Thoughts on a Tsugami TMA8F Mill Turn? or other small mill turn

[the_r1_kid]

I worked as an AE at an Okuma/Tsugami dist for 8 years. I saw a lot of shops struggle when getting into a B-axis style mill turn machine. Some were customers we sold Multus machines to, others bought our competitors machines (Nak, DMG, Mazak, etc.). The only way to justify the high price tag of these types of machines is to reduce operations and setup time, especially for job shop type work. There were a few common issues that seemed to be the most relevant to successfully implementing this type of machine.

1. Software. The customers that had better software had better results. The ones that didn't struggled to get good code and prove out programs in a timely manner. They took days to prove a program rather than hours. This was a decade ago so they may have improved, but Mastercam was the biggest culprit. Gibbs shops also seemed to struggle but I think that was more because of the local dealers greedy post development process. Customers with Esprit or other high end mill turn software had significantly reduced times getting new parts processed. The better the software's simulation, the better the results at the machine.
2. Lathe operators versus mill operator. Many times shops they would stick these machines in their lathe department and put 2 axis lathe operators on them. These are complex machines that need very capable operators/machinists to make them productive.
3. Refusing to learn/use all of the options available in the machine. The Okuma Multus comes with their CAS collision avoidance software. Most builders have something like this now. It takes a little up front work to model your tools and holders, but once it is done you can run through program in high speed machine lock mode to prove them out and check for collisions. This is way faster than a machinist sitting with their hand on both knobs and watching code go by while. At my current job we use the CAS in all of our Okuma millturns. Most of our parts are 5-20 minutes cycle times and we can prove out most new parts in under an hour including setting up CAS for new tools and jaws.

Thank you thats great insight. I really hope mastercam has matured their mill/turn. I'm going to start with mastercam, But if I have to I'll eat it and pivot to Esprit or NX.

 

[the_r1_kid]

My machine came with microcentric (B65) collets closers both front and back, the chucks were never installed, they are a low profile design.
Might actually gain some travel if installed. The Z travel with the head kicked isn't that bad, I have a 3.00 plus long part that we drill out the center with an insert drill.
Machine is really rigid handles milling with ease. Has soft break and a disk type hard brake for clamping C when milling.
Lots of offsets and good memory (maybe options), my machine has high pressure through coolant also.
I program using Fusion and blend handwritten code into that, hardest part is getting all the correct codes for stopping starting C.
This machine likes a program that has robust safe start codes before a cycle and after, I think it is baked in to keep me from hurting it.

Thats good to know. 3" is about the max length of part that ill need to end drill. Whats your guess for max length of stock stick out of the collet you can have and still work on the end with a stubby tool holder and reasonable length tool?
You are more patient than me. I've been there, I don't think I have the patience to hack posts together into something working any more

 

[YoDoug]

Thank you thats great insight. I really hope mastercam has matured their mill/turn. I'm going to start with mastercam, But if I have to I'll eat it and pivot to Esprit or NX.

So as far as Mastercam and their Millturn, one of the last projects I worked on before leaving the dist was a turnkey on some Multus U3000 machines. For the most part the code was decent. There was a few issues that would cause a machine crash that I ended up finding work arounds. Also the importing of tools and custom chuck/jaws for simulation was horrible. I have heard they have improved that as that project was 6+ years ago. I really didn't care for the way they handled program sync and wait codes, but the machines you are looking at are only one channel so that is not an issue.

 

[gregormarwick]

For programming millturns, Featurecam is excellent. The FC workflow is exceptionally well suited to these machines and complex parts are effortless to program. The post system is second to none and it's very possible to get 100% perfect code with a little effort.

The huge, unavoidable, grotesque elephant in the room is Autodesk. But if you can live with selling your soul to the devil, Featurecam is absolute bliss with a B axis millturn.

 

[SD&M]

3. Refusing to learn/use all of the options available in the machine. The Okuma Multus comes with their CAS collision avoidance software. Most builders have something like this now. It takes a little up front work to model your tools and holders, but once it is done you can run through program in high speed machine lock mode to prove them out and check for collisions. This is way faster than a machinist sitting with their hand on both knobs and watching code go by while. At my current job we use the CAS in all of our Okuma millturns. Most of our parts are 5-20 minutes cycle times and we can prove out most new parts in under an hour including setting up CAS for new tools and jaws.

Hi Doug:

Are you using the CAS on the machine, as well as whatever tools are at your disposal in TS or Esprit? Are there advantages to using the CAS that aren't available in s/w?

 

[Macturn]

Putting in a good word for NX here. Use it for a Macturn 250W with a bottom turret and another B axis Millturn and I have no complaints. Synch mark and dwells are done through Synchronisation manager graphically , drag and drop. Clean safe code plus ISV will then simulate the posted G code all inside a seamless CAD/CAM environment. Postprocessor and machine kits are available or your reseller can build one for you if one isn't available.

The NX lathe module is overlooked because of its CAD and milling prowess but it is equally powerful.

