Indexable tool holders

Hi

A while ago I received as a gift a set of 8mm mini turning tools

thought I would try them out today.

I tried to turn 1 inch dia free cutting mild steel and got a very poor surface finish

I was running abt 700 rpm on my Super 7 fine feed 4 thou per rev

the indexable tool holders where not cheapo ones but a good make

what im I doing wrong

Hi Martin,

Not easy to say without seeing your results. Carbide tools want high speed, have you tried increasing the speed? 700RPM for a 1in. diam. freecutting steel is approximately what you might use with a good HSS tool.

Carbide tools also need a rigid setup. I use carbide for roughing and turning hard materials (castings), for finishing I use HSS.

Thor

Hello Martin, Increase the spindle speed 150% and use a good depth of cut as carbide tooling will not cut a fine feed. The carbide tool shears and does not cut like HSS.

Check that the edges of the tool are not chipped as that will give poor finish. The turnings may come off the job hot and blue and that is situation normal.

Clive

Hi Thanks for the replies I will try a higher speed and coarser feed

Should I use any cutting oil ?

Best Wishes Martin

Martin/Thor/Clive - I might end up regretting starting on this, but here goes anyway.....!

The comments re speed and rigidity w.r.t use of carbides are commonly expressed, but they're not the whole story.

Speed is easily dealt with - carbides will cut quite satisfactorily at low speeds. Very low speeds - if they wouldn't do that then they wouldn't be capable of parting off, facing off, or drilling.

I suspect the idea that they need high speeds originates from manufacturers' recommendations that to improve finish one should increase the speed - someone has heard this in the past, and it's been handed down ever since.

Well, the recommendation is correct, but it's being taken somewhat out of context. A common cause of poor finish is the formation of a built up edge (BUE) on the tool tip, caused by material from the workpiece becoming welded to the tip. The formation of BUE depends on the material being cut, the material of the tip, and the temperature at the interface between the two. The normal recommendation is to increase the cutting speed, which increases the temperature at the interface and takes it above the region where welding can take place.

Industry isn't interested in going slower, so that recommendation would not be welcome! We, on the other hand, very often can't increase the speed sufficiently. So do the opposite, and slow down! The interface temperature drops BELOW the welding range, and good finish results.

To further illustrate this effect, we've all seen it many times, albeit without realising what's happening. Imagine facing off a 4" disc - good finish at the outside where the speed and temperature are high, then it falls off part way across as the temperature enters the critical region and BUE forms, and comes back to good when the speed and temperature falls below the critical region. If you were to double the speed for another cut with identical depth of cut and feed, you would find that the 'poor' finish region now occurred at half the diameter.

As far as the tendency to produce BUE goes, somewhat crudely and arbitrarily...

Aluminium/HSS - AAAAGH!

Steel/HSS - Not so bad

Steel/Tungsten carbide - Better

Steel/Titanium carbide - Good

Steel Titanium nitride - Gooder. Sometimes.

So the 'need for speed' is not intrinsically linked to the carbide itself, it's linked to the avoidance of BUE. The suggestions to increase speed will have an effect if BUE is the cause of the problem, as long as you increase it sufficiently to get out of the BUE region, and that depends on the actual tips you have. If you're comfortable with the S7 at top speed, go for it, but if you're not used to this, be aware that the carriage does tend to approach the chuck surprisingly quickly!

Clive's suggestion re increasing depth of cut - yes, try that, as taking more metal off will increase the interface temperature and might help you get away from the BUE region. But as far as not liking fine feed is concerned... well, that depends on the tip. A new Sumitomo CCGT060602 in T1200A titanium carbide will take off less than a thou. at 0.002"/rev, but one designed for turning tyres on 12" scale loco wheels would need a bit more than that!

You could also try going slower, of course, but not so low as to need back gear.

But when trying different rpm, keep the depth of cut and feed the same, otherwise you'll be introducing additional variables into the mix, each of which will affect the interface temperature, and possibly the finish that results. Which would lead to confusion.

