Facing surface finsh as Vo becomes zero.

Hello,

Long time reader first time poster.
I am having trouble maintaining good surface finish when facing off parts on my lathes.
The problem: the last 10 mm when facing a part is rough.
The set up: okuma lb 12, max rpm 2500, constant surface speed Vo.240, ceratip cnmg120804 cermet tool, Ap 0.2, 0.12 m/rev feed.
The material : s45c (AISI 1045 equivalent)

I know its a limitation of the max rpm of the machine but if any one has any advice i am keen to listen. Any tooling recommendations?

KabutoMike said:

Hello,

Long time reader first time poster.
I am having trouble maintaining good surface finish when facing off parts on my lathes.
The problem: the last 10 mm when facing a part is rough.
The set up: okuma lb 12, max rpm 2500, constant surface speed Vo.240, ceratip cnmg120804 cermet tool, Ap 0.2, 0.012 m/min feed.
The material : s45c (AISI 1045 equivalent)

I know its a limitation of the max rpm of the machine but if any one has any advice i am keen to listen. Any tooling recommendations?

Click to expand...

.
some inserts need enough speed to get tip hot to get a shiny surface. too slow often get bue or built up edge of part material forming on cutting edge and breaking off many times per second
.
if you go much slower finish often dull but its more even looking. i try not to get shiny and dull finish side by side, cause often there is often a height difference, dull finish being lower
.
transition speed where finish goes shiny varies with material and part shape. often you got to go either a lot faster or a lot slower to get a stable even finish. at least thats been my experience

KabutoMike said:

Hello,

Long time reader first time poster.
I am having trouble maintaining good surface finish when facing off parts on my lathes.
The problem: the last 10 mm when facing a part is rough.
The set up: okuma lb 12, max rpm 2500, constant surface speed Vo.240, ceratip cnmg120804 cermet tool, Ap 0.2, 0.012 m/min feed.
The material : s45c (AISI 1045 equivalent)

I know its a limitation of the max rpm of the machine but if any one has any advice i am keen to listen. Any tooling recommendations?

Click to expand...

Live tool. Abrasive, even. Or a shearing operation, pushed or pulled AFTER done with turning. If it matters.

WHEN it does, a second-op is usually needed as the cheaper method, no way around it.

A separate cutter or abrasive (or laser, EDM, waterjet.. yadda yadda..) is the only way you can get SFM independent of radius out of a spindle.

Well a "product" of the RPM & AND the wheel or cutter's own, but there you have it.

In theory, a lathe and single-point tool approaches the need for infinite RPM as it approaches zero radius, and there is No Fine Way to actually deliver "infinite" RPM, nor even close-to.

Even if one could do? The "turning" tools and their cutting edges no longer work as expected.

Catch 22. "Minimize" the teat the best you can do. JFDWT and final-final your finish some other way. No magic on-tap. Not on conventional "turning".

Now.. if a milling-cutter, saw, or endmill were generating that face, working off a powered rotab? Overlap can be done. No teat.

Y'see why I said "live tool"?

KabutoMike said:

...The set up: okuma lb 12, max rpm 2500, constant surface speed Vo.240, ceratip cnmg120804 cermet tool, Ap 0.2, 0.012 m/min feed.

I know its a limitation of the max rpm of the machine but if any one has any advice i am keen to listen. Any tooling recommendations?

Click to expand...

Start by changing your feed to per revolution, not per minute. Your RPM is increasing as you near center, the chipload is not keeping up.

Play with your SFM, finish allowances, run it dry, try a smaller TNR if you are still having problems.

edit to add: you don't mention anything about the workpiece, but if you are chucking a bar down the spindle, it can move around and affect the finish too. Same thing if chucking with soft jaws that aren't bored appropriately.

You want to leave enough finish allowance to make it break a chip all the way to the center, you need some rigidity in the setup.

guest said:

Start by changing your feed to per revolution, not per minute. Your RPM is increasing as you near center, the chipload is not keeping up.

Play with your SFM, finish allowances, run it dry, try a smaller TNR if you are still having problems.

Click to expand...

.
agreed usually lathe is feed per revolution not feed per minute. different gcode

I also would not be using cermet inserts for mild steel like 1045. Certainly change the machine to run in IPR. Your depth of cut should be fine. 2500 RPM should be plenty. Feed rate with that size radius of say .12 mm/rev. .005 in/rev.

I mean, you probably will never get down to the center to be "shiny" smooth but aesthetics and surface finish do not always fall in line.

Just to add some details. And thanks for the comments so far.

I goofed the original post, the feed is 0.12 mm/rev not 0.012 mm/min. Sorry.

The work is held in soft jaws which were bored correctly with almost no stick out. I am not worried about chatter or work holding problems.

The roughness is only noticeable with the eye and is a purely asthetic problem. It gets a quick polish on a soft wheel then blacked (黒染め i am not sure of the process name in english). But the part is visable and its somthing i would like to make look good.

