Help with wear comp

[Tkrohn45]

I am trying to figure out how to utilize wear comp between Mastercam and our machines. I will give my situation:

I have a part where I have to machine a boss of .75 +0/-.0005, .093 depth. I used a 3/16 5 flute flat endmill carbide with AlTiN finish, we have a probe in the machine to measure tool diameter and length. I enter the exact diameter from my machine into Mastercam. I left .01 from my rougher, and did 2 passes at .005, 1 at .0001 and 1 spring pass. Material is 1044, I ran rpm at 10K, and feed at 25 ipm. Machine is a Mazak 410B-II with Mazatrol Matrix Nexus controller. 

The part comes out at .751, the way we rerun stuff now is we change the "leave on walls" parameter in the toolpath on Mastercam and repost until the measurement comes out good. We may do that a couple times. 

I want to know how to post out once and use wear comp to be able to make quicker adjustments and skip posting out multiple times. I have been trying to research but am finding a hard time researching my specific situations. 

[AHarrison1]

In the tool offset page of the control there should be columns for dia wear offset and length wear offset.

When using wear control in Mastercam then there should be zero tool diameter set in control.

When adjusting for wear offset to remove more material a minus wear is entered into the wear offset for that tool.

So in your case you are measuring .751 then -.001(diametric) in entered into wear offset (This is on A HAAS control)

I don't know if the wear offset on your machine is set radially or diametrically.

[Tkrohn45]

1 minute ago, AHarrison1 said:

In the tool offset page of the control there should be columns for dia wear offset and length wear offset.

When using wear control in Mastercam then there should be zero tool diameter set in control.

When adjusting for wear offset to remove more material a minus wear is entered into the wear offset for that tool.

So in your case you are measuring .751 then -.001(diametric) in entered into wear offset (This is on A HAAS control)

I don't know if the wear offset on your machine is set radially or diametrically.

So in my control's tool offset page, I have like 2000 sets of offsets, but they aren't described as anything. Just has a column for No. and a column for Offset, I can only type in the Offset column 

Then in Mastercam, are you saying that the tool diameter would just be 0? or if its a 3/16 endmill set at .1875?

[RaiderX]

program in master cam to nominal .74975 with wear comp on.

run with zero comp in your table on machine

measure and insert the amount of comp to achieve feature nominal.

I say zero comp assuming you are using a carbide end mill that usually will run small, this tool will also need to be running true. this will allow you to run it as is and cut oversize and have room to comp to your feature size. (sneak it in).

[AHarrison1]

2 minutes ago, Tkrohn45 said:

Then in Mastercam, are you saying that the tool diameter would just be 0? or if its a 3/16 endmill set at .1875?

The latter, Mastercam will have the tool Diameter. Your posted code would then have work piece dimsion plus half the cutter diameter.

Does the offset column effect tool diameter or length?

[Tkrohn45]

27 minutes ago, RaiderX said:

program in master cam to nominal .74975 with wear comp on.

run with zero comp in your table on machine

measure and insert the amount of comp to achieve feature nominal.

I say zero comp assuming you are using a carbide end mill that usually will run small, this tool will also need to be running true. this will allow you to run it as is and cut oversize and have room to comp to your feature size. (sneak it in).

The issue I am having is figuring out how to use tool offsets with our post. If I turn wear comp on it'll put in G41 codes. After that I am not sure what to do to actually use a tool offset.

 

23 minutes ago, AHarrison1 said:

The latter, Mastercam will have the tool Diameter. Your posted code would then have work piece dimsion plus half the cutter diameter.

Does the offset column effect tool diameter or length?

I am not sure, I tried looking into it. I couldn't find any specific information. My guess might be that it is both, depending on if you use a D or H in the program?

[MWearne]

Have a look at this video...

https://blog.caminstructor.com/mastercam-cutter-compensation

 

[AHarrison1]

9 minutes ago, Tkrohn45 said:

I am not sure, I tried looking into it. I couldn't find any specific information. My guess might be that it is both, depending on if you use a D or H in the program?

Sounds like you are going to have to do some trial and error with A test block.

[Tkrohn45]

35 minutes ago, AHarrison1 said:

Sounds like you are going to have to do some trial and error with A test block.

I did just that, I understand it more now. I think I can comfortably work with tool offsets. not sure if it'll be easier or less of a headache for what we do at the shop but I at least understand it.

[AHarrison1]

Good to hear... the understanding bit at least..:)

[Matthew Hajicek - Singularity]

The way I do it is I program for the nominal sized tool (.1875 in your case), even if the tool measures a little small (which it usually does).  While proving out the first part, If it's for a tight tolerance feature, I'll put +.002" in the diameter wear offset, run the program, then measure the feature.  If it comes out .0025" over, for example, I subtract that amount (so wear offset shows -.0005") and rerun the tool.  Usually comes out dead nuts, or maybe a couple tenths under since deflection force was lighter.   Next part will usually be a couple tenths larger than the first prove-out part, since it has the full deflection force.  Using skim passes (0.0000" stepover) takes out most deflection and improves surface finish, and I find modern, good quality cutters don't mind taking as little a cut as you like; they'll make shavings on a skim cut.

[Charlie Pierson]

Ditto what Matthew said.