[SpookyDad]

Is it possible to put a chamfer on an opening without changing to a dedicated chamfer bit? Can a hole be countersunk?

I noticed on the menu that there is a "new chamfer" item but it seems
to be grayed out all the time.

Neil

[ger21]

With a straight bit? Yes, but the results won't be too good. You just make multiple cuts, stepping down and over with each pass. A ballnose bit would be better, but if you're changing bits, you might as well use the correct bit.

[LongRat]

I don't see that option on the menu (Sheetcam 3.1.23)?
Even with a dedicated tool, I have been programming it as a standard slot drill and offsetting it by manual calculation. Is there a 'proper' way of doing this?

[locost_cam]

There isn't an option to chamfer without using a V bit. If you use a square or ball nosed cutter the chamfer won't come out all that good, even if you do step down. If you are doing this because you don't have a V bit, try a countersink. As long as you don't use a high feedrate it works surprisingly well.

Les

[LongRat]

I do have a 90 degree V-tool, but I can't work out how to use it to chamfer a boundary 'properly' without tricking the software into thinking it is a square ended tool offset vertically slightly. If I do tell it the tool is a V-cutter, and I cut the profile with a zero finishing offset and a defined depth value, surely that would cut no material off the workpiece? Maybe do this with a negative fin offset?

[locost_cam]

SheetCam doesn't currently compensate for the cutter V angle. There has been some discussion of this on the Yahoo list. If the outside profile has all external corners (e.g the outside of a square) then simply do an outside offset and set the cut depth to whatever you want your chamfer to be.

If your shape has inside corners (e.g the inside of a square hole) then you have to cheat a bit. As a round cutter can never cut a square inside corner, the finished shape of the part will not be exactly as per the drawing. If you do a simple chamfer as above you will find that the inside corners don't chamfer correctly. To get around this problem, define a 90 degree tool but set the tip diameter to be equal to the diameter of the cutter you used to cut the shape. Now make the cut depth deeper by half the difference between the true tip diameter and the value you entered (this formula only works for a 90 degree cutter). By making the cutter diameters the same, the chamfering cutter will follow the exact same path as the cutter used to cut the part so the chamfer will come out even.

[LongRat]

Understood. That is basically what I have been doing, I'll continue with it in that case.