A Puzzle

[gcode]

I posted this on eMC and have stuck out so I thought
I take a break from the political wars and try it here

The machine is a Mori Seiki NT600, 2008 vintage horizontal 5X lathe

The post is from Postability and outputs solid code

The tool path is a simple 3+2 high speed 3D roughing toolpath.

This is the startup code.

When running this code the machine alarms out with a X axis overtravel

at the first motion after calling out G68.1

N6
(ROUGH 1ST DETAIL -B- 11.380 RADS)
G17
M45
T1012
( T12    -  .375 DIA. CARBIDE BULL MILL 1.0FL .03CR  -  H12.    -  D12    -  D0.3750 "  -  R0.0300 " )
G330
G361 B-40. D0.
T1013
G54
M69 (UNCLAMP C)
G28 H0.
U-2. W-2.
G49
G68.1 X.0001 Y0. Z0. I0. J1. K0. R50.
G43 H12.
G97 S7500 M13
G00 X2.6186 Y2.9491 C0. <---- The machine moves  +X -Z and over travels in X
Z10.
M68 (CLAMP C)
M8
Z4.5483

Vericut emulates this motion perfectly ... only the B axis blows through the roof

of the machine, stopping about 10 feet above the spindle

 

After much trial and error with Vericut I got it to run by making these edits

M69 (UNCLAMP C)
G28 H0.
U-2. W-2.
G49
G68.1 X.0001 Y0. Z0. I0. J1. K0. R50. <----- enable tilted tool plane
G43 H12.
G97 S7500 M13
G00  Y2.9493 C0 <---------- start the comped motion with Y and C axis only
X2.6186 Z10.         <----------- output the comped X and Z values
M68 (CLAMP C)
M8
Z4.5483

This runs perfectly  in Vericut and at the machine.

This makes no sense to me.

Can anyone shed some light on this?

I've gone back through proven files and we've run G68.1 toolpaths multiple times

with no issues at all.

I'm thinking a parameter in the machine ( and in Vericut) are not set properly.

[Jeff]

I've gone back through proven files and we've run G68.1 toolpaths multiple times

with no issues at all.

Can you load one of those older programs and see if you get the same result? Or would that not tell you anything?

[gcode]

Can you load one of those older programs and see if you get the same result? Or would that not tell you anything?

I put this up on eMC
Ron answered the question
I need a post edit

if Y = 0
first output should be
X Y C
Z

in Y does not equal 0
first output should be
Y C
X Z

It's seems stupid, but that is exactly the behavior I'm seeing
on the machine and a CGTECH built Vericut machine

 

[Jeff]

Ahh, I haven't been to that site but maybe 3 times since "the great exodus" took place.