Boring chatter (on the lathe)

I want to bore a hole 18mm deep and about 84mm diameter in the end of of a 150mm diameter 100mm long EN1A round bar. The work was set in the 4-jaw:

and I started out by drilling to accept the 12mm boring tool.

Then I started boring with a 0,4mm tip CCMT insert at 200rpm with 0,2 mm/rev feed, and an 0,5mm DOC. All went smoothly until I got to about 40mm diameter, when horrible chattering set in.

My first thought was that it was to do with increasing surface speed as I opened the bore, so I reduced the rpm, but that didn't help.

I'm struggling to understand why there should be such a dramatic change in behaviour over such a small interval. Maybe some sort of resonance?

Robin.

At a guess I would say the overhang from the chuck isn't helping much. I think I would try an HSS boring tool and drop the speed right down.

Paul.

If you have a fixed steady, use it to support the end of the job.

200rpm might, counterintuitively, be a bit slow for insert tooling. Try speeding up to 400 or so. Plus inserts dont like light cuts so you might try deeper cuts.

At that diameter and depth you might even get in there with a normal turning tool at a suitable angle which could be more rigid.

Bigger boring bar needed.

As Hopper suggests, a turning tool may have enough clearance.

Jim

Try it taking cuts off the face working from middle to outer edge then a final cleanup along teh 80mm dia. Although a bigger bar would help you are not going that deep so overhang will be minimal. Somethines you just hit a diameter that at a certain speed starts to ring, modulating the varii speed pot can help.

200rpm when only at 40mm dia is slow, I'd be about 800rpm at the full 80mm dia, 1mm DOC

If you've got a 3-point steady that'll accommodate such a large diameter, that would help. Failing that, I think it's necessary to accept that the op's being done in less than ideal conditions and look for whatever mitigations are possible.

At 18mm deep I'd say it isn't really a boring bar job. I'd look to modify an HSS turning tool as Paul Kemp suggested by sweeping away enough LH side clearance to avoid contact for about 20mm, and point it straight into the face with a little bit of plan trail angle, make sure it can cut across the bottom face at well, and that it's very sharp so as to minimise cutting load. Jason's way of starting in the centre and then boring with reversed feed using light cuts away from the chuck also has a good chance of working. You might need a couple of very light cuts to start with to skim off the chattered surface to stop it copying itself to the next passes, or OTOH it might work better to dig beneath the chatter - I think I could only tell by trying it.

Have you checked the tip, sometimes a tiny flake comes off that's hard to see?

I now only use steel inserts on hard spots. Try CCGT, much sharper.

To save confusion my suggestion was to cut across the axis from ctr to outside not backing out of the hole. Doing it this way the cutting speed at the tool's tip will constantly be changing so it will move through any speed/diameter related resonance

For an 18mm deep bore, it would be best to have only 20mm of the bar projecting and set the saddle stop to prevent the toolpost from hitting the work. As the nornal indexable boring bar has the tip height much lower than turning tools, a 16mm bar would be a better choice. The gibs on the saddle if adjustable and the gibs on the cross slide and compound should be checked. If you can change the insert for another grade, it's worth a try.

I am currently modifying a 25mm boring bar to fit in a larger toolpost which will be attached directly to the cross slide of the Smart & Brown model A which will greatly stiffen up the boring of holes bigger than 40mm. Even at 25mm diameter, the Sandvik bar is marked at 100mm for maximum depth.

Edited By old mart on 06/09/2020 15:59:27

have you an example of this, All the catalogues I have seen that have the insert sloping still set it so the tip is on ctr height where it contacts the work

Absolutely correct JasonB.

I was refering to the tip height relative to the bar height. There is an example of a Glanz 12 mm bar from Chronos with the tip height about 6mm from the base. Ebay 333281987078. The 25 mm Sandvik bar I have has the tip height at about 12mm. I have shims to fit under all my 20mm bars, wheras all the 20mm turning tools are reduced to 17.53mm to use without shims.

