Announcement

Collapse
No announcement yet.

[IMG] Turning threads in steel: badly torn finish with ground and honed HSS

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • #31
    It sure looks like a case of bad material, since the SS turned out so nicely. Have you tried turning or facing the same material? If you have problems with that, it would definitely point to a material problem.

    AIUI, setting the compound angle to 29.5 degrees causes the cutting tool to do most of its cutting on the left side, but it also just barely shaves material on the right. If it is set greater than 30 degrees, it will leave steps on the right side for each threading pass. Having the tool ride on the right side also helps with rigidity, as it prevents the tool from springing to the right.

    Here is my first attempt ever at threading, 3/8"-16, in a piece of steel (probably 1018):







    This was done on my Harbor Freight 9x20 lathe using a hand-sharpened HSS tool bit. You can see that I may not have had the compound set quite right, so there are ridges for each pass. I think this is the threading tool I used:

    http://pauleschoen.com/pix/PM08_P76_P54.png
    Paul , P S Technology, Inc. and MrTibbs
    USA Maryland 21030

    Comment


    • #32
      At end of your compound passes (less one) do a light simple plunge cut with the tool set at 30 degrees. That will clean it up any ridges etc.

      Comment


      • #33
        Right below your cutting edge, looks like no clearance..
        I mean the side toward the chuck.
        Side rake on top of tool should be ok, just makes it harder to check with the guage while grinding.
        Last edited by 754; 11-10-2017, 08:35 PM.

        Comment


        • #34
          I share the questions with regard to the very edge area where the honing is done. That must still have some clearance rake.

          Also, the side is nice, but the top of the tool is not very good-looking. Maybe the edge is not as sharp as it could be as to the top. And also maybe the cut material is not getting away cleanly, and may be getting re-welded onto the part. It does not look like classic re-welding, but ......

          Originally posted by lakeside53 View Post
          At end of your compound passes (less one) do a light simple plunge cut with the tool set at 30 degrees. That will clean it up any ridges etc.
          But his back-side edge is obtuse angle, not a cutting angle. So making it try to cut is maybe not so good.

          Also, something looks wrong with the pictures. The material that is smeared, looks like it is "smeared forward" with the rotation, and not "smeared back" in the direction the tool should have pushed it against rotation. Otherwise looks a bit like the way a built-up edge tears away.

          And again, is the threading tool ground with slight angle to account for the thread helix? It does not always seem as if that would be so important, but.....
          Last edited by J Tiers; 11-11-2017, 12:58 AM.
          2730

          Keep eye on ball.
          Hashim Khan


          It's just a box of rain, I don't know who put it there.

          Comment


          • #35
            Originally posted by 754 View Post
            Right below your cutting edge, looks like no clearance..
            I mean the side toward the chuck.
            Side rake on top of tool should be ok, just makes it harder to check with the guage while grinding.
            This what I'm seeing as well, not sure if this is an artifact of the photo or not but this could be responsible for the torn effect left by the tool bit, especially in soft gummy steel. I have found that when cutting these types of steels that just the slightest variation of the cutting edge geometry can make a surprisingly huge difference in finish quality.

            I see that the facing cut on the end of the work piece has a much more satisfactory finish. What can you do to the thread cutting tool bit to achieve similar geometry/results?


            Home, down in the valley behind the Red Angus
            Bad Decisions Make Good Stories​

            Location: British Columbia

            Comment


            • #36
              Take a piece of bar stock, put it in the chuck.
              Now using your threading tool cut a wide chamfer with the tool.
              Tell us what happens... if it can do that nicely it won't cut good threads....

              Comment


              • #37
                Originally posted by 754 View Post
                Take a piece of bar stock, put it in the chuck.
                Now using your threading tool cut a wide chamfer with the tool.
                Tell us what happens... if it can do that nicely it won't cut good threads....
                I don't get it?
                Location: Helsinki, Finland, Europe

                Comment


                • #38
                  Originally posted by 754 View Post
                  Take a piece of bar stock, put it in the chuck.
                  Now using your threading tool cut a wide chamfer with the tool.
                  Tell us what happens... if it can do that nicely it won't cut good threads....
                  I think you meant that if you CAN'T do that....


                  That's not a bad way to try different speeds and infeeds to determine the optimum settings.
                  At the end of the project, there is a profound difference between spare parts and left over parts.

                  Location: SF East Bay.

