Turning on a Horizontal Machining Center

First of all, let me say that I am not currently in need of this technique. I'm am just curious about how the heck you do this.

I saw this video today while killing some time and have to say that I think it's pretty cool.

How do you program this? I understand the basic math behind it, but the excel and decel to keep it timed correctly. Maybe you have to start off the part in Z then move in? Maybe I just answered part of my question, but I know that you have to keep the orientation of spindle perfect to the XY position. How do you program that? Is this an option of some sort? I feel like I am missing something.

Hopeful I posted this link correctly.

YouTube - New Okuma MA-600H CNC Horizontal Machining Center ID#5373

This was posted a year or so ago. IIRC it was a special routine / option unique to that machine control.

Let me add that if I ever wanted to try this my machine is a Makino A-88 Horizontal Machining center with a Pro-3 control, or basically a 16i with all sorts of bells and whistles.

Yeah - that was new released at IMTS 2006 I think.

I am sure that it is a canned cycle. You don't need to figger all that out.


I think someone else has that out on an HMC now as well. Also - I have seen something like that used on a transfer machine a cpl yrs ago as well.


----------

Think Snow Eh!
Ox

It's interpolation just like anything else, except it's tied to the spindle encoder. Lots of gee-whiz.....but not very technically difficult.
Mazak had different concept on that at IMTS this year.

I used to work in the building that that demo was shot in.....


Husker

I thought that you might have been around that Husker.

Alright, so I got the idea that it's a special cycle. Seems pretty simple but if the machine isn't setup for it then it really can't do it.

I was hoping, in the back of my mind, that since most machine nowadays have an encoder on the spindle (for rigid tapping) that this was something most machines could do and I was just over looking how to program it, sort of like the first time you macro program or rigid tap. While I have been a machinist for a long time, I love it when I learn a new trick.

Too bad because I am sure that somewhere down the line this would really come in handy.

If only there was a way to cheat it. Something like programming in IPR instead of IPM which would tie in the spindle and the XY movements. I can only imagine what would happen if things are not orientated correctly.

Oh well, better luck next time.
Thanks for the replies!

I thought the video you posted was gonna look more like this:
YouTube - Methods Machine Tools Matsuura Cublex-25 Mill-Turn 5-Axis

Matt:

I would think that you would have some hdwr requirements that need to be met first.

1) Loads of low end trq. Likely a geared head.

2) Fast X and Y rapids. (Linear?)


I doubt that the macro is all that involved other than processor speed to be able to keep up?


---------

Think Snow Eh!
Ox

It's not particularly unique. MY Kitamura HX400 can do it and it goes back to 2002

YouTube - Kitamura's CNC Turning Function

I noticed Mori has it on their horizontals at IMTS as well.

It is a relatively simple interpolation issue. While it allows the ability to generate certain tapered profiles, it is quite slow compared to other methods of achieving the same result. I had the mori guy at the show look at me and tell me there was no other way to machine the part they were demonstrating. I laughed and said, I'll bet you your machine.... For all the time it took to single point turn it, and it was a relatively small feature, I'd have had a tool ground to the profile and come in fro the side and interpolated it and moved off and been done. Just like milling a thread with a thread mill. Sure it doesn't work for onesee twosee parts, but for thousands like you would do on a horizontal.... puleeeeze. Don't you hate it when someone says theirs is the only way....

Okuma Turncut

Been using this function on our Okuma MA600-HB for a while now.
It was a £15k option comprising of.....
Software
Uprated servo's
Cooled ballscrews
Glass scales.

I posted the video below when we first got the machine.
With the WNMG boring bar it machines......
OP1~15° taper, straight bore 60mm deep, 20mm rad, 45° taper
OP2~Scroll face
OP3~ O/D profile.

YouTube - Turncut

The cycle is turned on with a few G-codes and then programming is done in XZ as on a lathe. There is no canned cycle (eg G71) so each line is programmed manually. Macro programming helps loads here. Also you cannot change rev/min once the cycle is active. Single point taper thread turning is easy when you don't have the reqired tapered threadmill. Just use a threading bar from the lathe with the correct insert.

I'm just proving out a new job this week. A forging weighing 210kg. It needs milling and turning. It's kind of a large tube with a flat baseplate, to put it simply. The milling is as normal. The turning reqires an O/D of 295mm, 80mm long with a 15° taper on the front face. Then at the bottom of the forged bore there is 16mm depth to come out. This requires a 230mm bore leading into 7mm x 45° taper (with 3mm connecting rads) and machining the bottom face, which is 680mm deep. Handling and setting up/re-jigging this kind of component all adds valuable time and can cause alignment errors. Mill and turn in one set up will save loads of time. The turning will be slower than on a lathe but we don't have a machine to take anything this size.