Now the website says it was too long, so the bit about rigidity comes in the next posting!

Turning to rigidity (and this is bound to rattle a few cages!) - if a machine/tooling/job setup is rigid enough for HSS, then it's rigid enough for carbides!

The need for rigidity depends upon the forces generated at the tool tip, which depend on the force needed to shear the material (referred to as the specific cutting force), the depth of cut, and the feed. For a given material, depth of cut and feed, it is INDEPENDANT OF THE TOOL MATERIAL. Taking ten thou. off steel at 0.004" per rev. will require the same force at the tool tip whether the tool is HSS or carbide.

In fact, in certain circumstances, the forces with a carbide tool will be LESS than those with an HSS tool. Say your Myford has a 1h.p. motor and you want to shift the steel as fast as possible, using the full 1h.p. (I'm neglecting power and gear train losses here) An oft-quoted and reasonable figure is 1 cu.in. of steel per minute per h.p., so you can do this in one cut at lowish speed using an HSS tool, resulting in a certain force at the tool tip, trying to deflect it downwards.

Alternatively, do it with carbide in 3 cuts at one third depth of cut and three times the rpm, still removing 1 cu.in. of steel in one minute (neglecting time to wind the carriage back, of course!), still using 1 h.p.

Now: Power = Torque x RPM

And: Torque = Force x Radius

Hence: Power = Force x Radius x RPM

And since the RPM is now three times greater than before, the force at the tool tip is only one third of that required to shift metal at the same rate as the HSS tool.

So, assuming that Martin and his machine can get good finish on FCMS with HSS, speed and rigidity are not the causes of his poor finish with the carbide tools. If his S7 is in good condition, then I know for sure that 700 rpm on 1" diameter FCMS is fast enough, and the machine is rigid enough, to give good results. We need to look elsewhere for the cause of his difficulties.

Some questions for Martin:

1) Is the machine (bearings, chuck, slides, everything) in good nick? If not, you need to fix it! Not for carbides, but for all cutting tool materials.

2) Do you get good results with HSS? If not, put away the carbides until you've sorted out things for HSS.

3) Are you an experienced user of your lathe, or still near the bottom of your learning curve? If the latter, see 2) above!

4) Do you know the exact details of the tips that are fitted to your tools? If so, please advise. If not, throw them away. Use of an inappropriate tip is, in my experience, the commonest cause of poor results for model engineers.

5) How do you set the tool to centre height?

6) Can you describe the swarf? Not bothered about colour, it's the form that matters, it will give clues as to whether or not your tool is cutting within it's design envelope. Very short comma shaped chips, short spirals less than say 10mm long, longer spirals, continuous spirals, wirey flat strips with a tendency to wrap themselves around everything?

Martin:

Use of cutting oil. No, definitely not. Carbides need either a full flood of coolant, or nothing at all.

Dripping/brushing it on risks causing rapid temperature changes at the tip, which can lead to micro-cracking of the carbide and premature failure. Also the temperatures that can result when cutting without full flood can cause the coolant to dissociate into unknown chemicals - better not to risk that!

Hello thanks for the info these are the answers

1 yes the machine is in good nick bearings slides etc

very well looked after

2 I get a mirror finish with HSS I grind all my hss blanks myself and use a diamond stone

to get a nice edge

3. Iam a experianced lathe operator been using lathes for nearly 40 years

as a hobby and for a living but have never used inserts have used wimet carbide tools

for cast Iron

4.Yes these are the tools in the set

1 turning and facing 90 degrees with 95 degrees approach Right Hand

2 same as above but Left hand

3 turning with 75 degrees approach right hand

4 same as above but left hand

5 I use a gauge with a spirit level

6 longer sprials

Best Wishes Martin

The fact they are in a set makes their quality questionable, all the name brand holders will not be in sets despite you saying they are a good make.

Can you say what make they are and what make and spec the inserts are. Photo swould be handy too.

