weird insert problem

so i turned a 30 mm free machining steel piece to 16 mm over 90 mm:



i turned the insert around for the job to use a new edge and this is what it looked like when i was done:







dead sharp, though, giving superb finish.



what has happened? its a sandvik coromant dnmg 15 06 16-15 insert.

(dnmg 444-15, 415 p-k15 7n467292. whatever that stuff means.)

the only "mistake" im aware of i made is going too slow, starting at 800 rpm.

any thoughts?

Looks like maybe the cutting edge is above centerline?

Positive carbides are inherently weak. It seems like the increased speed sometimes helps get rid of vibrations in the cross-slide that want to chip the carbide, and rather forces everything into a more stable setup.

They are also sensitive to certain operators technique. I have never pinpointed the exact difference but have co workers who can wreck the insert almost every time they use the lathe.

You might also try putting the long symmetrical axis of the insert dead square to the part rather than like a ccmt.

Which way was the chuck spinning?

His problem is NOT the bad broken edge. That's actually why it is GOOD finish.

Look at it closely in the picture of the broken part. Look at the edge near it where not broken. The broken place is sharp like HSS in comparison, the rest of the insert is more dull. Not ONLY that, but the way it broke forms a sort of chipbreaker, which is probably improving the finish by not rewelding a built up edge onto the part.

So I think the broken part just happened to form a very good edge for this material. Naturally, since you stopped the turning, you will probably never get back to that "magic" condition. But you have a suggestion of what that material wants. It apears to want dead sharp HSS with a chipbreaker. Unless of course, you can get a grind on carbide just like it.

insert was dead on center and i was taking 2-3 mm cuts and powerfeeding. seemed easy, chips were just flying off. so did it break because i wanted to get to the shoulder? then i should remember to use this tool straight in the future.

Roughing down from Ø 30 to 16 I should do with a WN insert, negative geometry, SCEA minus 5 degrees*; 240 m/min or 787 surface feet per minute cutting speed which calls for 2728 rpm on the first cut of Ø 28 (depth of cut 1 mm). At Ø 16 spindle speed would mount to 4774 revolutions per minute.

Mild steels, structural steels, are chip welders, means the single chips are melted together into long bands. To overcome this you set the tool inclined for a rather skiving action. Carbide inserts work best when enough energy is converted. You press the steel too slowly on a DN insert but should better race it. D-form inserts, by the way, are special inserts for threading actually, the corner angle is 55 degrees destined for Whitworth and pipe threads.

Inserts have different chip breakers. Get in touch with one manufacturer and become informed. It’s also about coating(s), fastening, holders, coolant, rigidity and power of your lathe.

My 2"
______________________

*Allows face and plain turning

Ditto..

HSS and free machining steel work well, why bother with a hard dull plow, when a soft (sharp/tough) knife can handle the material??

i dont use hss for general work (sometimes when parting off), its not worth the time and effort. and again, this was free machining steel (11smnpb30+c) that comes off almost by itself. the insert should have lasted for hours, not seconds. i dont think d-type inserts are for threading, as a matter of fact they are my favourite go to inserts for general work, on angled holders you can face with.

well, i guess i just had a bad insert. on the other hand i had used the first edge for a while.

and btw, my lathe is old (reiden) and does good work. i dont like to run it above 1400 rpm.

Did this material happen to be a piece of free machining stainless, like 303 or 416? Stainless will crater tooling quite quickly if the coating is not specifically for stainless. Sandvik makes an insert coating specifically for stainless, it is kind of a coppery color, easy to not mix up your inserts, it is quite distinct.

The other thing I can think of is that the chip breaker isn't right for free machining, it may be rolling the chip in such a tight curl that it comes round and scrubs the insert right under the cutting edge, leading to notching and failure. This can be alleviated by changing the attitude of the tool so that the curling chip comes up and scrubs against the shoulder of the cut. But a different chip breaker style may also solve the problem. Sandvik has a system for describing the intended usage of their inserts for finishing, medium and rough turning.....I don't recall the syntax at the moment, I'd have to check their catalogue.

inserts are made for specific feeds and speeds and depth of cut. they work poorly or have short tool life when out of recommended range.
.
coolant to prevent chip welding to cutting edge and taking chunks of carbide off with chips is often needed too

Regardless of what people are saying about using HSS or whatever because it's free machining steel, this should NEVER happen to a good insert in free machining steel (or any steel for that matter).

