Fanuc tool lenght offset question

[Mechanica-Art]

Good morning, 
I have worked on many control types in my years of programming, so I am not a novice. I have over thirty years of CNC programming, process development, working with manufacturing cells, and I teach Machine technology at a local trade school. I have worked with Haas, Yasnac, Meldas, Mazak, Fanuc to name a few over the years. The Haas and Yasnac are my favorites, very user friendly and logical. I feel that I am just not seeing something in the Fanuc control in regards to tool length measurement and setting at the machine, and hoping some one can shed some light on the matter for me... 

My method for tool length offset at the machine (dynamic measurement) is as follows:
1) I measure off the machine table on top of a 1-2-3 block, the 3" side. 
2) Set all the tools at this point, enter the lengths into the height offset registers.
3) I them measure from the top of the measurement block to the top of each of my work piece Z-zero planes and set my work offsets as required, G54 vise one, G55 vise two and so on...
4) If I need to change a tool it is always measured on top of the block as listed above.

Easy method, fast accurate and no fuss to get a job running. 
On the Haas, and other controls I just enter the length coordinate of the machine "Z-axis" directly into the length offset register and it is done. 

My question is this; I notice on a Fanuc control, it will add what ever active work offset G54-G59 Z values to the tool length when you write it into the register Why Why why?? and how to get it to stop doing this???

This has frustrated me for years, I wonder if any one knows how to make it read only from the machine coordinate system. The Haas control has two parameter settings for tool length offset, Fanuc, and Haas when set to Fanuc it does exactly as described above. I tell every one who has a Haas to turn the Fanuc style off....

Over the last several years I have worked on Okuma and Haas machines so it has been a while since I worked on a Fanuc.

[Guest]

Haven't measured a tool in this manner in years...

Gage Length settings only

[mkd]

Haas also has this (seemingly idiotic) setting also. but it is easily turned off.

not sure how to turn off on fansuc.

[Newbeeee™]

4 hours ago, JParis said:

 

Gage Length settings only

+1

although I've never done it any other way...

[jlw™]

This is so that you can touch a tool off on your workpiece.  Very handy actually, you can match faces so well you can't tell it's two different pieces.  I use a 1in gage block on top of my workpiece, teach it 1in above wherever it's at.  If it's G45 Z0. I teach 1in.  If it's G54 Z-1.2 I teach it -.2.  Super simple, quick and easy for when you need to match faces tighter than your presetter will hold.  You can also use it to set workpiece Z from the tool.

Any who, always more than one way to skin a cat.

[Colin Gilchrist]

Maybe I'm missing something, but why don't you simply use "Tool setting" Work Offset Number? Set G59 to use "0.0" for XYZ. It's even easier if your machine has Extended Work Offsets. Just use G54.1 P48 as your "setting" offset.

If you want to get more creative, use Macro B, and create a Macro to copy the active work offset values to a safe location, and another Macro to copy them back. For example, save G54-G59, into G54.1 P43-P48. Then, call a second Macro to restore all three values to each offset.

Then you can clear the offsets (save), set your tools, and restore the offsets. It would take a single line of code in MDI to store and retrieve the values.

[civiceg]

What series of control, are you hitting Input C to store the value for the tool offset?

It should be a simple parameter change.

[RonC.]

20 hours ago, Mechanica-Art said:

My method for tool length offset at the machine (dynamic measurement) is as follows:
1) I measure off the machine table on top of a 1-2-3 block, the 3" side. 
2) Set all the tools at this point, enter the lengths into the height offset registers.
3) I them measure from the top of the measurement block to the top of each of my work piece Z-zero planes and set my work offsets as required, G54 vise one, G55 vise two and so on...
4) If I need to change a tool it is always measured on top of the block as listed above.

Easy method, fast accurate and no fuss to get a job running. 
On the Haas, and other controls I just enter the length coordinate of the machine "Z-axis" directly into the length offset register and it is done. 

My question is this; I notice on a Fanuc control, it will add what ever active work offset G54-G59 Z values to the tool length when you write it into the register Why Why why?? and how to get it to stop doing this???

