Turning long thin work on slant bed CNC

Ray51 · Jan 19, 2021

My first post and rather a difficult one to address. I was advised by a good mate to come here, as he said, if the answer is out there, this forum will have it.

The issue I am trying to solve is turning 304 stainless bar on a Puma 2600Y slant bed CNC. The job requires parallel turning 300mm long * 14mm diameter and so far its been a pain in the butt. I have managed to reduce most of the vibration, but not enough as I still need to put the job in a manual lathe to polish it satisfactorily enough for delivery to the customer.

Being a slant bed, there is no steady rest available for it. Currently I'm running a WNMG with a 0.8 nose radius as the roughing tool at 160mpm and a clamped spindle speed of 750. Finishing is with a DNMG 0.4 nose radius at 180mpm and a clamped spindle speed of 500

DouglasJRizzo · Jan 19, 2021

Ray51 said:
My first post and rather a difficult one to address. I was advised by a good mate to come here, as he said, if the answer is out there, this forum will have it.

The issue I am trying to solve is turning 304 stainless bar on a Puma 2600Y slant bed CNC. The job requires parallel turning 300mm long * 14mm diameter and so far its been a pain in the butt. I have managed to reduce most of the vibration, but not enough as I still need to put the job in a manual lathe to polish it satisfactorily enough for delivery to the customer.

Being a slant bed, there is no steady rest available for it. Currently I'm running a WNMG with a 0.8 nose radius as the roughing tool at 160mpm and a clamped spindle speed of 750. Finishing is with a DNMG 0.4 nose radius at 180mpm and a clamped spindle speed of 500

There are straddle type tools that can utilize the Y axis and straddle the part as you cut. I think Sandvik makes one.

implmex · Jan 19, 2021

Hi Ray51:
Have you considered trying to knock together a quick and dirty roller box tool?
Or maybe buying one if you can justify the cost?
It might take a good bit of screwing around to get it to cut a consistent diameter, and it;s a one-shot deal in that you can't take a second cut but it has been known to work well once the kinks are worked out.
For inspiration check out how old fashioned manual turret lathes were set up for long skinny turning...box tools were common in bygone days.
Something like this:
Boyar Schultz box tool with carbide insert conversion cutting 01 tool steel. - YouTube

Here's a Youtube link to a more modern one on a CNC lathe:
Tangi Flow Roller Box 2015 1 - YouTube

However, if you have a lot to do, you may still be better off overall finding a vendor who has the gear to do this easily.
This cries out for a Swiss or a centerless grinder.
These machines can do a far better job than you'll ever do on a conventional lathe, without even breaking a sweat, so there comes a time when it stops being worthwhile to keep breaking your head over it.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Milland · Jan 19, 2021

You might try roughing with whatever method works to ~14.5mm, start turning the finish diameter from the live center end about 15mm in, then draw back and reposition to the right, and M0.

At that point, you'd want Y to be at the final diameter, and using some "miraculous" fixturing manually attach a pair of small sealed ball bearings that will perform a follower function, starting from the pre-turned 14mm and then riding on the freshly cut surface as you finish the cut length.

You'd then have to M0 again, manually remove the follower bearings, and finish facing or tool retraction.

How you set up the follower bearings is a matter of available fixturing, precision needed, etc. A really fancy setup could swing the bearings in using spare M codes and a servo-driven pivoting mechanism, but unless this is a recurring job I doubt you want to get that fancy.

Something similar using rubbing blocks of a good plastic might work, especially if you could flood them with coolant to both lubricate and flush chips away to keep them from getting embedded.

Just some idle thoughts, hopefully someone has a better/simpler approach.

Bobw · Jan 19, 2021

More info please.

1) starting stock diameter.

2) TOLERANCE!!!!!

3) Tail stock.. Si or No?

mmurray70 · Jan 19, 2021

I do 1/2" stainless shafts fairly often at about 9" long. I only need to take off about 10 thou, finish size is 12.5mm or 0.492.

I run about 1000 rpm, use razor sharp aluminum tools (ground inserts) to reduce forces. I think the feed is around 0.004, but not 100 percent sure now. I usually take one pass, and then a spring pass at same depth. Gives pretty good finish. Light sanding after and its good to go.

Edit: Also box tools are pretty neat. I bought one to try on this job, but never did get around to trying it. Got it running pretty good on cnc by the time box tool showed up lol

Ray51 · Jan 19, 2021

Thanks fella for all your solutions, one of which I'm sure will work for the future as we get a lot of jobs of this nature (we custom make temperature thermowells)

Bobw said:
More info please.