J

As has been said already carbide will take a fine feed with no problem and also sets of carbide tools tend to not be of the best quality.

Tony

Hello Martin, thanks for the answers. 1 - 3 bode well for success with carbide tools.

Re 4 - I was hoping you would be able to provide the designation for the tips themselves, rather than the toolholder shapes. Something like Sumitomo CCGT060202-NSC T1200A. It's the -NSC bit that's of particular interest as this identifies the geometry of the chip breaker arrangements moulded into the tip, which in turn determine the ranges of feed and depth of cut for which the tip is suitable.

If you haven't got that information, your answer to 6 provides some guidance - you were cutting on the edge of the tip's envelope, or a little out of it. Have a look at this diagram, cribbed from a Sandvik publication, I think:

Tips are designed to produce comma shaped chips that are easily removed from the machine, and don't clog things up, and they would produce such chips if being used within their intended feed and depth ranges. Longer spirals suggests you're slightly outside the range for the tips you have. That's generally ok, a bit outside the envelope (in any direction) works fine in my experience, but as you are having some difficulties it would be better to have the tip cutting within it's range for now. So adjust feed and depth until you find a combination that gives comma chips.

Now to question 5 - mmm, no experience of those devices, but I can see a potential problem if either the lathe isn't perfectly level, and/or the chuck doesn't hold perfectly concentric - the tool tip could be off centre height. Carbides can be VERY touchy about centre height - get them even slightly above and you're in trouble as they'll be rubbing as well as cutting, which gives a poor finish. You might get away with ever-so-slightly high with a sharp HSS tool, but not with a carbide tip, as they don't have sharp edges. Sumitomo specify +0.000"/-0.0015". That's for a front mounted tool of course, reverse them for one in the rear tool post.

If you have a height gauge I would suggest that you use that for now, and aim for a thou or so below centre. But one thing NOT to do when setting a tool to height is to use the old trick of trapping a rule between the tool and the work - this kills carbide tips, stone cold dead. Micro-cracking again. Never let a tip contact stationary metal, they don't like up 'em, Mr Mainwaring, they don't like it up 'em.

Pah! Call that swarf?

My record is over eight feet of tightly coiled stainless steel, that's real swarf.

Neil

<who won't mention that it was a somewhat shorter length of swarf that snaked into the control box and blew up the PCB on his mini lathe>.

Pah! Call that swarf?

My record is over eight feet of tightly coiled stainless steel, that's real swarf.

Neil

Something like this?....

Yes, that's swarf. Nasty stuff, gets into lots of places you wouldn't want it to get into ..!!! I'll stick to chips with everything!

Something I forgot to mention, another check for a carbide tip cutting correctly, as intended. Watch the formation of the chips (or swarf, if you haven't got it right!), and you should see the waste material being directed to the left of the tool, in the direction of the un-machined surface. If it's going the other way, right and towards the newly machined surface, then a) something is wrong, and b) it can cause poor finish if it contacts the newly-cut surface.

Cabeng: Blimey, those are some of the best posts I've ever read regarding the use of insert tooling, not just on this forum, but anywhere.

I tend to use insert tooling as a matter of course on my centre lathe, with HSS and gauge plate used for specials and form tools. Generally I can get a finish on the order of 1-2µm Ra, but it's not as consistent as I would like. Your posts have certainly illuminated a few lightbulbs for me. I wondered why the finish changed from state to state, and then back again when facing a large diameter. Plenty to think about. I think I need to pay more attention to what I'm doing, rather than 'winging' feeds and speeds, based on experience.

Being a technical pedant I would point out that for consistency of units power (W) equals torque (Nm) times angular velocity (in radians/second), rather than rpm.

Now, a question on turning aluminium (6082) if you don't mind. I use Korloy CCGT-09T30x-AK inserts, specifically for aluminium. Generally the swarf exits stage left, which is good, and I get an excellent finish. But apparently at random the swarf can suddenly create a birdsnest, which gets trapped between the tool and work, giving a dull finish. Any advice?

