V Carve Creating Steps

I am having an issue when doing a two step carve using an end mill and a v-bit. I designed my project in VCarve Desktop and I am trying to clear out a square that I can then inlay another type of wood into. I have set it up to do a vcarve (60 deg) with a clearing tool (1/4" end mill). I am using homing to make sure that my X and Y are the same between bits and using a touch plate to do my Zero. The problem I keep having is the VCarve isn’t smooth. It is creating steps. I am not sure what I am doing wrong and I am hoping you guys can help me.

Is the V-bit a true 60deg bit? Not 59 or 61deg?
Is the point of the v-bit a very fine point or does it have a small flatspot?

It is a Freud 60 degree v bit and I have read some reviews on it and they have all said it has a flat bottom. Could that be the issue?

The flat bottom is the issue. When you tell the software you have a 60° v bit, it assumes a 60° angle from a fine point. Instead, you have a bit with that fine point chopped off, but you’re zeroing your z as if the angle is there. So the software thinks the bit is higher than it is, causing it to carve too deep.

The workaround is to calculate how much height is “missing” from the tip of your bit, and when you zero your bit, leave that much gap between the bit and the top of the workpiece. Time to brush up on your highschool trigonometry. :slight_smile:

Left, a true V-bit with infinite fine point which is the basis for calculations.
Middle, an actual V-bit with a flat tip (most have some degree of flatness to them)
Right, an actual V-bit, zeroed at flat spot, ignoring the height difference between infinite and actual tip. Will ride deeper => wider cuts and dog bone effect on sharp corners.

(Updated to pic to see changes is dimensions, in mm but they are arbitrary. Sorry Kim :wink: )


That image perfectly illustrates what I tried to say.

Er… I liked the original version better.

Are there any recommendations on a true V Bit that is out there? or else how do I make that calculation and account for it when using a touch plate.

There a lot of them out there.
Here is one source that I use.

Because it’s a 60° bit, what’s “missing” is an equilateral triangle… so a profile view of the missing piece is a triangle with sides the same as the diameter of the flat part of your bit… Half of that is a 30-60-90 triangle, and the height you want to calculate is going to measure half of the diameter of the flat tip of your bit times the square root of 3.

So if you accurately measure across that tiny flat bit (or check the bit’s packaging to see if it says what the flat diameter is), divide by two, and multiply by √3, you’ll have your missing height.

Then just do the homing sequence, but before telling Easel that it’s zeroed, raise the bit by the amount you calculated.

1 Like