[Colbolt2]

I have a Fanuc Series 0i-TC on a Lathe
I program the following G71 cycle with a .050 clean up pass.
The control shows that the tool is leaving .067 for clean up pass
Then when it takes the clean up pass, the control shows the tool going right to 1.000
However, it does not remove any material, thus the part is .067 big.
Any ideas would be greatly appreciated.

I run this same program on Funac Controls 18-T. 18i-T and OT and they run perfect.
I also run the G71 on a boring cycle and it works great.


:1111
(CONTOUR)
G00G99G96S500T1212
G50S1500
M03
M08
G00X4.010Z.2
G71U.1R.025
G71P10Q20U.05W0.F.015
N10G0G42X1.0
G01Z0.0F.015
G01Z-.7497F.015
G03X3.75Z-5.8125R12.9412F.015
G01X3.896Z-7.6F.015
G01X4.0F.03
U.05
N20G40U.05
G70P10Q20
G28U0.
M30
%

[dcoupar]

Are the R and T values correct for Offset 12?

[Colbolt2]

dcoupar,
Thank you for your reply:
I have a .0312 in R while using a CNMP432 insert. That seems that is incorrect as it should be .015.
I am not familiar with the T value. Can you explain please?

[ghyman]

If you program using radius comp, then the R value for the tool offset in this case will be .0312... The TNR for a 432 insert is 2/64" = 1/32" = .0312"

[dcoupar]

The T value tells the control where you set the virtual tip when you touched off the tool. Most likely it should be a 3 for OD turning towards the chuck.

[Colbolt2]

ghyman:
Many Thanks. So it was set correctly. My bad. Spinning to many plates.

dcoupar:
Can I ask where in my the G71 program one would insert a T. I have never used a T

[Colbolt2]

dcoupar:
Are referring to the Z axis when you speak of the T?. If so yes, that is set correctly.

[fordav11]

you say the program runs fine on another machine so it has to be a parameter issue.

[dcoupar]

ghyman:
Many Thanks. So it was set correctly. My bad. Spinning to many plates.

dcoupar:
Can I ask where in my the G71 program one would insert a T. I have never used a T

The 3 goes in the T column of the Geometry Offset for #12... see attached.

[Colbolt2]

Thank you .
I will double check this entry

[Colbolt2]

I did check this entry.
It was set to zero.
I have many different size parts to run with this cycle on this machine.
I will be setting up another size today. I will update my progress.
What I did was run the G71 program and then wrote a additional program to come clean the part up to size.
I will see what happens when all the entries are input correctly.
Thanks for all your time.
Hope I can return the favor one day.

[Colbolt2]

fordav11
Yes, this program works on 3 other Funac controls and has worked for about 17 years.
I purchased this Femco as a back up to my TU-30 Ikegai Lathes.
I just need it to do a secondary operation.
I will continue to attempt get it to do what I need it to do.
UNFORTUNATELY When I purchased the machine the machine tool salesmen told me that the machine manuals were on line.
Not true. So I do not have any programming manuals for this machine.

[fordav11]

the guy wasn't lying. 0i-TC manuals are there if you look hard enough in the right place while the moon is at 30 degrees above the horizon.
anyway you can find it attached.....

[Colbolt2]

Fordave11
I can not believe I did not find that.
Perhaps I did not even look for it.
Regardless, many thanks for taking time out of your day to attach that and send it to me.
It is very much appreciated.

[Colbolt2]

I have an unrelated question.

Is there a way to get the chuck to not spin during our dry run cycles?

*****UPDATE TO MY QUESTION******
We just removed the M03 and the dry run cycle worked as needed.

[Colbolt2]

UPDATE ON MY G71 PROGRAM
I followed the advice from the all that responded and SUCCESS!!
I entered the value 3 in the T section of my offsets and the program now runs the finish cycle.
Thank you so much to all !!

[fordav11]

to save editing, you can use block delete on the M03 to skip it.
/G97 S200 M3

in CUSTOM/AUX, some machines have a STM item that will ignore any STM functions too when enabled.