Program Z work offset probe with macro?

[teachme]

Application:
We're milling raw stock sheets with small variances in thickness. We're milling hundreds of sheets, so measuring each one isnt an option.

The goal:
Probe the fixture Z height then,
Probe the stock Z height then,
Write a program to calculate the difference which equals the actual stock thickness.

Question:
After we get this stock difference Z offset, how can we plug it into the Z work offset via a macro?
Or is this only possible manually?

 

[BrotherMacros]

Hi,

This is possible. It depends on what probe you are using and the machine type. I would look at the probe manual for a specific macro that the probe programs are referencing dimensions to. Some manufacturers want you to pay extra for measurement programs. You could avoid paying the extra money by probing and sending all the data to one work-offset like G59. Use that offset as a sort of "scratch paper" for storing dimensions.

Example:
Probe routine- fixture
#500=#5233 (write G59 z-value to macro #500)
Probe Routine- Part
#501=#5233 (write new g59 z-value to macro #501)
#502=[#500-#501] (variable #502 is storing the difference)
#5223=#502 (write the difference to G54 Z-offset)

Check with your manual or machine dealer about what macros are not being used, typically #500's are not used but every machine is different.

Helpful list of variables.
Fanuc system macro variables and macro programming

Good luck!

 

[teachme]

Hi,

This is possible. It depends on what probe you are using and the machine type. I would look at the probe manual for a specific macro that the probe programs are referencing dimensions to. Some manufacturers want you to pay extra for measurement programs. You could avoid paying the extra money by probing and sending all the data to one work-offset like G59. Use that offset as a sort of "scratch paper" for storing dimensions.

Example:
Probe routine- fixture
#500=#5233 (write G59 z-value to macro #500)
Probe Routine- Part
#501=#5233 (write new g59 z-value to macro #501)
#502=[#500-#501] (variable #502 is storing the difference)
#5223=#502 (write the difference to G54 Z-offset)

Check with your manual or machine dealer about what macros are not being used, typically #500's are not used but every machine is different.

Helpful list of variables.
Fanuc system macro variables and macro programming

Good luck!

Super appreciate this. We're using a Haas with a renishaw probe. Wasnt able to find anything specific to this.

 

[13engines]

Not sure if and how this applies to a Renishaw Probe on a Haas, but the standard Inspection Plus O9820 Stock Allowance probe routine will measure and store up to 6 X,Y or Z positions for you. It will put the Max in #144, Min in #145 and variation (stock allowance) in #146. How-what-where is stores the individual measurements you'd have to run it and find out.

You say part of your needs is measuring the fixture. Not sure why you have to measure the fixture every time, as don't Fixed-In-Place Fixtures, as the name implies, have a fixed location including height? Meaning measure once and done?

 

[LockNut]

Not sure if and how this applies to a Renishaw Probe on a Haas, but the standard Inspection Plus O9820 Stock Allowance probe routine will measure and store up to 6 X,Y or Z positions for you. It will put the Max in #144, Min in #145 and variation (stock allowance) in #146. How-what-where is stores the individual measurements you'd have to run it and find out.

You say part of your needs is measuring the fixture. Not sure why you have to measure the fixture every time, as don't Fixed-In-Place Fixtures, as the name implies, have a fixed location including height? Meaning measure once and done?

This! Wouldn't it be easier to just probe the top of the part every time? Done? Or are we missing something?

Also, a Renishaw probe uses #500 macros for the calibration data. You DON'T want to overwrite that.

 

[angelw]

This! Wouldn't it be easier to just probe the top of the part every time? Done? Or are we missing something?

Also, a Renishaw probe uses #500 macros for the calibration data. You DON'T want to overwrite that.

My thoughts entirely. Further, I can't see the point of registering the difference between the two surfaces (small value) in a work offset unless it was Offset G52 and Setting 33 was not set to Yasnac Mode.

@teachme
Please explain for what purpose you had in mind for registering only the difference between the two in a work offset.



Regards,

Bill

 

[teachme]

My thoughts entirely. Further, I can't see the point of registering the difference between the two surfaces (small value) in a work offset unless it was Offset G52 and Setting 33 was not set to Yasnac Mode.

@teachme
Please explain for what purpose you had in mind for registering only the difference between the two in a work offset.



Regards,

Bill

Ill try to answer the other 2 comments here as well.

The goal was to probe the fixture once and set it as a global variable. Then use it to subtract from the stock heights, which will exceed hundreds of parts. Maybe I wasnt clear enough in the OP.

@Bill, not sure if this is what youre asking, but the difference between the fixture and stock height, will give me the total thickness of the stock.
So our sheets are 5 mm ±0.2 mm thickness.
The parts on the sheet have to be milled to 3.4 mm ±0.02 mm thickness.

So rather than measuring each sheet, and settings those numbers manually for each sheet, I was hoping to let the probe do the work.

 

[13engines]

I'm just not following the logic. Are you stacking the sheets on top of each other like albums on a record player, and peeling one off after each run? If not, then what is the problem here?

Measure the fixture and set its coordinates in G54. It has a Zero Reference corner or feature right? Include the Z floor of the fixture in your G54 setting to represent either the bottom of your part, and program your part with positive Z values, or set Z zero at 3.4mm above the fixture floor, and program your parts so Z0. equals the top of the part when finished. Then just keep the clearance plains of your tools above the worst case scenario of your stock thickness.

What I'm saying is... unless the tools are being run at the very breaking point of their existence, what will 0.2mm mean to any depth of cut you've got going? You have a fixture derived reference point in Z, or at least I think or hope you do. Why not use it and forget about the minor stock variations? Work from the bottom up so to speak, as the top of things is a small variable that should be easy enough to ignore.

I must be missing something. This is all so simple, and I'm having a hard time making it difficult enough for a probe routine to be added in the mix.

 

[angelw]

@Bill, not sure if this is what youre asking, but the difference between the fixture and stock height, will give me the total thickness of the stock.
So our sheets are 5 mm ±0.2 mm thickness.
The parts on the sheet have to be milled to 3.4 mm ±0.02 mm thickness.

So rather than measuring each sheet, and settings those numbers manually for each sheet, I was hoping to let the probe do the work.

Hello teachme,
Yes, I understand that, but how does the total height of the stack (difference between the fixture and the top of the stack) equate to a Work Offset. That value on its own doesn't relate to where Z Zero is, unless, as I suggested in my previous post, registered in G52 (Child Offset, common to all Work Shift Offsets). I can see that working, because the value registered will be combined with whatever the primary Offset thats being used.

However, less work (in terms of math carried out by the control) would be done by simply probing the top of the stack to adjust the Work-shift Offset for Z Zero.

Regards,

Bill