[rideredcr]

I recently purchased a desktop CNC mill. I am using bobcad v17 to write my programs. I am using Mach 3 to run my mill. I'm farely new to CNC and working to better my skills with programing. My issue is with G41 and G42. I can not get my mill to compensate for the cutter(which is a 0.25 endmil). Here is a partial of my program I wrote. Can someone tell me what I'm doing wrong.

N10O1001
N20G00G17G40G49G80G90
N30G70
N40T1
N50M06
N60G54X0Y0M08
N70G43Z2.H1
N80 T1 M6
N90 G42
N100 G00 X0.7425 Y0. Z-0.01
N110 G01 X0.7425 Y0.
N120 G02 X0.7425 Y0. I-0.7425 J0.
N130 G00 Z0.1

[Al_The_Man]

You did enter the tool dia in the tool offset page did you?
Al.

[cbr_speedster]

Add a D1 to the program to pick up the offset.

N100 G00 X0.7425 Y0. Z-0.01 D1

I generally use the same D offset number as my tool length offset.

[Al_The_Man]

I ran it through the simulator to test and also looking at the code, no XY move will take place with those coordinates?
Al.

[rideredcr]

The mill wants everything programmed in incremental mode. As far as the tool offset page goes, Ill have to figure out where to enter that info.......still learning BobCad and Mach. I thought I had it set, but maybe I'm not on the right page

[rideredcr]

So D1 is entered on line N100, not N90?

[ger21]

If you call T1 prior to the G42, then the diameter in the tool table for tool #1 will be used.
You can also do
G42 D1
or G42 P0.125
where P is the tool radius.

In order for comp to work in Mach3, you need a lead in move at least as long as the tool radius.
Try adding
N85 G00 X0.45 Y0. Z0.1
prior to the G42.

[cbr_speedster]

This is the code I have to interpolate a 1.735 dia. hole .010 deep starting from center of the hole.
Many machines require an X & Y move to activate cutter comp correctly. Don't put the tool diameter in the diameter offset. If the hole is programmed with the proper tool dia. then the diameter offset is only used to dial in the tolerance or adjust endmill diameter discrepancies. Say for instance it's programmed with a .250 endmill but the tool is really only .240. Then you would add -.005 to adjust the .010. If the tool is oversize like .260 dia. then you would put +.005 in the D1 offset. This is for a Fanuc control where on a HAAS you put the total differance, not half.

Here's the code for ramping in on a line:

N35 T01 M06 (.250 CARBIDE ENDMILL TOOL 1)
N40 M08
N45 G00 X0.0 Y0.0 S6112 M03
N50 G43 Z1.0 H01 D01
N55 Z0.1
N60 G01 Z-0.01 F10.0
N65 G41
N70 X0.7425
N75 G03 X0.7425 Y0.0 I-0.7425 J0.0
N80 G01 X0.0
N85 G00 Z0.1
N90 G40

Here's the code for ramping in on an arc:

N35 T01 M06 (.250 DIA. CARBIDE ENDMILL TOOL 1)
N40 M08
N45 G00 X0.0 Y0.0 S6112 M03
N50 G43 Z1.0 H01 D01
N55 Z0.1
N60 G01 Z-0.010 F10.0
N65 G41
N70 X0.1 Y-0.6425
N75 G03 X0.7425 Y0.0 I0.0 J0.6425
N80 G03 X0.7425 Y0.0 I-0.7425 J0.0
N85 G01 X0.0
N90 G00 Z0.1
N95 G40

[rideredcr]

Thx Guys