 

[YoDoug]

Hi Doug:

Are you using the CAS on the machine, as well as whatever tools are at your disposal in TS or Esprit? Are there advantages to using the CAS that aren't available in s/w?

We do use CAS on the machine. We have all of our tools modelled and we use the CASME command to load chuck/jaws/workpiece in each program. We also model everything in TopSolid. The biggest advantage to using the CAS is collision avoidance. We don't have actual Gcode verification so while it rarely happens, there are times that CAS catches something that TopSolid missed. The other big advantage to CAS is you can run through a program in machine lock in high speed. A program that has 15 minutes of runtime and would take and hour or so proving it out with both hands on the knobs, will simulate in a minute or two in machine lock. If the CAS looks good I will start it and let it run. I don't feel the need to stop at every tool and keep my hands on the knobs or run it slower. We just recently started making waternecks in our Multus U3000 and the CAS was a big time saver in proving the program. Pic below

https://imgur.com/QG1uH8A

 

[PitterPatter]

I bought a TMA8F last year, big buy for a small shop like mine, took the gamble and it is paying off and freeing up my capacity on other machines. Prevents me from making over runs. And changing over jobs is fast as hell.

It should handle Titanium and Alum like nothing. I run mostly aluminum and 316 SS.

The machine is extremely rigid and accurate, cuts through 316 SS like nothing.
Comes with Heidenhein glass scales for the X axis.

Came with high pressure, chip conveyer, foot switch, and a mist collector.

Thats good to know. 3" is about the max length of part that ill need to end drill. Whats your guess for max length of stock stick out of the collet you can have and still work on the end with a stubby tool holder and reasonable length tool?
You are more patient than me. I've been there, I don't think I have the patience to hack posts together into something working any more

The longest part I ran was approx. 4" inches. Had to buy a .500 EM approx. 6" long to contour a corner radiis around the part. I think you should be fine. See below.

Esprit spits out really good code. Just the learning curve is ridiculous...

Only gripe is that touching off tools and backworking set-up is a chore. And you get very limited work offsets. Wish it had handle-jog-through program. Single block is the only next best altnertive to prevent crashes.

Otherwise. I fucking love this machine.

(Couldn't afford everything else that was on the market..)

 

[Springy]

I bought a TMA8F last year, big buy for a small shop like mine, took the gamble and it is paying off and freeing up my capacity on other machines. Prevents me from making over runs. And changing over jobs is fast as hell.

It should handle Titanium and Alum like nothing. I run mostly aluminum and 316 SS.

The machine is extremely rigid and accurate, cuts through 316 SS like nothing.
Comes with Heidenhein glass scales for the X axis.

Came with high pressure, chip conveyer, foot switch, and a mist collector.


The longest part I ran was approx. 4" inches. Had to buy a .500 EM approx. 6" long to contour a corner radiis around the part. I think you should be fine. See below.

Esprit spits out really good code. Just the learning curve is ridiculous...

Only gripe is that touching off tools and backworking set-up is a chore. And you get very limited work offsets. Wish it had handle-jog-through program. Single block is the only next best altnertive to prevent crashes.

Otherwise. I fucking love this machine.

(Couldn't afford everything else that was on the market..)

Reviving this oldish thread with more questions - what does the tool touch-off process involve that makes it so laborious? I would have thought on a millturn like that, it'd be the easiest part of the whole process. Anything in particular about the backworking setup that's also difficult, or are you just talking about machining soft jaws...?

Also, does it have integral motor spindles or are the spindles belt driven? And what CAM are you using for it?

 

[PitterPatter]

Reviving this oldish thread with more questions - what does the tool touch-off process involve that makes it so laborious? I would have thought on a millturn like that, it'd be the easiest part of the whole process. Anything in particular about the backworking setup that's also difficult, or are you just talking about machining soft jaws...?

Also, does it have integral motor spindles or are the spindles belt driven? And what CAM are you using for it?

Unlike touching off a mill, there isn't a macro program to call to automatically touch off your tools to the tool setter.

Need to call up the tools, manually jog it to the setter and jog the tool to measure.

Since the machine is compact, careful consideration needs to be made when setting the work offset to avoid smacking the head into the main spindle. Each tool on the sub spindle work may need a bunch of separate work offsets. I have had to use all G55-G59 to make sure my drills have enough travel.

I don't remember if its integral. I will take a look.

But otherwise, Esprit has a solid post processor and support.

 

[Springy]

Unlike touching off a mill, there isn't a macro program to call to automatically touch off your tools to the tool setter.

Need to call up the tools, manually jog it to the setter and jog the tool to measure.

Since the machine is compact, careful consideration needs to be made when setting the work offset to avoid smacking the head into the main spindle. Each tool on the sub spindle work may need a bunch of separate work offsets. I have had to use all G55-G59 to make sure my drills have enough travel.

I don't remember if its integral. I will take a look.

But otherwise, Esprit has a solid post processor and support.

Thanks for the info. Why do you need separate work offsets on the sub? Is it not sufficient to be careful with the retract/clearance planes?