How to set offset correctly to mill threads with cutter comp on

[lakeside94]

I have posted a program from BobCad for my 2004 TM-1 to mill internal threads. I was advised to post the program with machine comp ON IF I wanted to make extra passes on the thread to open it up. I could then use the tool wear field to offset the cutter out and open the thread up.

My question is: in the HAAS tool offset screen, do I use a positive or negative number for wear and should I be using G41 or G42 in the post (with climb milling)?

Also, can I / should I post the code with BobCad system comp OFF if machine comp is ON?

Thanks,
Don

Similar Threads:

• Need Help!- cutter comp for mill
• Centroid Mill Cutter Comp Rule
• Getting the post to add 20 to the cutter comp offset
• Haas mill stops moving when using tool offset and cutter comp
• X2 Slot mill and cutter comp. don't work?

[djr76]

I program with comp on and just adjust the tool size.

[Machineit]

G41 will move the tool to the left side of the programed path and G42 will move the tool to the right side of the programed path.

I prefer to use negative numbers that to me tell me the tool is actually smaller than what it should be. But, you can do it either way.

This is a code I use all the time for some parts. This is a post makes internal threads about 2.635" in diameter for parts I make. This operation is done using a thread mill, so it has only one pass to complete all threads. If you are single pointing then you would have multiple passes going down. I used G42 and any adjustments to make the threads larger is done in the last column for the wear in geometry, by entering a negative number. Example, this thread mill makes the slightly too small, so I set it to -.002".

Note that you must invoke cutter compensation in a straight line move. Here it is called up in the eighth line, an X Y move. You need to cancel it in a straight line too, X, Y, or Z or the machine will throw an error message.


G00 G90 G80 G40 G54
T3 M06 (.285 THREAD MILL)
(SET WEAR TO -.002 TO START)
S7500 M03
G00 X0.675 Y0.
G43 H03 Z0.1 M08
G01 Z-0.3125 F20.
G42 D03 X0.675 Y0.5
G02 X1.175 Y0. I0. J-0.5 F10.
X1.175 Y0. Z-0.375 I-1.175 J0. F20.
X0.675 Y-0.5 I-0.5 J0.
G01 G40 X0.67 Y0.
G00 Z0.1 M09
G00 G91 G28 Z0. M05

So, bottom line, you can use either G41 or G42 and use a + or- sign as you see fit.

PS: You can always add the cutter comp after the code is posted by just adding it to a straight line move. I do it all of the time. Just put the G42 D03 in a straight line move. Oh, and I did not mention that you have to add the D01, 2, 3 ext to the line so the control know what tool to use for the compensation. The tool number used does not have to be the same number that the tool actually is. There are some programs I have that call up a different tool offset than is actually being used, because I need two different offsets for the same tool.