[dlenardu]

I have been trying to get the chamfering setup to work but have been unsuccessful. I have a .5" diameter endmill with a 45 degree chamfer on it. I have been trying to put a .030" chamfer around a hole but I can't seem to get it to work. If I try to change the depth then it seems to go and make the hole wider. It seems to look like it is doing everything correctly on the simulation but when it does the machining it doesn't come out correctly at all.

[sqatch]

Is your bit a 45 or a 90?

[andre-dolphin]

In the tool definition, the angle is the included angle, so for a normal chamfer tool this would be 90 degrees, 45 per side.

ATB
Andre

[sqatch]

He had defined 45 which give you a 22.5 cut.

[dlenardu]

It is a 90 degree tool which is 45 degree per side. I tried doing it both ways using 90 degree and then I changed it to 45 degree and still couldn't get it to work properly

[sqatch]

Try increasing the lead to 0.250" .

[dlenardu]

When I change the lead to .25" I get an error saying the chamfer tool dimensions are inconsistent

[andre-dolphin]

I produced a drawing based on the Gcode output.

The key sizes are the X1.078 start point of the radius and the Z depth of 0.078

You will see that this produces a chamfer size of 0.030"


ATB
Andre

[dlenardu]

So is this something that I am going to have to do every time I want to chamfer something? I was using this circle as something simple to try out first, especially since I have found myself wanting to put a bevel on milled out pockets before. I have a part that has an irregular shape and would also like to be able to put a chamfer all the way around it. I guess I was just hoping that since it had a chamfer setting that I would be able to use it and let the cam do the work

[andre-dolphin]

That's exaclty what you can do - just give it the depth of the chamfer and let the cam systems calculate the tool offsets in XY and Z.

The reason for posting the drawing was to show that the cam system was producing the correct numbers.

The XY and Z dimensions were created by the post-processor, I then drew the tool from these numbers to show that the numbers generated were correct, and would produce a chamfer of 0.030".

ATB
Andre

[dlenardu]

Ok, well the problem must be my tool then because I cannot get it to work. This is the tool I'm using

Enco - Guaranteed Lowest Prices on Machinery, Tools and Shop Supplies

[sqatch]

If you increase the lead to 0.249" you dont get the error message. See if this works for you, it seems to run ok in my cam.

[dlenardu]

If you increase the lead to 0.249" you dont get the error message. See if this works for you, it seems to run ok in my cam.

That worked perfectly. Thanks, I don't know why I didn't think of going .001" smaller to test with

[sqatch]

I dont know why it does that, maybe it does'nt like an infinite point. No problem helping you out because you problem may be my problem some day.

[andre-dolphin]

We found a slight rounding error in the code that calculated this. It's been fixed.

ATB
Andre