[glbreil]

When setting up a single block G71 turning cycle or G72 facing cycle is it the line prior to the G71/G72 that determines the stock size and how much metal needs to be removed?

G00 X1.300 Z.1
G72 P2 Q3 U0 W0 D00100 F.012
N02 G00 Z0
N03 G01 X0

So in this example is it correct that it is going to face off .1" in .010" passes and if I changed the first line to read G00 X1.300 Z.050 that it would then face off .050"?

Thanks Gary

Oh, and does the D word need the leading zeros or would 100 do the same thing?

Thanks again, Gary

[sinha_nsit]

z clearance would result in air-cutting at the specified depth of cut.
Similarly, in G71, X clearance would give air-cutting till the OD of the workpiece is reached.
I do not give X clearance in G71, and Z clearance in G72.
I use 2-line cycles. I believe 1-line cycles would do the same.
So, the answer to your question is YES.

[fordav11]

a simpler way to look at it is when using G71 position the start X point at the same diameter as the material size and position the Z start point in front of the material by about 0.05" or so
with G72, position the start X point above the material size by about 0.1" and position the Z start point in line with the face of the material
this results in no air cutting when using G71/G72

[glbreil]

Thanks for the replies and I understand about the air cutting, I was just trying to make sure I understand what tells it the actual cutting start point.

So that brings me to one more question. Say I have faced off a new piece of stock using G72 and now with the same tool for simplicities sake I want to transition to G71 and turn the profile. What is the best way to transition from one to the other. Is it as simple as doing a rapid move to the new starting point and calling the G71 or does the previous cycle need to be canceled in some way?

Thanks Gary

[sinha_nsit]

Just call G71 after changing the start position suitably.

[sinha_nsit]

Maybe I should elaborate more ...
G codes are grouped into various groups based on similarly in their functionality. G codes belonging to group 0 are one-shot or non-modal codes. These remain active only in the block they are called. If needed again, they would need to be commanded again. All other G codes are modal codes. These remain active till replaced by some other code from the same group. At anytime one code from each group remains active (except Group 0 codes).
G70-G76 belong to Group 0. Therefore these automatically get cancelled in the next block.