 

I've been here before, it's been a while for me, since I've set tools this way,

but the only other thing  I would do,  that you didn't mention was I would hand write a tool offset program to go to

a certain place on table to set tools, this program was in every machine we had. it set the tools in same place, and use G53 command to get machine coord.

instead of involving G54-G59 workshift.

hope this helps..

[Mr.ZX]

This is the Mechanica-art guy from above I could not log into my account for some reason so this is my work account to reply.........

In the past I would create my own macro programs to read the values into the height offset registers, worked great! 

Yes I have been trough all the scenarios as above. I currently use a set point on my machines (Okuma) to measure tool length offsets. Very accurate when machining molds..... And have used the "G59 0,0,0" method in the past.  The controls are at the school and are on Sharp CNC machines. Fanuc 21i. Does Fanuc have a parameter that will read only from the machine position? I called Fanuc directly and they did not really know....  I just need to know if Fanuc has a method or parameter, or have I been missing something all these years......

 

I really do not like to teach the students to measure tools off the top of the part. It creates to many variables when using two vises multiple work offsets and so on. Measuring off a set point from the table is the most accurate and simple method in my opinion.  It also teaches the students about the machine, work coordinate, and length offset  systems and how they work with each other in a program.

[Guest]

 

            There are four principal methods in general use for “telling” the machine where the location of the part is relative to the machine’s home positions for the Z axis. There are others but these are the most common and most preferred.

 

1. Distance from the Spindle Face/Gage Line at Z Home to B-Axis Centerline of Rotation. Parts are programmed relative to Centerline of Rotation. This will ALWAYS be a negative number and will be written to the preferred Work Offset(G54~59, G54.1P1~P48, etc…). In addition, the tool length with be the distance from the Spindle Face/Gage Line to the tip of the tool. This will ALWAYS be a positive number.
   1. Setting this is relatively simple. Remove the tool from the spindle (I prefer to call T0 M6 so that there are no tools even supposed to be in the spindle). Get a 1-2-3 Block, a 3” or 4” Gage Block whichever is easiest to acquire. Set the Machine in “Handle Mode”. Go to the Work Offset Page and cursor down to the preferred Work Offset. Using the hand-wheel, Jog the Z Axis in using the X100 increment getting it within 4-5 inches of the Pallet Edge(depending on the Gage block size). Stay away about 1.0”. Place the Gage Block between the Pallet Edge and the Spindle face moving it in closer still in the X100 increment. Once you’re within about .1” to .05”, set the increment to X10. Once you get within about .010, set the increment to X1. Sliding the gage block between the Pallet Edge, the Gage Block, and the spindle face, you want them to just barely touch being careful not to put too much pressure on the face of the spindle. You should feel a very slight drag. Once you are comfortable with the feel, exit handle mode.You’ll need to do some math on a calculator now. Take the size of the pallet and divide by two. Add the size of your Gage Block to half of the size pallet (ex. 5.9055 for a 300mm pallet plus 4.0 for my Gage Block = 9.9055). Press the Axis Letter “Z” and key in 9.9055, then press the (ex. Z9.9055), then press the “MEASURE” softkey that appeared as you pressed the Axis Letter Z. This will now calculate the distance from the machine home to the center of rotation. You may need to fine tune this number as it may change slightly during cutting conditions.

 

 

2. Distance from Spindle Face/Gage Line at Z Home to Z Part 0. Parts are programmed with no regard to Centerline of Rotation. This will ALWAYS be a negative number written to the preferred Work Offset(G54~59, G54.1P1~P48, etc…). In addition, the tool length with be the distance from the Spindle Face/Gage Line to the tip of the tool. This will ALWAYS be a positive number.

