[jdgromi]

Hello dcoupar

I have try your modifications and the result still a sharp edge.

10 G0 X1,6 Z,06
20 G71 U.06 R.02
30 G71 P40 Q70 U.04 F.01
40 G0 G42 X1.42
50 G1 Z0 F,008
60 G3 X1,5 Z-.04 R.04
70 G1 X1,6
80 G70 P40 Q70
90 G0 G40 X4 Z3 M30

Is it possible that a parameter of controller would be wrong?

Best regards
J-D

[dcoupar]

Please try one more thing:

10 G0 X1,6 Z,06
20 G71 U.06 R.02
30 G71 P40 Q70 U.04 F.01
40 G0 G42 X1.35
50 G1 Z0 F,008
55 X1.42
60 G3 X1,5 Z-.04 R.04
70 G1 G40 X1,6
80 G70 P40 Q70
90 G0 X4 Z3 M30

[jdgromi]

Hello dcoupar

I have fixe my problem like this
10 G0 X1,6 Z,06
20 G71 U.06 R.02
30 G71 P40 Q70 U.04 F.01
35 G42
40 G0 X1.36
50 G1 Z0 F,008
60 G3 X1,5 Z-.07 R.07
70 G1 X1,6
75 G40
80 G70 P40 Q70
90 G0 X4 Z3 M30
I NEED A RADIUS .04, I HAVE A RADIUS OF 0.03 ON MY INSERT
THE SUMM OF TWO = 0,07 FOR R IN MY PROGRAM
Is it OK?

[angelw]

Hello dcoupar

I have fixe my problem like this
10 G0 X1,6 Z,06
20 G71 U.06 R.02
30 G71 P40 Q70 U.04 F.01
35 G42
40 G0 X1.36
50 G1 Z0 F,008
60 G3 X1,5 Z-.07 R.07
70 G1 X1,6
75 G40
80 G70 P40 Q70
90 G0 X4 Z3 M30
I NEED A RADIUS .04, I HAVE A RADIUS OF 0.03 ON MY INSERT
THE SUMM OF TWO = 0,07 FOR R IN MY PROGRAM
Is it OK?

What you have done, is that you have created a program with coordinates that don't require Tool Nose Radius (TNR) compensation. As you have still specified G42 in your program, I suspect that you have incorrect data registered in the associated offset registry, or that you're calling an offset that has a zero value for the TNR.

One thing to remember, is that not all Fanuc controls will interpret TNR compensation in a G71 cycle, but the G70 cycle does. Accordingly, using G41/G42, and the corresponding coordinates that don't take into account of the TNR, in a G71 roughing cycle is allowable so long as there are no concave forms where the back of the tool will over-cut. It just means that the finish cycle will have to take more material in areas that are effected by TNR compensation.

In your latest listing of your program, you can drop the G42 altogether and you will achieve a 0.04 radius. When programming a radius and taking into account the radius of the tool, you do as you have done in your example and effectively program the TNR centre relative to the centre of the arc required.

Cutter Radius Compensation is just about mandatory on a machining centre, as its via this function the size of features can be regulated when using the periphery of end mill type cutters.

In contrast, size of a turned workpiece is overwhelmingly regulated by the X Wear or Geometry offset and not the TNR of the tool being used. As the calculations to incorporate the TNR in the actual program are relatively simple when manually calculated, and somewhat irrelevant, in terms of difficulty, when a CAM system is used to generate the program, I practically never use TNR compensation when programming for a lathe. The only advantage of using TNR compensation, in my opinion, is that the physical TNR of the cutting tool can be changed without having to reprogram the tool path. And a major negative is that in most Fanuc controls TNR compensation is not considered in the G71 roughing cycle, which will lead to grief if the profile contains any concave forms.

Regards,

Bill