[helocat]

Posting my first programs from my CAM package. I have four canned Haas posts to chose from, two with with cutter comp. The one ending in MM I can see by testing a post is in millimeters. So I am using the other w/o MM. I wish to use cutter comp, however the post starts off with G40 then I never see G41 or G42 in the code. With a typical Haas post with cutter comp on what should I be seeing?

Can someone post a sample opening block of code with cutter comp on please? I think this would help.

The comp should change from left and right based on the direction the tool is traveling correct? (outside profile vrs. a pocket)

Or does the Haas control automatically use cutter comp. in the tool settings page when you enter the actual tool size?

Thank you,

Mark

[Matt@RFR]

Hey Mark. What CAM package are you using? Someone may allready have a post they would be willing to share, or you could go to the specific forum for your software on this site and ask questions.

Starting with G40 is good. It just makes damn sure that no cutter comp is being carried over from a prior operation, especially if you've been messing around in MDI. I have my post set to put G40 before every toolchange.

This is a typical format for me for the beginning of each tool:

(END OF LAST TOOL)
G0 Z.25 M9
G40 G80 G90
M6 T2
M3 S12000
G43 H2
G0 X4. Y-2. M8
Z.25
G1 Z-.75 F500.
G41 D2 X3.75 Y-1.875 F85.
X-.25
G40 X-.5 Y-2.
G0 Z.25 M9
G40 G80 G90
G53 Z0.
G53 X-10. Y0.
M30
%

The comp should change from left and right based on the direction the tool is traveling correct? (outside profile vrs. a pocket)

Not correct. G41 is cutter comp LEFT, G42 is, ofcourse, cutter comp RIGHT. Picture looking through the spindle, through the center of the tool, down onto the part. For direction, it's just like sitting in a car...allways facing the direction of travel. You see the edge you need to finish, and you want the cutter on the left of that edge, use G41. In other words, when we drive a car here in the US, we are in the left lane no matter which direction we are headed...that's G41. Japan drives their cars in G42.

Or does the Haas control automatically use cutter comp. in the tool settings page when you enter the actual tool size?

No, G41 or G42 need to be called every time you want cutter comp to be active. G43 must be called every time a new tool is used to set it's length offset from the numbers in the offsets page.

[helocat]

Matt@RFR Thank you for your help on this. I will look closer in the programs tool set up, cutter comp must be there as an option to turn on.

I am using Alibre CAM right now.

Thank you for sharing the code it is helpful.

Mark

[HelicopterJohn]

Hi Helocat,

First, I am a hobbyist machinist and not a Cutter Comp Expert.

Matt is correct on his advise to check out a specific forum for you CAD/CAM Software. The sample shown below is utilizing (Machine Comp) in the ONECNC Software. Their are other options and those may require modifications as it relates to the diameter in the offset page of the HAAS control. I would advise you to contact your CAD/CAM Software dealer directly for advise on how to accomplish this.


I have attached a sample of where cutter comp is established in the ONECNC CAD/CAM system and a sample associated post for that particular operation. It may help you find where it is done in your CAD/CAM software system. I used cutter comp to accurately size the slot in this part.

Hope this was of some help.


John