Deckel Maho DMC 80 FD Mill-Turn with Siemens 840D solutionline FD

[martin.schachtner]

Hi. I´m a Fusion 360 Beginner and have some questions.

A customer of mine has a DMC 80 FD with the Siemens 840D solutionline FD control.

Does the general Siemens 840D Post support this Machine type? Does it work?

And the main question, how can i program this in Fusion? With the Setup for Milling or Mill-Turn? I thought the Mill-Turn is only for Lathe Turning machines? And how is it possible to create a machine model for the simulation?

Sorry for so much questions, but i´m a little bit confused about mill-turning in Fusion 360.

Thanks a lot and much greetings

[serge.quiblier · Accepted solution]

Hello  

Here are some answers to your questions.

Does the general Siemens 840D Post support this Machine type?
Not without modification, as the milling post is only supporting milling toolpaths.
And trying to use a siemens turn mill post will be wrong, see the explanation below.

And the main question, how can I program this in Fusion?
It can be programmed by defining a turn mill setup in Fusion, creating the operations in the same setup.
Their properties will be identified by the post, so that we can generate the gcode correctly.

With the Setup for Milling or Mill-Turn?
As I said the Mill Turn setup.

I thought the Mill-Turn is only for Lathe Turning machines?
Tricky thing, there is 2 sort of these hybrids.
a - The lathe that think it can mill the part. (Mori Seiki, Doosan, Nakamura ....)
Acting by default as a lathe, and needs to be instructed to "switch" to milling mode by command like C axis enable, polar mode activation...
We use a base turning post to support them, adding function to deal with the milling part.
b - the milling machine that think it can turn the part (as the FD, Willemin Macodel, Chiron, some Mazak)
By default this is a milling machine, we can instruct the machine to "switch" to turning mode by a Cycle command.
In this case, we start with a milling post, adding logic to activate the turning mode when needed.

And how is it possible to create a machine model for the simulation?
The simulation can be created by the Machine Builder module in Fusion, but you need to get the 3d machine model from the customer.
In the current state of the machine simulation, you won’t be able to simulate turning toolpath, only the milling ones.

Cheers,

______________________________________________________________

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

[martin.schachtner]

Hello Serge,

thank you very very much for the explanation. It is really a tricky thing to work with. Your Info helped me definetly to understand the situation in Fusion 360 and to support my customer.

Thanks a lot and much greetings

[serge.quiblier]

Hello @martin.schachtner 

when I am speaking about switching to turning, it means:

In the onSection function, we need to detect if we are outputting code for a turning operation.

Either via

currentSection.type == TYPE_TURNING

or

currentSection.checkGroup(STRATEGY_TURNING) returning true or false

Then the controller needs to be informed via (on the latest firmware) a call to

Cycle959 for example, or else a specific function from the machine builder.

Siemens manuals can be found by looking for Siemens DocOnWeb.

Cheers

______________________________________________________________

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