can/ how do you do cutter comp in CNC12? [yes - instructions in post SOLVED]

[rk9268vc]

can/ how do you do cutter comp in CNC12?
I have been poking around the menus and im not seeing a spot to do it, only height offsets

I think I want to use G41 and G42 somehow, but idk how. Im using Fusion for CAM

Can someone point me to a tutorial on how to do it if its possible?

Thanks!

[tblough]

Chapter 10 in the users manual covers cutter compensation in Intercon. Chapter 12 describes the use of G41/42.

[rk9268vc]

Chapter 10 in the users manual covers cutter compensation in Intercon. Chapter 12 describes the use of G41/42.

Thanks,

Do you have any experience using G41/42 with Fusion?
How good is CNC12 at figuring out which side of the line it should be cutting on?
I see that it can do look ahead, but what if I am dialing in a slot that is only 3 thou wider than my endmill, will it just skip over it?

Thanks

[tblough]

Sorry, I use Intercon for simple items and. SolidCAM for complex parts. In Intercon you need to tell it which direction you are cutting. In SolidCAM, cutting side is determined automatically.

CNC12 just reads g-code and uses what is programed.

[rk9268vc]

Sorry, I use Intercon for simple items and. SolidCAM for complex parts. In Intercon you need to tell it which direction you are cutting. In SolidCAM, cutting side is determined automatically.

CNC12 just reads g-code and uses what is programed.

yeah im not using intercon

So can you not use cutter comp if running gcode from another cam program?

I know like with a tormach mill, in fusion you tell it to handle cutter comp in the controller, then in pathpilot (CNC12 for tormach) it handles cutter comp.

[tblough]

If the g-code has cutter comp commands they will work. Most CAM systems have a checkbox along the lines of "use cutter comp" in the machining strategy dialog. Checking that includes the appropiate cutter comp commands in g-code.

You need to decide if you are using diameter or wear compensation and enter the appropriate values in the Centroid tool table diameter values.

[rk9268vc]

If the g-code has cutter comp commands they will work. Most CAM systems have a checkbox along the lines of "use cutter comp" in the machining strategy dialog. Checking that includes the appropiate cutter comp commands in g-code.

You need to decide if you are using diameter or wear compensation and enter the appropriate values in the Centroid tool table diameter values.

so if i want to use wear compensation, do i enter -.001 into the tool diameter table (for example)?

[rk9268vc]

ok i figured it out

In fusion select cutter comp type "wear"

Then in CNC12 under Setup->Tool->Offset Lib.
Enter the CHANGE from nominal in DIAMETER into D#

positive value makes it think the cutter is bigger than nominal, negative makes it smaller.

EXAMPLE:
Cutting a 1in x 1in square with a .500 endmill
using cutter comp type wear

Enter 0.01 into tool diam results in a 1.010 wide square (cuts .01/2=.005 oversize x2 edges)
Enter 0 in D# results in a 1.000 wide square
Enter -.01 results in a .990 wide square (.005 in x2 edges)

if you use a 1/2 in endmill that measures .510 in diameter, enter .01 into D# in table to get a properly sized part
if you use a 1/2 in endmill that measures .490 in diameter, enter -.01 into D# in table to get a properly sized part

In Fusion

In CNC12