                  Comment


                  • #39
                    Originally posted by J Tiers View Post

                    But his back -side edge is obtuse angle, not a cutting angle. So making it try to cut is maybe not so good.

                    .
                    I was referring to PStechs post above mine.

                    Comment


                    • #40
                      Originally posted by danlb View Post
                      I think you meant that if you CAN'T do that....


                      That's not a bad way to try different speeds and infeeds to determine the optimum settings.
                      Just remember that you need to account for the helix angle. Some of the coarsest standard threads like 1/4-20 UNC have almost 4 degrees helix angle. If you grind the relief angle to 7 degrees you have effectively only 3 degrees relief angle left on the leading edge.
                      Location: Helsinki, Finland, Europe

                      Comment


                      • #41
                        What I am saying, is test that edge, see if it works.

                        Comment


                        • #42
                          Originally posted by Illinoyance View Post
                          The steel you are using is prone to galled or torn threads when cut at low surface speed. It may not be feasible to run fast enough to get a decent finish. In the shop where my son worked the shop foreman ordered the cheapest steel he could get to make some short shafts. In order to get sufficient speed to cut smoothly the RPM was so high the Z axis servo couldn't keep up, resulting in drunken threads. Try to get a steel better suited for machining. Others have posted their preferences. All are better suited for threading than what you use. Hot rolled and 0.2% carbon are a lousy combination.

                          Take a tip from pipe fitters. They die cut threads in really gummy steel all the time. They always use dark cutting oil that contains lots of sulfur. They seem to get decent threads at low speeds most of the time. Try the dark oil.

                          One of my favorite materials to machine is cold finished 1144 (Stressproof). Because of its sulfur content it is not recommended for welding.
                          Thanks for the tips. That's an interesting story regarding the drunken threads and servos that can't keep up. I've heard of Stressproof steel, but never seen it. At any rate, many of the things I make are welded after machining, and as such, general purpose mild steel is what I often use. I'd love to have some heat-treated 4140 or equivalent to experiment on. I do have some "hard" mystery steel that my Sandvik file will barely cut, but I've been too cheap to use it, and it's also mixed in with the rest of the mystery steel drops in cardboard boxes scattered along the floor.

                          Originally posted by MattiJ View Post
                          I did some test runs on crappiest S355 cold drawn stock they sell around here.
                          HSS tool with couple of passes with 0.2mm plunging straight in:



                          Nasty nasty... decrease the cutting depth to 0.04mm per rev and 0.02mm for last 5 passes:



                          The one on the left is turned with HSS tool and the one on the right is turned with ER16 VP15TF carbide insert.
                          Took probably 3 times longer with the pretty sharp sharp HSS tooling because it was tearing a lot more compared to insert. Insert tool did tear some but it was nowhere near as bad.
                          On some parts of the thread the finish looks great on the piece turned with HSS tool but there is still tearing marks visible. .The one turned with insert has more constant finish from thread to thread but doesn't look as nice as the piece turned with HSS in the best parts.

                          Both run @100rpm and last few finishing passes @ 40rpm.
                          Very nice results, very nice. I especially liked the first image which looks like a mirror copy of my results. What diameter and pitch were you threading?

                          Originally posted by PStechPaul View Post
                          It sure looks like a case of bad material, since the SS turned out so nicely. Have you tried turning or facing the same material? If you have problems with that, it would definitely point to a material problem.

                          [...]

                          Here is my first attempt ever at threading, 3/8"-16, in a piece of steel (probably 1018):



                          This was done on my Harbor Freight 9x20 lathe using a hand-sharpened HSS tool bit. You can see that I may not have had the compound set quite right, so there are ridges for each pass. I think this is the threading tool I used:
                          Come on now, how can free material be bad? Things that are free are not given away because they cause more problems than they solve. Right? Nice results on your threading job!

                          Originally posted by 754 View Post
                          Right below your cutting edge, looks like no clearance..
                          I mean the side toward the chuck.
                          Side rake on top of tool should be ok, just makes it harder to check with the guage while grinding.
                          I measured the clearance below the "primary" cutting edge by eye, and I got 5-6 degrees. That seems low to me, and I might have to try clamping a piece of steel on my bench grinder tool rest to cut more on the bottom of the tool for the next time.

                          Originally posted by J Tiers View Post
                          I share the questions with regard to the very edge area where the honing is done. That must still have some clearance rake.

