No announcement yet.

4130 steel - simply poor machinability or...

  • Filter
  • Time
  • Show
Clear All
new posts

  • 4130 steel - simply poor machinability or...

    Along the lines of the thread started by FJK... Can anyone give me a hint on turning 4130 steel? I'm using a plain bearing lathe in good condition. I've been working with 1018 steel and O1 the last few days. After changing to 4130, I simply can't work out a satisfactory finish. The work looks "torn", shows "rings" around the OD. Nowhere close to the finish I was getting on the other material. I'm using the same speeds I did for the O1 work... 930 rpm. That works out to about 87sfm. I tried slowing it down quite a bit; that helped buy not tremendously. Is this just "what it is" with HSS cutting tools and 4130, or is there a tool geometry change that is recommended for 4130? I've never considered O1 to be an attractive material to turn, but the finish was far nicer than this. Am I expecting too much? This is the best I can get it:

  • #2
    Its not the same material but looks very similar to what I had before trying a shear type edge and slowing the feed down to never did get to where I had hoped but a great improvement.

    I am sort of chalking "not getting to where I had hoped" down to not having the backgear available so still pretty fast (254 rpm v. the 86 rpm I think would work best) and more so having no way to slow the feed a bit more...slowest I can feed is .0031 ipm and I like to go about half that...


    • #3
      I've never dealt with 4130, but here are a couple of thoughts that may be applicable: are you using cutting oil? If not, get some high-sulpher cutting oil and slather some on. That might help.

      Make sure your toolbit is, as we say in Maine, "wicked sharp." If you're not doing it already, try going over the toolbit with a medium to fine India stone or similar after it comes off the grinder. Or a medium to fine diamond stone. A slight radius on the toolbit might help. Polish that sucker right up!

      Or it may just be the nature of the beast. Some steels are certainly more machinable than others.
      Try to make a living, not a killing. -- Utah Phillips
      Don't believe everything you know. -- Bumper sticker
      Everybody is ignorant, only on different subjects. -- Will Rogers
      There are lots of people who mistake their imagination for their memory. - Josh Billings
      Law of Logical Argument - Anything is possible if you don't know what you are talking about.
      Don't own anything you have to feed or paint. - Hood River Blackie


      • #4
        High feed rate, Higher speed. Something about Chrome Moly-41 steels just loves this. I hit my 4130 and 4140 at about .005 to .008IPR and about 150 SFPM or a bit more. I get a finish that is just unbelievable. You kind of have to "push" through the toughness of the Molybedenum or it oushes back, creating the ridges of resistance.

        On my 13 inch lathes (240V), I actually hear the machine settle in to a load type of situation where them machine actually sounds very smooth and a high but not excessive load is present.

        I do the same with D1.
        CCBW, MAH


        • #5
          Yep. Higher feed, higher speed, and more depth of cut.

          I _FINISH_ at .0035" - .005" per rev.
          Try roughing at .005" - .008" per rev.
          For HSS, I'd try .012" - .02" DOC and see what it likes.
          Double your speed and start there...


          • #6
            And this is why I like coming to this site...I would have gone completely the wrong directions


            • #7
              Im starting to like using a lathe file on my 1018 steel when it does that and I want a good finish.. Does not take much off at all before the finish looks really good.
              Play Brutal Nature, Black Moons free to play highly realistic voxel sandbox game.


              • #8
                Originally posted by Black_Moons
                Im starting to like using a lathe file on my 1018 steel when it does that and I want a good finish.. Does not take much off at all before the finish looks really good.
                Yup, those jack screws I posted in my other thread a few days ago were from 1018, and with a little detail work after sizing them they turned out beautiful.


                • #9
                  I think you need to check your SFM calculations.
                  Starting point for 4130 on a home lathe is 50 FPM
                  I believe I see a 1/2" collet ?
                  .5 x 3.14 (PI) = 1.57
                  12 /1.57 x 50= 382 RPM

                  Hold your left hand against the carraige feed handwheel to keep a drag on the feed. This produces a better feed "Pattern" (cancels gear feed variations)

                  Put a small radius on the tip of a very sharp M42 (HSS) tool bit.
                  Stone, stone, stone.....