Cermet inserts bad for mild steel? Any good recommendations. I have had a go at TiN and carbo nitride coated carbide with terrible results. Would a wiper type help? All tooling across all our machines are negitive rake, would a positive tool help? At the moment the CNMG has a -5 deg lead angle (kapr 95 deg) would a positive lead angle help pull the chip away from the work at lower surface speeds?

I can get mirror finished on the face down to the last 10mm then it turns to crap.

KabutoMike said:

I can get mirror finished on the face down to the last 10mm then it turns to crap.

Click to expand...

You can surely beat 10 mm. Even beat half a mm, razor-sharp HSS-Cobalt.

Even so, the long and short of it is that if you want a polished look? Then "polish" or Diamond/CBN finish is wot you do.

Not sane to expect to single-point turn clear to "zero".

Want a nice look? Just drill and tube-set a small cubic Zirconia gemstone at the center. Or a blinking purkle LED.

"Turns to crap"? We've all heard about those automated Japanese toilets by now. How about a pink nano-sphincter, or a gilded tapeworm scolix, or a miniature Bronzed shit-eating-grin, or..

thermite said:

You can surely beat 10 mm. Even beat half a mm, razor-sharp HSS-Cobalt.

Even so, the long and short of it is that if you want a polished look? Then "polish" or Diamond/CBN finish is wot you do.

Not sane to expect to single-point turn clear to "zero".

Want a nice look? Just drill and tube-set a small cubic Zirconia gemstone at the center. Or a blinking purkle LED.

"Turns to crap"? We've all heard about those automated Japanese toilets by now. How about a pink nano-sphincter, or a gilded tapeworm scolix, or a miniature Bronzed shit-eating-grin, or..

Click to expand...

Thanks for the advice, and humor.

Do you know any big brands (kyocera, sandvik, sumitomo ect?) that make HSS (cobolt M35?) inserts?

Trying to get this done in a single operation as its of hundreds of parts being made, where adding more operations is cost prohibitive.

I have no problems getting good finish down to the last few mm in SUJ2 (52100) or SCM440 (4140) so i was seeing if there were any hints on getting these slightly gummier steels to shine.

Thanks.

KabutoMike said:

Thanks for the advice, and humor.

Do you know any big brands (kyocera, sandvik, sumitomo ect?) that make HSS (cobolt M35?) inserts?

Trying to get this done in a single operation as its of hundreds of parts being made, where adding more operations is cost prohibitive.

I have no problems getting good finish down to the last few mm in SUJ2 (52100) or SCM440 (4140) so i was seeing if there were any hints on getting these slightly gummier steels to shine.

Thanks.

Click to expand...

CNC is not my bag. Other-than HSS-Cobalt/Stellite isn't, either, nor "inserts", in general. One HAND grinds & hones these and HAND adjusts for that sort of tight finish spec. Too old to care to deal with the "inserts" learning-curve, meself.

Next door down the hall, some other Pilgrim(s) will assuredly know.

"Gummy steel" is easy, though. Prolly why you haven't already had more specific guidance?
It just dasn't DO "mirror finish" in one go all that well at room temperature.

That's why we CALL it "gummy". How much budget ya got for a liquid Nitrogen or CO2 chiller system?

Or .. just pay the barely even measurable pittance per part to use a friendlier alloy is all. You've blown any savings already just in researching bad options. "GIGO" applies. Garbage IN. Garbage OUT. Next go, you will know in advance, yah?

Otherwise, any decent alloy, steel or otherwise, PM "community" expertise can sure as God made little green apples get you way TF under a "few mm". A "few thou" should be possible. IF yah got the spindle for it.

Poor choice of materials for a given expectation is still a poor choice. Can't fix that any more easily than one can fix stupid. Costs you time. Time is money. Decent steel? Pretty damned CHEAP, actually. That's why we use so much of it!

Change your G50 to the max for the Chuck.
Leave about 16% of the TNR for the Finish pass.
Face away from centerline.
Use a smaller TNR.

This won't solve the problem completely, but it will get you down to the 1mm or less area. Why aren't you using all the RPM?

R

What is the od facing size?

On a manual lathe I’d use something like this probably :

tpux insert - Google Search

I know it as a TPUX insert. Can probably get chipbreaker similar for a holder shape you have. Bear in mind for triangular inserts there are left and right hands.
Where I used to work that was the best offering for this situation. If your not facing off from a large diameter do a light cut at a slow speed. Usually comes off shit hot. Dunno what their like at high cutting speed, but moderate speed left a smooth finish. Never had the speed to find out.

I light cut as in .05mm at a slow like 30m/min speed might get you what you want. Might take too long though. I was thinking about this the other day, depending on the size your facing from, and your machine, it might work out similar in time including spinning the chuck up and down to speed from 2500rpm.

litlerob1 said:

Change your G50 to the max for the Chuck.
Leave about 16% of the TNR for the Finish pass.
Face away from centerline.
Use a smaller TNR.

This won't solve the problem completely, but it will get you down to the 1mm or less area. Why aren't you using all the RPM?

