What's new
What's new

Turning Parts With variable OD / Polygonal Turning ?

christie628

Plastic
Joined
Nov 12, 2018
I'm interested in moving a part from our 5 axis cnc's to a lathe with live tooling and polygonal turning capabilities.

Now cycle times on the 5 axis machines are approx. 1.5-3 min depending on the particular part. I would prefer to keep the same cycle times or close to. I've never programmed or ran a lathe so any advice is welcome.

The whole point is to move this part to full automation but with current work holding making it unreliable (on the 5 axis cncs) during part exchanges we could work hold better in the lathe's (given they can even cut something like this competitively)

Tolerance's are (+- 0.005) Average part Dia 15"

Thank you.
stp blade.JPG
IMG_0429.jpg
 
Hello Christie, Welcome to the board!

What YouTube examples of this kind of turning I just got done watching doesn't look much like your part. Same concept I suppose but regardless it looks like it happens pretty doggone quick. What is your part? Is that just for looking at or does it have a mechanical function?

Brent
 
I doubt you are going to improve cycle time. Obviously you can get more Automation.

Polygon Turning is not as fast as Cylindrical Turning. The saw type shape you are considering is going to be painfully slow Turning. But Milling on a C-Axis Lathe still gives you Automation.

R
 
Hello Christie, Welcome to the board!

What YouTube examples of this kind of turning I just got done watching doesn't look much like your part. Same concept I suppose but regardless it looks like it happens pretty doggone quick. What is your part? Is that just for looking at or does it have a mechanical function?

Brent

Brent,

For most polygonal turning the live tool is setup inline with the spindle but what i was wondering about putting the live tool at a 90 to the main spindle.
I think it could be done if the X axis can actuate fast enough while staying in time with the main spindle.

The part does have a mechanical function . Its a tillage blade for agriculture. We make a lot of parts at smaller margins vs a few parts at large margins.
My deal is we are selling all of our equipment in the next month and are completely updating our shop. I just want to be sure we are going in the right direction.
 
Lirlerob1,

On the c axis lathe i would have to look into a machine like a Mazak vari axis or so it could contour with the tooth profile.
Were really not wanting to invest in a mazak yet for this project we were looking more towards Haas ( I know its the throw away machine and everyone hates them ) but for the investment it works better for us to run them hard for 5 years and then sell to update keeping up with technology and keeping newer equipment. The choices we are looking at are the UMC750SS machines and ST35Y lathes.

I might have answered my own question as far as running these on a haas lathe but i just wanted to pick someones brain who has lathe experience.
blade varible tooth.JPG
 
Okay just to be clear; just because it in a Turning center doesn't mean the Operation is Turning. "Polygonal Turning" is an actual thing with Turning Tools (not Milling Tools). Milling in a Lathe is still Milling.

A couple different ways you can do this;
1. B-Axis Lathe$$. With a B-Axis you can orient the Milling Tool from the Face of the Spindle anywhere you want from -10º to 190º.

2. C-Axis Lathe with Milling Tool oriented Parallel to the Spindle. (will be required at least for the Periphery of the part)
3. C-Axis Lathe with Milling Tool oriented Perpendicular to the Spindle.

In 2 and 3 the Lathe itself has the Motion control you need (XYZ and C) it's 3-D surfacing. It's just a question of Metal Removal Rate and a good enough post. For number 3 (Milling Perpendicular) you could also use a Tapered Endmill. Luckily you can't get a Live Tooled Lathe with only Perp. or Parallel--you get both. :popcorn:

You could also use a Face plate on an Angle, and a Straight Endmill Perpendicular, because it's a round part.

R
 
Can you get an end mill ground to the profile, and set it up in a vertical mill?

Should be able to pull it down on a vacuum table if it is about 14" diameter, or more. Depending on the aggressiveness of the cut, and cutter condition. ??
 
Isn't a lathe that could do those milling features on a 15" part cost a small fortune?
 
Honestly, you want to put them on a gear cutter, you need one capable of bevel gears and you need the correct cutters - setup, but it would spit those out fast!
 
As litlerob1 said, that's not a polygon turning optimized shape. I'd be really tempted to try doing that on a mill with a rotary table driving an horizontal arbor where ~10 disks were stacked with spacers, then (as mentioned) profile with a tapered endmill.

You might have to revise tooth profile a little bit to optimize the process, but you could save a lot of time swapping in arbors already set up with fresh blanks. Dress the backside of the disk with a abrasive belt to knock down the burrs, then send it on to H/T and painting.
 
At 15" OD, you're going to be loading these by hand anyway, so not much in the way of lathe automation. I'm not sure I see the benefits of moving away from a decent sized 5-axis mill (e.g. UMC-750 as you've mentioned) vs. a live tooled lathe.

Changing milling tools in a lathe is much more cumbersome than in a mill, and you can fit a lot of redundant backup tools in the mill to keep it running.
 
Gosh, I have a hard time with the idea of tying up a 5x mill for such a (no offense) plebeian part.

What about a rotary and water jet or plasma cutter? I mean, this is turning over dirt, it's not ultra critical. If it's got to be pretty follow up the burning/jetting with a simple robot with a belt grinder to smooth the striations from cutting.
 
