Force "H" and "D" to equal "T", at the machine (Fanuc 31i)

[Niezingerly]

I am searching for a topic, and can't find it.

 

I remember someone mentioning it, somewhere, but...

 

So, here I go...

 

I want the control (Fanuc 31i A5) to force the H value and the D value to be the same as the T Number, no matter what is in the program.

 

Just the other day, someone fat fingered the value for the H value, at the machine, and well, part, meet spindle.

 

It's weird what "H " does to things...(that's H with a "nothing" value after it.) ("Hmmm" says the control, "my tool has no length...OK, here I go...")

 

 

 

I believe there is a setting or parameter to force the control to do this, but I can't find the topic that had the info.

 

Any help appreciated...

 

Thanks.

[Glenn Bouman]

It is in the control def.

 

 

Or just add these to lines to your post processor.

 

tloffno$ = t$ #Diameter Offset No

tlngno$ = t$ #Length Offset No

[JayM]

It is in the control def.

 

 

Or just add these to lines to your post processor.

 

tloffno$ = t$ #Diameter Offset No

tlngno$ = t$ #Length Offset No

 

+1 to Control Def. Definitely the preferred and more flexible method.

[Guest]

THE best method would be to go into your machine's tool change MACRO and the line immediately after the M6 add the following;

 

#506=#4120

 

Then in your part programs, you just use H#506 and D#506 (or pick your favorite 500+ MACRO Variable just make sur eir's the same as the =#4120 section) and you'll be GTG

 

JM2CFWIW.

 

Do it this way and you'll NEVER have the wrong offset active unless you do it on purpose.

 

[scooke4073]

THE best method would be to go into your machine's tool change MACRO and the line immediately after the M6 add the following;

 

#506=#4120

 

Then in your part programs, you just use H#506 and D#506 (or pick your favorite 500+ MACRO Variable just make sur eir's the same as the =#4120 section) and you'll be GTG

 

JM2CFWIW.

 

Do it this way and you'll NEVER have the wrong offset active unless you do it on purpose.

 

 

 

or you could skip the step of writing from one variable to another......H#4120 or D#4120

[dforsythe]

or you could skip the step of writing from one variable to another......H#4120 or D#4120

 

This is the way to go.

[GoetzInd]

or you could skip the step of writing from one variable to another......H#4120 or D#4120

 

May be a slight problem if you're pre-calling tools......

 

Mike

[dforsythe]

all the machines i have ran use one vaiable for the tool in the spindal. pre call tools do not matter in this case.

[GoetzInd]

#4120 is current "T" value. I believe most builders have there own way of passing down the tool that's actually in the spindle. Makino for instance has a M code that passes info to a #500 variable including current and next tool numbers.

 

Mike

[john316]

 

Or just add these to lines to your post processor.

 

tloffno$ = t$ #Diameter Offset No

tlngno$ = t$ #Length Offset No

 

This is the way I've done it since v5 so there's no worry about it working right or forgetting to set it. You can also add a "+" value in the post if you want to add a specific number to the tool for the D or H

[Niezingerly]

Thanks to all for the input.

 

A co-worker of mine wrote a macro that forces the H to equal the T number. This is what we were looking for.

 

Thanks again...

[Guest]

May be a slight problem if you're pre-calling tools......

 

Mike

Newp... as long as you do it IMMEDIATELY after the M6 in the Tool Change MACRO it's all good.

[GoetzInd]

Newp... as long as you do it IMMEDIATELY after the M6 in the Tool Change MACRO it's all good

 

James, I'm talking about if you forgo copying the #4120 to a 500 variable.

 

Mike

[rocheey1]

Thanks to all for the input.

 

A co-worker of mine wrote a macro that forces the H to equal the T number. This is what we were looking for.

 

Thanks again...

 

macro ? as in a nethook/mcx vbscript, to modify the settings in an operation, or something to directly manipulate the Gcode ? I personally have had limited success doing it from the operations

[Niezingerly]

He wrote a Macro at the machine, that runs on the machine, to force the H to equal T.

 

Sidenote: Our Mastercam / post are set to output T, H, and D all the same number. That's not what was going on here...

 

The reason this is going on is that an operator modified the T call, to call another tool. When he went to modify the H value, he missed the fact that he deleted the value, instead of changing it to match the T number.

 

This is why the spindle crashed into the part. To the control, the tool had zero length...

 

 

So, this was not to be done in Mastercam. Our output is good. It was just one of those one off "...oh, I'll just change the tool call..." moments, and it bit us.

 

Old file, non-standard tools...

 

Anyhow, thanks again for all the help.

 

 

Just for kicks, here is the macro code for on the machine...

 

 

%

(G43 & TOOL HEIGHT COMFIRMATION PROGRAM)

(TEST FOR G43 VALUE)

(OVERWRITE H# WITH T# IF NEED)

(TEST FOR A TOOL HEIGHT VALULE LESS THAN 3.0", EQUAL TO ZERO, OR NULL VALUE)

(LAST UPDATED 10/08/2013)

 

IF [#4008NE43]GOTO665 (Is G43 Active? )

IF [#4120EQ0]GOTO664 (Is T# Equal To 0)

IF [#4120EQ#0]GOTO664 (Is T# Equal To Null)

IF [#4111EQ#4120]GOTO555 (Is H# Equal To T#)

G49 (CANCEL TOOL LENGTH COMPENSATION)

G43H#4120 (ACTIVATE TOOL LENGTH COMPENSATION)

N555

IF [#5083LT3.0]GOTO666 (Is Tool Height Less Than 3.0)

IF [#5083EQ0]GOTO666 (Is Tool Height Equal To 0.0)

IF [#5083EQ#0]GOTO666 (Is Tool Height Null)

GOTO777 (N777)

N664#3006=175(T# IS NOT EQUAL TO H#)

GOTO777 (GO TO N777)

N665#3000=175(**ERROR** G43 IS NOT ON)

GOTO777 (N777)

N666#3000=176(TOOL HEIGHT LESS THAN 3")

N777

M99

%