Fanuc 16i tool length default value

[left coast lefty]

Since we are now using a Speroni tool presetter, obviously the values are a positive number. Is there a way to get the offset table to default to 99? A couple of crashes due to a zero value have already occurred.

[GoetzInd]

Put some logic in the the tool change macro to check if offset is below a certain amount or 0. If so, alarm or M00. Pretty easy and safe.

 

Mike

[left coast lefty]

Thanks Mike. I have never messed with the tool change macro, but it sounds like a god idea.

[generaldisarray]

We are also having a problem since switching to positive tool offsets.

G49 causes Z to move in the negative direction to cancel the offset.

Not if the offset was canceled first with G91 G28 Z0.

On a Fanuc 18i

[crazy^millman]

Okay so change the output at your tool changes to either do that then call G49. I have used positive tool offset for years and IMHO is the only way to go, but it does require you to think about what is going on through out the whole process. By having the post output the code they way you are looking for then you should be good to go.

[generaldisarray]

So i guess we will have to modify our posts to remove g49 before tool changes?

 

Is there not a parameter?

 

All our existing programs have g49 called in the beginning like g40 g20 g90

[within a thou]

Why not just remove the G49 all together. It's not needed if your first move in Z on the next tool is your G43 line. I agree positive offsets are the way to go since you can do a quick tape measure check to make sure the tool was touched off and isn't a value from a previous tool.

[Allan]

Fanuc Parameter #5009 bit zero.

 

If set to 1 will create motion when cancelling the height comp

If set to zero will cancel the height comp, without motion.

[generaldisarray]

Why not just remove the G49 all together. It's not needed if your first move in Z on the next tool is your G43 line. I agree positive offsets are the way to go since you can do a quick tape measure check to make sure the tool was touched off and isn't a value from a previous tool.

Exactly

it is just the existing program mod for us, We have lots of existing proven programs

[generaldisarray]

Fanuc Parameter #5009 bit zero.

 

If set to 1 will create motion when cancelling the height comp

If set to zero will cancel the height comp, without motion.

fanuc 18i parameter manual b-63530en/03

" 5009 bit 0 = GSG---in the mode of tool compensation direct input B, the offset write input signal is input 0-from machine side 1-from pmc side"

[Allan]

I thought we were talking Fanuc 16i like the thread title.

 

Hang on I'll look in the Fanuc 18I manual

[Allan]

I thought we were talking Fanuc 16i like the thread title.

 

Hang on I'll look in the Fanuc 18I manual

 

 

 

Manual the same....wording in your is different.

[generaldisarray]

I thought we were talking Fanuc 16i like the thread title.

 

Hang on I'll look in the Fanuc 18I manual

 

 

 

Manual the same....wording in your is different.

same wording

but it is 5008 bit 6 (so is yours:)

excellent

i knew i could get the answer here

but it does not say next block with motion?

[generaldisarray]

5003 bit 6 LVK was 1 tool length offset value not cleared but held by reset. I changed it to 0-cleared by reset.

There should be no easy way to call a tool offset in program and then a g49 w/o a reset in between.

[within a thou]

Exactly

it is just the existing program mod for us, We have lots of existing proven programs

 

Then why not make it a company policy that before any program is ran G49 is searched and removed. After it is gone add a note to your program header that says proven program by adding a character to that and then you know it is gone.

[BBprecise]

You could also just set up a Macro call using an G code. Put G49 in parameter 6050 (or any available parameter between 6050 and 6059). Create a program with correct O word (O9010-O9019 respectively) like this,

%

O9010(G49 BYPASS)

M99

%

The Macro call has priority over standard code so the macro prg gets executed 1st. You can see what it does, nothing. We have 3 VTL's, 2 ram style and 1 turret style. The ram style use an M6 to tool change (like a mill) but the turret operates like a standard lathe and calls a tool with T06. To interchange between machines with the same prg I did the same thing for the M6. Works like a charm.

 

We don't use a G49 on any of our Fanuc based mills.