[mooreaa]

Hey guys,

I've seen a few videos where the tools are setup on the mill bed and the part is held in the spindle to allow turning operation on the mill.

I would like to learn more about this method and wanted to find out a couple things.

1) What jigs are out there for holding the tools on the bed? Or do people make their own custom tool holders? If so, can someone recommend an article or tutorial on designing such a fixture?

2) How are the parts being programmed? Do you have to re-configure the CAM software / Mach3? I can see how this can be done manually but I am hoping to run a part though the software and am not sure where to start looking.



Thank you,

Aaron

[dsdmax]

tosatool - makes one. they are also a tormach approved vendor. they about about 850... so you might want to look into designing one yourself. That said - usually when i am in your situation and i am asking questions hindsight generally indicates i would have been better off buying instead of trying to build. though i still enjoy the learning experience of the building -just not usually the quickest or most cost effective solution (my manual mill to cnc conversion is a great example and i am still going to buy one - still stuck on ihcnc or tormach).

[SCzEngrgGroup]

Here's how I plan to do it, and it's dead simple to make your own:

Welcome to Mill2Lathe!

Regards,
Ray L.

[mooreaa]

Hey guys, thanks for the response. What is the theory behind programming for this? Do you have to trick the cam software to flip axis somehow? or is there a cleaver way to take the cam output for a lathe and use it on a mill?

I'm pretty new to my CNC but I am proficient in Solidworks so I've been keen on finding a method to program this mill lathe using the CAM software.

For the fixture I agree that the rigs look pretty simple. As this is an exercise initially, I'm wondering if I may even just try to hold one of the turning bit in my vice (please someone tell me if this is dangerous for any reason before I try this).

[TXFred]

The axes are the same, actually. Z on a lathe is along the spindle's axis, same as on a mill.

X is across the axis on a lathe, same as on a mill.

Picture your Tormach laying on its back, and suddenly it looks a lot like a lathe.

There's more to it than that, of course. You need to get Mach unlocked and make a bunch of configuration changes in order to get it working smoothly.

The Y axis of the mill presents an issue, since a lathe program doesn't do anything with Y. I've got a project going on right now that should fix this. I need to do a bit more testing and debugging before I post it up here. So far, it handles gang tooling like a champ. It should work very well with a Mill2Lathe style tool holder.

Frederic

[beanbag]

U don't need to configure Mach3, but u should have a CAM program that knows how to output for Lathe ZX, which is the axes u will be using. The CAM program also need to know how to take the cutting tool's shape into account. SprutCAM can do this. Tormach has a tutorial on this.

[TXFred]

The Duality post for Sprutcam is meant to work with Lathe XY, not ZX. It's strange, but that's how they set it up.

And yes, you do need to make changes to Mach3's configuration.

Frederic

[TXFred]

As this is an exercise initially, I'm wondering if I may even just try to hold one of the turning bit in my vice (please someone tell me if this is dangerous for any reason before I try this).

I forgot to reply to this bit. It's not dangerous, and is a very good way to hold a single lathe tool for testing purposes.

Frederic

[beanbag]

The Duality post for Sprutcam is meant to work with Lathe XY, not ZX. It's strange, but that's how they set it up.

And yes, you do need to make changes to Mach3's configuration.

Frederic

Hmm, I used the Vertical Lathe post and made no changes to Mach.

[apeman88]

I turned a few things on my Tormach with one lathe tool in the vice and a R8 chuck in the spindle. It works great. I hand coded the G-Codes though. Attached is a piece I turned on the Tormach earlier this year.

Ken

FYI... this is a Marposs Touch Probe Holder I made earlier this year.

[TXFred]

Hmm, I used the Vertical Lathe post and made no changes to Mach.

I love eating my words. They're delicious!

I'm curious how you did this. What I'm understanding is, and please correct me when I'm wrong:

You set sprut to Lathe, XZ. And you have a post processor called Vertical Lathe.

When you say you didn't change Mach at all, does that mean you just fired it up in Mill mode and ran lathe code?

I'm running the basic version of Sprut with the encrypted postprocessors. The only ones I can use are the Duality Lathe and the Tormach Mill posts. That limits me somewhat, but the Duality post appears to work quite well. Since Mach's Duality config uses the mill's Z axis as X, and the X axis as Z, some configuration changes to Mach are necessary. Also, coolant is disabled in this config, because they don't want users hosing down their Duality lathes.

Frederic

[BlueFin]

This video is old news, but it is how I use the mill as a lathe. Built the tooling holder and hand wrote all two pages of G Code. Took me 6 weeks to figure it all out, but I had never seen a cnc before and jumped into this as my first project.

Tormach vertical turning brass - YouTube

[beanbag]

I got the Vertical Lathe post from Tormach. I forgot if I found it on their webpage, or if Eric sent me a special link. The biggest drama is setting up the part in sprut cam.

