[GITRDUN]

Been probably 20 years since i have done any serious programming on a Fanuc lathe control so i need a little help.
Can someone explain to me what im doing wrong? I want the machine to rough an OD down to size leaving a small amount for finish pass. Everything works fine except i am getting an extra rough pass that takes 0.0 depth of cut before it runs the finish pass.
Here is an example program of what i am doing.

T0101 M3 S500 M8
G00 X5. Z.1
G71 P1 Q2 U.05 D.1 F.012
N1 G0 X4. Z.1
G1 Z0
N2 X5. Z-1.
G70 P1 Q2
G28 X6. Z2.
M30

What happens is it moves to X5. Z.1, then moves to X5.05 to add for the finish allowance, then moves to X4.85 and begins roughing at .2 per pass. But regardless what the DOC is it always makes a last roughing pass at X4.05, then makes another pass at X4.05, then runs the finish pass at X4. .
If i leave out the finish allowance and G70 finish line it will make a final roughing pass at X4., then make another pass at X4. .

Dont know what im missing.

[sinha_nsit]

I will confirm later, but I think this is normal behavior for type II which does not leave steps like what type I does.
Delete Z1 from N1 line, to invoke type I, and you will not see any overlapping motion.

[fordav11]

In Type II there is no last pass. Because the cuts blend out there are no steps so a final clean-up pass isn't needed.
I seem to recall this behavior is a bug in the software.
It shouldn't make 2 passes at the same diameter.
If you can get access to a later rev of the software then upgrade it, otherwise there's not much you can do to fix it.

[angelw]

Been probably 20 years since i have done any serious programming on a Fanuc lathe control so i need a little help.
Can someone explain to me what im doing wrong? I want the machine to rough an OD down to size leaving a small amount for finish pass. Everything works fine except i am getting an extra rough pass that takes 0.0 depth of cut before it runs the finish pass.
Here is an example program of what i am doing.

T0101 M3 S500 M8
G00 X5. Z.1
G71 P1 Q2 U.05 D.1 F.012
N1 G0 X4. Z.1
G1 Z0
N2 X5. Z-1.
G70 P1 Q2
G28 X6. Z2.
M30

What happens is it moves to X5. Z.1, then moves to X5.05 to add for the finish allowance, then moves to X4.85 and begins roughing at .2 per pass. But regardless what the DOC is it always makes a last roughing pass at X4.05, then makes another pass at X4.05, then runs the finish pass at X4. .
If i leave out the finish allowance and G70 finish line it will make a final roughing pass at X4., then make another pass at X4. .

Dont know what im missing.

Hello GITRDUN,
I suspect that the control is a FS10 to FS15 due to the single G71 block format in your example. The format for these controls included a Rough Cutting Margin, specified with I and K addresses, in addition to the Finish Allowance specified with U and W. When using Type II G71 cycle, irrespective of whether a Rough Cutting Margin is specified, a Rough Cutting finish cut is performed, leaving the Finish Margin specified by U and W, after all Roughing Cuts have been completed. Accordingly, the action of the the cycle as you've described is performing as it should.

Regards,

Bill

[GITRDUN]

Aha, that makes sense. I will try that out and see if thats the problem. I didnt see any reference to an I and K value in anything i read about G71 cycle. I am remembering why i never liked Fanuc. But then again i was raised on Okuma G code which always seemed much less technical to me.

[GITRDUN]

That was it. I switched the U in the G71 line with an I and removed the G70 line. Runs perfect.

[angelw]

That was it. I switched the U in the G71 line with an I and removed the G70 line. Runs perfect.

Hello GITRDUN,
That may be an acceptable work around for you, but it circumvents being able to make a finish pass with a different (finishing) tool, as no Finish Allowance is being left.

Regards,

Bill

[GITRDUN]

If a seperate tool needs to be used or the RPM or feedrate needs to be changed for the last pass you can still put a U value on the G71 line and use the G70 finish pass. No need for it in most cases for what we do but will need to be used occasionally.

[lenny09]

I am having the same issue with a Fanuc 32i-Model A

If I add the WO on my N1 line it will make an extra pass for no reason.
If i remove the WO from N1 line. Tool path runs fine except it will leave steps on my angles and clean them up on the last pass.
I'd rather run it with no steps but i'm having the repeat last pass issue.

Any help on fixing this would be greatly appreciated.

G0X6.45Z.15T0101
M8
Z.0366
G96S600
G71U.2R.025
G71P1Q2U.02W.005F.016
N1G1X3.9701W0
Z.0316F.016
X4.1717Z-.0692
G3X4.19Z-.0912R.0313
G1Z-1.0783
X4.5017Z-1.2342
G3X4.52Z-1.2562R.0313
G1Z-4.1
N2X6.45
G0
Z.15M5

[sinha_nsit]

As suggested by Bill, insert I,K apart from U, W.
The manual does not explain it well.

[lenny09]

Ok I tried the suggested but no luck.


Did the following.

G0X6.45Z.15T0101
M8
Z.0366
G96S600
G71I.2R.025
G71P1Q2I.02K.005F.016
N1G1X3.9701W0
Z.0316F.016
X4.1717Z-.0692
G3X4.19Z-.0912R.0313
G1Z-1.0783
X4.5017Z-1.2342
G3X4.52Z-1.2562R.0313
G1Z-4.1
N2X6.45
G0
Z.15M5