[ggundrum]

I am running a Bridgeport XV1000 with a Fanuc Oi-MC controller and a 24 tool vertical carousel.

I have ~50 different tools that I use on a consistent basis, and each tool is assigned a corresponding tool number (1 through 50). On my Haas I am able to tell the machine that I am taking tool 1 out and putting in tool 40, but I can not figure out how to do this on my Bridgeport.

There are 200+ tool offset entries available in the controller, and I have to believe they wouldn't have made these available if you can only put tools 1-24 in the carousel. I am aware of the method of using T1 H40 D40, but I would much prefer not to do it this way. It would not be uncommon for me to have to use tool 1 and tool 40 in the same operation, and I don't want to have to reassign tool numbers for each part I grind.

Also, in the operator's manual for the Fanuc controller, there are example codes that show the use of T100 and higher, but no where does it say how to put tool 100 in the machine, so that a T100 M06 line in MDI brings that tool into the spindle.

It doesn't make sense!?!? Thanks in advance for your help.

[samu]

I have an idea with macro programing. Does it have a tool change macro? Suppose that you reserve a set of 24 consecutive variable in the range of the 500's (they remain after power off). In those variables, you write your tool number 1 to 50. The first variable represent T1 for the machine the second T2 the third T3.....

When a tool change is called, you execute a simple macro that look in the 24 variable you have reserved for the tool number called. Once the variable number is found, you subtract to it the (first assigned variable number -1) and you get an equivalent number (1 to 24) that can be read by your machine.

You can also create a custom M or G code that load automatically the value in the assigned variable.

I don't know if you are familiar with macro programming, but if you want more detail or explanation, let me know

[ggundrum]

I have very limited experience with programming Macros, atleast on Fanuc contollers. I think I get what you are saying though, the program would read "T25 M06", but the macro would automatically convert that to "T1 M06" and keep the H25 and D25, is this correct?

The only issue I see with that is, what if I need to run T1 and T25 in the same program?

Thanks for your help, I wouldn't be opposed to using Macros to accomplish this, but definitely not experienced enough to write myself.

[samu]

it's not a problem if you want to use T1 and T25 in the same program. Cause if you do so, you won't put T25 in the pot of T1, suppose you have reserved the variable #501 to #524, and you put T25 in the pot of T3, you write(by hand or via a custom code) 25 in #503.

It will be a pleasure to write a macro for you, but I don't know when i can find the time to do it.

If your machine use a tool change macro, we have to integrate my idea inside the tool change macro.

Do you already have some variable reserved for whatever?
If you don't use tool change macro,more exactly, if M6 does'nt call a custom macro, it will be very simple

something like that should work

%
O9020 
#1=501    				(THE FIRST VARIABLE NUBER YOU RESERVE)
WHILE [#1 LE 524] DO1  		(LOOP UNTIL IT FIND OR LOOK ALL THE RESERVED VARIABLE)	
IF [#[#1] EQ #20] GOTO 10		(IF IT FIND IT)
#1=#1+1				(LOOK THE NEXT VARIABLE)
END 1
#3000=1 (TOOL NOT FOUND)		(DISPLAY AN OPERATOR MESSAGE ''TOOL NOT FOUND'')
M99
N10 #1=#1-500				(CONVERT TO READABLE T NUMBER)
M6 T#1
M99
%

It assume that you reserved #501 to #524
and you have to set a parameter to call this program by m6

[samu]

Do you try it, i'm curious and like to play with macro, i'm really interested helping you. keep me informed

[norbert.barnard]

Hi,
your statement explain your understanding (or miss-understanding) of tool lenght compensation activation.
"The only issue I see with that is, what if I need to run T1 and T25 in the same program?"

1. on Fanuc cnc for a milling machine the T-code is only used for managing the collection of the requested tool no. from the caroucel, i.e. indexing of the caroucel.

2. tool lenght compensation is only actived with the "H" code, i.e. "G43 Z_ H_"

3. therefore, the max. number for a T-code is alway's equavilent to the max. no. of pots in the magazine and the requierd compensation(geometry and wear) to be used is alway's called with the "H" code.

T1M6
G43Z100.H1
.
T2M6
G43Z100.H48
.
.

have fun.
norbert

[samu]

I am aware of the method of using T1 H40 D40, but I would much prefer not to do it this way.

He seems to understand like it should, just trying to use another method that is not Fanuc standard .


your statement explain your understanding (or miss-understanding) of the problem we try to solve.