What's new
What's new

TL-1 G71 Question

r2784c

Plastic
Joined
Jul 28, 2022
Hey guys,

I ran a simple program using G71 canned cycle on a TL-1, and for some reason when I was done the diameter of the part was 40 thou undersized. Instead of 1.02" it was 0.980". All other dimensions were fine.

Here is the section of relevant code. I am focusing on the sign of the U (finish allowance) parameter, but after double checking I believe that positive is the correct sign. Not sure what is causing the undersize condition.

Any thoughts are much appreciated.


G54 G00 X1.6 Z0.1 (START POS)
G71 P10 Q20 U0.02 W0.01 D0.03 F0.01
N10 G41 G00 X0.8572 Z0.1 (BEG OF PROFILE)
G01 Z0.
Z-0.0714 X1.
Z-3.45
N20 G40 G01 X1.5 (END OF PROFILE)
 
Last edited:
Positive X finishing allowance in external machining is correct.
There can be an error in X tool offset.
Call the tool with offset, and do a straight turning at 1.0. check if you obtain 1.0
 
Hey guys,

I ran a simple program using G71 canned cycle on a TL-1, and for some reason when I was done the diameter of the part was 40 thou undersized. Instead of 1.02" it was 0.980". All other dimensions were fine.

Here is the section of relevant code. I am focusing on the sign of the U (finish allowance) parameter, but after double checking I believe that positive is the correct sign. Not sure what is causing the undersize condition.

Any thoughts are much appreciated.


G54 G00 X1.6 Z0.1 (START POS)
G71 P10 Q20 U0.02 W0.01 D0.03 F0.01
N10 G41 G00 X0.8572 Z0.1 (BEG OF PROFILE)
G01 Z0.
Z-0.0714 X1.
Z-3.45
N20 G40 G01 X1.5 (END OF PROFILE)
You should be using G42 not G41. For ID turning towards the chuck ( from Right to Left) TNR Comp is to the Right (G42), irrespective of whether the Tool is at the rear or the front of the machine. When the tools are at the back of the machine, its easy to visualize that the TNR Comp is to the Right and when the tool is at the front of the machine, its easy to mistakenly think that the tool needs to Compensate to the Left.

Right Hand OD Turning Tools at the back of the machine will be Upside Down and clearly, they have to be compensated to the Right. With the TL-1 and other machines that have the tool and X+ at the front of the machine, think as if the Tool Post and X+ axis were to be rotated from the rear of the machine, about the Centre Line of the machine, so that the Right Hand OD tool is now at the front of the machine with the tool now Upside Up. Effectively, the view by the operator is also rotated about the Centre Line of the machine, so that now the tool is being viewed from the floor looking up. From this viewpoint, its easy to see that the Compensation direction will still be to the Right of the Tool Path and therefore, G42.

Change G41 to G42 and your issues will be solved.

Regards,

Bill
 
Last edited:
Sinha. Double checked tool comp. All is well.

Bill, I agree that I need a G42, not G41. But I am still a little fuzzy on how for the profile I have programmed the G41 would result in the diameter of the part to be smaller. As I understand how the comp works, the machine either shifts the tool tip left (G41) or right (G42). Left being the -Z direction and right +Z.

With my program the chamfer and the final X move should be impacted by the erroneous G41 call, but the rest of the profile is just a -Z move. When moving solely in the z axis isn't tool comp essentially nullified until in reaches an intersection with a X movement?

Thanks
 
Your approach move turning on G41 puts the tool tip radius on the other side of your X value. That's why it's small.
 
Sinha. Double checked tool comp. All is well.

Bill, I agree that I need a G42, not G41. But I am still a little fuzzy on how for the profile I have programmed the G41 would result in the diameter of the part to be smaller. As I understand how the comp works, the machine either shifts the tool tip left (G41) or right (G42). Left being the -Z direction and right +Z.

With my program the chamfer and the final X move should be impacted by the erroneous G41 call, but the rest of the profile is just a -Z move. When moving solely in the z axis isn't tool comp essentially nullified until in reaches an intersection with a X movement?

Thanks
You have the wrong concept of TNR Comp with your description regarding Z only. Its Left or Right of the Tool Path. Imagine yourself walking along the tool path described by your program. The correct Tool Nose Radius Comp direction to use is the direction of the side of the tool path you have to walk so as to not step on the workpiece. With a Right Hand, OD Turning Tool, machining towards the Chuck, you have to walk to the RH Side of the Tool Path. With a machine that has the Cutting Tool and X+ at the front of the machine, as with your lathe, you have to view the Tool Path, walking upside down.

Its exactly as Booze suggests. Because you have specified G41 (Comp to the Left), the tool will cut on the Left Side of the Tool Path and that's where the workpiece is. Accordingly, the workpiece will be cut undersize.

Regards,

Bill
 








 
Back
Top