Need programming help: 041 Interference in NRC on Fanuc 21i-TB lathe G71/70

Hi All

I have an Ajax apollo lathe with a Fanuc 21i-TB control and am attempting to profile the attached part using the following program section;

(PROFILING TOOL);
;
T0808 G96 S1200 M3;
G0 G40 G95 X47. Z1. M8;
G4 U1.;
G71 U1. R.1;
G71 P10 Q20 U.1 W.05 F.3;
N10 G0 G42 X0. Z1.;
G1 Z0. F.15;
G3 X27.71 Z-24. R16.;
G1 X24.06 Z-27.16;
G2 X28. Z-34. R4.94;
G1 X45. Z-38.5;
X46. Z-39.;
N20 G0 G40 X47.;
G70 P10 Q20;
G0 Z50.;
M9 G40;
M5 G30 U0 W0;
M30;

The tool I have is a dnmg 93degree turning tool with 0.8 tip radius, and is setup as type 8.

The Interference in NRC error happens when the program gets to the G70 command. The G71 roughing cycle seems to work fine.

I am not a professional programmer, i usually only do simple programs. This is the first time that i have tried machining an undercut and used type 2 roughing cycle.

I have seen a couple of old posts about this error, but they didnt help.

I have tried moving the G42 command outside of the roughing cycle, just after the dwell line, and messing with additional moves when I call G42, but cant fix the problem.

Any help would be appreciated.
Thanks,
Tom

NearEnuff said:

Hi All

I have an Ajax apollo lathe with a Fanuc 21i-TB control and am attempting to profile the attached part using the following program section;

(PROFILING TOOL);
;
T0808 G96 S1200 M3;
G0 G40 G95 X47. Z1. M8;
G4 U1.;
G71 U1. R.1;
G71 P10 Q20 U.1 W.05 F.3;
N10 G0 G42 X0. Z1.;
G1 Z0. F.15;
G3 X27.71 Z-24. R16.;
G1 X24.06 Z-27.16;
G2 X28. Z-34. R4.94;
G1 X45. Z-38.5;
X46. Z-39.;
N20 G0 G40 X47.;
G70 P10 Q20;
G0 Z50.;
M9 G40;
M5 G30 U0 W0;
M30;

The tool I have is a dnmg 93degree turning tool with 0.8 tip radius, and is setup as type 8.

The Interference in NRC error happens when the program gets to the G70 command. The G71 roughing cycle seems to work fine.

I am not a professional programmer, i usually only do simple programs. This is the first time that i have tried machining an undercut and used type 2 roughing cycle.

I have seen a couple of old posts about this error, but they didnt help.

I have tried moving the G42 command outside of the roughing cycle, just after the dwell line, and messing with additional moves when I call G42, but cant fix the problem.

Any help would be appreciated.
Thanks,
Tom

Click to expand...

Hello Tom,
Unfortunately, when using TNR Comp at the control, things can't be NearEnuff.

Even without the Interference Error, the part will not come out as you would like and expect. Starting from X0.0 will result in a tit at the start of the Ball, With a 0.8 TNR it would have to be at least X-1.6 (X-1.61) and then a Linear Move to X0.0 before stating your first Circular move.

The reason the alarm is not being raised in the G71 Cycle is that TNR Comp is ignored in that Cycle and executed in the G70 Cycle. Because your cutting a profile with a Concave Feature, the area of the Ball past 12 o'clock will be over-cut by the trailing edge of the Tool and therefore, the part is Toast before the G70 Cycle is executed. Accordingly, you will have to either specify a quite large Finish Allowance with "U" to try and avoid the over-cut. The W0.05 is only exacerbating the over-cut, or and this would be the best solution, calculate your program profile with compensation for the TNR included in the Profile Path.

The last moves in your profile path, as shown in the code snippet following, are 0.50 radially in X, while the TNR is 0.8.

G1 X45. Z-38.5;
X46. Z-39.;
N20 G0 G40 X47.;

That is not going to work and I suspect that's what is raising error.

Following is a Roughing/Finishing Profile that will work. Set the Tool up as a Type 03, ie, the Leading edge of the Insert for Z and the point on the TRN closest to the machine Centre Line for X.

G00 X47.0 Z10.0
G00 X47. Z2.0 F1.0
G71 U1. R.1;
G71 P10 Q20 U0.5 W.05 F0.3;
N10 G00 X-1.600 W0.0
G01 X-1.600 Z0.000 F0.20
G03 X27.493 Z-25.202 I-0.000 K-16.800
G01 X23.844 Z-28.361
G02 X27.140 Z-34.091 I3.585 K-2.070
G01 X44.361 Z-38.649
G01 X46.663 Z-39.800
N20 G01 X47.0
G70 P10 Q20
G0 Z50.0 M09
M5 G30 U0.0 W0.0
M30

0.1 Finishing Allowance is too small for a 0.8 TRN. If your were cutting Mild Steel, you would probably find that the surface finish was not great. Also when using the G71 Cycle were a Concave Feature is included in the Profile, you usually have to increase the Finish Allowance in X if a Finish Allowance is specified as a + value in Z. The Finish Allowance in Z in not applied in both directions, only the direction specified by the W value in the second G71 Block. Accordingly, a Z+ Finish Allowance may cause over-cutting with the Trailing Edge of the Tool in Concave Features if not enough X Finish Allowance is specified.


Regards,

Bill

Thanks Bill,
Great explanation, way more detailed than I was expecting.
I see where i am going wrong.
I shall try that program, calculating the toolpath seems a sensible way to save a lot of headaches with tnr alarms.
This job was a bit beyond my capabilities, but i am learning (hopefully).

Thankyou again.
Tom

This will help in learning G71/G72 ...
https://www.amazon.com/dp/B01FOPN3RW