Cutting to different depths and avoiding flipping

as requested on support…

Given a design which wants to be cut at different depths:

one would work up multiple pockets which will achieve the desired effect.


First, set up the job:

we will use 1/4" stock, and cut the various pockets to half that depth.

Then import the geometry:

and if desired, set the image on the background for reference:

One can see the necessary two levels in the text object, but the rattan background should be let into the back, so we will need to add geometry for that — fortunately the design is symmetrical, so we can do this on the same side that we do the text on and just flip during assembly:

Choose “Offset Vectors”:

and set it to “Inside” and a suitable distance:


We then cut the inside features first:

There are multiple possible approaches — one can use a medium size tool which allows balancing detail against material removal rates, or cut as an Advanced V carving with pocket clearing, since that will capture all of the detail, or cut with a large and a small endmill, using REST machining to as to get sufficient detail — one could also combine these techniques.

First, the advanced V carving — when creating toolpaths, be sure to use the “Edit…” and then the “Select Tool” buttons to choose a material/machine combination which is suited to your setup — if need be, edit any settings as needed:

If you don’t understand a setting or a term, check the videos at:

and see the glossary at:

and if need be, check in at

Once the toolpath is set up, check the 3D simulation:

and if need be, iterate.

Since the slope of the V carving will reduce the area available to the rattan, we go ahead and to an inside contour along the outer design only:

using a tool which is small enough to fit everywhere along the design:

which previews as:

We then cut out the interior shapes:

which might need tabs — if they do, add them:

placing them where they will be easily cut away.


Then assign an inside Contour toolpath which starts at the bottom of the previous pocket and cuts to the full depth — since the depth of the cut is equal to the diameter of the tool, it should be workable to just cut the slot:

which previews as:

Lastly, we cut out the larger outer part — since an 0.25" tool won’t fit into the finer details, we use a 1/8" tool, since the depth of the cut will be twice the diameter of the tool, we need to add offset geometry and cut as a pocket down to tab height (0.0625"):

Offset Vectors

offsetting to the outside by endmill diameter plus 10% or so


Select both the offset and original geometry:

and cut as a pocket down to tab height:

which previews as:

and we add tabs:


lastly we assign an outside Contour toolpath which starts at the bottom of that pocket and cuts the outside of the original geometry through, leaving the tabs:

which previews as:

and should cut to match.


Thank you so much for sharing this!

My pleasure!

One thing which was left unstated/assumed is that the larger part would be flipped over after installing the rattan/backing so as to hide the seams/edges.


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