Help with turning 4140

Investigator said:
I'm trying to turn some 4140 bar on my 12" logan lathe. The surface finish looks rough, literally. Looking at it up close it looks like the metal is tearing off. The 4140 is supposed to be annealed. It is 2" round bar, I am turning at 250rpm. I am using HSS bits for cutting. I am turning down the OD, as well as making an internal 60* cone. I have tried lighter cuts, and deeper cuts. The RPM I reached by reading the Niagra Tools slide rule they send out.

It turns and cuts, the shavings are very tight spirals, sometimes 2 inches long. I am feeding at the slowest feed rate on the lathe.

What can I do to make it better?
Click to expand...

Cutting speed for 4140 annealed is about 60-200 sfm when using HSS. A lot depends on how your tool is ground but I would suggest you try slowing your speed to about 125-140 rpm and increase feed when roughing. How much feed? That depends on the tool and how the finish turns out with that tool. 4140 likes deeper cuts at only moderate speeds and a higher feed rate with carbide but with HSS, it is very much dependent on the tool's geometry and I find it cuts better at lower speeds when roughing. When finishing, I crank it up to about 1100 rpm and take light cuts and get a really good finish. Most harder carbon steels are like this - rough slow, finish fast.

If you choose not to show us your tool, that's fine but I would suggest you try this grind: 10 degree side and end relief, 20 degrees of side rake and 12 degrees of back rake. The relief angles are conservative to provide strength under the cutting edge. Side rake is boosted a little to reduce cutting forces and improving chip clearance. Back rake is slightly increased and together with the increased side rake, will reduce cutting forces and greatly reduce cutting temperatures. As you know, 4140 is not that hard to cut but it can work harden if you dwell in the cut. By increasing the rake angles, you improve chip ejection to keep temps down and by increasing feed you also increase chip ejection.

I also suggest you try reducing the lead angle of your tool when roughing. If you grind a general purpose shape, try turning the shank of the tool a few degrees off perpendicular, toward the chuck. This is the equivalent of reducing speed and increasing feed just with the tool angle alone and this may help. When doing finishing cuts, increase speed and turn the tool slightly toward the tailstock and slow down your feed. You finish should improve.

As Benmychree said, 4140 is not that hard to cut. It has a machinability rating of 66%; kinda hard but not that hard. Oh yeah, depths of cut depend a lot on the rigidity and HP of the lathe but I would try a 0.050" roughing depth of cut, slow the speed to about 140 rpm and play with feed until the tool cuts well. When this stuff cuts well, it will show you a clean finish at low speeds and a really nice finish at high speeds.
 
Last edited:
I'll snap a photo of the tool bit, and the parts I have made so far. I am making several of the same thing, cone baffles for suppressor.
I shaped the bit on a grinder, then finished it up, cleaning it up on a belt sander.
I've been busy at work, and haven't even been in the shop this week. I'll get pics posted tonight.
 
I have heard that annealed 4140 while softer does not machine as nicely as HT (28-32). I know HT is pretty hard on tooling and wears it out quickly, but I can get pretty good surface finishes. I have never machined annealed 4140.
 
The attached video may be helpful.

Daryl
MN
 

Attachments

  • Fundamental Aspects of Metal Cutting - Cincinnati Milling Machine Research Dept. Feb 1950 - Yo...mp4
    30.5 MB · Views: 40
Some photos:

This is the part i'm making
20180223_173729.jpg
20180223_173737.jpg

Here is the bit for the inside:
20180223_173846.jpg
20180223_173855.jpg

this is the outside bit:
20180223_173929.jpg
20180223_174010.jpg
 
I'll comment on the tools but I hope you understand that I'm trying to help, okay?

Both of your tools have zero rake, meaning the tops are flat. That's okay but the tools will cut with pretty high cutting forces and they will cut hot because the chips are not being evacuated from the cut very quickly. Basically, they are functioning like form tools and as I'm sure you know, form tools cannot handle heavy cuts because they cut with a lot of resistance. Accordingly, the finish is poor with a tool like this unless you take really light cuts.

If I were going to do a 60 degree inside taper like that, I would use a boring bar. Even one of those cheap Chinese brazed carbide boring bars will make short work of that taper. If you want to grind the tool then give yourself more side relief, at the very least 8-10 degrees to reduce rubbing. In use, angle the tool so that it cuts with the side edge, up near the tip.

I would suggest you grind your external turning tool a bit differently. Rather than trying to describe how to do it here, I hope you don't mind having a look at this thread: https://www.hobby-machinist.com/threads/models-for-grinding-hss-lathe-tools.62111/. Go to post #104 and have a look at how the turning tool is ground. That tool has tool angles of 15 degree all around but for your tool I would shape it the same way as in the post but use the angles I listed in my post above. In other words, follow the sequence in the pictures in that post but change the table angles.
  • Set the grinder tool rest at 10 degrees and grind the side and end as shown in the pics.
  • Once the side and end are done, re-set the tool rest to 20 degrees and draw a line at a 12 degree angle on your tool rest and grind the rake angles as shown in the pics.
Hone the side, end and top to remove the grind marks and put a small radius at the nose of the tool. To do this, put a small flat at the tip of the tool that follows the angle at the nose. You want the flat even from top to bottom. Then gently round the flat and blend it into the side and end of the tool. Give the tool a final hone on top and you're ready to cut.

I know this tool will cut 4140 well. I have a tool that is similarly shaped and it cuts as it should. For roughing, angle the shank of the tool so it is angled toward the chuck by about 3-5 degrees. For finishing, turn it towards the tailstock the same amount and take light cuts at higher speed.

I think that work piece is a difficult thing to make because you don't have a lot to hold on to when cutting the external taper. It looks to me like you have under 1/4" to grab on to and that is an issue because the material is rather hard and the work can slip in the chuck. Assuming you will cut the internal taper first and then chuck it up to turn the outside taper, you will need to take light cuts to keep from ripping the part out of the chuck. The tool, if ground as I described, should be able to take light accurate cuts (0.010 - -.020" deep") without too much cutting force and you might get away with it.

Let us know how it goes.
 
If your tool is changing color when sharpening it you are getting it too hot. Keep it cool when grinding. Too hot and you lose the hardness and tool will dull quickly.
 
You must log in or register to reply here.
Back
Top