Greetings,

I run a swiss with live tooling/poly milling capability.
Yeah, you *could* do it on a machine like this, but looking at it, I think you're probably best served to do it on a standard 3 axis VMC with a tapered end mill.
Couple of reasons:
15" part. You're going to be hand loading, unless you spring for a robot. So no real speed savings there.
Agricultural blade: no need to hold turbine tols. Put a camlock system on your table, rig up a pair of camlock jigs that hole two or three of these things, and load one while the other cuts. Use a tapered end mill, and you're off to the races. Shouldn't take all that long to cut.
No way I'd waste a 5 axis machine knocking these things out.
Ever thought about having them drop forged? Or a grinder with a guide? (rotary holder with cams kind of thing.) That kind of low angle taper could be done pretty easily by a custom cam'd grinder.

Best of luck,
Brian
 
I could see it being done with a dual/spindle dual/turret w/ a gantry and some custom work holding. gantry loads raw disk in the sub, one turret chamfers the bolt circle and tree pans out the hub circle, other turret is drilling out and chamering bolt cirlce on the main.
Both turrets go back position behind the main, bring the sub over and do a press with the Z2 holding a torque. then upper and lower would both take 180deg of the disk with either adjustable angle holders or radial holders with an angled endmill. robot grabs finished from main (expanding mandrel) goes up, sub loads the main, gantry back down and loads sub with blank.

changing tools wouldn't be that bad. I would go with the BMT 12k turrets and use the radial HSK holders. Set off line pretty easy and popping the HSK into the radial holders should repeat length within a few thou...
 
At 15" OD, you're going to be loading these by hand anyway, so not much in the way of lathe automation. I'm not sure I see the benefits of moving away from a decent sized 5-axis mill (e.g. UMC-750 as you've mentioned) vs. a live tooled lathe.

Changing milling tools in a lathe is much more cumbersome than in a mill, and you can fit a lot of redundant backup tools in the mill to keep it running.

I thought a minute after I posted, and I agree with the above post 100%. Must Lathes don't have 7.5'+and- in Y for sure. That doesn't mean you can't do it. And it isn't like you can bar feed them sooooo?

R
 
HI Christie,

I thought about your problem on the drive home, and came up with a way to do it reasonably fast, on a basic 3 axis VMC, **without** expensive custom tapered end mills.

It was hard to tell from the picture: are the disks 'belled' a little, like disker wheels are? If they are, or can be, that'd be helpful.
The reason: I'm imagining bolting these things down to a big plate jig, via a bolt through the hub. If you then screw down against a slightly belled form, you'll get better tension at the rim than just trying to clamp on a flat disk.

But either way, the big trick is climb milling. Not climb milling like the opposite of conventional, like you normally think of it, but taking a normal end mill, and climbing up in the Z axis as you proceed sideways. If you don't care that your cut profile has a slight 'cup' to it, it's a good way to cut a form that's tapered in Z, just the way your parts are. You just cut a bunch of paths that converge from the edge of the disk towards the center point, and climb up in Z as they go. It'll take a little fiddling to get exactly the form you want, but I've done *lots* of this with 2" shell mills, and they work great. The closer to flat the cut is, the less cupped the tool mark is. Looking at your wheels, you might need something like a 1" cutter to get those teeth you're using, but it should work just fine, and is probably at least as fast, if not faster than anything you're doing on a 5 axis. While *not* using custom tooling, and *not* tying up a much more expensive machine.
It does take a little fiddling in CAD to figure out the tool paths, and then probably some hand-tweaking of the CAM tool paths to get them to do what you want, but it's do-able.

Hope this helps
Brian
 
Followup:
If the disks are flat, 'up' climbing is going to cause a fair bit of chatter, since you're pulling up in to air. You *can* do it "down", and press into a jig face, but at that point, a shell mill probably really will work better. You just have to be very careful about your down ramp angle, so you don't over-run the depth of the insert 'stick-down' below the face of the shell, before you traverse into cut material.
The good news in terms of that, for your part, is with a decent sized shell, you probably start off at least half way off the edge, and the thinness of the disk means you probably don't have any real risk of bottoming out the mill, but you do need to be aware of that as a problem when you're calculating your ramp angle.

Best of luck,
Brian
 
I really like this thread, to see the different ideas that you machinists (which I am not) come up with. I learn a lot from threads like this.

I do have a story about polygonal turning tho, lol. I had a customer years ago turning stem pinion forgings between dead centers with tight tolerances on the bearing diameters. They called me in because there were three flats about a 1/4" wide down the length of the parts. This was after a bad crash and they had aligned the lathe with a test bar between centers to zero with z-axis travel. They showed me a part and I told them there is no way that came out of that machine. So they run a part and sure enough, three flats.

I start indicating things and find that the headstock got knocked out real bad towards the operator, and all they did was move the tailstock to match the headstock, so both were pointing towards the operator. When a test bar was spun between the dead centers it had zero run-out, but the parts had three point contacts forged in both ends. When a part was spun between the dead centers it went bumpity bump. That was one for the books.

I should have kept one of those parts to put on my mantel. :)
 
Hi All new here.
I did an exercise in polygon turning on a 2 axis fanuc 21tb lynx200
very rough and not accurate due to a number of factors.
main one being clearance issue of the turning tool.

YouTube

regards
Jorg
 
I could be Wrong, but I thought that Polygon turning involved synchronizing the main spindle and a live tool perhaps at an integer speed ratio.
Here at 20 seconds..
YouTube
 








 
Back
Top