Calculating "zero" with Radius tool...

[CyborgCNC]

Hi all,

I just wanted to double check on something, before I do something stupid, and crash...

So, using end mills (Mastercam X2), (flat, bull etc) I know that the "zero" Z-Axis point usually is the top of the part (if I am off course cutting in the Negative z-direction).

Using Mach3, I have a touch probe, and I can very accurately do that, never had an issue. Depth cuts are spot on.

My question is now I want to use some "profiling" bits (like for example, a .25 Radius bit) to create a radius around a part, AFTER I cut it say with an end mill.

Since I need to change the mill, what is the "zero" point for a profile bit? How does one calculate this, to make sure that the machine cuts at the proper depth, and not ruin the part?

Do I lower the radius bit to the point where I want it to start cutting, and tell the machine that is the Zero point?

I am sure I am missing something simple, but wanted to check with the experts here, before doing something stupid....

Thanks all in advance for any insight!

[Superman]

Originally Posted by CyborgCNC So, using end mills (Mastercam X2), (flat, bull etc) I know that the "zero" Z-Axis point usually is the top of the part (if I am off course cutting in the Negative z-direction). My question is now I want to use some "profiling" bits (like for example, a .25 Radius bit) to create a radius around a part, AFTER I cut it say with an end mill. Since I need to change the mill, what is the "zero" point for a profile bit? How does one calculate this, to make sure that the machine cuts at the proper depth, and not ruin the part?

**On Machine**
for corner rounding cutter, Z-zero is the centre of the radius. This is theoritically the end of the tool. Many would gauge the end of the tool and then make the value smaller when proving off the program while cutting the part
**In Mastercam**
the base diameter is the calculated tool diameter and is important, The depth to cut the contour is incrementally deeper by the radius form

ie base diameter is 0.24" with 1/8" corner rounding tool radius
profile level is at Z-0.5" ( this is the upper face the rads are on and the level your profile is drawn at)

retract = 0.1
top of stock = -0.5
depth = -0.5" absolute (or 0.0 increm)
wear comp ON
XY offset = 0
Z allowance = -0.125" ( the form tool radius )

lead in/out
line 0.1
arc 0.1 sweep 90°
and copy left to right

Program should output a Z depth of Z-0.625 and give a profile pass identical to a 0.24" diam tool