What kind of tols/roundness specs have you been able to hold with this routine so far?

Maybe your parts are fairly open tols? Or have you found the limits?

Doo you find that a bigger offset on the bar offers advantages? I would think that the closer the tool is offset to the actual size desired = less slide travel, should likely = some better roundness specs if nothing else?


----------------

Think Snow Eh!
Ox

Tolerance

No more that 0.02mm out of round. Not been asked for any tighter.

You're bang on there, Ox.

Roundness is not a problem but trying to get the cutting speed up is. The offset bar is deffinately the best way. The least amount of XY travel the better.
I use a spread sheet supplied by machine tool seller to work out max revs. Up to 2m/sec (axis travel) will hold 0.02mm roundness, although I've found higher still stays within stated tolerance. Up to 4m/sec can be run for 15mins. And above 4m/sec will alarm out~over speeding~.

On the forging that is on now, we made an offset O/D tool similar to the one in the video in the first post. We used a 25mm shank WNMG turning tool and used 2mm DOC and 0.5mm/rev feed. Spindle was running about 100 rev/min. I think that gave 90m/min cutting speed on a 295mm dia. A bit slow but it chewed it off.

It's fun to use too.

4M/sec?

You have GOT to have linears on that then eh?
(motors)


------------

Think Snow Eh!
Ox

Looks more like a "Cool Factor". Although if you have a need for it, I guess it become a priceless option.


Tooling comes loose or a drive hiccups and that becomes a nasty mess...to say the least.

Ooops

Ox said:

4M/sec?

You have GOT to have linears on that then eh?
(motors)


------------

Think Snow Eh!
Ox

Click to expand...

Ooops, yeah should be....acceleration = 4m/sec²

Just making sure you're paying attention.

The formula used in the spread sheet is (not checked it, just use it).......
a=acceleration
d=interpolation diameter

n = 60*1000 SQR(d/2000*a) /(d*Pi)
a = (n²*d*Pi²)/1800000

I'm outta my league here, not even owning a horizontal, but is that really "turning?" The work isn't rotating, so you don't have the control over concentricity that a lathe spindle normally provides.

It seems more like an external boring bar than anything else, although the simultaneous spindle-X-Y coordination is pretty impressive. Heck, is there any reason you couldn't do ovals, cams, or custom profiles with that kind of technology?

Pics

CCC....tell me that doesn't look like it's been turned






It's a compromise of course. It's more like a horizontal borer but more versatile. You can get lathes that mill but we needed a Horizontal. Fortunately we could put a "turning" function on it. There's plenty of milling on the other end of the part. Then I can tool change, spin the job around and turn that end in a few minutes. How much handling would it take to put it in yer lathe and turn it? More than a few minutes. With the Horiz, the 2nd op is being loaded while the machine is still cutting. So the machine never stops. While loading this in a lathe the machine is stood.

Incidently the bore at the front was done with a boring head. Plunge in, and out. Quick, yep. But that's a £600 tool dedicated to that one bore and can do nothing else. Yet the turncut tool can turn many outside dia's and face, rads, angles etc....within reason.

Tried doing the bottom bore/face today but found out the jig's not sturdy enough. Needs beefing up. Had to make a boring bar 680mm long 125mm dia. Made the 50 taper look small. I think I'm finding the limits!




We also do face grooves with it. Drawing specifies corner rads on top and bottom of groove. Mill it and you need a custom tool (for each size/spec), turn it and you just use a common face groove and program in the corner rads.

CCC....I id see a video of an oval face groove. There's no function on ours for this but have noticed you can scale the axis in the program. Might not be very accurate but suppose it could be done.

http://www.bankbottom.co.uk/video/test2.wmv

I'm going on a bit now, aren't I. I'll get my coat.

I would think that at $30K - that would be an option that I would have on mine! If your running much work on big HMC (CNC HBM?) this could make a LOT of difference if it holds as good as you say!


Some bells and whistles are just that, and others are werth ringing and blowing. I'd ring this one!


------------------

Think Snow Eh!
Ox

I'm not trying to be negative - that's some very impressive capability, and nice work on your part.

I think people will be expanding it in the future to shapes that aren't round. Somebody on here a while back needed an odd-shaped groove for a seal in the face of a part. Tool marks needed to be parallel to the groove, so end milling was out - this thing could pull it off, in theory at least.