Siemens 5 axis turn-mill fusion 360 post.

[trevor7RDJL]

Wondering if anyone can help me out with this problem.

We have a Hermle c42 u 5 axis mill turn using siemens 840D, I have a post that can generate this milling side of things, however when I try to combine turning and milling within the same program it throws up the error:

Error: Turning toolpath is not supported by the post configuration.

Failed while processing onOpen().

Does anyone know a way to configure the post to allow turning and milling?

Thanks in advance

[serge.quiblier]

Hi @trevor7RDJL 

this is not an easy thingd to do.

But it is not impossible.

We already have some Simens post for turn mill machine. (A lathe that know how to mill)

But the logic is the same for a mill turn machine ( A milling machine that know how to turn the part)

Step one will be to alter the post capabilities from:

capabilities = CAPABILITY_MILLING | CAPABILITY_MACHINE_SIMULATION;

to

capabilities = CAPABILITY_MILLING | CAPABILITY_MACHINE_SIMULATION | CAPABILITY_TURNING;

Then inside the onSection, and potentially in the defineWorkplane / setWorkplane functions, some changes may be required.

Because if the currentSection.getType() == TYPE_MILLING, or TYPE_TURNING you will have to activate different controller functions, inside the onSection function.

For example, on the Hermle, using a Siemens controller without the OPERATE system, the commands ttcon, ttron, turnof had to be used.

They select or cancel the turning mode, or turning mode with inclined axis.

The OPERATE version uses Cycle800 and ttron.

The post will have to be modified, to deal with feed rate in unit per revolution, and not only unit per minute.

You can take a look at the controller turn mill post for help on that subject.

If you don’t intent to use the roughing canned cycles, and to drill in turning mode, you don’t have tons of work to do.

It will be mainly tricks to avoid passing in some functions.

For example in turning mode, we don’t want to output a Cycle800 for switching a tilted workplane.

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[ITS-CNC]

Hello guys,

I have almost the same problem, I don't know if I'm expressing myself too well. I have a chiron 800 mil tower, with siemens, I have some product blades and some operations require processing in full 5 axes, the machine is capable of doing this but the postprocessor is not, I tried with one of 5 axes and it generates my ABC and I have only A and B are needed, C being attached to the V axis. I tried with a mill-turn processor but I get the error: "Direction is not supported for machine configuration."
Can you help me set up this post-processor to give way to the project?
I didn't find anything related on this topic anywhere else, except here, that's why I didn't open another topic