1) starting stock diameter.

2) TOLERANCE!!!!!

3) Tail stock.. Si or No?

25.4mm

+/- .1

Tailstock in place.

wmpy · Jan 19, 2021

So, you're using a tailstock and still getting vibration? Then I'd look at your finishing insert. Make sure it's a sharp geometry meant for low-pressure finishing. Maybe switch to a 0.2 mm radius. And then look at how much material you're leaving with the rougher. This may be a case where it's better to leave more material so that the part has more rigidity. Heck, you might be able to put in a ground, positive finishing insert meant for Swiss turning and take the whole cut one pass at a slow feed.

TheBigLebowski · Jan 19, 2021

I have recently been thinking about methods for turning thin parts and came up with an idea.

For turning long very skinny parts, wouldn't it be easier if they could be slightly tensioned between the tailstock and chuck. (rather the compressed)

Is there any good reason this isn't done?

norb · Jan 19, 2021

I have a Tangi Flow box tool that I used to turn some stainless rods from .5 to .250 dia. about 6 inches long for threading with a geometric die head. It worked well.

gregormarwick · Jan 20, 2021

Going from 1" to 14mm is a higher DOC than I've personally done before, but I've had surprising success on long skinny parts by taking one pass to size using a VBMT/VCMT. With the fairly large stock diameter there might be enough rigidity to get away with it, definitely worth trying. VBMT1604 has enough edge length.

The quality of the live centre, condition of the bearings, has a pretty significant effect on the outcome when doing this.

Whatever you end up doing, positive geometry inserts are an absolute must for something like that. The WNMG is about the worst case scenario for what you're trying to do, and the DNMG is marginal depending on what the top rake geometry is like.

Booze Daily · Jan 20, 2021

You might try doing it Swiss style. Rough and finish 1” of length at a time. The stock size should be able to support that.
If you arc in and out of your finish cut there probably won’t be much of a transition mark.

Kiwi 'smith Dean · Jan 20, 2021

Trying to do 14mm diameter at 300mm or longer length is going to create chatter at some point. It's similar to the problems with profiling rifle barrels.
Once the diameter to length ratio gets too long, you usually have to go to some sort of fixed steady rest in the mid-section, or a follow-steady. On tapered barrels it's often a pneumatic or hydraulic follow steady.
Pinch turning or balanced turning (dual 'balanced' cutting edges) can work well if set up right.

On some CNC lathes you also have a variable or ocsilating spindle speed option on the control, for getting a better finish on long parts that would normally chatter badly if a bad resonance starts to trash your finish. Google 'Haas SSV' on youtube for an example of that.

Dean.

SIM · Jan 20, 2021

Light cuts can lead to chatter...especially in 304SS. I'd start by roughing, leave .2-.3 per side then finish with a sharp ground cemented carbide tool. Or maybe a positive sharp carbide insert meant for aluminum.

at +/-.1 tolerance another choice would be to leave a substantial amount on shaft for one heavy last pass to size. The material itself offers the support.

As its outside the norm its trial and error..adjust and try again.

Ox · Jan 21, 2021

Booze Daily said:
You might try doing it Swiss style. Rough and finish 1” of length at a time. The stock size should be able to support that.
If you arc in and out of your finish cut there probably won’t be much of a transition mark.

Tapering in / out, or in his case - arc, will yield a good part, but it will leave witness marks as the arc/taper in and out produces different ship loads, and thus - while the major part of the turn may be shiny, the ramp segments always come out cloudy.

If you spin some emmory over it in the end anyhow - that would trump any concerns here.

I think that the EU is almost on mainland US by the sounds of Staten Island. :eek:

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

Think Snow Eh!
Ox

SIM · Jan 21, 2021

Ox said:
I think that the EU is almost on mainland US by the sounds of Staten Island.

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

Think Snow Eh!
Ox

Hey, make sure you smile when you mention Staten Island....

Search

Largest Manufacturing Technology Community on the Web

Search

Turning long thin work on slant bed CNC

Ray51

Plastic

DouglasJRizzo

Titanium

implmex

Diamond

Milland

Diamond

Bobw

Diamond

mmurray70

Stainless

Ray51

Plastic

wmpy

Hot Rolled

TheBigLebowski

Aluminum

norb

Cast Iron

gregormarwick

Diamond

Booze Daily

Titanium

Kiwi 'smith Dean

Cast Iron

SIM

Titanium

Ox

Diamond

SIM

Titanium

Similar threads