Tool length offsets Fanuc O-M

[Chevy427z]

Hi Folks.

I've been dealing with this ever since I was introduced to Fanuc controls years ago and just dealt with it, but decided that it's time to get the record set straight (in my mind anyhow). I know that it's been discussed in the past but I can't find those threads again.

My O-M is mounted on a mid 90s LeBlond-Makino 4 axis mill.

I set my tools by touching off on top of a 6" block which sits directly on the machine table. I input the relative position in the tool offsets. Then I use a dial indicator to find the difference from the top of the 6" block to the top of my part and input that difference into the G54 Z register.

The machine puts the tool exactly where it needs to be (in Z) but the on screen "position" is never correct.

If I touch off the tool directly on top of my part, input the relative position into the G54 Z register, and zero in the tool length offset, the machine puts the tool where it needs to be (in Z) and the absolute location shows properly on the "position" screen. Obviously, I can only do this with one tool, but would love to be able to get the same result with multiple tools. What am I missing or doing wrong?? Many thanks for looking!

Edited: added some pictures incase someone recognizes an error in my math or methods.

Mark

 

[Milling man]

What am I missing or doing wrong??

Maybe offsets?

 

[706jim]

On the old Fanuc 6 you could just press "Z input" and the offset value would enter itself into the table. Maybe try that?

 

[Chevy427z]

On the old Fanuc 6 you could just press "Z input" and the offset value would enter itself into the table. Maybe try that?

Great suggestion! Thank you! Wish it was that easy. Must be a step above the O-M as when I hit Z to input "Z input", all I get is a "6" as that's the Z button. Appreciate your response!

Mark

 

[13engines]

The actions of the Absolute Display are controlled by Parameter. Maybe even a MTB Keep Relay. Can't remember which. Look in your machine manuals and/or Fanuc Parameter Manual to find out.

Your setup routine is okay, except that you should be paying attention to Machine Position and not Relative when setting your numbers. Relative and Machine may match, but not always. Think of your Relative as a DRO. Something you can play with to set Position Zeros as the need may arise. Honestly... in running a mid 90's OM machine for a couple decades, I've never used Relative, and barely have the need for Absolute except when I'm bored and want to watch numbers change.

When your tool is in position on the setup block, and your cursor is next to the current tool offset number, try EOB Z INPUT. (Think Control/Alt/Delete) This will enter the current (Machine) position into your Tool Offset Table. Note that this will include anything you have in your SHIFT register, so be careful about that. If you were to put Z6.0 in your SHIFT register and measure your tools, it would enter your Tool Offsets as if you had touched them off on the table. Be sure to set Z SHIFT back to Zero when done.
Note when you measure a tool to your Work Piece using your 2" block, be sure to add -2.0 to the number you put into G54Z.

 

[Chevy427z]

The actions of the Absolute Display are controlled by Parameter. Maybe even a MTB Keep Relay. Can't remember which. Look in your machine manuals and/or Fanuc Parameter Manual to find out.

What's an MTB Keep Relay?

Your setup routine is okay, except that you should be paying attention to Machine Position and not Relative when setting your numbers. Relative and Machine may match, but not always. Think of your Relative as a DRO. Something you can play with to set Position Zeros as the need may arise. Honestly... in running a mid 90's OM machine for a couple decades, I've never used Relative, and barely have the need for Absolute except when I'm bored and want to watch numbers change.

Excellent point. I have been using relative for years, maybe why I've always had grief setting tools. My machine position has always been in metric since I bought it and never pursued changing it. Maybe I should look into that first. Assuming it's a parameter. I am away from the machine and manuals now, so I will look that up later.

When your tool is in position on the setup block, and your cursor is next to the current tool offset number, try EOB Z INPUT. (Think Control/Alt/Delete) This will enter the current (Machine) position into your Tool Offset Table. Note that this will include anything you have in your SHIFT register, so be careful about that. If you were to put Z6.0 in your SHIFT register and measure your tools, it would enter your Tool Offsets as if you had touched them off on the table. Be sure to set Z SHIFT back to Zero when done.
Note when you measure a tool to your Work Piece using your 2" block, be sure to add -2.0 to the number you put into G54Z.

