Broke another bit and yet another unsuccessful carve. 
My pass depth is set to .25 but it digs in aggressively to over .5" and thus breaks the bit. What setting could this be?
I would first look at what vcarve thinks the size of the stock is. If the stock size is too small the first pass will be too deep. Next I would make sure that vcarve’ idea of z=0 is the same as the machines. Then before I broke any more bits I would look at the gcode to see what Z for the first couple of cuts is and make sure that it is reasonable. The safe Z is set to 3.73 inches. It is hard to tell from the pictures but that piece of wood could be thicker than that.
Thanks for the reply Paul. This is rectangular stock to cut a car model (7.1W x 4H x 16L) so I set the diameter in the project settings to the widest part at 7.1"…the car model being wider than it is tall. Maybe it should be set to 4" instead?
How does the safe Z correlate with the pass depth? TBH I’ve always just accepted what Vcarve shows.
I am having a hard time parsing your reply.
Is the stock itself wider than 7.5 inches at any point? Note that this is measured across the diagonal of a rectangular piece. Note that if you had a 7.1 x 4 inch rectangular piece that would give you a 8.14 inch diagonal. It doesn’t matter (for this question) what the model width is, though how you get the alignment of the stock to the model right seems like a challenge.
What did you set your stock size to?
Safe Z is the retraction height for an indiscriminate move. You have told the software that there is no stock, and no jigs, obstructions above 3.7 inches.
I also forgot to suggest that you check your z = 0 location. Could be a tool length/Z 0 sort of problem.
Oh boy - I think I realized what’s been wrong. I’ve just been using the longest edge of the stock as the diameter (in this case 7.1") when in fact I should be using the diagonal (8.14") as you pointed out. 
Essentially I’m telling Vcarve its about an inch shorter in diameter so that’s probably why it’s cutting into the stock more than the pass depth setting of .25".
I have the Z in the software and machine set to the center axis.
I’ll report how it goes. Thanks again the help Paul!
One thing that is very useful both in Mach4 and in CNC12 is the toolpath simulator. It will show you X, Y, and Z in the toolpath display, and where the tip of the tool is on all of those. Whenever I have a tricky job that I’m doing (or something I’m trying for the first time), I load up the Gcode and jog around the toolpath and compare my real tool location to the simulated one.
This has saved me many bits, as well as some very expensive pieces of wood. I’ve been doing some unorthadox things this last week and this checking process has saved my bacon several times.
1 Like
If you are telling vcarve that you have round stock, how are you going to align the wide part of the model to the wide part of the stock?