# Help with turning 4140



## Investigator (Feb 20, 2018)

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?


----------



## benmychree (Feb 21, 2018)

Are you using a cutting oil or other lubricant? using the lowest feed rate may not be the best thing.  I use Tap Magic as a cutting oil on nearly everything so far as steel is concerned, it can make a huge difference. Make sure your tools are on center, and too slow of a cutting speed is not good.  4140 ann is not difficult to cut compared to mild steel.


----------



## Alan H. (Feb 21, 2018)

Make sure your bit is ground properly.  Try bumping the speed up to 400 rpm and as already said use a mist coolant or oil. 

Can you post a photo of the HSS bit showing its grind? 

The 4140 should have a good finish.  I like turning it a lot.


----------



## dlane (Feb 21, 2018)

Higher Rpms ,radius cutter, smaller= faster speed, where was steel made , pics?


----------



## Technical Ted (Feb 21, 2018)

You stated is was supposed to be annealed... What color are your chips? This will help you determine how hard the 4140 actually is... If running HSS it's probably best if they come off a straw yellow or silver rather than blue/purple. I have run my best, high quality HSS lathe tool bits (usually with Cobalt added) at higher speeds and gotten away with it, but if you're using a low/normal quality HSS then you might be loosing the cutting edge if running too fast. If using an import HSS, you're most likely better off running even slower yet. 

Also, when grinding your cutting tool, the harder the material the less top rake you want. Another thing is that, typically, the cutting speeds most charts list are suggested maximum speeds. I always use 60-80% of those speeds and adjust from there. I'm not running production and I like my tools to last a little longer. Sometimes, running slower helps to break the chips because they have time to cool off and become more brittle. Of course, sometimes you need to run faster to break them. Go figure... I hate long stringy chips. As others have suggested, cutting oil or coolant will help as well.

YMMV,
Ted


----------



## Investigator (Feb 21, 2018)

Thanks for the replies.  I am using a blank I ground myself, I got the blank when I bought the lathe.  It is marked Fagersta WKE 4 Sweden.  I am using non-detergent 30W oil as it turns.


----------



## Investigator (Feb 21, 2018)

The chips come off in tight curls and are uniformly dull silver in color


----------



## cg285 (Feb 21, 2018)

benmychree said:


> using the lowest feed rate may not be the best thing.  Make sure your tools are on center, and too slow of a cutting speed is not good.  4140 ann is not difficult to cut compared to mild steel.



+1, + more doc if possible


----------



## Investigator (Feb 21, 2018)

DOC was usually .030" to .050"
What would be the recommendation for DOC and feed rate?


----------



## pdentrem (Feb 21, 2018)

Your depth of cut is fine. RPM per the charts for 2” is between 136 - 382. Everything else will depend on the tool geometry. A HSS tool has to be sharp. I ground mine with at least 10 degrees of side angle and a chip breaker, fairly square to the work and a small nose radius. As I was only roughing the shafts prior to finish grinding to size, surface finish was not taken into consideration. A finish pass would of been required to make the surface smoother.


----------



## pdentrem (Feb 21, 2018)

Incase you have not seen this. I also suggest to use a fine diamond stone to finish sharpening to tool as a regular grinding stone leaves a rough finish that needs to be improved to get the best finish on the steel.

https://sherline.com/Wordpress/wp-content/uploads/2015/01/grinding.pdf


----------



## mikey (Feb 22, 2018)

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?



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.


----------



## Investigator (Feb 22, 2018)

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.


----------



## Robert LaLonde (Feb 22, 2018)

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.


----------



## Uglydog (Feb 22, 2018)

The attached video may be helpful.

Daryl
MN


----------



## Investigator (Feb 23, 2018)

Some photos:

This is the part i'm making





Here is the bit for the inside:





this is the outside bit:


----------



## mikey (Feb 24, 2018)

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.


----------



## bluechips (Feb 24, 2018)

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.


----------



## pdentrem (Feb 24, 2018)

Check out Mr Pete’s YouTube video series.

Here is another blog
http://www.machinistblog.com/grinding-lathe-tools-on-a-belt-sander/


----------



## Chuck K (Feb 24, 2018)

Are you certain that is 4140 you're turning?


----------



## Investigator (Feb 24, 2018)

mikey said:


> 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.
> 
> ...



Mikey,
I appreciate all the help, no offense taken.  I realize I don't know much about it.

I did try a cheap boreing bar with inserts, I had trouble with the last few cuts because of diminishing clearance. 

I will look and try to regrind my tools this weekend.


----------



## Investigator (Feb 24, 2018)

Chuck K said:


> Are you certain that is 4140 you're turning?



It was sold as 4140, I have no way to confirm.


----------



## Chuck K (Feb 24, 2018)

Investigator said:


> It was sold as 4140, I have no way to confirm.


The only reason I ask is, it looks like it's turning real gummy.  It's hard to tell looking at pics.  If you have an extra piece you might try experimenting with the grind of your tool, feeds, and speeds until you have something that works.  4140 should leave a nice finish.


----------



## mikey (Feb 24, 2018)

Investigator said:


> Mikey,
> I appreciate all the help, no offense taken.  I realize I don't know much about it.
> 
> I did try a cheap boreing bar with inserts, I had trouble with the last few cuts because of diminishing clearance.
> ...



Hey, nobody knows how to grind lathe tools when they first begin, believe me. Give it a go and if you can grind the tool with the angles I suggested I think you will be pleased with the results. I also suggest you buy yourself a set of those brazed carbide Chinese boring bars. They only cost about 10 bucks for the set and, when sharpened with a diamond stone, will cut that tapered bore easily. Do let us know how it goes, okay?


----------



## pdentrem (Feb 24, 2018)

I would believe that the tearing raggedy look to the surface is due to the 0 degree side rake that the tool currently has. Need more like 10-15 degrees to make it more of a knife edge with a small radius on the tip.


----------



## pdentrem (Feb 25, 2018)

Here is the HSS tool I ground on the bench grinder. It has been changed to a sharper cutting edge but this should help you out. I was feeding this fairly square to the shaft to help reduce chatter and deflection away from the tool.


----------

