Fanuc Height Offset Lost/Reset

So, I was squaring up a block today. G54 Z0 was set on the floor of the vise, so I could face mill to the exact height I needed very easily. Turned on G43 height offset so I could get this done.

Squaring up my block all happy, I hit reference return Z to send the spindle home and my height readout mysteriously changes as soon as it gets home. G43 stays active, but the actual value on the Absolute (G54) position is lost. Canceling height offsets with G49 leaves the number the same. Hitting G43H5 again brings the height offset back.

It seems like a very very unexpected behavior... do I have some funky parameter set?

I made a video for everyone's enjoyment:

I didn't listen to the audio, so I may have missed something, but your situation doesn't sound unusual to me. Typically when you ZRN the machine, the Z-values will change, at least in my experience. Truth be told, I never gave much thought to the "WHY" of it.

Are you not using a simple program to face the parts in this situation? In such a case - assuming a single pass across the face, this is how I would treat it...


O1234 (SIMPLE FACE PASS PROGRAM)
(G54 X0. IS...)
(G54 Y0. IS...)
(G54 Z0. IS FLOOR OF VISE)

#110=5 (FACE-MILL) I'm a big fan of calling tools & H-codes this way - less chance of screwing them up and crashing.
#112=1.25 (THICKNESS OF PART) Easier to edit it here, than the program somewhere, IMO.

N10(FACE TOP OF PART)
G0 G20 G17 G80 G90 G40
G91 G28 Z0 G30 If that's better for toolchanges
T#110 M6
G0 G90 G54 X0. Y0. S1000 M3
G43 H#110 Z[#112+1.] Calls corect H-offset, and stops 1" above the part...
M00 (CHECK TO MAKE SURE CUTTER IS 1-IN. ABOVE PART) Safety check - Can't crash a machine after a fat-finger quick-edit!
M3
M8
G1 X6. F35.
G91 G28 Z0 M8 Again, G30 if it's better.
G90 G53 X-10. Y0. M19 Send table to unload position by the door. Change X value as needed.
M30

Jashley73 said:

I didn't listen to the audio, so I may have missed something, but your situation doesn't sound unusual to me. Typically when you ZRN the machine, the Z-values will change, at least in my experience. Truth be told, I never gave much thought to the "WHY" of it.

Click to expand...

It just seems very strange to me that the machine would stay in G43 tool length comp mode, but basically obliterate the actual tool comp from the coordinate system. Firs off - it isn't logical to cancel G43 when you send the spindle to home in the first place, but even if that is what Fanuc wanted to do - leaving the machine with G43 active, but essentially canceling it causes a misinformation condition that could really screw someone in the tookas.

I'll put it this way - if the machine switched to G49 after hitting Ref Return in Z, I wouldn't be posting this. That it stays in G43 is the sorta fucked up thing.

Are you not using a simple program to face the parts in this situation? In such a case - assuming a single pass across the face, this is how I would treat it...

Click to expand...

It was a lumpy, saw cut thing that had to get ~.35" removed from one face, .02 from another and skim cut on the last pair. I am so not comfortable enough in Finger Cam yet to be fast enough to beat whirling around the MPG a little bit!

O1234 (SIMPLE FACE PASS PROGRAM)
(G54 X0. IS...)
(G54 Y0. IS...)
(G54 Z0. IS FLOOR OF VISE)

#110=5 (FACE-MILL) I'm a big fan of calling tools & H-codes this way - less chance of screwing them up and crashing.
#112=1.25 (THICKNESS OF PART) Easier to edit it here, than the program somewhere, IMO.

Click to expand...

Neat tip, Thanks!

gkoenig said:

It just seems very strange to me that the machine would stay in G43 tool length comp mode, but basically obliterate the actual tool comp from the coordinate system. Firs off - it isn't logical to cancel G43 when you send the spindle to home in the first place, but even if that is what Fanuc wanted to do - leaving the machine with G43 active, but essentially canceling it causes a misinformation condition that could really screw someone in the tookas.

I'll put it this way - if the machine switched to G49 after hitting Ref Return in Z, I wouldn't be posting this. That it stays in G43 is the sorta fucked up thing.

Click to expand...

Hello gkoenig,
The action of a physical Reference Return (via Reference Return Button) is determined in the PLC program (PMC in Fanuc Speak) by the MTB. The G Codes on the Control Screen is a List of the Last G Codes executed and addressed by Fanuc, but could also have been (should also have been) addressed by the PLC.

It nearly goes without saying, that when either a Manual, or programmable (G28) Reference Return is performed, the program will be executed either from the beginning of the Program, or from the start of a Tool Operation, where the Tool Length Offset will be re-established. Seldom and foolhardy in my opinion, would one be part way through a programed operation, execute a Manual Reference Return and then start from the same place where the Program was terminated without calling the Tool Length Offset again. Accordingly, if you were to Start the program from the appropriate position prior to the Tool Length and Work-shift Offsets being applied, there should be no issue.

Regards,

Bill