[eng101]

Hello, after taking a skim cut I measure and enter the diameter and press X dia measure.

But, when I run the program the tool does not even come close to the material. the z axis offset is fine. Am I missing some thing? Are there any Prep G code I should place at the begining of the program or is there a setting I need to change?

[txcncman]

Touch tool to known diameter or make a cut. Back off in Z only. Measure diameter. Press X Diameter Measure. Follow prompts. Input measured diameter and press Write.

[djm77]

Take your cut, wind clear in Z only. Take measurement. Press X dia Measure, then input your known diameter and hit write/enter. If you are doing it the other way around it will only have the 'X dia measure' dimension in the offsets page.

[KenFoulks]

Both answers are correct.

You are entering the diameter, then pressing X DIA MEAS. Press X DIA MEAS first, then enter the diameter, then press WRITE/ENTER.

[eng101]

Thanks all. Pressing X measure first, enter Diameter, Press read/write works.
Next Problem, After roughing using G71 finish pass is over cutting about .03 in the Z-axis. Any ideas, I have attached the program.

[txcncman]

What value are you putting in for tool nose radius for each tool? Saying it is over cutting in Z means little without a part print to compare the program to.

[Geof]

In addition to entering the tool nose radius you also have to enter the Tip Code for the Tool Tip Orientation and direction. You should find this mentioed around page 58 of your manual. The wrong Tip Code can result in overcutting.

[eng101]

Well, when I call up T0101 and MDI G00 Z0.00 the tool goes to the zero face of the part. The tool nose radius is set @.0312 and I am using tool tip 2.
This being a TL1 lathe the tool holder is located -X of the center of the spindle. Given a basic roughing cycle such as this, what would cause over cut of the z axis only. This cycle is only roughing step cuts.

[txcncman]

Still no part print.

If last line of cycle is a Z move, it will cut a straight line using the quadrant of the tool tip touching the radius of the part. Yes? So any resulting shoulder will measure an additional tool nose radius longer.

[garylb]

and I am using tool tip 2.
Th

shouldnt it be tip code 3 for od turning not 2?

I have a TL2 and use tip code 3 for od and 2 is for id

[djm77]

I think it should be tool tip position 3 also.

The other thing I noticed, is that you are using G41. If you are OD turning which it looks like you should be using G42. The Toolroom lathes are a bit back to front when looking at TNC. The graphics are the same, with them both being set up as though the tool was at the back of the machine as in our SL30 not at the front.

I also noticed that you use G40 on the X movement on the last line of your G71 cycle. This may be causing the TNC to be turned off on the line before which is your last Z movement. (Not certain about this though)

I don't turn my TNC off within my canned cycle, I do it when sending it home so my last X movement in my G71 cycle allows for the TNC, ensuring that all my Z's are correct.

I would think the most likely thing is the Tool Tip position needing to be 3 and your TNC to be G42

[andre_77]

G00 Z0.08 X3.15
G71 P101 Q102 U0.0156 W0.005 D0.031 F0.012
N101 G42 G00 X0.9425
G01 Z-0.787
X1.2598
Z-1.494
X1.7306
Z-1.888
X2.563
Z-3.315
X3.15
N102 G40 G01 X3.25
M05

[KenFoulks]

I would think the most likely thing is the Tool Tip position needing to be 3 and your TNC to be G42

This is correct. Change these two things and you should be good to go.