Mastercam for Millturn

[Shiva.aero]

How good is Mastercam for Millturn machines?

I moved from Esprit to Mastercam recently and I am very satisfied with the Mastercam. I am primarily a 5 axis user and I don't know about Millturn functionality in both the softwares.

One of our supplier recently purchased a Millturn and during a discussion I suggested Mastercam for CAM. They told that the Machine-tool vendor itself suggested to go for Esprit CAM. The same argument I heard from another supplier who uses Millturn machines.

I can list out no. of advantages of Mastercam over Esprit in 2,3 & 5 axis Milling. Simply I can't believe Mastercam is lagging in Millturn.

Can somebody please share their experience on 'Millturn with Mastercam'? Has anybody moved from Esprit/other CAM softwares for Millturn/Multitasking machines?

[gcode]

Mastercam Mill Turn is only available for specific machines\

Some ( maybe all??) supported machines are listed here

Look for this note at the end of each machine description

Quote

Note: This post requires the Mastercam Mill-Turn module to be enabled.

 

I have no personal experience with it, but know people who use it and like it

You can also find some pretty vocal rants about it here on eMC

[So not a Guru]

1 hour ago, gcode said:

You can also find some pretty vocal rants about it here on eMC

To be fair, you can find some vocal rants on just about every subject .

But, in truth, this is one of the finest forum I've ever belonged to.

[Shiva.aero]

4 hours ago, gcode said:

Mastercam Mill Turn is only available for specific machines\

Some ( maybe all??) supported machines are listed here

Look for this note at the end of each machine description

I have no personal experience with it, but know people who use it and like it

You can also find some pretty vocal rants about it here on eMC

Just in the other thread, it was mentioned that Mastercam is non-kinematic based CAM. That is Mastercam doesn't depends on the machines.

Then how come MC supports some machines & not support some other machines?

By support do you mean only post?

[Colin Gilchrist]

1 hour ago, Shiva.aero said:

Just in the other thread, it was mentioned that Mastercam is non-kinematic based CAM. That is Mastercam doesn't depends on the machines.

Then how come MC supports some machines & not support some other machines?

By support do you mean only post?

You're not aware of the full picture.

Mastercam Mill-Turn uses a new 'Machine Layer', called Mastercam Extensions. This is both a Simulator and a Post Processor. There is a 'link' between the Simulation and the original Mastercam File, but there are limits to how much of the data is shared. The machine file (literally called the "Dot Machine" file), is where the machine kinematic information is stored and manipulated. For example, when you set a token to drive a different machine mode like pinch turning, you'll see the simulation changes to show the change to the machining process. 

Inside Mastercam Extensions, you set 'Tokens' which drive the output of machine options in the NC Code. These are things like coolant output. The Extensions product also supports Multi-Stream output, and allows you to Sync Operations, which controls the output of Sync and Wait codes. Then, after you set the tokens and syncs, you Simulate the process. This shows you doing things like Pinch Turning, or parking the turret, while performing another operation. 

Once you've created the process in Extensions, you post the NC Code. This is done through a  MP.NET Post, which is Mastercam's new Post Language for use with Extensions. Currently it is only used for Mill-Turn machines, because that is just how the development has evolved. Also, only your Reseller and CNC Software has a Development License for MP.NET, so you can't just modify your own Post.

That said, you really only need Mill-Turn if you are driving a B-Axis Lathe, with full 5-Axis. If you have a 4X lathe, where you are limited to a single code stream, and a maximum of 4 simultaneously driven axes, then you can use the Generic Fanuc 4X MT_Lathe Post and Machine Definition. Even dual spindle, dual turrent lathes can be driven by that Post. But the limitation is > no Simulation.

Every software has strengths and weaknesses. Mastercam is no exception, but the overall ecosystem is by far the most powerful for a broad range of users. There are several other packages that I've used, and I like a lot about each one. But with Mastercam, I know I can buiild or buy a Post for just about any machine.

I've always been a fan of Simulation that runs the actual G-code, and drives the simulation based on the actual NC Program that will run on the machine. This was traditionally NCSIMUL, VERICUT, ICAM, and CAMplete. The difference between them, is that CAMplete also did the NC Code generation extremely well. However, since the acquisition by Autodesk, I doubt they will remain 'independent' much longer.

