No announcement yet.

Fun with CNC thread milling [photos]

  • Filter
  • Time
  • Show
Clear All
new posts

  • Fun with CNC thread milling [photos]

    One of the founders of the company I work for has a Coles hit'n'miss engine. It has a drip oiler on a long pipe that reaches down through the water tank to lubricate the piston. The pipe had 3/16-40 Model Taper Pipe (MTP) threads on the end that had gotten irrepairably bent (see lower left of the following photo).

    I offered to fix it. I decided to cut off the bad threads and splice on new threads. I was averse to buying an expensive MTP thread die for a one-time use, and I don't have a taper attachment on my lathe. Instead, I milled the threads using a thread mill in my Deckel FP2NC CNC milling machine with Deckel Dialog 4 control. The associated photos tell the story.

    The threads came out better than any I could ever dream of cutting with a die. The Dialog 4 can do helical interpolation, but not spiral interpolation, which is needed for taper thread milling. To work around this issue, I made a mathematical model of the pitch spiral of the thread and broke it up into helical segments, four per turn. Each segment had a slightly different radius, but the end points of each segment coincided. Although the centers of the best-fit segments are mathematically off the center of the intended spiral, the offset is less than 0.00005", so negligible as far affecting the actual CNC g-code commands. I used Mathematica software to model the spiral and also spit out formatted g-code. I programmed these helical segments into the Deckel by downloading from my laptop.

  • #2
    Great looking work and a good description of the job. Nice fix too.
    Jonathan P.


    • #3
      I love thread milling, once you have done some you are hooked.
      Using multi vee cutters a lot of work is just one pass and is far quicker than screw cutting and you get that sexy run out at the end.

      Multi cut thread mills are horrendously expensive so I cheat and used either taps with all the flutes except one removed or for larger or external thread I use one die piece out of a Coventry die head.

      You only need one pitch to do all threads of that pitch and if you tilt the die slightly in the holder it will do a tapered thread in one pass.

      Sir John , Earl of Bligeport & Sudspumpwater. MBE [ Motor Bike Engineer ] Nottingham England.


      • #4
        So, am I understanding this process correctly... the workpiece is altogether stationary, and the CNC is revolving the rotating cutter around the workpiece, whilst simultaneously lowering (or raising) the cutter at the proper rate for the given thread lead?

        I assume the thread is cut to full depth in one pass ...?

        My town used to have a machine tool trade show every October, where I could see a lot of neat stuff. But they discontinued that a few years back. I miss that.


        • #5
          lynnl, you are correct on both counts.


          • #6
            rklopp, Thanks for the interesting post and pics! I'm especially impressed by the work and ingenuity to create the spiral.

            Originally posted by lynnl
            So, am I understanding this process correctly... the workpiece is altogether stationary, and the CNC is revolving the rotating cutter around the workpiece, whilst simultaneously lowering (or raising) the cutter at the proper rate for the given thread lead?
            ...this requires just three axis? on the tooling in a diy environment, any reason other that time that a home made single point tool wouldn't work (other than time)?


            • #7

              John S i have seen these run out threads on stuff from ww-2 how did they do this in the days befor cnc?


              • #8
                Yup, three axes required, {X,Y,Z} all moving at once. You could indeed do it with a home-made single-point tool like a lathe boring bar for threading, provided you could hold it in the mill spindle. You could also do it on a Bridgeport with a Vetcoa rotary table. On these, the table rises as it turns. When I was in school, they had an antique thread miller that looked like it was born in Whitworths shop or about that era (only slight exageration). It used a 60-degree horizontal mill type cutter, the mill spindle was tilted at the thread lead angle, and motion was coordinated through change gears. Neat machine. OSHA nightmare.
                Last edited by rklopp; 11-13-2006, 08:57 PM.


                • #9

                  In production, you can use a regular mill. The only move is a single axis into the cut, and the fixture lets the part revolve as it's moved up the pitch distance in one complete revolution.

