Problem- lathe offset problem

[crazycnc]

Hello all,
I have an older Takisawa TC-20 lathe with a Fanuc 21-Tb control. This morning I started it up and referenced it to the limit switches like always. However when I start the program, the Z axis is off about 5 inches and the X axis is off about half an inch! I am positive that no offsets or anything else was changed since last night. Does somebody have a clue as to what is going on? There are no alarms or errors or anything.

Thanks,
Lorne Martin

[HuFlungDung]

Does the amount it is off position correspond to anything, such as a missing tool offset? When you see what appears to be a random error, it is often useful to think "ok if this is a random error, is it repeatable and why is it this exact value?"

[crazycnc]

no, the numbers don't seem to correspond with anything that I can see. I have the technician coming shortly, see what he makes of it.

[stevo1]

I ass u me that you did a couple of power cycles and re-referencing of the machine correct? Is it off by the same number everytime you do that?

Stevo

[crazycnc]

Yes it is

[stevo1]

5” and .5” is a lot to be off. That is not just a simple miss of a marker when referencing the machine.

I have to side with Hu on this. Are you positive that you are not missing something? Do you use your G54-G59 to where maybe someone put something in there? You also want to check your common work coordinate N00. This effects all movements.

Stevo

[HuFlungDung]

A thought: if you happen to have used a G10 in the last program, and for some reason, did not have a line of code to reset it correctly, it will leave its last commanded entry and could throw things off. Just something else to check.

[crazycnc]

Ok, something flaky is going on here, the service guy got me to re-measure one of the tools, all good, the offset number stays within a few thou of what it was, but for some crazy reason, everything's good again. Either I'm going crazy or the machine is. I'm running again with my fingers crossed.

[sinha_nsit]

Possibly you are not the only person handling the machine, and somebody wants to have some "fun" with you.

Note down the work offset values for future reference, just in case ...
It is also possible to manipulate "work shift" on a lathe, which would shift the WCSs by the specified amount, without changing the work offset values.

[crazycnc]

while we are on the subject of lathe offsets, let me ask another question.
A lot of the parts that we make are 2 sided parts, we face the first side, maybe drill a hole, bore it out, then we flip the part around and do something similar to the other side.
What I usually do is make a main program that looks something like this:
:0100
M98P0101
M5
M00
G00X5.0Z9.0
G50X5.0Z9.062
M98P0102
G00X5.0Z9.062
G50X5.0Z9.0
M5
M30

From this main program the two subprograms are called, one for each end of part, the second one being 60 thou closer to the chuck than the first one to compensate for facing the first side.

This works ok, but I never did like the fact that my Z9.0 is always dependent on the length of the tool I am using, and I never know for sure where the absolute position will be. We used to have a Mori Seiki lathe that had G54 to G59 coordinate systems but the Takisawa we have now does not support this. The only command I know of to shift the coordinate system is the G50 command. I know I could always use G28 to return to machine zero, but I don't like going back so far. I would like to be able to return to a specific absolute position for each tool change, and then between the two sides of each part, also shift the coord system by 60 thou.

Following is a typical subprogram:
O0101
(145 SPINDLE TUBE)
(CCLNR-124 GENERAL TURN - KC 240)
G0 T0909 M8
G99 G96 S950 M3
G0 X2.7 Z0.1 S950
X2.7072
Z-0.0778
G3 X2.6224 Z-0.0954 R0.06 F0.012
X2.5376 Z-0.0778 R0.06
G1 X2.401 Z-0.0095
G2 X2.355 Z0.0 R0.0325
G1 X-0.125
G3 X-0.245 Z0.06 R0.06
G0 Z10.0 X5.0
(1.5 UDRILL)
G0 T0101
G99 G97 S1600
X0.0 Z0.1 S1600
G1 Z-3.5 F0.0073
X0.03
G0 Z0.1
Z10.0 X5.0
(A16-DCLNR4 GENERAL BORE - KC 730)
G0 T0303
G99 G96 S1460
X1.5626 Z0.1 S1460
X1.562
X1.7052
G1 Z-0.756 F0.01
X1.562
G0 Z0.1
X1.8484
G1 Z-0.756
X1.7052
G0 Z0.1
X1.9916
G1 Z-0.0531
X1.9906 Z-0.0539
G2 X1.98 Z-0.0712 R0.0312
G1 Z-0.756
X1.8484
G0 Z0.1
X2.1348
G1 Z0.0191
X1.9982 Z-0.0491
X1.9942 Z-0.0514
X1.9916 Z-0.0531
G0 Z0.1
M9
Z10.0 X5.0
(CCLNR-124 GENERAL TURN - KC 240)
G0 T0909
G99
M99
M30

If somebody has any ideas, please let me know.

[dcoupar]

When you Reference Return your machine, are there values in the Machine Position display? If so, on a 21T-B, these are set in prm 1240.

Your machine may have the "Second Reference Position" option. It works like G28, but you can move it by changing a parameter. 1241 contains the metric values for G30. 1242 for G30 P3, and 1243 for G30 P4.

So at the start and end of your program and each tool index, you can command G30 U0 W0 instead of an absolute position.

You might try to MDI G30 W0 to see if you get an alarm. If not, using G30 might help.

[crazycnc]

Yes, thank you very much that works exactly the way I want it to. G30 is not listed in my manual but it works on the machine! Now, is there another G code for points 3 and 4? Not sure what I would use it for, just curious.