4340

[DavidB]

Hi all,

I would like some advice and any info on Material 4340.

 

How best to cut it dry ?coolant? lathe tool geometry?

 

The stock is diameter 25mm (1") by 375mm 15" long.

The stock bar has to be turned down to 12.7mm (1/2"),by 360mm (around 14")long.

We currently get this job machined out side but they refuse to it as they can not get any tool life.

I have been asked to look at it and see if we can machine it inhouse.

 

[crazy^millman]

Well it is tough but not impossible to machine. If you are going to cut that small of a diameter for that long of a length on a CNC lathe I would get a follower to help support the shaft while you are cutting it. If you are doing it conventional most lathes have a follower you can use. I would look at normal carbide to machine it unless it over 35rc then I would look at CBN to cut it. I would go with a .01 to .005 finish cut also will help the tool to last longer for finishing and a real pain to take off small amount unless you toolpost grind it in. I would go aggresive on the cut for roughing if you got the machinen to push it. I am thinking upwards of .018" to .025" with upwards of 450sfm.

 

Good luck and we use yo cut 12" dia material down to 2-15/16" by 78" long leaving a 11-1/2" header for the paper rolls. We could produce 10,000 lbs of chips in one week on 3 lathes. Our roughing tools where WNMG-632 inserts on 1-1/2" toolholders for extra rigidity.

[DavidB]

I have n/c machines to do it in but none have a steady.I was thinking about turning it in say 3 sections to keep the stock a bit more rigid.The shop that was doing the job had a double chuck machine. The chuck at the tailstock end pulled it out of a bush that was in the machine end chuck.We haven't got that sort of machine.Would you cut it dry or wet?

 

Thanks for the reply

[Quickmike]

I'm not sure, but maybe this could be run on a swiss type lathe. I think that this type of lathe has the capability of pushing the stock thru the collet, or something like that. Another idea would be to see if it could be centerless ground. I'm not sure how many pieces are going to need to be made, but just a couple of ideas to kick around. I also not sure if either of these prcesses would work but maybe someone else here might know for sure.

[DavidB]

We grind the shafts after turning between centres.We have always done this,but the turning was done outside now we are going to try doing the turning inhouse.On normal N/C lathes.

[McRae]

Material group for this type of an alloy steel will help you make some impressive parts. If you are grinding after the fact, I would use a CNMG or similar insert. If you are deforming too much, use something a little sharper in the profile like a "D" style knife edge from Sandvik. Their steel grades are great and I think the only pitfall that I can forsee is the notching on the insert at the depth of cut line. If you want to get a little fancy, change the depth of cut as you go and distribute some fo the wear along the edge of the insert.

 

Good luck - Nothing smells better than cutting at full powers and making alloy steel chips pop off of a workpiece.

[crazy^millman]

+1 Andrew love the steam bellowing out of a machine cutting the stuff. I could fog the place up in a matter of mintues. We would have to fill the coolant tank every day when running the stump shafts as I use to call them. I would leave like .1 with the WNMG and then set-up the next shaft. I use to let the shaft normaize overnight before finishing them just to be safe.

[Harryman]

4340... Oh yeah, I remember that stuff.

 

It has strange magnetic properties and gets an odd red dusty coating if left laying around too long.

[DavidB]

So I asume cut it wet?

 

The biggest problem is the part bends over such a long length.The part is stess relieved after turning then ground.

 

[crazy^millman]

Well sounds to me you got that job figured out then just a matter of hitting that bad boy a running. I would cut it wet but make my mixture double what you normally do to help get lubrication to the cutting edge.

[Harryman]

You can cut the stuff wet.

 

The length is going to be the problem. If you can't support it someway this will be you>

 

You could go at it in several steps sticking the bar out a few inches each time and holding it with a center, but I doubt you'll be able to turn 14" between centers in one shot. Three or four whacks ought to do it. The stock will have to start out pretty straight if you regrab several times. If the stock is very straight, you'll be very successful given that you'll be grinding for real finish.

 

A relatively heavy finish pass is required for a good finish, approx .02" per side and that will tend to limit unsupported length on a small diameter. HTH

[chris m]

I don't know if you're checking both of your threads, but I'll post in both:

 

We turn 4340 all day every day at 34-36 Rc using Sandvik WNMG 432 MM4015 inserts to rough and Valenite WNMG 431 GF SV315 inserts to finish. We use the Valenite because Sandvik doesn't make an insert that'll break a chip at the speeds / feeds we need to run for our finish requirements. If you can run a little more feed I'd try a CCMT 32.50 or 32.51 UF525 or 5015 [525 doesn't take vibration].

 

We rough at 450 SFM and finish at 550SFM but if your material is softer or if your tolerances aren't too tight you can for sure go a little faster.

 

As mentioned in the other thread, I'd rough a couple inches, then finish it, rough a couple more inches, then finish that; if you're gonna grind it anyway you shouldn't be too concerned about little steps between chunks.

 

Good luck and be sure to tell us what your results are so we can all learn.

