Cutter comp on haas mill

[rellim_63]

We have a new vf-6 with probing. On the older haas without probing I can use cutter comp (wear when programed) with no trouble.

 

However I went to use cutter comp today on the machine with probing and I had no luck. For some reason when I programed the wear into my cut, (.750 mill) it looked to change my path by half diameter.

 

Any help would be appreciated.

[crazy^millman]

Need to see how the macro was set up for the math. The might be an option to change by diameter, radius or increment for the macro and need ot set the option according to match what you are doing.

 

HTH

 

BTW Welcome to the forum.

[gcode]

check your parameter settings

Haas controls have switches that define cutter comp behavior.

You should be able to set them to match your older machines

[Pilot Plant Supervisor]

The Haas probe will enter the actual diameter of the tool in the offsets. You need to set comp to "control" in Mastercam for this to work. "Wear" comp would need to see 0 in the offset for a nominal sized tool.

[rellim_63]

I will look in to the settings for wear offset, but I will try the control setting first. Thank you.

[JeremyV]

We have a VF-6 at the company and we use mastercam for everything, with the exception of cutting the jaws.

 

With that said, we use geometry as probing tools with the presetter puts the tool diameter into geometry. If you are using mastercam to program your stuff, you dont need any tool dia number in geometry unless you are wanting to increase or decrease the size of whatever you're making. But i don't use diameter probing at all. Even the carbide disc itself gets worn out in 6 months- a year; u'll have a dimple in the center from all the probing of drills.

 

there is a setting somewhere that can change it from diameter to radius... i think

[BrianP.]

It is a combination of how you are programming in Mastercam and the Haas machine. Haas has a setting number 40 with which you can select diameter or radius. If you want to continue to use wear in Mastercam just probe length only not length and diameter. This will keep your diameter comp number as a zero. You will then just need to enter any wear offset for regrinds or adjustments.

[rellim_63]

I just changed my program to run "control" worked great thanks

[mc since v3]

If you are still interested, I rewrote the renishaw macro O9852.nc

so your wear offset is the difference between the size entered in the tool table and actual measured size. I.E. .500 endmill measures .498, offset will have a value of -.002 instead of .498

[Claytonic]

I'm interested! But 5 years late.

[Thad]

On 2/10/2014 at 4:42 PM, oceancnc said:

If you are still interested, I rewrote the renishaw macro O9852.nc

so your wear offset is the difference between the size entered in the tool table and actual measured size. I.E. .500 endmill measures .498, offset will have a value of -.002 instead of .498

 

12 hours ago, Claytonic said:

I'm interested! But 5 years late.

I did the same as oceancnc, with the help of this forum. It was probably 8-10 years ago though and I'm not sure if I still have it. I'll look through my stuff.

[Thad]

11 minutes ago, Thad said:

I did the same as oceancnc, with the help of this forum. It was probably 8-10 years ago though and I'm not sure if I still have it. I'll look through my stuff.

Oops, sorry, I just remembered it was for a Mazak with a laser tool setter.

[Claytonic]

Thanks for looking. 

 

I'll dig into if it bothers us enough.