                          Also, the side is nice, but the top of the tool is not very good-looking. Maybe the edge is not as sharp as it could be as to the top. And also maybe the cut material is not getting away cleanly, and may be getting re-welded onto the part. It does not look like classic re-welding, but ......



                          But his back-side edge is obtuse angle, not a cutting angle. So making it try to cut is maybe not so good.

                          Also, something looks wrong with the pictures. The material that is smeared, looks like it is "smeared forward" with the rotation, and not "smeared back" in the direction the tool should have pushed it against rotation. Otherwise looks a bit like the way a built-up edge tears away.

                          And again, is the threading tool ground with slight angle to account for the thread helix? It does not always seem as if that would be so important, but.....
                          The honing on the top of my tool is not perfect, or even great, but I use a similar method on other HSS tools for general turning and they usually cut well. I might have too little clearance in the front (left side) of the cutting tool, I'll look into that.

                          Originally posted by Willy View Post
                          This what I'm seeing as well, not sure if this is an artifact of the photo or not but this could be responsible for the torn effect left by the tool bit, especially in soft gummy steel. I have found that when cutting these types of steels that just the slightest variation of the cutting edge geometry can make a surprisingly huge difference in finish quality.

                          I see that the facing cut on the end of the work piece has a much more satisfactory finish. What can you do to the thread cutting tool bit to achieve similar geometry/results?
                          The facing cut was made by a Mitsubishi CNGG 120408 MJ VP15TF at a relatively slow surface speed and a "normal" feed. That's an interesting observation regarding small changes having a large impact. I guess one does not have a lot to lose by experimenting, maybe except in the area of hard drugs.

                          Originally posted by 754 View Post
                          Take a piece of bar stock, put it in the chuck.
                          Now using your threading tool cut a wide chamfer with the tool.
                          Tell us what happens... if it can do that nicely it won't cut good threads....
                          Sorry, I forgot to try that today while I was out in the shop and running the lathe.

                          Originally posted by MattiJ View Post
                          Just remember that you need to account for the helix angle. Some of the coarsest standard threads like 1/4-20 UNC have almost 4 degrees helix angle. If you grind the relief angle to 7 degrees you have effectively only 3 degrees relief angle left on the leading edge.
                          Good point, I'll have to look into this.



                          I had some free shop time today after I finished modifying a small Oilite (?) bushing for one of my customers International Harvester tractor transmission. I ground a new 60-degree included angle threading tool with the same 9-degree offset, but instead of giving it a side rake I instead ground in a back rake of about 10-12 degrees. The result was a somewhat improved finish, still threading at 125 RPM and feeding in @ 29.5 degrees between 0.20 - 0.02 mm. My photography got worse, however; I used my Samsung Galaxy S5 mobile phone instead of my DSLR. It actually has more megapixels, but megapixels aren't everything.

                          EDIT:
                          I only took one finish pass, the pass beforehand was probably fed in 0.05 - 0.06 mm. Do ye reckon' taking several finishing passes might have led to a better result?





                          EDIT2: Video filmed on my GoPro Hero 4, "narrow" angle of view. Random background music in the shop was supplied by Pantera for the occation. Note: the video is still uploading and will be ready about one hour from now on:

                          Direct link:
                          https://youtu.be/yZSJQYP0ddI

                          Embedded (maybe):
                          https://youtu.be/yZSJQYP0ddI

                          More embedding tries:
                          HTML Code:
                          <iframe width="560" height="315" src="https://www.youtube.com/embed/yZSJQYP0ddI" frameborder="0" gesture="media" allowfullscreen></iframe>
                          Last edited by Oyvind Ryeng; 11-11-2017, 03:15 PM.

                          Comment


                          • #43
                            You definetely need more finishing passes. I did more than ten! 5 passes with 0.04mm DOC and five more passes at 0.02mm doc. Before that it looked just like yours.
                            And about M20 and 2,5mm pitch or something like that.
                            Location: Helsinki, Finland, Europe

                            Comment


                            • #44
                              Very well, I'll make an effort to try that. Thanks for the clarification.

                              Comment


                              • #45
                                Be careful with back rake, as that is what changes the effective cutting geometry, and thus the actual angle of thread that you cut.

                                Any time the top of the tool is not perfectly radial to the work, you will have a change of geometry vs what is ground into the tool. The more off of radial, the larger that effect is.
                                2730

                                Keep eye on ball.
                                Hashim Khan


                                It's just a box of rain, I don't know who put it there.

                                Comment

                                Working...
                                X