4140 finish issues

Rogue_Machinist · Jul 6, 2020

Ive been machining for a while. And for some reason I cannot get my 4140 to finish nice. It doesnt need to be mirror but it cant look like its tearing. First picture is the finish im trying to attain (minus the scotch brite cross hatch).

Second photo is the tool I need to use because of a tailstock. Can a good finish be attained. Im leaving .03" for finish @2500rpm

Unless im doing something wrong its getting a "torn" finish.

Sent from my HD1925 using Tapatalk

Phil in Montana · Jul 6, 2020

What type of lathe? and are you using a tail stock and center, should be no problem...phil

Cole2534 · Jul 6, 2020

What's the tool's nose radius?

IME, if that's too fine you'll never get a great finish and feed also has part in the play.

Also- annealed or HT'd material? Prehard shines like a diamond compared to annealed, in my experience.

Sent from my SM-G981V using Tapatalk

Dan from Oakland · Jul 7, 2020

Need to know more- your tool nose radius, feed per rev and your surface speed or part diameter and rpm. From the picture, the feed is too coarse and your SFPM may be too low, but . . . . . .

Delw · Jul 7, 2020

I never liked those inserts on soft steels( unheat treated), try to get a positive insert and a .015 -.032 rad even an .008 would be fine. it will help a bit. then if need be hit it with 220 paper and coolant

OCTANE WORKHOLD · Jul 7, 2020

DNMG 431-PF 4315

You can try getting this insert as a sample from your area rep, it leaves the bright rainbow finish on every kind of steel. Minimum .017" DOC, .005 FPR, 1100 SFPM, and coolant for the best finish possible.

It has the added bonus of making tiny chips even at low feedrates. Surface finish on steel has a lot to do with DOC being greater than the insert radius, and SFPM, steel loves RPM.

michiganbuck · Jul 7, 2020

Fingernail shaving sharp.
A positive insert so it has some clearance under the cutting edge.
larger radius.
Some positive top rake angle.
Zero clearance under the cutting edge.
How is the part supported at the out end?

Plus check that holder to see no daylight under the insert at the forward edge of the insert.
Sometimes a snip of .002 -.003 shim at/under the forward of the insert can help a shot holder..

QT:[minus the scotch brite cross hatch).]

Going back and forth with Scoth Bright is not as good as one way travel with abrasive paper or closh IMHO.

A small radius is cutting a thread in tha part, having a grinder one can bump a small flat on the point...Small radius is for when the part print wants a small radius at the shoulder...

OCTANE WORKHOLD · Jul 7, 2020

michiganbuck said:
A small radius is cutting a thread in tha part, having a grinder one can bump a small flat on the point...Small radius is for when the part print wants a small radius at the shoulder...

Disagree strongly, a small radius is for taking deflection out of the cut and not requiring a large depth of cut for a finish pass. If you are roughing, yes you want some radius so the edge doesn't deteriorate instantly.

Making sure the insert is positioned properly is important like you said though, as well as part stickout even with a tailstock, machine rigidity, the list goes on.
If the insert I linked isn't a 100% improvement using the parameters mentioned, i'll buy you a steak dinner.

ChipSplitter · Jul 7, 2020

OCTANE WORKHOLD said:
Disagree strongly, a small radius is for taking deflection out of the cut and not requiring a large depth of cut for a finish pass. If you are roughing, yes you want some radius so the edge doesn't deteriorate instantly.

Making sure the insert is positioned properly is important like you said though, as well as part stickout even with a tailstock, machine rigidity, the list goes on.
If the insert I linked isn't a 100% improvement using the parameters mentioned, i'll buy you a steak dinner.

You guys are both right, I think...........

Buck is saying that a smaller rad will almost cut a thread if the feedrate is too high, hence the need to reduce feedrate or use a larger radius insert.
Octane, I think you're saying a smaller rad makes less deflection, which is also true.
IME the best results will be from a small rad with a very tight chipbreaker. (See notes below.)

For best finish, feed at 25% of insert radius IME. So a .015 insert would be about .004 IPR. And yes, you will need a tight chipbreaker.

Another thing that makes a difference is the rear clearance angle of the holder. IOW, a CNMG insert has 5 degrees clearance behind the radius instead of 45 like your tool appears to be. It's difficult to explain, but it has to do with the point of tangency on the insert radius and the straight section of the workpiece. (It makes the cusp size way smaller if the insert if almost heeling the workpiece.)

EmGo · Jul 7, 2020

If you just want shiny, jack up the speed.

ChipSplitter · Jul 7, 2020

EmanuelGoldstein said:
If you just want shiny, jack up the speed.

Are you taking DMF_Tom's place?

I can't believe he hasn't mentioned that yet.

EmGo · Jul 7, 2020

ChipSplitter said:
Are you taking DMF_Tom's place?

