Live tooling toolpath feed not correct

[JJackrabbit]

Got something strange going on in the millturn siemens post.

I have a part and do some axial 2d adaptive with live tooling.

Runs perfect

after 2d adaptive a 2d contour is finishing it

The 2d contour is perfect and spot on

But once I run/post the two toolpaths in the same program, issues happen.

The 2D adaptive runs fine but once it start with the 2D contour. It goes full speed mode over the contour.

When posting the toolpaths in separate programs...both run fine.

This is the code when posting both toolpaths in the same program.

N13044 X-26.876 Y-69.659 Z40.846
N13045 X-26.88 Y-69.665 Z40.95
N13046 G0 Z76
N13047 TRAFOOF
N13048 DIAMON

N13049 MSG ("; 2D Contour1")
N13050 DIAMOF
N13054 G0 C4=0.
N13055 TRANSMIT
N13057 G1 X-83.138 Y18.066 Z76 F1500
N13058 G0 Z66
N13059 G1 Z62 F1000
N13060 Z40.8
N13061 X-83.131 Z40.696 F800
N13062 X-83.111 Y18.067 Z40.593
N13063 X-83.077 Y18.069 Z40.494
N13064 X-83.031 Y18.072 Z40.4

And this is the code when posting the 2d contour in a separate program.

N16 MSG ("; 2D Contour1")
N17 T12
N18 M6
; Atorn - HPC ALU - 8mm
N19 DIAMOF
N20 SETMS(1)
N21 G97 S1=4500 M1=3
N22 G17 G90 G94
N23 G55
N25 D1
N26 G0 C4=0.
N27 TRANSMIT
N29 M108
N30 G0 Z76
N31 X-83.138 Y18.066
N32 Z66
N33 G1 Z62 F1000
N34 Z40.8
N35 X-83.131 Z40.696 F800
N36 X-83.111 Y18.067 Z40.593
N37 X-83.077 Y18.069 Z40.494
N38 X-83.031 Y18.072 Z40.4

When I compare the code in the 2D contour the "SETMS(1)" is missing.

I don't know if something at the end of the adaptive toolpath will override this?

[kuhnjst]

Just wondering if the setms1 is missing is it going into setms4 on its own as a default and feeding at mm/rev? But your live tooling head wouldn't turn on either if that was the case right? What post are you running siemens mill-turn.cps? I just wanna know how you got the TRANSMIT function to work properly?

[JJackrabbit]

Setms1  = live tooling

setms4 = main spindle

I think it maybe needs another setms1 when both programs are combined?

[kuhnjst]

I would think that would be a modal command but try the old copy paste trick and see?

[kuhnjst]

ok so my post spits out system1 both time (same endmill used) but it dumps the offsets and doesnt recall the tool (does this on a regular basis. Yes it almost causes wrecks)  but the setms1 is called at the beginning of each tool.

X73.9

G3 X74.2 Y-0.7 Z107.2 CR=0.3

G1 Y-0.4

G3 X74.2 Y-0.1 Z107.5 CR=0.3

G0 Z129.6

G53 X250 D0

G53 Y0 D0

G53 Z500 D0

MSG ("; 2D Contour6")

DIAMOF

SETMS(1)

G97 S1=5941 M1=3

G0 Z129.6

X74.2 Y0.1

Z119.6

G1 Z115.2 F333.33

Z107.5

G3 X74.2 Y0.4 Z107.2 CR=0.3 F1718

G1 Y0.7

[JJackrabbit]

I just check a different part. Which also uses a 2d adaptive and 2d contour.

That part runs fine (already made it).

I don't see any difference in the codes. Except for the positional moves.

I will check tomorrow on the machine and rerun my first toolpath to do some tests.

[JJackrabbit]

I have done some testing.

Once I post the toolpath as a seperate program.

It runs fine.

But once combined with other toolpaths it won't work.

The first toolpath works. But all following toolpaths will have this issue.

It will override the speed and will follow the toolpath at max feed. Causing the endmill to crash

I found out which is causing it.

When posting it as a separate program. It won't posts a " G97 S1=4000 M1=3" each time a toolpath operation starts.

And it runs fine.

But once combining it with other toolpaths.

I will post a g97 after each operation.

Once I remove the G97 it runs fine.

I'm curious how I can change this?

Another thing.

When posting single toolpath operation (2D contour with a circular pattern).

After repeat of the 2D contour it goes Z15 and repeats 

This is perfect

But when combining the toolpath operations after each repeat cycle it will go to it's home position and back to it's starting position. I don't want that.

G53 X418 D0
G53 Z549 D0

[kuhnjst]

Yep my machine is also doing this! not consistent though. very weird but yes caused me and my apprentice to ruin our underpants!

[JJackrabbit]

Interesting. 

How did you solve this?

I current modify the posted code to remove all G97 from live tool toolpaths.

But it's quite annoying to do.

[kuhnjst]

I deleted the G97 on the 2nd path. It was strange, So i'm milling flats (2x180) on the od, the 1st path ran fine. indexed to 180 and it took off like you was saying. After the machining op we weld 2 ribs on those flats then it comes back to me to mill the height of the rib then profile the od of the ribs. I copy and pasted the cycle from 1st op and changed my heights. The copied section DID NOT do this. The profile path around the rib did....But the other issue i have also showed up. Where it sends the tool home, turns of the comps, then heads back over with out comps active and tries to crash.

[JJackrabbit]

I don't have the last issues. But I also have to remove all G97's after each milling operation.

[kuhnjst]

So the post adds a g97 whenever it outs puts the spindle command. I cant find that in the post. I think if we could remove the g97 from that line the problem would go away. line below calls the g94 in the beginning but when it move to the next contour the g97 cancels out the g94 and off it goes! I was also told the 

 DIAMON

N13049 MSG ("; 2D Contour1")
N13050 DIAMOF

Might also be kicking the g94 out, goes from turning back to milling but doesn't get the feedMode again.

Any input from:

@aju_augustine

@seth.madore

 ?

[kuhnjst]

so i edited line 481 in the post to G94. Thoughts?