I so look forward to trying that EOB Z INPUT! Well aware of taking out the touch off setter height. I included the pic, but it got lost in translation. That was to show that driving the machine via the program, it went to the proper height (2", but the absolute display was off).

Thank you very much for your time and expert advice! Can't wait to try it now.

Mark

 

[13engines]

What's an MTB Keep Relay?

A Machine Tool Builder (LeBlond) Keep Relay is a setting in the control, (there are many) that affects how the machine operates. You find them in the Manufacturers Manuals. They will be listed under a K setting. Each Bit of an eight Bit Word will potentially have the ability to change how the machine acts in various situations.

My machine position has always been in metric since I bought it and never pursued changing it. Maybe I should look into that first. Assuming it's a parameter.

It's on the Main "Settings" page. It would do you well to get a Fanuc OM Operators Manual which will lead you through moving through all the different pages and settings on your control. The MTB Operations Manual is even better yet.

 

[Vancbiker]

Your 0 series control has to be a C model or later to switch the Machine Position display between inch and metric. A and B models can only display Machine Position in inch units if the machine is equipped with inch pitch screws.

 

[13engines]

Your 0 series control has to be a C model or later to switch the Machine Position display between inch and metric. A and B models can only display Machine Position in inch units if the machine is equipped with inch pitch screws.

Still learning...

 

[lowCountryCamo]

would this apply?

 

[Mtndew]

If I touch off the tool directly on top of my part, input the relative position into the G54 Z register

Have you tried using Machine position instead of Relative?
Are you zero-ing out the Relative position after homing out the machine?
There is a parameter that controls whether or not the ABS reflects the tool offset when a G43 (H) is commanded.

 

[lowCountryCamo]

or for absolute read out

 

[lowCountryCamo]

this is for fanuc 0md which I have and my readout includes TOL

 

[Chevy427z]

Have you tried using Machine position instead of Relative?
Are you zero-ing out the Relative position after homing out the machine?
There is a parameter that controls whether or not the ABS reflects the tool offset when a G43 (H) is commanded.

Happy to report moderate success!! It took a while to find the PWE (ability to edit parameters) then to find the right one (0063) and then input it properly (digit 0 - far right - needs to be a 1) Turned parameter editing off and POOF! 18 years later the machine position is reading English and not metric!

Yes, I am zeroing out the relative positions after homing, then hitting "MANU/ABS" to "lock" the positions. That's how I was taught so many years ago. Is that correct?

Thank you all so very much for your time and attention. On to see if "machine position" will help with my tool length offsets. Truly appreciated!

Mark

 

[Chevy427z]

or for absolute read out

View attachment 425661

Thank you LowCountry!
Not quite sure what that refers to.

Mark

 

[Chevy427z]

Still learning...

How do I determine which model mine is?

There is a software key (PWE) under parameters to enable parameter editing. And I was able to finally get my machine position to read in English after only 18 years of suffering. LOL Hopefully I can set my tools properly now.

Mark

 

[Chevy427z]

A Machine Tool Builder (LeBlond) Keep Relay is a setting in the control, (there are many) that affects how the machine operates. You find them in the Manufacturers Manuals. They will be listed under a K setting. Each Bit of an eight Bit Word will potentially have the ability to change how the machine acts in various situations.


It's on the Main "Settings" page. It would do you well to get a Fanuc OM Operators Manual which will lead you through moving through all the different pages and settings on your control. The MTB Operations Manual is even better yet.

Thank you! I do have the manuals. I've always found them too "techincal" to follow easily. I seem to lack the necessary patience, until I am forced into a corner.

Mark

 

[Vancbiker]

How do I determine which model mine is?….

Power on with the estop button pressed. There will be a number on the screen like..

04xxx-xx

Post that number and I’ll look it up.

 

[Chevy427z]

Power on with the estop button pressed. There will be a number on the screen like..

04xxx-xx

Post that number and I’ll look it up.

I didn't see it on any screen while powered up but I remembered seeing it while it was powering up. So I shut it down and brought it back up. Mine is 0452-04. Thank you!

Mark

 

[Vancbiker]

0452-04 is an 0 Mate MF.