Adding 20 to my cutter comp D number

[Doug Funny]

Greetings Gurus,

Why is my post adding 20 to my comp numbers? I looked through my control def and my post and I can't figure out why it's adding to the number. Attached is my Zip2go so you can tell me where my Bozo moment is.

TYA,

Doug

CUTTER-COMP.MCAM-CONTENT

[#Rekd™]

I didn't look at your file.

Is you Control def set like this?

 

[AHarrison1]

Check in your control Def

[Doug Funny]

17 minutes ago, #Rekd™ said:

I didn't look at your file.

Is you Control def set like this?

 

It was set to zero and it still adds 20, I also tried setting it to From Tool with the same result.

[#Rekd™]

Possibly you are looking at the Global Control def vs the local Control Def in the file?

[volitan71]

Line 775 of your MPFAN-3X-M5.pst file, someone changed:

fmt  "D" 4  tloffno$    #Diameter offset number

to read:

fmt  "D2" 4  tloffno$    #Diameter offset number

 

 

[Doug Funny]

31 minutes ago, volitan71 said:

Line 775 of your MPFAN-3X-M5.pst file, someone changed:

fmt  "D" 4  tloffno$    #Diameter offset number

to read:

fmt  "D2" 4  tloffno$    #Diameter offset number

 

Thank you!

 

 

 

[CookerJohn]

I am having the opposite problem of the original poster. I need to add 20 to the diameter of every tool. I have been manually changing the Dia. value in the toolpath.  Attached are photos of my control definition and a pic of the code my post processor is producing (I am using the MP Master post processor). 

I am programing for a Mori FM-1 3 axis mill, it lost its all of its parameters a while back.  After reloading everything thing, it requires +20 to all the dia. 

First time post, my apologies if I posted in the wrong spot, this was the most relevant thread I found. 

My MCAM is legit, Maintenace is current. 

[JoshC]

17 minutes ago, CookerJohn said:

I am having the opposite problem of the original poster. I need to add 20 to the diameter of every tool. I have been manually changing the Dia. value in the toolpath.  Attached are photos of my control definition and a pic of the code my post processor is producing (I am using the MP Master post processor). 

I am programing for a Mori FM-1 3 axis mill, it lost its all of its parameters a while back.  After reloading everything thing, it requires +20 to all the dia. 

First time post, my apologies if I posted in the wrong spot, this was the most relevant thread I found. 

My MCAM is legit, Maintenace is current. 

typically that change effects newly selected tools, so you may need to confirm that the toolpaths themselves have Dia offset 37 set, when creating future tools they should automatically add 20 to the d offset however your existing tools or tools that were already created may just need their tool settings offsets updated along with the toolpath offsets. 

[CookerJohn]

Thanks Josh!

That did the trick.