[deputydawg]

On our ST40-L, we frequently see tools cutting about 1/8" differently than programmed (possibly 4x TNR). Pressing reset, and restarting the process results in an accurate cut. Haas technicians are working with us on this issue, but lead us to believe this has never occurred before. If it is a programming issue involving compensation, it should still cut exactly the same each time, yet it doesn't. Has any one run into this situation before?

[Machineit]

You say "Pressing reset, and restarting the process," but does that mean you are restarting the program or restarting the machine?

If you mean that you are restarting the machine, I would look for an encoder problem/error.

If you are just restarting the program, then I would look for a programming error, like accumulating G91 moves.

What is your level of experience with this machine and how are you programming?

Good Luck----Mike

[cncfixxer]

I've had pre-load issues causing excessive backlash on some Bridgeport VMC's , Once the machine changed direction the position was not accurate. You may want to confirm your ball screws condition ... just a thought

[underthetire]

I would write a simple repeatability program to a test indicator and see what's going on. Then do the same test but index the turret in the test. 1/8" is a lot, not something like backlash. When you re start, are you also re zero returning the machine?

[ROBBY 68]

Sir
I've seen same issue on some ST machines, double check parameters for X axis.
There should be a thermal compensation value that isn't right.
Ask the Haas guys to verify this for you against original parameter list.
You'll find it there.
It is not related to programming or mechanical problem.
Robby

[deputydawg]

The machine was new this spring. Our prior lathe was "Fanuc compatible", so the old programs just need minor editing to run. It's not an issue of not cutting to the right diameter, but literally not cutting to the programmed diameter. We don't use G91, but Mike's thoughts about something accumulating seem possible since we get accurate results simply by re-running the process without any changes. This process for example sometimes does not finish the bore at 11.1", and the display shows that it is about 1/8" off. I see that the X value is the same when G41 is activated, but if that is the cause, would that make it run correctly most of the time, but not every time?

N06 (FINISH BORE)
T1010 M08
G00 X21.2 Z0.8075
Z0.1
G96 S1000 M03
G01 G41 X21.2 Z0. F0.006
X21.0625
G02 X13.128 Z-1.2492 I1.1688 K-10.636
G02 X11.1 Z-2.9599 I0.936 K-1.7107
G01 Z-6.5
X11.
G00 G40 Z.1
X23.7Z15.
M05
T1000M09
M01

[Machineit]

I assume you are running a main and a sub program since you are talking about multiple parts, but you are only listing one section. Post it all and we will be able to see where it accumulates maybe.

Mike

[deputydawg]

Here is the program from the lathe. The Back Face process was programmed to rapid in .100" away on X, but crashed into the part because it wasn't at the programmed diameter, so the operator changed that. The Rough Bore process does a tracer pass at the end, and stops at X 10.3", not 10.2" as programmed. Both the Finish OD, and Finish Bore sometimes leave about 1/8" on the X.

%
O00013 (CMS0013 FRONT COVER)
G54
G40
M41
G50 S300
T202
G00 X22.4 Z0.5
T202 M08 (ROUGH FACE)
Z0.41
G96 S800 M03
G72 P10 Q20 W0.01 D0.06 F0.014
N10 G00 Z0.
G01 X18.75
N20 Z0.1
G00 X23.
M05
T200 M09
M01

N1 (ROUGH OD)
G54
T202 M08
G00 X23.8 Z0.1
G96 S800 M03
G71 P30 Q40 D0.1 F0.014 U0.03 W0.01
N30 G00 X21.0375
G01 G42 Z0
X21.0625 Z-0.0125
Z-0.7473
X21.119
Z-1.1535
X23.225
X23.25 Z-1.166
Z-2.45
N40 X23.9
G00 G40 Z0.1
X24. Z15.
M05
T200 M09
M01

N2 (BACK FACE)
G54
T606 M08
G00 X23.9 Z0.1
Z-2.4
G96 S800 M04
G72 P50 Q60 D0.06 F0.014 W-0.01
N50 G01 X23.9 Z-1.7688 G42
X23.28
X23.255 Z-1.7813
X19.8
N60 Z-1.88
G00 X23.9
G40 Z0.1
X23.7 Z15.
M05
T600 M09
M01

N3 (ROUGH BORE)
G54
T1010 M08
G00 X10.3 Z0.1
G96 S800 M03
G71 P70 Q80 D0.1 F0.014 U-0.03 W0.01
N70 G00 X21.2
G01 G41 Z0.
X21.0625
G02 X13.128 Z-1.2492 I1.1688 K-10.636
G02 X11.1 Z-2.9599 I0.936 K-1.7107
G01 Z-6.85
N80 X10.2
G00 G40 Z0.1
G00 X23. Z15.
M05
T1000 M09
M01

N4 (FINISH OD)
T202 M08
G00 X21.0625 Z0.1
G96 S1000 M03
G00 X21.0375
G01 G42 Z0 F0.006
X21.0625 Z-0.0125
Z-0.7473
X21.119
Z-1.1535
X23.225
X23.25 Z-1.166
Z-1.85
X23.35
G00 G40 Z0.1
X23.7 Z15.
M05
T200 M09
M01

N5 (FINISH BACK FACE)
T606 M08
G00 X23.35 Z-1.88
G96 S1000 M04
G00 Z-1.7688
G01 G42 X23.25 F0.006
X23.225 Z-1.7813
X19.8
Z-1.88
G00 G40 X23.35
X23.7 Z15.
M05
T600 M09
M01

N6 (FINISH BORE)
T1010 M08
G00 X21.2 Z0.8075
Z0.1
G96 S1000 M03
G01 G41 X21.2 Z0. F0.006
X21.0625
G02 X13.128 Z-1.2492 I1.1688 K-10.636
G02 X11.1 Z-2.9599 I0.936 K-1.7107
G01 X11.101 Z-6.85
X11.
G00 G40 Z0.1
G00 X23.6 Z15.
M05
T1000 M09
M01

N7 (RELIEF GROOVE)
T1212 M08
G00 X21.22 Z-1.1535
G96 S600 M04
G01 X21.12 F0.003
X21.0625
X21.22
G00 Z-1.0593
G01 X21.12
X21.0625
Z-1.1535
X21.22
G00 Z0.1
G00 X23.7 Z15.
M05
T1200 M09
M30
%

[haastec]

I would write a simple repeatability program to a test indicator and see what's going on. Then do the same test but index the turret in the test. 1/8" is a lot, not something like backlash. When you re start, are you also re zero returning the machine?

Definitely do something like this. Make something simple with very few variables to help track down the issue.

If the machine runs good with a simple/basic program, then start comparing what is different and how the machine is reacting to the differences.
If it does not run good with a simple/basic program then check your parameters as was mentioned already.

Good luck and keep us posted!

[deputydawg]

The machine does not always run good with a simple program. A Haas Technician is going to update the software to the latest version tomorrow. I will mention the parameters to him when he is here. If it is a parameter set wrong, I would thick it would perform wrong every time start is pressed, but I've assumed wrong before. Thanks for the input, I'll keep you posted.

[deputydawg]

This morning, the Haas Technician loaded the software to fix the cutter comp issue. Thus far, all is well.

[deputydawg]

It's been about 6 months and our ST-40L is still running well after the software upgrade. Although the problem was a result of their Software Project #46614, which caused it to sometimes use an incorrect tool offset, they only corrected it, and did not address the $10,000+ of scrap and several late deliveries that resulted due to their software glitch.