Renishaw OTS tool probe cycle for HAAS can set both length and diameter offsets.

Too bad there is no choice: it only puts absolute measured diameter of the tool into D- diameter offset and makes wear offset=0

But if your programming is done with the center of the cutter, then you actually only need the difference between actual and programmed diameters of the tool.

I.E.: When probing 5/8Dia end mill, we get D=0.6248. You would normally have to subtract 5/8 from it and leave the -0.0002 difference.

But there is an easier way

Warning:Make sure you know what you are doing.
Make sure you backup all files you are going to modify.
I simply WILL NOT care about any damage done to your machine in any case.

• Go to settings and set  protect 9xxx programs from edit to OFF
• Go MEM and edit program O09852 (RENISHAW DIA. SET)
• Go to line N31 and replace
• Code:OLD
  .....
  N31
  #[ 2400 + #7 ]=  #8 / #156
  .....
  
  with
  
  Code:NEW
  .....
  N31
  #[ 2400 + #7 ]= [ #8 - #19 ] / #156
  .....
• Go to settings and set  protect 9xxx programs from edit to ON

Thats it.

Now when you probe tool for diameter, D offset will contain the difference between approximate Dia and actual dia of the tool.

Tags:HAAS Renishaw Diameter offset 9xxx