By continuing to use this site, you agree to our use of cookies. Find out more
Forum sponsored by:
Forum sponsored by Allendale Jan 24th

Boring chatter (on the lathe)

All Topics | Latest Posts

Search for:  in Thread Title in  
Robin Graham06/09/2020 00:34:16
874 forum posts
261 photos

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:

boringvmc_riser.jpg

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.

Paul Kemp06/09/2020 00:51:34
689 forum posts
18 photos

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.

Hopper06/09/2020 01:38:18
avatar
5505 forum posts
137 photos

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.

jimmy b06/09/2020 06:22:16
avatar
739 forum posts
42 photos

Bigger boring bar needed.

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

Jim

JasonB06/09/2020 07:11:35
avatar
Moderator
21435 forum posts
2448 photos
1 articles

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

Mick B106/09/2020 12:03:25
2018 forum posts
116 photos

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.

Dave Halford06/09/2020 12:15:15
1726 forum posts
19 photos

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.

JasonB06/09/2020 13:04:28
avatar
Moderator
21435 forum posts
2448 photos
1 articles

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

old mart06/09/2020 15:57:01
3345 forum posts
208 photos

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

JasonB06/09/2020 16:03:35
avatar
Moderator
21435 forum posts
2448 photos
1 articles
Posted by old mart on 06/09/2020 15:57:01:

As the nornal indexable boring bar has the tip height much lower than turning tools, a 16mm bar would be a better choice.

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

Baz06/09/2020 16:08:51
578 forum posts
2 photos

Absolutely correct JasonB.

old mart06/09/2020 16:37:58
3345 forum posts
208 photos

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.

Neil Lickfold06/09/2020 20:33:24
720 forum posts
127 photos

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.

blowlamp06/09/2020 20:59:22
avatar
1516 forum posts
98 photos

Use a milling cutter as your boring bar.

Martin.

Danny M2Z07/09/2020 08:19:10
avatar
936 forum posts
1 photos

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 *

Rod Renshaw07/09/2020 11:44:57
325 forum posts
2 photos

+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

Russ B07/09/2020 12:56:49
600 forum posts
26 photos
Posted by Robin Graham on 06/09/2020 00:34:16:

.....EN1A........

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.

....

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

Robin Graham07/09/2020 22:38:02
874 forum posts
261 photos

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

Robin Graham08/09/2020 21:51:48
874 forum posts
261 photos

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:

img_2407.jpg

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

not done it yet08/09/2020 22:39:31
6321 forum posts
20 photos

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

All Topics | Latest Posts

Please login to post a reply.

Magazine Locator

Want the latest issue of Model Engineer or Model Engineers' Workshop? Use our magazine locator links to find your nearest stockist!

Find Model Engineer & Model Engineers' Workshop

Latest Forum Posts
Support Our Partners
walker midge
BOLDON
Eccentric July 5 2018
emcomachinetools
Warco
cowells
JD Metals
rapid Direct
Eccentric Engineering
Subscription Offer

Latest "For Sale" Ads
Latest "Wanted" Ads
Get In Touch!

Do you want to contact the Model Engineer and Model Engineers' Workshop team?

You can contact us by phone, mail or email about the magazines including becoming a contributor, submitting reader's letters or making queries about articles. You can also get in touch about this website, advertising or other general issues.

Click THIS LINK for full contact details.

For subscription issues please see THIS LINK.

Digital Back Issues

Social Media online

'Like' us on Facebook
Follow us on Facebook

Follow us on Twitter
 Twitter Logo

Pin us on Pinterest