CMS Antares Post Processor Issue?

[Kanalje72]

Hi, I struggle with a (to me) strange behaviour when switching between different operations in an NC-program. I can run the different operations as separate programs but when I have the operations i one nc-program the machine stops due to "(Z)+ OVERTRAVEL ( SOFT 1 )"

Machine: CMS Antares 2615 PX5

Postprocessor: Fanuc (slightly modified by Autodesk support)

Operations: Multi Axis Contour

I think the error occurs when the machine reorient to match the next operation. I would be grateful for any ideas in how to solve this.

[licensKKGSY]

Rapid moves BETWEEN operations are not handled directly in fusion but by your post processor. Fusion only defines the retract height and rapid moves WITHIN an operation. This is just a  guess, but perhaps your post is set up to do axis prepositioning with TCP activated: once the machine has traveled to g53 Z0 (without prior reset of the rotary axis) and tcp is activated, the machine will attempt to pivot around the tool center point, without having the necessary Z-travel to do so. 

I have done quite some work with our SCM Hypsos 6018, with respect to this kind of stuff. If I'm right in my guesswork, the solution should be a simple change in the order of positioning and tcp.

Can you please share your post processor as well as a piece of NC where there is a change from one OP to another (obviously 3+2 or 5-axis)?

[Kanalje72]

Hello and I agree. These has been my thought as well even if I didn't now the word for it. I was not familiar with TCP concept but from your explanation and the behaviour in the machine it seems likely that this is the root cause for the unwanted halt. I'm keeping my fingers crossed that the solution is "simple" as you said. Please have a look at the attached files and see if it makes any sense 🙂

//Adam

[licensKKGSY]

Here you can see the bit:

N3275 Z-0.325
N3280 G28 G91 Z0.
N3285 G90

(MULTI-AXIS CONTOUR2 5)
N3290 G00 B-72.135 C90.
N3295 G49
N3300 G359
N3305 G00 G43.4 X-515. Y-92.482 Z9.675 H18

You want g49 (canceling tcp) before positioning your rotary axis.

I'm not a big post editing guru, so perhaps someone else could make the change in your post more quickly than I, as I'm too busy today, but if nobody chips in, I will make the attempt later and get back to you.

[licensKKGSY]

I think this bit has to be set to "true"  (it was set to "False") to force tool length compensation deactivation, when the one chooses to setup the post like it is here. The line number is 1769.

[Kanalje72]

I really appreciate the input and the suggestions but I also recognise my lack of skill and understanding of what happens if I edit the post by my self. I have contacted a professional to help me out. I will try to remember to give you feedback if I find a solution with the help of support.

//Adam