Nah, I didn't mention Excel or my salary ....

toolsteel · Jul 7, 2020

Looking at the condition of the holder....(we have some too).....I would also check your centerline.

michiganbuck · Jul 7, 2020

QT :[Disagree strongly, a small radius is for taking deflection out of the cut and not requiring a large depth of cut for a finish pass. If you are roughing, yes you want some radius so the edge doesn't deteriorate instantly.]

One thing they emphasized at Carboy school was to use the largest radius the job will tolerate.
Righty, horse power, and part print often determine.
One of our tasks was to choose the tooling with inserts for a certain part, after the class they demonstrated running the part on a big chucker that turned the part end wise, with it having many tool stations. Most of us got the radiuses wrong with picking the smaller radius...The machine was so heavy duty it could pull the larger radius.
The part included ID, Od radiuses, steps, shoulders, close and scale sizes. I can’t remember if it had a thread or not. likely it did.

angelw · Jul 7, 2020

ChipSplitter said:
Another thing that makes a difference is the rear clearance angle of the holder. IOW, a CNMG insert has 5 degrees clearance behind the radius instead of 45 like your tool appears to be. It's difficult to explain, but it has to do with the point of tangency on the insert radius and the straight section of the workpiece. (It makes the cusp size way smaller if the insert if almost heeling the workpiece.)

The point of tangency on the Tool Radius for a given surface is the same irrespective of the Trailing Angle of the insert being used. The OP's workpiece appears to be parallel, therefore, the point of tangency will be at the point on the Radius closest to the centre line of the lathe.

Surface Finish in Turning is a function of the TNR and the Feed Rate. A feed rate of 0.17/rev, using a 0.8 TNR, will result is a 1.6µm finish. A 5deg clearance angle of the trailing edge of a CNMG insert will be well clear of the scallop height of the surface finish; accordingly, no better finish will be achieved with the 5deg trailing angle of the CNMG vs the 50degs of the VNMG used by the OP. With a fine Feed Rate, an insert with a tight chip breaker is required to control the Swarf.

I suspect that the Finish DOC being used by the OP is quite small relative to the TNR being used. Rule of Thumb, the DOC for a finish cut should be at least the TNR being used. Less than that alters the vector of force and deflection forces are actually increased with a very small DOC. Whether that has an apparent negative result on the workpiece is closely linked to the rigidity of the set up, but is the reason that a torn looking finish will nearly always result if a spring cut is made on Mild Steel with Negative Geometry Inserts, using a relatively large TNR.

Regards,

Bill

Bill in PA · Jul 7, 2020

Last time I had any trouble with 4140 was because I inadvertently bought annealed instead of prehard. Could not figure out why I had to run the part twice as fast as expected to get a decent finish until I double checked the material invoice. :rolleyes5:

CNMG 431 or 432 work fine for me. Usually rough .125" to .250" DOC (diameter). Leave .025" - .050" for finish at .004" to .008" IPR.

Bill

litlerob1 · Jul 7, 2020

Turning 4140 is cake.

I DO disagree with most of the posts. "Sharp corner radius and light depth". "Rainbow finish"? First time I've heard that one.

IMO .0312"r X 17% feed, .07" DOC and 500 SFM (for the finish pass). If it's annealed more faster is gooder.

R

OCTANE WORKHOLD · Jul 7, 2020

litlerob1 said:
Turning 4140 is cake.

I DO disagree with most of the posts. "Sharp corner radius and light depth". "Rainbow finish"? First time I've heard that one.

IMO .0312"r X 17% feed, .07" DOC and 500 SFM (for the finish pass). If it's annealed more faster is gooder.

R

.07 doc is massive for holding tolerances on most machines that aren't incredibly stout. I wish the OP luck, let us know how you get on.

Hardplates · Jul 7, 2020

My experience has been, the only reason to run a larger radius is to increase insert durability. But the larger the tip the deeper the minimum cut to get the chip to break. If you are getting a phonographic finish you are feeding too fast. The only time I can think when it could be good to use a larger radius for finishing is in a high production environment, but even them I would think you would be better off with a small radius with a wiper behind it.

Finishing with a large radius may allow you to feed faster but at the expense of greater tool pressure, possibly chatter, push off, stringy chips and so on.

angelw · Jul 7, 2020

litlerob1 said:
Turning 4140 is cake.

I DO disagree with most of the posts. "Sharp corner radius and light depth". "Rainbow finish"? First time I've heard that one.

IMO .0312"r X 17% feed, .07" DOC and 500 SFM (for the finish pass). If it's annealed more faster is gooder.

R

Hello Rob,
I think some are confusing actual Surface Finish with the shine of the cut surface of the material. Surface Finish in turning is simply a relationship between Feed Rate and the TNR being used. Your cutting data would result in a 1.05µm, quite a good Surface Finish. There would be no advantage using a 0.7" DOC over .0312" (TNR value)

Regards,

Bill

4140 finish issues

Hot Rolled

Stainless

Diamond

Titanium

Stainless

Aluminum

Diamond

Aluminum

Titanium

Diamond

Titanium

Diamond

Titanium

Diamond

Diamond

Hot Rolled

Diamond

Aluminum

Stainless

Diamond

Similar threads