                  Think about a lathe application by putting a Dremel tool in the toolpost with the thread-form cutter in it. If I'd lock the spindle, move the cutter into the work, then unscrew the chuck (in my case 1-/2 x 8) I could mill an 8 tpi on something. Screwed of course for other pitches, but I've got one available.

                  "People will occasionally stumble over the truth, but most of the time they will pick themselves up and carry on" : Winston Churchill


                  • #10
                    I used to have a regular job with a 2" pipe thread.
                    This was a box machine frame.

                    We did a similar procedure, hand programmed, with the use of a sub program
                    repeated the requierd number of pitches for the appropiate depth.

                    M98 Pxxxx Lyyy

                    This was the call up for the program. M98 called the program, P the program number, and The L was the number of repeats of the cycle.

                    Of course, M99 canceled the cycle and returned to the base program. The values for X, Y, and Z were incremental.

                    I had a hand ground flycutter and used tool comp to hold the finish depth.

                    That roughed the thread and required a pipe tap to finish the taper.

                    Last edited by kap pullen; 11-14-2006, 12:25 PM.


                    • #11
                      Nothing to add but

                      Nothing to add but.. I am not a real machinist, I play one in the shop and do my own jobs.

                      Helical milling of threads has not gotten my attention yet, but...

                      Sharpening of milling cutters has .. using the same helical interpolation I can run a small stone down my mills mounted on a fixture on my mill table.. NOW I have to build a fixture to hold the kwik switch adapters to set endmill length, so why not allow it to bolt to the table. USING the helical threading wizard. I rarely use that end of the table anyways.

                      ALL the time I have been drawin up a complicated x-y-A rotational device to feed to the HF chinese lathe tool grinder, NO need now. I can combine two projects into one and go at it.

                      I do however like the Wizards in Mach3.. XP has gave me a fit trying to get my cnc mill back online.. It turns out to be a video problem on the Intel motherboard and XP.. The video driver keeps crashing. XP don't like it.
             I used the wizard, the first hole there? It was bored while I was thinking I had a .5 endmill I did not measure with the caliper, I found out the helical boring was off about two thousandths so I checked the endmill and found it was about .4845.. I adjusted the diameter of the wizard and ran it again.. It fit perfectly. Hole was a 1.51 exactly.
                      I did this yesterday, The laser is a Sears Lasertrac I dissasembled and reassembled onto a 1/2" aluminum plate to do laser scanning with the camera. It is great doing non-critical setups like a lengthwise piece of plate. I was milling nema 23 motor mounts yesterday. OTHER easier to adapt line throwing diodes are available now.. FOR about the same price as the sears.. HF has a level with a diode waffle line lens for about $10. I am now powering this from a usb plug off the pc 5volt power.

                      I have rewired my cnc bridgeport after my dog pulled the cables out, some of the plugs on the larken drives were broken. I am not real happy about that. I am looking for some terminals to replace the slip on/off header plugs Larken supplied.
                      God knows I loved Butch, but he was a pain at times. This new pup, he ran though the dog door plastic shutter slider that shuts it from the outside (broke it in two) I have to cut a new slider on the plasma table I guess.
                      He is about sixty pounds of trouble now. I went outside with the double barrel last night about two am and he decided to come into the front yard and watch me. We have some more dope heads that have moved into my neighborhood. "Butch kept them all ran back over the fence", Lex is non-combative unless Dad is pissed or giving off bad radio waves. He was snarling like a bear last night.. Later ten or so police cars and video cameras were at the bottom of my hill here. SO the problem went on down the street.
                      Excuse me, I farted.


                      • #12
               cnc thread milling video on youtube..
                        Excuse me, I farted.


                        • #13
                          rklopp -
                          That is absolutely the coolest! That's the kind of job that, if I had done it, I'd run an extra part just to keep in the "portfolio".
                          Sadly, I'm totally manual on all my machines, but the one thing that makes me yearn for CNC is all the various kinds of interpolation that can be done.
                          Thanks for the post and the excellent descripton of the work.

                          The curse of having precise measuring tools is being able to actually see how imperfect everything is.