G71 stock removal cycle

I am running a Citizen A20 with a Fanuc control and am trying to get a G71 stock removal cycle to work and am having trouble with it. The part has a radius on the end which transitions into a 8.5 degree taper and then into a .75 degree taper in a Z.528 long segment. I am not clear how to use the G71 but this is what I tried with the information I had.

(ROUGH FIRST SEGMENT)
G0 X.5 Z-.03
G71 U.04 R.02
G71 P1000 Q1010 U.003 W0 S1=#102 F#112 T02
N1000 G0 G41 X-.05
G1 Z0
X0
G2 X.0561 Z.0237 R.0278
G1 X.1226 Z.2463
X.12998 Z.52800
N1010 G40 X.5
T0

I am getting an alarm on the second G71 line that says, "PS0325 UNAVAILABLE COMMAND IS IN SHAPE PROGRAM " . I put a parenthesis around the G71 line to test the numbers and it ran just fine but I want the stock removal cycle so it doesnt take it all in one pass.

Does anyone have any suggestions for me or see something wrong with my code?

Jason

I've never used a Citizen machine before, but I've used Fanuc controllers on several different brands of machines. The first thing that looks out of place to me is the first G71 line. I've never seen that used in a G71 cycle. Also, the "S1=#102" looks odd to me. I'm not sure what the S1 represents. The G71 should have an address that represents the depth of cut per pass, which I've always known to be "D". And I don't believe the "=" is allowed. If "S1" is supposed to represent your depth of cut, I would suggest the format below. But like I said, I have no experience with Citizen machines. Hope this helps

(ROUGH FIRST SEGMENT)
G0 X.5 Z-.03
G71 U.04 R.02
G71 P1000 Q1010 U.003 W0 D#102 F#112 T02
N1000 G0 G41 X-.05
G1 Z0
X0
G2 X.0561 Z.0237 R.0278
G1 X.1226 Z.2463
X.12998 Z.52800
N1010 G40 X.5
T0

Thanks for trying to help. The first G71 line sets the depth of cut with the U.040. The S1=#102 defines the spindle RPM for spindle one. This is unique to the Citizen Swiss machines.

Try to command the special spindle commands and T-codes just before the G71 canned cycle. Also try giving it a specific feedrate and not a macro variable.

Here's the format that works for me:

Quote:

---

G71 U.187
G71 P101 Q102 U.01 W.004 F.018
N101 G0 X7.6726
G1 Z-.1837 F.012
X7.8526 Z-.2737
G3 X7.88 Z-.3068 R.0468
N102G1 Z-2.45

---

Let us know what you come up with

Never used a Swiss machine, but have used a few different Fanuc controls. I know for a fact that an OT control will not accept a 3 digit variable number for the F code in a G71. I have a little macro program that allows me to run any size material with one program. The feed output is #116. What I do is make #1=#116 just before the G71 call and use F#1 to get around that problem.

Quote:

---

Originally Posted by jmichaud1

I am running a Citizen A20 with a Fanuc control and am trying to get a G71 stock removal cycle to work and am having trouble with it. The part has a radius on the end which transitions into a 8.5 degree taper and then into a .75 degree taper in a Z.528 long segment. I am not clear how to use the G71 but this is what I tried with the information I had.

(ROUGH FIRST SEGMENT)
G0 X.5 Z-.03
G71 U.04 R.02
G71 P1000 Q1010 U.003 W0 S1=#102 F#112 T02
N1000 G0 G41 X-.05
G1 Z0
X0
G2 X.0561 Z.0237 R.0278
G1 X.1226 Z.2463
X.12998 Z.52800
N1010 G40 X.5
T0

I am getting an alarm on the second G71 line that says, "PS0325 UNAVAILABLE COMMAND IS IN SHAPE PROGRAM " . I put a parenthesis around the G71 line to test the numbers and it ran just fine but I want the stock removal cycle so it doesnt take it all in one pass.

Does anyone have any suggestions for me or see something wrong with my code?

Jason

---

Hi Jason,
Although this Thread has a bit of age about it, but did you find a resolve for your problem? If not, I suspect that the "S1=" is the issue.

Unless S1 itself is a Variable created by the MTB, then I believe the syntax should be S1#102

Although S and T arguments can be included in the G76 block, its much more common practice to call the Tool and Spindle Speed prior to the G71 cycle being launched. Accordingly, I'd do as suggested by "rpm3000", and specify these two addresses before calling the roughing cycle.

If you did find a resolve, it may be of interest to others with the same type of machine to know the answer.

Regards,

Bill

hi sir
we get alaram stock removal in G71 PS0325UNAVAILABLE COMMAND IN SHAPE PROGRAM
G71U1.R1.
G71P10Q20U.3W.2F.25
N10GOX77
G1G42X78..F.15
Z0.02
X80.W-1.F0.05
Z120.F.2
X128.
X130.W-1.F0.05
X140
N20G0G40U2.Z2.

Quote:

---

Originally Posted by Ram123

hi sir
we get alaram stock removal in G71 PS0325UNAVAILABLE COMMAND IN SHAPE PROGRAM
G71U1.R1.
G71P10Q20U.3W.2F.25
N10GOX77
G1G42X78..F.15
Z0.02
X80.W-1.F0.05
Z120.F.2
X128.
X130.W-1.F0.05
X140
N20G0G40U2.Z2.

---

I see 2 problems as posted. Block N10 has the letter O instead of number 0. X78 has 2 decimal points after it. I've never used G41/G42 so I don't know if there is a problem with that. I assume you have used G71 cycles on this lathe before. If not, maybe it takes a 1-block instead of a 2-block call. How old is the lathe? All newer ones I've ever programmed all use the 2-block call.