No announcement yet.

Threading question.

  • Filter
  • Time
  • Show
Clear All
new posts

  • Threading question.

    The basic question is how much in feed to apply on each pass. Most of my threading experience has been on 1” diameter parts with 16 TPI where surface finish was important. Well I was doing some 3/8 threads and it was taking too long. I realise that the final cuts need to be small as you creep up on the correct fit, but where do you start?

    I am in the process of building one of John’s swinging thread gadgets where you apply the in feed while the carriage is returning. At my experience level that is going to get the pucker string a little tight. I will probably start by working on imaginary parts but at some point I am going to have to get wet to learn to swim in the threading environment.

    Any instructions would be appreciated.
    Byron Boucher
    Burnet, TX

  • #2
    I'll probably get scolded but on steel I only feed .010 per pass


    • #3
      I use 0.010" in feed on the compound set to the controversial 29.5؛ angle. A final pass at a thou and it's usually a done deal.

      Another rule of thumb involves a constant times the TPI but that's way too much turn time math.


      • #4
        I use a similar technique to Joe & DP's. I usually start out @ .010 for 2 or 3 passes with a "free ride" between each new setting of the depth of cut. I then back off to about .005, then .002 & finally to .001.

        There are quite a few variables that impact my depth of cut decision.

        1) Type of material

        2) Thread pitch (course = more roughing cuts)

        3) Fit & finish requirements

        4) Machine condition

        Note I also use the compound set @ one-half the included angle of the thread (AKA slant depth) to set the depth of cut, except for extremely fine thread pitches (>32 TPI). For UN threads this is 30 degrees and for Acme it is 14 1/2 degrees.

        To get an idea of how deep to cut for UN threads look at your thread pitch gauge (fish tail). It has a chart of the double depth of the thread. Divide by 2 and use this number as a starting point to check the fit.

        There are also almost 500 videos available on YouTube demonstrating single point threading on the lathe.
        Last edited by Dr Stan; 07-25-2010, 04:29 PM.


        • #5
          Well, you could calculate it all... The principle is to have equal chip area (in the cross section).

          Now I start with 0.5 mm for the first pass and slowly reduce. A rule halfway correct is to feed in by square of the previous pass. So that would be 0.5 mm; 0.25 mm; 0.06 mm; ... But then, you get the next rule: You can't cut too few. For HSS, I don't go below 0.05 mm.
          The easiest way is to watch the chip. If it starts to crimple, reduce feed. It should flow nice.
          At the end, two or three spring passes and you are done.



          • #6
            As with everything else, it depends on many factors. Even regular turning depth and feed varies depending on the tool, the material and the machine rigidity, etc. So do like the big production boys and figure it out their scientific way - keep messing with the variables until it works

            One thing to keep in mind on threading vs' turning is there are a couple more speed bumps to consider. Assuming you're doing the standard 29.5° compound thing, as you feed deeper, the surface area of the cutting face increases so you can make the first few passes much deeper than the last several. The other thing is that for a small, fine thread, the thread form dictates a much "sharper" point than the big course threads. That makes the cutter more fragile and prone to chipping the tip, requiring a fresh grind or insert index. So with fine threads you're stuck with feeding in light enough not to break the dang cutter.

            So what's the magic number? If the tool chips, you went too deep. If it takes forever because you're feeding in too light, then bask in the fact that you are a cautious perfectionist. Once you figure out what works, maybe write it down or commit to memory for future recall


            • #7
              If you're using laydown inserts, the manf has tables for feed giving several variables. but.... if often goes like 12 12 10 10 9 8 7 5 5 (for a 13 tpi thread).


              • #8
                Regardless of what type cutter I am using I go by the chip load. I start with .010" feed with the compound and determine what the next in feed will be by how hard it cut and the chip load of the last pass. It's usually .010" for one or two passes then .002" to .004" for a few passes and then I have to back off to .001" to .002" depending on how it is cutting. I don't like to see it ripping metal out and the tool looking like it's not cutting smooth.
                It's only ink and paper