[behindpropeller]

For everything that I have made with our TM-2 so far, I have used in computer cutter comp.

I'm curious how cutter compensation relates to tools measured with the toolsetter.

Lets say I measure a .250" endmill and it comes out at .240". I understand that the computer driven cutter comp gives me .005 of stock uncut.

So now when I program with cutter comp and the tool is measured .240 does the haas just fix that?

I'm still learning, so these questions may be trivial.

Thanks

Tim

[CNCRim]

Program 1/4" standard like brand new endmill, and if the endmill is smaller from resharp then that can be done by cutter comp in the control.

[beege]

Comp is not going to fix your inside radii if they're not programmed, though. If you need a .125 radius and you've programmed your part to let the endmill create the radius by its size, (two intersecting lines) it won't put an arc in. You have to program an arc at the intersection so that the end mill will create the proper size radius. Just something to consider.

[tobyaxis]

For everything that I have made with our TM-2 so far, I have used in computer cutter comp.

I'm curious how cutter compensation relates to tools measured with the toolsetter.

Lets say I measure a .250" endmill and it comes out at .240". I understand that the computer driven cutter comp gives me .005 of stock uncut.

So now when I program with cutter comp and the tool is measured .240 does the haas just fix that?

I'm still learning, so these questions may be trivial.

Thanks

Tim

Depending on what your making it is known that standard endmills are .001 to .002 undersized in diameter unless you buy NC Qualified.

IMPO I use a finish endmill to Interpolate an arc rather than using a to size endmill. Doing this you can adjust the Comp for tool wear and always be sure your radii are correct.

Are you making things as a hobby or for customers??

[Ydna]

That definitely works best if you can menage it (without a long-extended small dia endmill). The cool thing is the Haas control will automatically adjust the feedrate for arc moves while CDC is on, to help ensure the cutter sees the same surface speed when making the arc move.

Also note (for the OP) the number you use in the CDC diameter register depends on how the part is programmed. If you program the tool's center locations (as you would without CDC) you can still use CDC with a slight modification to the program, however you'll still use a 0.0 in the CDC register.
Alternately if you program the final product's actual part locations rather than the tool center locations, then and only then will you actually put the cutter diameter in the CDC register.

It works the same both ways unless you have CDC interference problems with your locations.

[crabbass]

Something to consider. When I draw my parts in cad (for example a pocket with .125" radii in the corners.) If I intend to use a 1/4" endmill for finishing, (and if tolerances will permit) I will draw the corner radii larger (the bigger the better) usually just round up about .005". Then when setting up, I start the comp big (.255") and I won't get an error. I used this strategy alot when programming lathes. The .005" radius interpolation on a square shoulder when turning is dramatically smoother. It will help to reduce chatter in the corners by maintaining a smaller approach angle when entering the corner (Milling and turning).