V Carve Depth -- not going deeper

I have a thin stock I am attempting to vcarve the owner’s initial. In the toolpath I had the max depth set for .1 inch. (the stock is .5 inch). The carve was not deep enough.

I edited the toolpath and changed the max depth from .1 to .2. Saved the file. Went to CM to load new file (made sure I opened the changed file). Ran it again. It did not carve any deeper.

I tried it again – changed toolpath depth to .35. Saved the file. Went to CM to load new file (had new time stamp so I know the file saved). Ran the job again. It did not carve any deeper.

I did not move the stock or adjust the cutter at all. Why is it NOT going deeper when I change the tool path v carve depth?

Vcarve will only go deep enough to keep the tool tangent to two (or more) vectors. If you have a line that’s 0.100 wide, a 60° cutter will only go 0.087 deep, no matter what the max depth is set to.
The max depth comes into play when the curves are far enough apart that the tool can’t make contact on both sides at that depth. You don’t want this happening with Vcarve as now the carve isn’t matching the design. To limit depth use Advanced Vcarve.


On a simple vcarve you should bottom of stock. If you limit depth you get weird results. Using the bottom of stock on thin material can cause you to cut right through the stock. In those cases where you need to limit depth use advanced vcarve.

Simple vcarve works well on larger objects with 90/60 degree bits. However if you have fine lines using a 30/20/15 degree vee bits works better. If during the preview using a 90/60 degree and you can barely see the carving you need to use a smaller vee bit angle.

A simple vcarve goes down the middle of an object until the bit touches both sides of the object. Advanced vcarve can use a flat end mill to carve out flat areas and then the vee bit goes around the perimeter to get the vcarve effect. If the areas that are flat are too small for the flat end mill the vee bit will carve out those areas. If there are others big enough for the flat end mill only those areas are cut with the flat end mill. If nothing is big enough for the flat end mill all the carving will be done by the vee bit to the depth you limited it to.

1 Like

Another work around would be to just adjust your z zero, i.e. set zero run file if u would like it deeper, reset z zero in small increments until recieve exact look you want.


Good idea. I appreciate the response.

As mentioned, the width between vectors is the determining factor on how deep the bit will cut. You could make the letters fatter, but that may not be the look you’re going for. I would suggest running a narrower v-bit, such as a 30degree bit. I purchased a set of very cheap chinesium v bits on amazon for under 10bucks a while back. They last while with how little they get used.

More acute, not necessarily narrower.

A 30 degree V endmill which was 1/2" in diameter would still cut more deeply than a 90 degree V endmill.

1 Like

My geometry terminology is not to be trusted. That’s why we rely on you!

I was playing around and found that if I adjusted the tool path to start at .5mm it gave the desired results.

First pass some of the carves were little more than a scratch. I had the stick thickness set correctly and had the zero set barely touching the stock. It was a scrap piece so I adjusted the tool path to start at .5 mm. Ran it again and it came out great.

1 Like