If you go to a smaller 0.2 radius insert, it will get rid of a lot of the vibration and has a reduced tool pressure when cutting. For best results with boring bars, you actually want them about a thou or 2 max above centre height. When on or below centre height , the bending load on the bar, makes it take a bigger cut. When slightly above, the load comes down to the centre height and has almost no increase in cutter load. Technically it is reduced by a smidgeon depending on the diameter of the work piece.

Use a milling cutter as your boring bar.

Martin.

A big blob of 'Blu Tack' placed onto a boring bar works well to dampen vibrations due to it's strange 'Non Newtonian' properties.

This is not a joke, I learned enough about Blu Tack from an MEW article a few years ago to design a unique barrel tuner for a rimfire target rifle.

* Danny M *

+1 for the blutack. Even plasticine or putty will do at a pinch. I think it's something to do with the added weight changing the resonant frequency.

Rod

I get my inserts from Cutwel and live by thier recommended feeds/speeds/depths of cut using anything between the min and max recommended depending on the strength of the setup and part, but almost never outside of this.

 You are perhaps not by coincidence running almost a similar speed/feed to what I would use on my NC5330 coated CCMT tips (I use Korloy CCMT09T308-HMP) - keeping in mind I'm on a Colchester with 20mm tooling.

Feed's are recommended 0.1-0.3mm/rev, .....check

DOC 0.5-3.0mm ..... check.... but 0.75-1.00mm might solve your problem if your lathes up to it.

However...... 200rpm.........I would be aiming between 130-300 meters/min surface speed, you're under 30! As you approach 40mm you want to be SLOWING down to around 1000rpm (=130m/min) - if the chips aren't purple and bouncing off the ceiling, you're not doing it right.....

Worth noting.... my colchester has an automatic cutoff on the depth, so I can let it loose at 1000rpm&0.2mm/rev fairly care free, my Myford 280 has a graduated handweel on the saddle, when things are moving fast I mark the depth on the mm scale with big bright bold marker so I cut the feed when I get to the depth, requires concentration, and a knack......

Edited By Russ B on 07/09/2020 13:00:04

Edited By Russ B on 07/09/2020 13:03:30

Many thanks for advice. I was worried by a post I'd read somewhere (possibly practical machinist) which said that once chatter had set in you'd had it, because the texture (something like basket weave in my case) would just set the tool bouncing again. So I took a light skim with a CCGT insert to try and restore the finish to something more like normal. The CCGT inserts I have are grade H01 and intended for non-ferrous metals I believe, but it worked. Because I was close to finished size and the CCGT was cutting so nicely I just carried on with 0.25mm cuts and got where I wanted to be.

I still have the other end to do (it's a VMC riser, about which I have posted before) and shall try the tricks which have been suggested - I've obviously been wimping out on the rpm with CCMT inserts.

I'm not totally convinced that my problem is altogether to do with the rigidity of the tool though. I have often bored 50mm+ in 3" steel bar using the same tooling and not had the whisper of a problem. But in this case, with the mass of the 4-jaw and the work combined I'm hanging getting on for 40kg on the spindle. The lathe+stand is about 600kg. A significant fraction. The stand is sheet metal so not as rigid as it might be. It could be that I have (over)reached the lathe's capacity. At least as far as industrial speeds/feeds go!

Robin

Edited By Robin Graham on 07/09/2020 22:44:09

Just to let you know how it went...

Despite my worries about the lathe not being rigid enough, after some experimentation with speeds, cuts and feeds I found some sweet (and more sour!) spots. Because I was experimenting using manual feed I can't give numbers, but the general rule seemed to be (counterintuitively) that when the machine starts to complain, increase the feed.

Anyhow, I got there:

and made some blue chips in the process. By the time I'd finished the work was at 65 degrees C!

Thanks again for advice, Robin.

Edited By Robin Graham on 08/09/2020 21:54:06

If it was 65 degrees the spigot is likely under-sized, now it has cooled down.