    This is my manual way of producing rest machining.
2 Likes
7

The official way to address this is with the “REST Machining” Pro feature which was added in v7: