[barca03]

Hello all,

Does anyone know how to make the tool life count by the number of holes a tool drills instead of the number of times the machine brings the tool in?

We currently run Faunuc 16i and MSG-501 controls!

What we're trying to accomplish is to control a tool's life by the number of holes it drills rather than the number of times the tool is loaded into the spindle. Because of our product, some parts may require only 2 holes with let's say T1, and other parts will require 10 holes with T1.

[underthetire]

MSG 5xx is a fanuc I series as well. Mori typically uses tool load as a function of tool life, not number of times it's in the spindle. I would think a good macro writer could do something quite easy.

[chucker]

This is what I use change the 4 to the number of holes that the drill drills per part then put the max number of holes you want to drill in register #520 when the count in #504 reaches max number in #520 it will put the machine in feed hold and put a massage on the massage screen to change the drill I use this on my Fanuc and Mori the only differance may be the register number if you have to change them its best to stay in the 500 or above range so they cant be cleared by rest or powering down the machine

(other tools up here0
M1
(drill holes here)
#504=#504+4 (Change the 4 at the end to the number of holes per part)
IF[#504GE#520]GOTO3000 (put the max number of holes you want to drill in register #520)
IF[#504LT#520]GOTO4000
N3000
#504=0
#3006=1(CHANGE DRILL)
N4000
M1
(run outher tools here)

[barca03]

Thanks for the replies,

I like that idea "Chucker," I need to work on that a little. A single program runs anywhere from 3-10 different tools for one part. Plus, I'm not an expert at writing macros, and I need to sell the idea to my peers (this is actually the toughest part of all) before we can make it work.

Originally I thought we could accomplish this with the H codes, but I just found out what "underthetire" said, it only counts the tool load.

[samu]

What Chucker suggested is simple and should work, but it involve hand coding each program with that code. Using macro call with G code and modal macro call(G66), you can write a macro(one per drill cycle) that automatically count without having to modify any program.

Suppose that each drill cycle call a custom macro by its own G code.

G81 call O9010 (set prm 6050 to 81)
G82 call O9011 (set prm 6051 to 82)
G83 call O9012 (set prm 6052 to 83)
G84 call O9013 (set prm 6053 to 84)
G73 call O9012 (set prm 6054 to 73)
G80 call O9014 (set prm 6055 to 80)

Let's say that the amount of hole a tool can drill is stored in #500+tool number and the quantity of hole that a tool has drilled is stored in #550+tool number.

Each macro is essentially the same. Only the drilling G code is different.

O9010 (G81 macro call)
G81 X#24 Y#25 Z#26 R#18 F#9 K#6 (DRILL THE FIRST HOLE)
G66 P9200 (CALL THE MACRO THAT MANAGE THE COUNT )
M99

09200
IF [#[500+#4111] LE #[550+#4111] GOTO 100 (JUMP IF MAXIMUM HOLE HAS BEEN REACHED)
#[550+#4111]=#[550+#4111]+1
M99
N100 #3006=1 (CHANGE TOOL)
#[550+#4111]=0 (RESET HOLE COUNTER FOR CURRENT TOOL)
M99

O9014 (G80 MACRO CALL)
G67 (CANCEL MODAL MACRO CALL)
G80
M99


But there is a problem with cycle that contain a P word (like g82) because you cant pass an argument with P. You can use another letter instead but it involve to modify all existing program and it become a non-standard code. You can also add the modal call (G66 p9200) directly in the program just after the G82 block without G code macro call.(once again it involve hand coding)