It is still really hard to beat the combination of Mastercam + A Good Post Processor (In-House or Postability, no question) + G-code Simulation (NCSIMUL or VERICUT). I can literally program any machine with this combination. However, there is a cost involved. You have to buy the Post and the Machine on the Simulation side. This isn't cheap, but you really do get great value for making the investment. 

[Shiva.aero]

14 minutes ago, Colin Gilchrist said:

You're not aware of the full picture.

Mastercam Mill-Turn uses a new 'Machine Layer', called Mastercam Extensions. This is both a Simulator and a Post Processor. There is a 'link' between the Simulation and the original Mastercam File, but there are limits to how much of the data is shared.

Inside Mastercam Extensions, you set 'Tokens' which drive the output of machine options in the NC Code. These are things like coolant output. The Extensions product also supports Multi-Stream output, and allows you to Sync Operations, which controls the output of Sync and Wait codes. Then, after you set the tokens and syncs, you Simulate the process. This shows you doing things like Pinch Turning, or parking the turret, while performing another operation. 

Once you've created the process in Extensions, you post the NC Code. This is done through MP.NET, which is Mastercam's new Post Language for use with Extensions. Currently it is only used for Mill-Turn machines, because that is just how the development has evolved.

That said, you really only need Mill-Turn if you are driving a B-Axis Lathe, with full 5-Axis. If you have a 4X lathe, where you are limited to a single code stream, and a maximum of 4 simultaneously driven axes, then you can use the Generic Fanuc 4X MT_Lathe Post and Machine Definition. Even dual spindle, dual turrent lathes can be driven by that Post. But the limitation is > no Simulation.

Every software has strengths and weaknesses. Mastercam is no exception, but the overall ecosystem is by far the most powerful for a broad range of users. There are several other packages that I've used, and I like a lot about each one. But with Mastercam, I know I can buiild or buy a Post for just about any machine.

I've always been a fan of Simulation that runs the actual G-code, and drives the simulation based on the actual NC Program that will run on the machine. This was traditionally NCSIMUL, VERICUT, ICAM, and CAMplete. The difference between them, is that CAMplete also did the NC Code generation extremely well. However, since the acquisition by Autodesk, I doubt they will remain 'independent' much longer.

It is still really hard to beat the combination of Mastercam + A Good Post Processor (In-House or Postability, no question) + G-code Simulation (NCSIMUL or VERICUT). I can literally program any machine with this combination. However, there is a cost involved. You have to buy the Post and the Machine on the Simulation side. This isn't cheap, but you really do get great value for making the investment. 

Thank you very much for such a detail explanation!

Cost aside, is it possible to program in Mastercam for any "Millturn machine", with a good post processor from inhouse solutions / Postability and a good CAV software?

[Colin Gilchrist]

9 minutes ago, Shiva.aero said:

Thank you very much for such a detail explanation!

Cost aside, is it possible to program in Mastercam for any "Millturn machine", with a good post processor from inhouse solutions / Postability and a good CAV software?

Yes, 100% possible. As machine complexity increases, so does the cost for the Post, for the Simulation, and for the Training you'll need to get everything running smoothly. The more complex the machine, the less this is an 'off-the-shelf' process, and the more time it will take to dial in the Post and Simulation. I've seen a WFL build take 18 months to get a Post ironed out, and 24 months to get the bugs worked out for VERICUT. But that's one of the most complex machines there is. 

[Guest]

5 hours ago, So not a Guru said:

To be fair, you can find some vocal rants on just about every subject .

But, in truth, this is one of the finest forum I've ever belonged to.

It used to be an ok forum, it went downhill since they banned off topic for sure...

[Guest]

3 hours ago, Shiva.aero said:

Just in the other thread, it was mentioned that Mastercam is non-kinematic based CAM. That is Mastercam doesn't depends on the machines.

Then how come MC supports some machines & not support some other machines?

By support do you mean only post?

Mastercam by default doesn't take into account the machine kinematics, however post extensions from moduleworks can add this ability to a post and are available from some dealers. 

[gcode]

The 2022 HLE contains the Mill/Turn Module

You can install it and play with it at no cost or obligation

If you have 2022 installed all you need is an HLE license

which you can get  here

One word of caution, I have heard of cases of the HLE license causing issues with 

existing industrial software licenses 

I run a USB hasp and have no issues