Tool setting macro

[positiverake]

Any one have a macro to set tools on a fanuc om control its a takisawa mill, looking to touch off, set z length then go grab the next tool and repete.

[dcoupar]

Originally Posted by positiverake Any one have a macro to set tools on a fanuc om control its a takisawa mill, looking to touch off, set z length then go grab the next tool and repete.

This may get you started.

G65 P9050 S1. E5.

Will change to the first tool (S) pause for you to handwheel the tool to the touch-off then back to AUTO and cycle start. Repeats for tools 2-5 (E). No blank tools allowed.

[glovebox20]

Here is a sample code that I use for Fanuc OM's

%
:2021(TOOL SET MACRO)
(MACHINE NAME)

(#2000 + TOOL NUBMER= TOOL OFFSET)
(#5023= MACHINE POSTION, Z AXIS)

(#521= X MEASURE POSTION)
(#522= Y MEASURE POSTION)
(#523= Z GAUGE BLOCK THICKNESS)


N1
T1M6
(ADD CODE TO LET OPERTOR PUT TOOL IN SPINDLE?)
G0G40G53G90X#521Y#522 (MOVES MACHINE TO MEASURE POSTION)
M0(JOG MACHINE)
#2001=#5023-#523 (SETS ZERO HERE)
G0G28G91Z0
N2
T2M6
(ADD CODE TO LET OPERTOR PUT TOOL IN SPINDLE?)
G0G40G53G90X#521Y#522(MOVES MACHINE TO MEASURE POSTION)
M0(JOG MACHINE)
#2002=#5023-#523 (SETS ZERO HERE)
G0G28G91Z0
(Repeat Code for other tools)
M30
%

1. First, pick a spot to touch tools off. This spot sould NEVER change during the current setup(s) and alway reachable. Enter X postion (from machine postion) in macro #521, Y #522. What ever you want to use as your gauge block thickness (ex. old 1/2 End Mill shank), enter in macro #523.

2. Call up the tool you want to touch off (N#). (You may want to add a move after the M6 to let the opertor to put the tool in and out of the spindle.) When the machine is at "M0 (JOG MACHINE)", jog the machine near the touch off postion. Use your gauge block (ex. 1/2 End mill shank) and slowly rasie the tool up untill the gauge passes underneth. Go back to auto and make sure the cursur in the program is here "#20XX=#5023-#523 (SETS ZERO HERE)" and press cycle start. The program will write the Machine postion - the gauge block thickness into the tool offset# and home the Z-axis out.


3.When your finished touching your tools off, take a travel/test indictor and zero where you touch your tools off (without the gauge block, ex. 1/2 End Mill shank) and reset your Z Reltive Position to Zero. Go jog the machine to your new workoffset and find your Z Zero. The Z Reltive Position. is your Z workoffset value.


I find this easy to use. You can jump around to any tool or touch them off one after the other. If your using a standard tool list, you can add comments to let the opertor know what tool he/she is touching off (ex T3 1/2 END MILL). You may want the look in a Fanuc Opertor Manual about Macro programing for more info.



Tip:
O9001 Tool Change cycle.

You may want to add a O9001 Pgm. to make the M6 cycle easier.

Paramter #240 tells the machine what M code runs Program O9001. Enter 6 for M6.

%
:9001(TOOL CHANGE MAC #240)
#3003=1 ( SINGLE BLOCK OFF)
M9
G0 G28 G80 G91 Z0 M19
M1 (OPTION STOP)
M6
#3003=0(SINGLE BLOCK ON)
M99
%

Now when ever M6 is exctued, the machine will turn the coolant off, Home out the Z-aixs, Cancle Any Canned Cycle Command, and orantie the spindle. There is even a option stop to stop the machine if needed before the Tool Change. You may want to modify the code to fit your machine/needs.


Glovebox20

P.S. I also heard of an old trick using the "End Of Block" key. When you have the tool at your zero point, go to your offset page like you normaly would and press and hole "Z" key and then press the EOC key [;]. The control should enter the Z Retaive position the the Data input window. Now you can press "Input" to insert the value in the table. I never got it to work but my Brother swears by it. Maybe there is a parameter somewhere that I'm missing? I personaly like the "tool set macro" mothed better because it uses the Machine position, not the Reltive position

[positiverake]

Thanks I'll try it