Regards,

Andrew

Totally agree with Andrew J as what he wrote is almost exactly what I would have said. His turning experiences are exactly what I see too.

Cabeng has put on paper a full treatise of the why's and wherefore's of tipped tooling. Its sensible, balanced, and worthy of publishing to a wider audience. It might silence some of people that slag off carbide and say HSS is all the model engineer should use.

I know that some of the information he passed on is freely available in manufacturers catalogues and data sheets, but often only after you've registered and downloaded massive PDFs do you then discover you have to trawl through scores of pages of parts numbers just to find the odd page or two that mean something in plain english.

Cabeng, it would be great if you could submit an article to one of these two hallowed magazines. it would make the subscription good value on its own.

Ian P

Excellent suggestion - Andrew

Yes some very interesting posts there, thanks Cabeng.

The inserts Martin is using are CCMT 060204 but being of far eastern origin the chances of any more info on their spec is unlikely. The holders themselves are not by an industrial maker but one of our hobby suppliers and with the addition of some decent inserts will work fine, I have several of the same make holders.

Would it be possible for Caneng to suggest a few suffixes that we should look out for that would be suitable on hobby lathes

Andrew, variable speed helps here and my suck it and see approach to speeds. Any calculation of cutting rated can only be an average over the ever changing diameter when facing.

J

I'd like to second(?) the positive comments about Cabeng's guidance on the use of inserts. Very good advice for someone coming from a 'big' machine shop where inserts rule the roost. As my expertise is in the coolant/lubricant side I rarely get to see the results of tip changes.

Thank you Cabeng

Jerry

Thanks Cabeng. Some very useful information. I'll have to play a bit more with different forms of tip.

Just one question if I may: Does your +0.000"/-0.0015" tolerance on tip height apply specifically to facing where you are cutting down to zero diameter or to all turning?

The reason I ask is because if I'm turning a 40 thou diameter clock pivot then 1 thou height error will give a 3° change in clearance angle which could be very detrimental while the same error when turning a 5" diameter loco wheel would only change the clearance angle by 0.02° which would seem to be unnecessarily precise. Can you give more guidance, perhaps in terms of the angular error permissable?

Rgds.

Russell.

Jerry:

Very good advice for someone coming from a 'big' machine shop where inserts rule the roost.

Who would that be, then? Certainly not me! Strictly amateur at metal cutting, albeit in the original sense of the word amateur, meaning 'lover of'!

But I've been involved with the metal manufacturing trades for 40+ years, as someone who designs bits and pieces and then gets someone else to manufacture them. As my technical education and training included all the metal working processes, my designs could usually be made straight from the paper, but of course they could always be improved for manufacture, so the manufacturer was always welcome to help me refine things. That led to very good relationships with the machine shops, with lots of knock-on benefits for Home Office jobs!

One was helping me to sort out my parting problems and introduced me to carbide parting tools some 25 years ago. They introduced me to a local tool supplier, who in turn introduced me to a manufacturer's technical department, and it all developed from there. Whenever I had a problem, they not only helped me to sort it out, but also contributed significantly to my education in these matters. Provided tips for me to try out, and lots of technical information and back up, even to the extent of visiting a few times. Well over and above what the call of duty required. Sandvik even provided a copy of their book 'Modern Metal Cutting', even though it was officially out of print and unavailable!

Add to that a willingness to turn perfectly good bars of steel into nothing just to find out how things worked out, to photograph it all, then inspect tips under a microscope to look at their wear and failure characteristics to identify what was going wrong, and it all added up to something useful.

Thanks for the favourable comments, very much appreciated, But as far as articles are concerned, well... they were written some years ago, and offered to ME towards the end of David Carpenter's reign. I won't go into the saga here, but let's just say that after some considerable time things did not progress to publication. It wasn't a satisfactory experience, and I don't want to repeat it. Sorry!

Separate postings for replies to other comments/questions.