Tool in Spindle Macro Variable

[Grumpy Guy]

Fanuc 16 and 31i controls, what macro number desplays what tool number is in the spindle?

[Tony35]

#4120 i think. i dont have my book here. can anyone back me up on this

[Simtech]

Yup thats it ... 4120 = T code

[Grumpy Guy]

Thanks

[Tony35]

be careful if you stage a tool it will update to the staged tool number

[Grumpy Guy]

You know, I remember that there is a variable for the current tool number in the spindle, not the current tool. I know Mazak has this variable, but I can not find it in the Fanuc manual.

[exjay]

I've been looking for that fanuc variable for years (current tool number in spindle NOT the current staged tool which are not always the same) as we use a tool touch off macro I wrote that will not work if there is a staged tool. Anyone know it?

[Charlie Pierson]

You could write #4120 to another variable (say #149) and use #149 then the pre-stage won't mess things up

[exjay]

then I believe I need to have the line #149=#4120 in the tool change macro (our posted code stages a tool immediately after the tool change line M6T#)

which I already thought of. unfortunately I cannot access the tool change macro on this particular old machine. I believe its hard coded onto a flash card or some such thing. or am I missing something?

[Tony35]

you could create your own custom tool change program

set a program call with M or G code

just a thought

[Grumpy Guy]

I added the same line to my tool change macro, I used #500 instead of a 100 number. The value is retained at power off and reset, not always the case with the 100 number range.

The macro I wrote will retract, and also has other tidbits to measure and set tool lenghts, go to a specific area to measure on specific pallets, or just do a retrack routine. It works great for opperators who do not understand G code.

[Kyle Waters]

Can't you use #4111?

[Tony35]

#4111 is a h code variable

[Kyle Waters]

so this must be before calling the offset? I was thinking tool measurement after cutting.....

[Tony35]

no its a modal information variable

you could use it to check that the right h code was called or is currently active if you want to change it you need to pass it to a local or common variable

T2 example

#100=#4111 (#100 = 2)pass it to the common table

 

IF[#4111NE2]GOTO100 (check T2 H code number)

prog

N100#3000=101 (Wrong H offset)

 

if you want to check tool offset values depends on what offset memory you have for memory type c tool 1 (geometry offset) starts at #2201