[tontze]

Is there anyway to make HAAS automatically check if tool is broken or not after run ?) I got renishaw probes with probing macros, machine is HAAS vfl-6ss.

In the tool offset table you can specify howto probe the tool, and field where you can specify amount that tool lenght/diameter can differ while probing .. But how you call these from program(or is it even possible) ?

Or, if anyone has sub-prog or such for this, it would be nice to have them

Thanks in advance, Tomi

[pit202]

create your checking program from VQC , save as a normal program in memory eg. O00005 , replace M30 with M99
in your mill program after that tool is used

(...)

M09
M05
M98 P5

(...) next tool ect.

Peter

[haastec]

Automatic Tool Breakage Check (Macro option installed)
Look at parameters 81 -90 for M macro call (program #)
Assign any unused M-code to an open parameter and note the program number associated with it.
Example: Par 81 M macro call O9000 M45
Next create a new program using the number associated with the parameter
O9000;
#100 = #3026; (#3026 = register for current tool in spindle. Assign to #100 which is a visible register)
G53G49Z0M09; (Z-AXIS Safety Retract)
G00G90;
G65P9023A24.T#100H.02; (Renishaw tool breakage routine, H = tolerance of tool +/- compared to set value before alarming)
G103; (Resets block look ahead to default value)
M62; (Turns off touch probe)
M99;
This program will check whatever tool is in the spindle using a simple M45(or whatever) code placed anywhere in your program. Adjust H value to your liking.

Happy Probing!!

[gpcoe]

At the end of the tool cycle enter:

G91 G28 Z0;
G90 G49;
G65 P9853 B1. T#3026 H.02;
M1;

H being your tolerance on the length. #3026 is the variable for what tool is currently in the spindle. You can substitute it with the numeric value if you wish.

Greg

[haastec]

I had register #3026 copied to #100 so that I can double check what is going on with the machine as #3026 is a hidden macro register. Yes, you can substitute #3026 or #100 for a numeric value but it defeats the purpose of the program as you would have to repeat all of the code each time you wanted to use it.

My program is inteded to be used like a subprogram which is called up using only the M code the programmer chooses. Use this M code after any tool that you want to check and nothing else. Makes for cleaner programs, less chance of programming errors, and no editing if you tend to change T #'s from run to run. Note that this does center line of tool only.

But just like everything else, there is no 1 correct way to get the job done. Modify as you please.

[tontze]

Awesome, thank you very very much

[haastec]

Thought I would share.

I came across a procedure to incorporate tool diameter check and spindle reverse for the tool breakage procedure for those who may be interested.

Note: I have not verified this code yet myself so proceed with caution.

You program a normal tool breakage detect cycle. Then replace the P# with P9853, the A# with B1. and add an S and H for tool Dia and breakage tolerance. The finished code should look like this for a .5 endmill (tool #5 with a .005 breakage tol.). EX: P9853 B1. T5 S.5 H.005

Cheers!

[renrepjnr]

WITH THE NEWER OPTICAL TOOL SETTER, OTS YOU WILL HAVE TO USE THE TURN ON/OFF MACROS OR M-CODES.

G65P9853B1.T1(TOOL OFFSET TO COMPARE TO)S.75(DIAMETER OF TOOL IF YOU WANT TO OFFSET RADIUS AND SPIN IN REVERSE)H.01(TOLERANCE)

This code will measure a tool and alarm out if it finds the length more than the tolerance out. You can also program a M variable on the same line of a spare tool offset that will store a broken tool flag instead of an alarm... ie M200 will set tool offset 200 to a 0 if tool is ok and 1 if tool is broken and you can run some logic on the flag to make decisions.

G65P9853B1.T1S.75H.01M200
IF[#2200EQ1]GOTO100 (BROKEN TOOL GOTO N100)
GOTO200 (GOOD TOOL GOTO 200)
N100
(CHANGE TO REDUNDANT TOOL AND RECUT)
N200
(CONTINUE WITH PROGRAM)