Announcement

Collapse
No announcement yet.

Bulk threading advice

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

  • Bulk threading advice

    I'm contemplating embarking on a journey that involves externally threading the ends of a thousand or more 1/2" 304 stainless rods (may be a variety of hex, round, or square) in the #10-24 to 3/8-16 range. Rods could be 10-16" long with 1/2"-1" worth of thread depending on size.

    Based on personal experiences, I don't think I'm going to be single-point threading that quantity or turning a die by hand. I'm willing to spend decent money, but not a mint.

    What are my options and what are other good-idea bad-idea points?

  • #2
    Hire a pipe threading machine and get the right die cutters, they come in all threads as well as pipe, or a Coventry die head in the lathe if you have one, very fast.
    Mark

    Comment


    • #3
      Everyone will have a different gauge for "spend decent money", and the solutions you seek can range enormously.

      Thread rolling is the way to go. For perhaps $700 to $2000 you can get a good LMT-Fette thread rolling holder and dies. Geometric (brand) dies and holders for cut threads will be cheaper but cost more per part. Either way you chuck them in a lathe.

      Or, you can just send it off to a shop with a Hartford or other thread rolling machine.

      Comment


      • #4
        How to go about it best would depend on several factors: one off job or repeat business; firm price or customer shopping around for quotes; what machines you already have that may be used/adapted; tolerance on threaded portion; etc.

        Comment


        • #5
          I would think 304 SS would be a poor candidate for thread rolling, due to its work hardening tendency, ...no?
          Lynn (Huntsville, AL)

          Comment


          • #6
            The way I would do it on a manual lathe is use 5C collets, one for each size/shape of bar and a lever collet closer. You can make a spindle stop or an extended 5C collet stop to make all the ends come to the same place.

            On the other end, a turret with a box tool or hollow mill to cut the round part and an automatic die head for the threads. (Get both used on eBay for cheap). The die head pops open at the end of the thread when the turret ram hits a stop. No reversing of spindle required.
            With this setup you are looking at a few seconds per part for machining and quick and easy part changes. Make sure to get collets that are made a few thou. open. If they are on size when at rest it will be difficult to change parts.

            That's how we did it back in the dark ages.
            Last edited by Toolguy; 05-04-2015, 01:34 PM.
            Kansas City area

            Comment


            • #7
              Originally posted by Rosco-P View Post
              How to go about it best would depend on several factors: one off job or repeat business; firm price or customer shopping around for quotes; what machines you already have that may be used/adapted; tolerance on threaded portion; etc.
              These would be my thoughts as well.
              Rolled threads are of course stronger if the application requires this quality. Not knowing what margin you are operating with or where in the world you are located I can offer only a link to a company that offers this service, just as an option to look into. Many factors come into play that will determine if this is a viable option, location being a significant one as shipping costs can easily negate any savings.

              Here is one picked at random outlining their thread rolling service options. There are many more out there, contact one locally if that is an option.

              http://horstengineering.com/threadro...hread-rolling/
              Home, down in the valley behind the Red Angus
              Bad Decisions Make Good Stories​

              Location: British Columbia

              Comment


              • #8
                +1 for a Geometric head,a thousand parts sounds like a lot,but that is only a couple days production with one fitted to the lathe carriage less than a day fitted to a turret lathe turret.
                I just need one more tool,just one!

                Comment


                • #9
                  Originally posted by lynnl View Post
                  I would think 304 SS would be a poor candidate for thread rolling, due to its work hardening tendency, ...no?
                  There isn't much carbon in 304, and 80 Rockwell sounds like a big deal until you realize it's B and not C. My experience is gummy more than a Superman's kneecap type thing. I'm certainly up for input and I while I get mixed opinions when reading, it sounds like forming taps get more mileage in 304 than cut taps do. I'm figuring that might hold true for external threads.

                  Comment


                  • #10
                    Concentricity isn't a huge deal, so I figure a scroll chuck should work unless round bars want to spin. I agree a turret lathe would a natural fit for this but would probably only be an option if one popped up both cheap and local.

                    A certain auction site seems to have plenty of geometric type die heads with all the chasers I could want, so I have a bit of reading nighttime reading to do now.

                    I don't seem to have much luck with search terms for rolling die heads other than seeing videos posted and thinking "that looks incredibly easy".

                    As far as existing equipment, I've basically got a 3-in-1 in the garage with MT3 sockets, 3" chuck, and a 4-way tool post. It doesn't really have a problem turning 304 but I am having to teach myself how to grind chip breakers. I figured the length I'm threading fits on a 2" indicator easy and likely a 1" once when it is all said and done. I figure the process would be to use the tool as a stop, chuck the material, face, shoulder, chamfer, thread. It is just the threading that has me starting this thread. I'm sure whatever I do there's going to be a learning curve and some failed attempts.

                    Ultimately I figure I'm going to see what it costs to get it done and see what the cost difference would be over my time and labor. If somebody can do it for $0.50/piece over what materials could cost me, I'm not sure I could beat that if my time were free. If, on the other hand, the lowest I can come up with is $5.00/piece over materials, that would cover some nice tooling and a lot of my time.

                    Comment


                    • #11
                      Ok, this is part of what my shop does for a living....

                      In looking at our setup for costing, using a 2 head Landis...Our labor component for cutting 1/2-13 thread 1" long for 2 ends is about .38 per stud...

                      Now I know you have different diameters you have to do, so this is an unfair comparison.

                      But if someone came to me and wanted the 1/2 turned down for different thread diameters, I would decline the work first, but if they absolutely had to have it, we would then just use the CNC lathes and knock em out.

                      Speaking from personal experience, doing these manually will piss you off. Round oily bar is hard to hold at times...

                      Comment


                      • #12
                        Originally posted by cuemaker View Post
                        Ok, this is part of what my shop does for a living....

                        In looking at our setup for costing, using a 2 head Landis...Our labor component for cutting 1/2-13 thread 1" long for 2 ends is about .38 per stud...

                        Now I know you have different diameters you have to do, so this is an unfair comparison.

                        But if someone came to me and wanted the 1/2 turned down for different thread diameters, I would decline the work first, but if they absolutely had to have it, we would then just use the CNC lathes and knock em out.

                        Speaking from personal experience, doing these manually will piss you off. Round oily bar is hard to hold at times...
                        I really think it will be a single thread size somewhere in that range or, if it changes, it would be on something like >1k groups. Also the threading is only on a single end. I'm guessing at a minimum the other end would be faced and chamfered, but I ought to experiment and see how much of a form tool my wee little machine could cope with.

                        Are you turning then threading, or just directly threading dimensioned bar?

                        Comment


                        • #13
                          We are threading dimensioned blanks that are already chamfered. For a stud with a different body than the thread, what we call a step stud, we would cut the blanks in bulk, chamfer, then turn down, then thread on a cut threader. With just one end, a lathe operation make more sense.

                          Comment


                          • #14
                            Not knowing what this part is all about I don't know if this is practical or not but when I need something like this I drill and tap the end of the larger bar and run setscrew in the end to produce the male thread part.

                            Comment


                            • #15
                              Originally posted by APEowner View Post
                              Not knowing what this part is all about I don't know if this is practical or not but when I need something like this I drill and tap the end of the larger bar and run setscrew in the end to produce the male thread part.
                              That's an excellent idea and could be the fastest option for the machine I currently have. I would just have to work out how to change tools for facing, spotting, drilling, and tapping between the toolpost and tailstock.

                              Comment

                              Working...
                              X