                  A. Setting this is relatively simple. Remove the tool from the spindle (I prefer to call T0 M6 so that there are no tools even supposed to be in the spindle). Get a 1-2-3 Block, a 3” or 4” Gage Block whichever is easiest to acquire. Set the Machine in “Handle Mode”. Go to the Work Offset Page and cursor down to the preferred Work Offset. Using the hand-wheel, Jog the Z Axis in using the X100 increment getting it within 4-5 inches (depending on the Gage block size) of part Z 0. Stay away about 1.0”. Place the Gage Block between the part face and the Spindle face moving it in closer still in the X100 increment. Once you’re within about .1” to .05”, set the increment to X10. Once you get within about .010, set the increment to X1. Sliding the gage block between the Part Face, the Gage Block, and the spindle face, you want them to just barely touch being careful not to put too much pressure on the face of the spindle. You should feel a very slight drag. Once you are comfortable with the feel, exit handle mode. Press the Axis Letter “Z” and key in the length of your Gage Block (ex. Z4.0) then press the “MEASURE” softkey that appeared as you pressed the Axis Letter Z. This will now calculate the distance from the machine home to the face of your part. You may need to fine tune this number as it may change slightly during cutting conditions.

 

 

 

 

3. Distance from Spindle Face/Gage Line at Z Home to B-Axis Centerline of Rotation set in Common Offset AND Distance from Centerline of Rotation to Z Part Zero written to the preferred  Work Offset (G54~59, G54.1P1~P48, etc…). Parts are programmed with Part Zero relative to centerline of rotation. This will ALWAYS be a negative number. In addition, the tool length with be the distance from the Gage Line/Spindle Face to the tip of the tool. This will ALWAYS be a positive number.

                  A. Setting this is relatively simple. Remove the tool from the spindle (I prefer to call T0 M6 so that there are no tools even supposed to be in the spindle). Get a 1-2-3 Block, a 3” or 4” Gage Block whichever is easiest to acquire. Set the Machine in “Handle Mode”. Go to the Work Offset Page and to the Common Work Offset. Using the hand-wheel, Jog the Z Axis in using the X100 increment getting it within 4-5 inches of the Pallet Edge(depending on the Gage block size). Stay away about 1.0”. Place the Gage Block between the Pallet Edge and the Spindle face moving it in closer still in the X100 increment. Once you’re within about .1” to .05”, set the increment to X10. Once you get within about .010, set the increment to X1. Sliding the gage block between the Pallet Edge, the Gage Block, and the spindle face, you want them to tough slightly touch. Be extremely careful not to put too much pressure on the face of the spindle. You should feel a very slight drag. Once you are comfortable with the feel, exit handle mode.You’ll need to do some math on a calculator now. Take the size of the pallet and divide by two. Add the size of your Gage Block to half of the size pallet (ex. 5.9055 for a 300mm pallet plus 4.0 for my Gage Block = 9.9055). Press the Axis Letter “Z” and key in 9.9055, then press the (ex. Z9.9055), then press the “MEASURE” softkey that appeared as you pressed the Axis Letter Z. This will now calculate the distance from the machine home to the center of rotation. Now, your programmer most likely will need to tell you the Z value from Centerline to Part Z0. Input this positive value in the preferred offset. You may need to fine-tune this number as it may change slightly during cutting conditions.

 

 

 

4. Distance from Z Home Position (with tools in the spindle) tip of each tool to part Z. Each tool will have a negative Z value in it’s corresponding tool length offset. This the least preferable and least flexible of the four methods mentioned.

                  A. Setting this is simple but not flexible if you plan to use tool breakage/tool length measurement, or if you plan to use tools on multiple jobs/setups. Start out by zero returning the machine. Go to the “Position”, “All” or “Relative” screens. Press the letter “Z” on the operator panel and the “Origin” and “Exec” softkeys. You want the Machine Z to match the Relative Z. Now go to the Tool Offset Page, cursor down to the appropriate tool length offset (making sure you are in the “Geometry” Column). Set the machine in Handle Mode and move to the Z0 surface of the part. Press the letter “Z” on the operator panel, and the “Input C.” will appear. Press this soft-key and it will write the relative value (a large Z- value) to the highlighted offset. Or, if you choose you can type it in manually.