G43

[captain_K]

Some help would be great!

I'm using Mach 3 with the 'Tool Table' setup with all my tool #'s and offset lengths. Everytime I make a Madcam post for Mach 3 I have to manually go back in and enter in: G43 H4 (or whatever the tool number is after H) before each tool change. This is so Mach 3 will apply the tool length offset for the corresponding tool that will be changed.

So my question: is there anyway to automate this in the Post from Madcam?
Or, is there another way to do this so I don't have to edit each post manually?

I know Master Cam has an option to add this into the post. For instance in the post in front of a tool change, lets say tool #7, it will put a G43 H7 automatically in for you.

[JOM]

Hello captain k,

It is possible to add G43 H"toolnr" in the post processor tool change section.
The variable “toolnr” is the tool number from your saved cutter.

Below is a post processor for mach3 with G43 for tool length compensation.

1.0_031210
*FILE_NAME*
Mach3_Gcode
*FILE_EXTENSION*
txt
*FILE_DEST*
c:\postfiles\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
3
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*RAPID*
G00"x""y""z"
*END_SECTION*
*RAPID_APPROACH*
"x""y""z"
*END_SECTION*
*RAPID_RETRACT*
G00"x""y""z"
*END_SECTION*
*APPROACH*
G01"x""y""z" F"feedz"
*END_SECTION*
*FIRST_CUT*
"x""y""z" F"feed"
*END_SECTION*
*CUT*
"x""y""z"
*END_SECTION*
*TOOL_CHANGE*
("toolname")
M6 T"toolnr"
M03 S"speed"
G43 H"toolnr"
*END_SECTION*
*TOOL_STOP*
M5 M9
*END_SECTION*
*PROGRAM_START*
G00 G49 G40.1 G17 G80 G50 G90 G64
*END_SECTION*
*PROGRAM_END*
M30
*END_SECTION*
*LINE_START_NUMBER*
1

Joakim

[captain_K]

Thank you Joakim -

I just inserted G43 H"toolnr" into my Mach 3 post processor and everything works perfect!

Thanks again!