Select LAthe ZX before you import the part. Import the part.
You have to turn on the "show machine axis" (That little green machine button at the bottom) and align the part with Z, according to the coordinate system shown in the bottom left corner of the screen. Then fiddle around with workpiece setup, coordinate system, etc randomly until something works.

The post will spit out g code in x and z, and also make y=0. Yes, I had to go in the code and manually edit out the m998s and g43 m6, etc. I used G54 and G55 for my two tools. Mach will then run this code without knowing any different.

[mooreaa]

@TXTFred - Good to know that its not dangerous. I am gonna get some lathe bits (see below) and give this a try first before figuring out any sort of rig.

@apeman88 - Very nice finish. Glad to see such promising results from this process.

@BlueFin - Ran across this video before and glad to see you here talking about it. I like the simplicity of your rig and I may try to replicate this for my first tool post.


Sounds like many of you are doing the G-code by hand which makes sense since I'm seeing the challenge with configuring the software to post/run the code. One immediate issue I see is tool-length offset in Mach3. Since the gang tools are going to be in different orientations and such, the x-y-z points for all these tools are going to be vastly different. Some tools will be point up in the Z like drill bits, Some tools will be pointing in -x. The tools positions will be scattered either across the y axis, x axis or both depening on the gang tooling setup. This seems like its a very different operation than a lathe on its side but maybe I am over thinking things? Maybe I just need to setup each of these operations in a different coordinate system and some how probe these points to setup my work offsets?

I may just be better off taking the plunge and trying it as you guys all seem to have done. I am trying to order some lathe tool bits to start off with. Trying to find the right toolset / cutoff blade to use. Saw some posts suggesting the use of 1/2" lathe shank tools though I'd like to hear from some of you guys on which tools you have used successfully.

Regarding Mach3, and unlocking it. Are you talking about being able to access Mach3's configuration menu which Tormach seems to hide from its users? How do I get access to that menu? I presumre they hide it for good reason as it is a "home cnc" but I'd love to be able to get at the inner workings to better understand my machine.

[apeman88]

Thanks! I was happily surprised with the results as well. Before I started, I was afraid cutting Stainless may be a challenge with this setup. As for tooling... since my plan from the very beginning was to clamp only one tool in the vise... I went on eBay and found the best deal possible for the beefyist lathe tool... ended up with a 1.5" lathe tool complete with a bunch of inserts.

Initially, I did consider using CAM to code... but it seemed a lot easier to hand code since it's only 2 axis and I'm only using 1 tool.

I say just jump in... you can get a R8 chuck on eBay for under $100.

Oh... one mistake I made was coding for cut in one direction and mounting the lathe tool in the vise in the opposite direction. The tool was rubbing instead of cutting and actually rubbed the stock out of the chuck before I realized it. A simple M4 fixed it. So make sure you setup/design your jig for cut in the direction you want.

Good luck!!

Ken

[300sniper]

if you are hand writing the program, wouldn't setting a work offset for each tool work? instead of calling a new tool, call out the work offset. that way you have the proper location and height.

[BlueFin]

Yes cut direction is something to consider, as looking at the mill I placed my tools on the left hand side, don't know why I did this, but required me to do buy reverse rotation drill bits so the spindle would not have to stop after turning in reverse. Didn't do any tool offsets or any of that stuff, used a dial indicator and mapped out the tooling, then programmed the move heights in my self. You also have to prgram for Z axis backlash as you move around up and down. Took me forever to visualize with my minds eye every Z axis reversal and where to add or subract .0015" of backlash in the z. Otherwise things would rub.

[TXFred]

if you are hand writing the program, wouldn't setting a work offset for each tool work? instead of calling a new tool, call out the work offset. that way you have the proper location and height.

Yes, that does work. But it means that you have to define each work offset each time you set up the tools.

If you have a gang tooling setup, and a tool table defined for it, then you only have to set up a single work offset. And it also means that you can use output from a CAM program without needing to do any edits.

Frederic

[beanbag]

Yes cut direction is something to consider, as looking at the mill I placed my tools on the left hand side, don't know why I did this, but required me to do buy reverse rotation drill bits so the spindle would not have to stop after turning in reverse. Didn't do any tool offsets or any of that stuff, used a dial indicator and mapped out the tooling, then programmed the move heights in my self. You also have to prgram for Z axis backlash as you move around up and down. Took me forever to visualize with my minds eye every Z axis reversal and where to add or subract .0015" of backlash in the z. Otherwise things would rub.

Right, and also the backlash in x, if you are interested in holding some kind of diameter spec.

[David Bord]

I understand that latest version of sprutcam has a mill based lathe function?

If so, and they get it to work well, that would be killer!

Has anybody used this?

David