Announcement

Collapse
No announcement yet.

Interesting way to knurl...

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

  • Interesting way to knurl...

    This video impressed me. It is using linuxcnc G33 thread cutting gcode.



    The gcode.

    Code:
    G8
    G53 G0 X0
    G53 G0 Z0
    M6 T3 G43
    
    #<workpieceDia> = 0.700
    #<workpieceRad> = [#<workpieceDia>/2]
    #<safeXOffset> = 0.025
    #<safeX> = [#<workpieceRad> + #<safeXOffset>]
    
    #<knurlStartZ> = 0.000
    #<knurlLen> = 0.25
    #<knurlLeadIn> = 0.010
    #<knurlDepth> = 0.002
    #<knurlPerDia> = 28
    #<knurlAngle> = 30
    #<knurlEndZ> = [#<knurlStartZ> - #<knurlLen>]
    
    #<rpm> = 100
    
    #<pi> = 3.142
    
    ; The surface is the circumference of the workpiece
    #<workSurface> = [#<pi> * #<workpieceDia>]
    
    ; Given a knurl angle, calculate Z feed given <workSurface>
    #<feedPerRev> = [TAN[#<knurlAngle>] * #<workSurface>]
    #<feedPerMin> = [#<feedPerRev> * #<rpm>]
    (debug, feed per revolution: #<feedPerRev>; per min: #<feedPerMin>)
    
    ; thread _width_ is equal to distance traveled in one rev, i.e. <feedPerRev>
    #<threadWidth> = #<feedPerRev>
    ; Thus, TPI will be 1/<threadWidth>
    #<tpi> = [1/#<threadWidth>]
    
    ; To do a n-start thread, we need to start each thread
    ; <threadWidth>/n further back (Z+) than the prior thread
    #<nStartZOffset> = [#<threadWidth>/#<knurlPerDia>]
    
    
    M3 S#<rpm>
    
    #100 = #<knurlPerDia>
    #110 = [[#<knurlPerDia> * #<nStartZOffset>] + #<knurlStartZ> + #<knurlLeadIn>]
    (debug, knurl lead in: #110)
    
    G0 Z#110
    G0 X[#<workpieceRad> - #<knurlDepth>]
    
    O100 WHILE [#100 GT 0]
       (debug, start Z: #110; feed: #<feedPerRev>)
       (calculate the lead in for the knurl AFTER this one)
       #105 = #110
       #110 = [#110 - #<nStartZOffset>]
    
       ;G33 Z#110 K#<feedPerRev>
       ;G1 Z#<knurlEndZ> F#<feedPerMin>
       ;G1 Z#105 F#<feedPerMin>
       G33 Z#<knurlEndZ> K#<feedPerRev>
       G33 Z#105 K#<feedPerRev>
       ;G0 X#<safeX>
       G0 Z#110
       ;G0 X[#<workpieceRad> - #<knurlDepth>]
    
       #100 = [#100 - 1]
    O100 ENDWHILE

  • #2
    Is this quicker than 'put knurling tool in machine, switch on, advance tool into work, withdraw tool, switch off?
    'It may not always be the best policy to do what is best technically, but those responsible for policy can never form a right judgement without knowledge of what is right technically' - 'Dutch' Kindelberger

    Comment


    • #3
      That is a pretty cool way to knurl. It doesn't put any stress on anything.............unfortunately it's beyond the capabilities of my Clausing 5900 and most other guys machines too.

      JL...............

      Comment


      • #4
        That was pretty cool. I happen to have an Emco 120 (not the 120p as in the video) so I may give her a try. Thanks for the code... JR
        My old yahoo group. Bridgeport Mill Group

        https://groups.yahoo.com/neo/groups/...port_mill/info

        Comment


        • #5
          It looks like there's a lot of rubbing going on, because the insert doesn't have enough clearance to handle the big lead angle on the "threads." I'd like to see what happens on 4140 pre-hard instead of aluminum. Regardless, it's a very slow way to go compared to usual upset or cut knurling. I sometimes cut straight knurls with a thread mill and an indexer when I want them to come out like jewelry, but that is also a very slow method.

          Comment


          • #6
            Lay the insert tool over to match the helix angle and it would be fine.
            I just need one more tool,just one!

            Comment


            • #7
              Yes, it's slow, but it also has no more feed pressure than a cut of equivalent depth, and requires no setup from the operator - on a small lathe, I'd bet a 2-minute 'knurl' cycle is faster than turning the part under NC, then either mounting/setting up a scissor knurler, or moving the part to a second op machine for scissor knurling. All bets are off with a cut knurl.

              I have actually done rudimentary knurls using this method before, by indexing the stock in the chuck a fixed amount then doing a left hand, and right hand, threading pass with a relatively coarse pitch. It was *very* slow but it was only ever intended to be an experiment. Shallow DOC; the tool had highly exaggerated side clearance - 30 odd degrees per side, maybe more. I only had the patience to do 4 passes, though.

              Comment


              • #8
                Originally posted by Richard P Wilson View Post
                Is this quicker than 'put knurling tool in machine, switch on, advance tool into work, withdraw tool, switch off?
                Yeah, it takes way more time.

                I can see a use for it though. Aluminum is difficult to knurl the conventional way. Little flecks of aluminum get pounded into the work piece. If you color anodize a dark color like black, white spot are left on your work where the flecks dislodge in the process. This is why you seldom see diamond knurls on aluminum parts like instrument knobs, etc.

                Comment


                • #9
                  Nobody seems to be talking results. If its a deeper more crisp knurl, then it doesn't matter how long it takes.
                  Reserve it for those special projects.
                  John Titor, when are you.

                  Comment


                  • #10
                    Pffft...Linux geek showoff.






                    VERY impressive!
                    Milton

                    "Accuracy is the sum total of your compensating mistakes."

                    "The thing I hate about an argument is that it always interrupts a discussion." G. K. Chesterton

                    Comment


                    • #11
                      This is the Home Shop Machinist site so we need an appropriate mechanical method, something like this driving the lead screw back and forth...

                      Comment


                      • #12
                        Seems to me you could do the same thing on a manual machine by bolting an indexer to a faceplate to index the start of each thread. This assumes you have the tpi capability of course.

                        Comment


                        • #13
                          Originally posted by wierdscience View Post
                          Lay the insert tool over to match the helix angle and it would be fine.

                          That would only work if the tool cuts in one direction in the Z axis,
                          but it goes forward and back. It is cool, but I am not sure how not
                          to make it rub. Agreed, if it were anything other than aluminum,
                          it might break the insert. A + for effort though.

                          -D

                          PS- I mean, yes you could grind the tool for clearance, but it would
                          have little edge support. Would have to be a symmetrical clearance grind.
                          I am thinking oil groover tool.
                          Hey I bet a cnc lathe could cut oil grooves in bushings pretty easily.
                          A properly grooved for oil bronze bush works very well, given oil.
                          Hmmm.
                          Last edited by Doozer; 09-29-2015, 08:41 PM.
                          DZER

                          Comment


                          • #14
                            It could be done with a rotary tool like an engraver bit or 90 degree point endmill.

                            Comment


                            • #15
                              a crude affair. Show me a cnc lathe with live tooling that cuts a knurl with micro features such that from one direction you see an image of James Watt and the other Tesla and I'll be impressed
                              Last edited by Mcgyver; 09-30-2015, 09:15 AM.
                              .

                              Comment

                              Working...
                              X