 

C

[McRae]

Chris, Great feed back on the chip breaking - this is some excellent knowledge to pass on and something that an insert salesman will waste hours on "Testing" at your plant.

 

Thanks, I will remember you in my will.

[DavidB]

Chris greta info thanks,

 

What feed rates are finishing?

 

I cut the first test piece and the swarf was very stringy.

 

[DavidB]

Chris also roughing feed rates?

 

I cut the roughing at .3mm/rev at 1.5 doc.

 

I left 0.5 doc for finishiing. at .1mm/rev

 

[chris m]

You guys with the metric stuff...

 

David, a 'good' feed rate depends alot on what you have for a chipbreaker on the insert.

 

The roughing feed you have shown looks pretty good, I'd go for more DOC [up to 3mm radially] if you can get it without vibration because you'll definitely see better tool life. Its doubtful that you can get that much DOC with your long part but try stepping up about .25mm at a time and see where you get.

 

As far as the finish feedrate goes you look like you're in the ballpark depending on the nose radius of your insert; if you're using a .0156R insert you're about where I'd be. If you can live with a little coarser pitch to your finish I'd probably try up to .20mm to see if the chip will break. I usually like to stay under 1/2 of the nose rad for feedrate in finishing but that's not a total requirement.

 

We usually leave between .12 - .25mm radial stock for finishing so it looks like you're in the zone there, too. The 'nest' of chips hanging on the tool can be a pain in the a$$ on the applications, you should work with your insert manufacturer of choice to get something that works well for you.

 

C

[DavidB]

Chris,

 

I looked in the Sandvick book the WNMG -MM is there first choice for stainless steel medium machining.But it doesn't come in the grade 4015?

 

It comes in 4015 in the WNMG -PM wich is there first choice steel medium machining.

 

Thx David

[chris m]

Sorry, that's a typo; PM is the geometry

 

Some of the stainless grades like the MM2015 actually don't work too badly because they're molded pretty positive; you might want to test that too.

 

C

[DavidB]

Im doing night shift at the moment 6pm till 6am.

 

The positive is I get to use the forum when most of you people(USA) are using it to,and i don't have to wait a day till I get a responce

 

[Philcott]

David,

 

I use the sandvik 4015 grade as well. Right now I have a job up using 650SFM, .09 radial DOC, and feeding at .014IPR . This works quite well for us breaking the roughing chips into nice little blue "6's". It is not a CRAZYMILLMAN rate of removal but is required here for two reasons. One is I get $#!t from everyone if I fill the shop with blue smoke and the other is due to lesser experienced operators running the machine and not really having the experience to HEAR when an insert is about to breakdown and change the insert before catastrophic failure.

We also use Kennametal CNMG432RN KC9125 for roughing this stuff with great success. pretty much same speeds and feeds.

For finishing we like to use cermet inserts and we get long life and stable cut sizes. This won't work on the part you are doing due to it's length and dia. but we cut at 1100SFM .006IPR. I haven't figured out the birdnest of chips on the part yet either. Stringy chips suck.

Good luck.

 

Phil

[McRae]

quote:

---

I haven't figured out the birdnest of chips on the part yet either. Stringy chips suck.

Good luck.

---

I can already see the cause, your tool nose radius is larger than your radial depth of cut. If your process will allow it, the stock allowance for finishing should be increased - or - the nose radius decreased. The chip will then land across the chipformer on the insert and you will be able to start to control it.

 

The other way to control this is to change the insert geometry slightly so that you use a chipformer with a shorter land. Similar to a change in the Sandvik PMK line from a PM to a PF. Also of note - the stainless grades have different geometries that are designed for stringly materials - word of caution though, they are softer so you will need to slow down a little.

[DavidB]

What sort of RPM do you guys have on your Lathes?

 

If i use a cutting speed of 230 m/min.

Thats 5767 Rpm.

If you guys are turning small Diameters at the cutting speeds your suggesting 450-650 SFM,you must have some quick spindles.

 

Im limited to 5,000 rpm.

Okuma LB15 fastest machine

Okuma LC40 4000 rpm

 

[Philcott]

Good point David.

I do max out the lathe at 4000 so at small diameters I am no where near the proper SFM. Above 20mm dia. or so the faster speeds work well. There is not much that can be done other than use a different grade for the small diameter jobs.

 

Phil

[chris m]

David, at that .500 diameter you'd need 4200 RPM to run at the 550SFM that I'd recommend for finishing. That is pretty fast, for sure, but it sounds like you're pretty close. When running up that fast just make sure that your workholding can handle it: air chucks typically crap out around 3000-3500 depending on size and top jaw mass but hydraulic chucks and collet chucks will usually handle more RPM than the machine has available.

 

As for RPM:

 

The Okumas are all Big Bore machines so I'm limited to 3800 on those

 

The Hardinge T51 has 4500 I think [i've run 4200 with the 10" 3-jaw on there, sounds like a jet dragster]

 

The Hardinge T42 has about 6000 but I've only ever run about 5400 without chickening out

 

The Mori-Seikis are OLD so I think we have about 2000 RPM there

 

The Okuma-Howas are 3500

 

C