                  Check the slop on your spindle bearing by putting an indicator on the work piece when stopped and push the workpiece with your hand . If it moves with a light force of maybe 5 pounds, you will not get a good finish without using abrasives

                  Green Bay, WI


                  • #10
                    Rich mentioned the starting point for 4130 on a home lathe is around 50 fpm. Is there some where a person could find the starting point for other materials?
                    In breaking down your equasion for spindle rpm's I take it that the .5 is the dia of the material, and 12 would be 1 foot? Please don't laugh, I never really knew how to calculate speed and feed rates.
                    I'm just glad there's a place I can ask a simple question and not have some one thinking I'm to mentally challenged to be on a machine forum.


                    • #11
                      Okay, playing around with aspects here. Both of these are at 1725rpm. DOC for each was .5mm (.200"). Yes, the collet and original stock is 1/2"; however, the turned portion is much closer to 3/8". I used that as the basis for calculating the sfm since it was the diameter I was turning at that resulted in the previous photo. For reference, the second cut shown here resulted in a final diameter of ~.310".

                      First, used 1/64" radius HSS. Sped up the feed but this is all manual. I really can't even estimate a number for feed. Needless to say, though, it was faster than I have been using. Not slow. Not "fast" (that gets the spiraling ring effect).

                      This is the same feed but now with a 1/32" radius.

                      Both are remarkably better than my original tries. The surface feels "smooth" to the touch. It just looks more dull with a residual "tearing" look than my usual material. Both radius examples have this characteristic.. I still think the stuff stinks compared to what I can get with 1018 No doubt this is a great improvement, though, over my previous attempts. Thank you. Strange how it reacts so differently than other steels from my experience. I even looked it up for double check reference in Machinery's Handbook. It lists 85sfm and suggests to "slow feed" and "increase nose radius" to tackle a poor finish with HSS. Guess you can't always follow the book as it were. Strange for sure. I honestly can't say I'm truly satisfied with the finish, but I can call it acceptable without a doubt. It'll also easily clear up with some abrasives. Good enough.


                      • #12
                        Originally posted by catman81056
                        I'm just glad there's a place I can ask a simple question and not have some one thinking I'm to mentally challenged to be on a machine forum.
                        No trouble. I never listed diameter in the original post. I see this has led to some questions. All speeds are equated in my shop by the "cheat" equation. That is, it replaces Pi with the numeral 4. Here is the equation:

                        Surface Feet per Minute * 4 รท Inch Diameter.

                        My lathe is all metric, but I exclusively use the above equation because I am only familiar with SFM and not Meters per Minute. Hence I am a bastard---working in millimeters and calculating in inches at the same time!


                        • #13
                          I had the same issues with my SB Heavy 10. I tried everything. finally, when the bearing noise was loud enough, I replaced the thrust bearing. all these issues went away.

                          It is not only Axial play, radial play is also an issue, check the axial play in your spindle. Check the condition of your thrust (bearings).

                          You need to have both axial and radial to get a good finish.

                          Jim B.
                          Jim B


                          • #14

                            try googling "feed and speed", "feed and speed rates", something like that...there are a few calculators out there where one can just plug in numbers (rpm etc.) but you will need to "cross reference" to materials as the numbers are different...those material numbers are found in reference sources like Machinerys Handbook. Sometimes you can find information that can give you a place to start,
                            would be an example and though they don't give an exact number they do list "Machinability" which is listed as some percentage of AISI 1212 with that being 100%.
                            if you are using inserts, those manufacturers will most often give suggested rates of feed and speed based on a number of parameters


                            • #15
                              Small diameter with large DOC. You might want to try supporting the work with a tail stock center to see if things improve further.