How to modify post for homing?

[mactec54]

Hi Lasershop

You should put G91G28Z0.X0.Y0. before the M30
I don't know why you would want to go to home at each tool change, as this would waste a lot of time

To go to home for each tool change you would have in your code T1M6 or T2M6 this will take the Z to the tool change position

If you want the X & Y to move as well then just put

T2M6 The T2 means tool number 2
G0X0.Y0. You can give the X & Y any number just to move them were ever you want them, Like X-3.Y-2.

You can do a G91G28X0.Y0. but that is not a good idea to do after a tool change

[Lasershop]

Originally Posted by mactec54 Hi Lasershop You should put G91G28Z0.X0.Y0. before the M30 I don't know why you would want to go to home at each tool change, as this would waste a lot of time To go to home for each tool change you would have in your code T1M6 or T2M6 this will take the Z to the tool change position If you want the X & Y to move as well then just put T2M6 The T2 means tool number 2 G0X0.Y0. You can give the X & Y any number just to move them were ever you want them, Like X-3.Y-2. You can do a G91G28X0.Y0. but that is not a good idea to do after a tool change

Spindle has to be up for the quick change to work. Have had many projects where the tool change may be a longer tool and would definitely crash if it were not homed. The Bridgeport only has a 5 inch quill. You have really helped alot. Thanks.

[JOM]

Hello Lasershop,

Here is a post processor for Fanuc 0M that use G28 before tool change and before program end.

//MadCAM_POST_2003-12-10
*VERSION*
1.0_031210
*FILE_NAME*
Fanuc 0M
*FILE_EXTENSION*
nc
*FILE_DEST*
c:\postfiles\
*FILTER*
0.01
*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*
F10000
G1"x""y""z"
*END_SECTION*
*RAPID_APPROACH*
"x""y""z"
*END_SECTION*
*RAPID_RETRACT*
F10000
G1"x""y""z"
*END_SECTION*
*APPROACH*
G1"x""y""z" F"feedz"
*END_SECTION*
*FIRST_CUT*
"x""y""z" F"feed"
*END_SECTION*
*CUT*
"x""y""z"
*END_SECTION*
*TOOL_CHANGE*
G00 G91 G28 Z0
T"toolnr" M06
T"toolnr" M06
S"speed" F"feed" M03
F10000
G90 G1"zhome" G43 H"toolnr"
*END_SECTION*
*TOOL_STOP*
M5
*END_SECTION*
*PROGRAM_START*
%
O"pgmnr"
G40 G54 G80 G90
*END_SECTION*
*PROGRAM_END*
G00 G91 G28 Z0
M30
*END_SECTION*
*LINE_START_NUMBER*
1

I hope this will help,
Joakim

[Lasershop]

Originally Posted by JOM Hello Lasershop, Here is a post processor for Fanuc 0M that use G28 before tool change and before program end. I hope this will help, Joakim

You guys are great! Thats what Im talkin' about. Ill get this coding figured out but I sort of need to reverse engineer an example to understand it.
Thanks, RonO

[Lasershop]

Just had to read the help file a little more..

*PROGRAM_END*
G00 "zhome"
G00 "xhome""yhome"


Now whatever coords you enter in the post processor "home position" ends up in your cut file. Whithout adding this it has no effect.
RonO