Machining 4140

[Dissenter]

Hello to All!

I need some advice on machining 4140. We are using Tungaloy Trigon inserts with a nose radius of .02 -.03 to turn and bore this material. Can someone suggest any speeds and feeds? How about depth of cut?

Currently the programs are set (from the previous programmer/operator) to cut around 200 SFM at .01. He programmed the depth of cut at .078 (which is per side). To me that is a huge amount to be taking off.

I came from running Star Swiss machines to this company and I don't know this material very well. Any suggestions would be appreicated.

Thanks!

[MDLang]

I run mills not lathe but I can say for sure that that suface footage is way to slow. I'd be thinking more in the 600 -900 sfpm range.

Our shop has been experimenting with tungaloy inserts over the last few months and the operators are loving them.

Mike

[DareBee]

I must disagree.
4140 has an RC hardness of 30.
200SFM is running on the safe side of things though, you could get up to 350 - 400SFM.
Ideally you should be getting this info from your "Tungalloy" supplier instead of a bunch of web lurking Toolies

[Tim S]

4140 comes in at 30 Rc only if you order it that way. It also comes annealed. All of these things depend on the HP of you machine, the style of chipbreaker you are using and type of piece. If it is 4140 Ann I would run at 600 - 800 SFM and a DOC of .100 - .125 for roughing. Feed at those specs would be about .015 IPR.

[Geof]

4140 is an alloy steel that will work harden so a good depth of cut and feed, which is what you have, is needed. Also machining dry is sometimes a good idea to keep the chip hot enough that it loses strength. Your program speed of 200 fpm minute does seem on the low side but maybe the machine runs out of power trying to cut faster. I would suggest going with the existing program until you have a feel for it. You might find that on the machine you are working with slow speed and heavy cut are the best solution for shortest cycle time because this is what the machine can handle. You might be able to double the speed but if you had to drop the DOC down to 0.035" to avoid overloading the spindle overall you are going slower.

[Dissenter]

Thanks to All of you for the answers. If I may be a bit more specific....

I am programming a ProtoTrak VL console on a Southwestern Industry lathe. I believe the chuck is 14".

We handle anything between the diameters of 3" up to 15". The part lengths vary.

I know 200 SFM seems low, but when some of the material is out of whack, it causes a serious interrupted cut and may take two passes to have a nice even cut.

I have been experimenting with speeds and feeds and find that a 250 SFM at .014 seems to be a nice medium, however....the owner wants to boost the speeds (go figure). So technically I am running the machine faster than the previous operator, but it doesn't seem fast enough.

I will boost it to the 300 SFM then start to move to 400 and up.

At those speeds, should I keep the depth of cut (DOC) between .100 - .125?

Thanks again!

[ctate2000]

You can run RC30 4140 in the 600 SFM range with no trouble. Depth of cut will depend on the chip breaker. Good start would be .1-.125 and feed .01-
.015 if chip breaker will allow. If the material runs out enough to cause interupted cut then go deep enough to eliminate interuption. That size machine holds at least a 1.00 shank tool. That means you can run a .375 IC insert. You should be able to go .187 deep if necessary. If part runs out that bad you need to examine the set up and the material. You will may have to back down the speed and feed some as you go deeper but not too much. 300 SFM is too slow.

[cdlenterprises]

300 is rather slow. I've run 300 series stainless at 600 and 17-4 at 650 +. Those are in an enclosed CNC with a good coolant supply though. I'd try 600-800 sfm @ .012-.016 ipr. These are guidelines however. Know your limitations(ie: machine, fixture, etc.) You can only go as fast as your equipment (and your gut) will let you. Bottom line: go as fast as your comfortable with and DON'T get hurt.

[Dissenter]

Thanks for the reply.

I have been programming the SFM to 350 and IPR around .014. If I push the IPR to .016, the inserts seems to get a bit hot and do not cut properly. They seem to push the material.

Now, for another question: I have been using the drilling event on this lathe with the ProtoTrak software. The lathe is a 2640 using the ProtoTrak VL. My question is: What is the maximum diameter drill that I can use before the machine may stall? The service rep. said I could use a 3-1/2 spade drill and I should not have a problem.

However, (and I don't agree with this), my supervisor believes that anything above a 1-5/16 diameter should be placed in the tailstock and drilled from there. I think not! At the correct speed and feeds this machine should be able to drill and not have any problems with the carriage.

Thoughts?

[HuFlungDung]

How many horsepower have you got?

I'd maybe be leary of using a 3.5" spade drill in the turret, but I have not seen how massive your machine is. The thrust requirement is fairly high, IMO for spade drills. By comparison, a carbide insert drill usually takes far less thrust. An insert drill will also eat lots of horsepower because of the rpm and feedrate required at that rpm, but it will make a hole pretty quickly. I have used a 1.5" Kennaperfect drill in a manual 10 hp lathe @1500 rpm drilling C1045. This is where I learned how an insert drill feels so far as thrust requirement is concerned.

[ajl6549]

Originally Posted by Dissenter I need some advice on machining 4140. We are using Tungaloy Trigon inserts

Typically, your insert manufacturer should be able to tell you what s/f to run 4140 at. Since this depends heavily on grade, geometry, coating and sub straight. How ever, also keep in mind that 4140 has wide open metallurgical tolerances which means, what works perfectly this time may not the next.

[HuFlungDung]

FWIW, on heavy roughing cuts in 4140 HTSR, I keep the SFM around 350fpm when machining dry, and get pretty decent insert life. With coolant, I would boost this to about 450fpm. When you get down to light finishing cuts (maybe .030"), then you can go to beat hell, as fast as the chart says the insert will handle.

The higher surface speeds capable with milling are because the tool is not subjected to continuous immersion in the hot zone under the chip. It takes a massive mill to subject a tool to a real roughing cut similar to what a lathe commonly does. If you get to that stage, you'll be back down to 400 SFM with the mill in 4140.