[vincent.pomerleau]

Hello!
When I work on milling, with my renishaw probe, I can position workpiece on table and just probe the angle to make a skew compensation in my program with G68 (coordinate rotation) and it's useful! I have long shafts to make on the CNC lathe with tailstock and of course I always have a little taper. There is this kind of compensation on Fanuc 0i cnc lathe for this? For now I correct the 8 diameters on my part manually in the program.

[fordav11]

normally just change the X values in the program and put X and Z on each line even if movement is only in Z. Or add U value for taper adjustment or use macro variable.
example.....

G00 X50.0 Z2.0
G1 X50.002 Z-50.0

or

G00 X50.0 Z2.0
G1 U0.002 Z-50.0

or

G00 X50.0 Z2.0
G1 X[50.000 + #100] Z-50.0


to make program adjustment easy, always use R value for arc radius, not I/K. With R you can adjust X/Z small amounts and the path of R will automatically be adjusted to the end coordinate. With I/K you will get an 'out of tolerance' alarm because the end point of the arc no longer lies within the reach of the I/K center point.


Or re-align tailstock ;-)

[vincent.pomerleau]

Thank for reply!
My tailstock is not so bad, it's just my part is 17" long with tolerance of +-.0002 on diameter. For now I use the macro as you write in your post, I just don't like to manual edit program and I have 9 diameter to modify in each part, but I think for now it's the best solution! I didn't found anything to compensate taper in fanuc manuals, it's surprise me, there a lot of useless functions in these controllers!!

[sinha_nsit]

The same thing can be done using G90 also, with an appropriate value for R, to compensate for the taper. Actually, the machine would be doing taper turning which would result in straight turning if R is made equal to the taper which is seen in straight turning.
The G90 method would be desirable if there are a number of passes.