What's new
What's new
By:
Advanced search…

Haas TL Lathe Compensation problems

M

Marcusdad

Plastic
Joined
Apr 20, 2020
Good morning
I have a question regarding a strange problem with our TL2 lathe. Whenever I program using the TNR compensation G42 for turning a part I have a problem with the Z value. On the final pass and the G70 cycle, the tool radius is added to the Z length of the part. For example. If I have a simple part that’s turned back to Z-2.500” it will rough out to 2.497” as I’m leaving .003” on the W value in the G71 cycle, but on the final pass, it will add .031” to the length. The .031” is the tool radius being used in the offset. The machine somehow is adding the .031” to the length only, diameters ( X values) are fine and unaffected. So instead of finishing at Z-2.500” it will finish at Z-2.531”, which causes a bump. Why is this adding to the Z-axis only? I tested some older programs that I ran successfully months ago and now these are also affected.
Could this be a parameter setting that got changed in error? In case I was making a programming mistake, I entered a sample program from the HAAS manual and it does this same strange action.
Any help you could send me will be greatly appreciated.

Best regards,
 
Are you using a tool tip number? I don't know if Haas lathes use them, but it sounds like it may be using tool tip 8.
 
That is how TNR supposed to work.
You normally want to plan your ramp-off move accordingly, but would need to see your actual code.

For the record, I love G70 cycle and use it just about always.
I absolutely despise the G71, and never ever use it.

With that said, the following code:
G00 G42 X0 Z.1
G01 Z0
G01 X1.
G01 X1. Z-1.5 ( tool is at Z-1.5 )
G01 X2.
G01 G40 X2. Z.1

vs.

G00 G42 X0 Z.1
G01 Z0
G01 X1.
G01 X1. Z-1.5 ( tool is at Z-1.531 )
G01 G40 X2.



Note the difference in the G40 placement.

Oh, and one another thing. Yes, Haas uses tool tip directions, and you should be at Dir 3 ( kinda F'd up Haas method on the TL, but ... )
Looks like you have it set correctly as with Dir 8 your overtravel would be .062 .
 
As mentioned earlier, i think you are cancelling cutter comp to early. I don’t cancel it until i am completely off the part at least double the tnr amount.
 
Marcusdad said:
Good morning
I have a question regarding a strange problem with our TL2 lathe. Whenever I program using the TNR compensation G42 for turning a part I have a problem with the Z value. On the final pass and the G70 cycle, the tool radius is added to the Z length of the part. For example. If I have a simple part that’s turned back to Z-2.500” it will rough out to 2.497” as I’m leaving .003” on the W value in the G71 cycle, but on the final pass, it will add .031” to the length. The .031” is the tool radius being used in the offset. The machine somehow is adding the .031” to the length only, diameters ( X values) are fine and unaffected. So instead of finishing at Z-2.500” it will finish at Z-2.531”, which causes a bump. Why is this adding to the Z-axis only? I tested some older programs that I ran successfully months ago and now these are also affected.
Could this be a parameter setting that got changed in error? In case I was making a programming mistake, I entered a sample program from the HAAS manual and it does this same strange action.
Any help you could send me will be greatly appreciated.

Best regards,
Click to expand...

Hello Marcusdad,
As others have stated, the departure move from TNR Comp needs to be planned, as much as the Start Up needs to be planned. Invariably, you will have fewer issues if you can cancel TNR Comp when the tool is clear of the workpiece, however, if this can't be done, then the Vector of the next element of the workpiece can be specified in the G40 Block with I and K

G00 X50.0 Z3.0
G42 G00 X48.0
G01 X48.0 Z-10.0
G01 X54.0 Z-23.0
G01 Z-50.0
G40 X60.0 Z-48.0 I5.0 K-5.0

The above departure from TNR Comp describes an element of the workpiece at 45degs from the last coordinate visited when in TNR Comp Mode (X54.0 Z-50.0). "I" in the I and K set is specified as a radius value.

SeymourDumore said:
For the record, I love G70 cycle and use it just about always.
I absolutely despise the G71, and never ever use it.
Click to expand...

Hello SeymourDumore,
G70 is a finishing Cycle, normally used in conjunction with G71, G72, G73 Roughing Cycles. Are you just using it to execute code earlier in the program and then return to from whence the G70 Cycle was executed?

Regards,

Bill
 
Last edited:
Bill

Dohhh...
Just re-read my post and realized that I'm dyslexic.
Of course I meant the other way around. :dopeslap:
 
You must log in or register to reply here.

Similar threads

M
G37 (Measure Tool Offset) Does Not Update Offsets
2
Replies
23
Views
677
rjwalker1973
rjwalker1973
Z
Okuma tool nose compensation
Replies
6
Views
185
zschary
Z
J
Lathe form tool program help.
Replies
16
Views
965
EmGo
EmGo
M
how to write a program to check tool diameter with Renishaw NC4
Replies
0
Views
256
Mavs84
M
G
Sample Servo Bar program for multiple parts
Replies
7
Views
535
rjwalker1973
rjwalker1973








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top