Something is most definitely wrong.
Over center or wrong chuck direction (we've all been there on that one) is where I would start.

Edit: The way even the chips look "torn" like the surface finish, and the fact you can plow through 2-3mm on your crosslide dial quite easily when spinning in reverse, I'd say that's the problem.
Index the insert, confirm chuck rotation and try again. I'd wager the problem is gone.

Looks to me like an impact fracture

From rough handling

yes, to me too, like anciant man making tools.





well, i think i know what happened. the insert was not seated properly. i was able to put a piece of cigarette paper between insert and shim. the gap was invisible. cant remember this ever happening. so do i have to clamp down inserts before tightening from now on?

i played with the broken insert and im able to take off 0.01 mm with it. its a keeper.

dian said:

i was taking 2-3 mm cuts

Click to expand...

You mean depth of cut two to three millimeters?

I could not match that insert number exactly with anything in my paper catalogue. I was looking for a 2 letter designation at the end of the description which would be an indicator of its intended feed range, where W is wiper, F is finishing, M is medium, R is roughing. I also see nothing describing the grade of the insert, but maybe it is different in a metric catalog. Are these some old inserts you picked up on Ebay?

Bingo.
We call this a pressure crack and it comes from dirt in the holder when side one is clamped or just not seating it right..
Note how the blown out area is not remotely connected to the cut but lines up with the top of the pocket and you didn't get this on the first edge used.
The "I turned the insert around" was the big clue to me here.

There is one other way to get something like this and it is pressing land cracks but you just don't see those coming out of Sandvik and it would have taken out more of the center also.
Bob

yes, depth of cut. i noticed the box in the drawer and thought i would put them to use, no idea where they came from. 415 is not in the current catalogue, maybe is was superseded by 4015. if its between p and k15 it seems to be for general use.

and btw there was no dirt, i have a habit of cleaning the holder with q-tips. i was not avare an insert would not seat properly when you torque down the screw.

I really don’t want to be rude or aggressive or anything but there is a handful of things you seem not to know.

One of them is: no Q-Tips. Why? The fine cotton linters easily get caught on burrs, even on sharp edges and they collect debris that then sits under the insert. Clean with toothbrush and pressure air. Fingers must be clean, too. Tighten insert clamp firmly but not with brute force. Apply a little grease to threads, always to the moving thread.

Two: The smaller the corner angle, the weaker the insert. I have broken many V types and the D type comes next. 2 to 3 mm cuts are simply too coarse for a D insert. With a C, a W, an S or a R you can go that deep.

Three: As has been said, chip breaking form, coatings, and hardness of inserts should be known. As long as you go guessing you will have inconveniences like this. I once had a job as CNC turner in a place where I found C inserts in drawers for estimated 6000 Francs, one type only. Nobody cared about technical details of tools. Before buying inserts one should know what material is machined at what speed and feed. Then one reads what a manufacturer offers in the respective field. I had to turn quite different steels there, from simple structural to Inconel alloys.

Four: Segregate finishing from roughing. Use sturdier tools for roughing, inserts with bigger corner radii such as 0.8 mm or 1 mm, and sharper tools for two equal passes. Thinner chip, greater speed, slow feed rate. Wiper inserts have the so-called Kolessow-Ryshkow bevel. They produce a smooth surface and last longer. Skiving with an inclined HS bit works wonders.

Five: Switch to HS, if you cant’ or don’t want wo speed up your Reiden. Carbide inserts shouldn’t be used at less than 80 m/min. Calculate spindle speed from velocity of cut in mm divided by circumference of cut. V[SUB]c[/SUB] can be taken from tabellae the insert manufacturers publish. Depending on work size and coolant conditions one can cut mild steels at up to 300 m/min and more. With HS tools the limit is at 42 m/min in free machining steel.

i have done 6 mm with dn inserts.