R

Click to expand...

Thank you.
I will try to go from inside out. I normally don`t like to run this direction as the lead-in is below x 0 so the works rotation is backwards in respect of the tool for short time as you make the initial cut.

I am using all the RPM i can with the chuck at 2500. The spindle will go to 3500 but i am not going to try.

Number 2, Thanks for the reply.

OD is 35mm with a 1.5 mm chamfer.
The program runs the facing op in constant surface speed G96 Vc 240 m/min.

KabutoMike said:

I am using all the RPM i can with the chuck at 2500. The spindle will go to 3500 but i am not going to try.

Click to expand...

Good grief! "hundreds" or even multiple hundreds, but not thousands and multiple thousands is even "manuals can still do this" turf!

I have 1942 and 1944 vintage all-manual lathes that can do 2500 RPM, an early 1970's that can do 3,300 RPM or so, and you are wingeing over using a modern CNC as it was BUILT to be run?.

Not clear why you haven't got at least "access to" 5,000 RPM or better, anyway even if it had to be subcontracted?

"Who dares, WINS".

You need to fill-in some gaps in your GENERAL understanding of turning, machine-tool, and tooling capabilities.

You aren't taking the sound advice of several expeienced folks handed you "for free". Best go and read-up on your own dime, yah?

Alloys as well.

Quit wasting your time trying to get fine jewelry-grade finishes off of "gummy" steel with low/no effort as a by-product of fast, cheap throughput on an uncooperative alloy.

Those are mutually exclusive - even antagonistic - goals.

One of them has to be adjusted or compensated for "somehow", if not all three "rebalanced".

TANSTAAFL

"There Ain't No Such Thing As A "Free" lunch!" - most especially if you will not even open the damned WRAPPER of what has been offered, if that was somehow overlooked?


PS: "Quote more wisely" while yer at it. No amount of chewing-on will correct an underbid.

We just EAT those, as the closest thing to a "free lunch" as can be counted on, empty of nourishment, or worse-than-zero! Welcome to reality. You surely ain't the first.

speed where inserts go from dull to shiny finish needs the heat at cutting edge. heat helps part material from sticking and the bue or built up edge is what causes a difference in height
.
most times for my work its not so much the mirror finish its the difference in height as dull surface is often lower .015mm. often i have to make finish all dull (go slower) and have part same height all dull finish rather than shiny and dull variations
.
also sometimes i get part vibration that gives bands of shiny to dull to shiny variations. sometimes its a part vibration problem too which depends on part shape.
.
sometimes changing inserts its extra shiny for a short distance (at lower speed) with the new inserts. of course that adds cost changing inserts more often. the data suggests going faster and having to recut and or change inserts more often is most times slower and more expensive. that data is hard to prove cause sometimes it works and part is all shiny and sometimes it doesnt work or you get shiny and dull variation. getting 100% reliability can be very difficult to get.
.
but sometimes you have to deal with other people who like shiny parts. hard to describe but who wants to be thought of as not capable of making the shiny "better" parts even if the others who are making the shiny parts are taking longer to make the parts and at higher tooling costs. nobody wants to be thought of as not good enough a machinist and cannot make shiny parts like somebody else does. like hearing the "Bob is not as good a machinist as Joe" based on shiny appearance and not on cost to make part. it can be difficult to go against a visual preference that makes little logical sense.

Thanks. Your negativity made me laugh. Merry Christmas.

Great! i appreciate the reply.
I will check running some different depths and see how much BUE if any is deposited.

KabutoMike said:

Thanks. Your negativity made me laugh. Merry Christmas.

Click to expand...

Nobody is being "negative" but he who will not use what he already has according to multiple offers of better ways to USE what he has - plus a rather modest extra spend.

May the coal in your stocking at least be low-sulphur high-grade "metallurgical" of such esteemed reverence that a traditional maker of Daikatana might happily trade you polishing services of "gummy material" for the exchange of!

"Win-win" after all!

How's that for "positive" Christmas cheer?

KabutoMike said:

Thank you.
I will try to go from inside out. I normally don`t like to run this direction as the lead-in is below x 0 so the works rotation is backwards in respect of the tool for short time as you make the initial cut.

Click to expand...

You can also change the code manually. It isn't a huge hiccup. Actually the Tool should not be below centerline, it should be at exact centerline. Change the lead in to Perpendicular instead of Arc.

G0X-double the TNR
G1Z0
X33.5
X35Z-1.5
blah
blah
blah

KabutoMike said:

I am using all the RPM i can with the chuck at 2500. The spindle will go to 3500 but i am not going to try.

Click to expand...

Oh come now my son. It's a little bity Machine. And it's rated at an RPM for a reason. It isn't stamped on the tag for no reason. I have run Okumas for years and years, I run them all at the rating they have on the tag (especially when it's just a piece of plain old round bar).

This is a 432mm Chuck that gets run at 3000 RPM every day!!!!! It's never flew over the cookoos nest.


R