Announcement

Collapse
No announcement yet.

threading tool

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

  • threading tool

    I purchased a new Dorian threading tool holder with a 60 degree carbide insert. I have used it on stainless and mild steel material and both times a small piece of the insert chiped off on the right side of the insert. I have not taken over 8 thou.cut on material at one time.The insert is square with the material using the fishtail as a guide. Has anyone had this problem before? Any suggestions

  • #2
    I have one of those, but have not had that problem.

    Chipping of carbide is usually from an impact, or from a buildup of material that gets torn off. Are you sure you don't have a rough edge building up on the work that could act like an interrupted cut and cause a chip?

    Also since the carbide inserts don't cut well at fine cuts, I don't think the 29 1/2 degree threading tool rule will work too well. Didn't for me. (brazed carbide is OK, if I hone it. I don't hone inserts)

    The 8 thous is OK, but much less is dubious, I suspect. If you do the 29 degree deal, the right side is just grazing, and the DOC is pretty small even at an 8 thous advance. Carbide inserts don't work like that very well.

    I just pushed the insert right in straight with the crossfeed, and it worked better. Insert cuts deeper on both sides then instead of just rubbing. Might chatter though.

    Maybe trying to do the 29 1/2 degree thing gave uneven heating, or a buildup, etc, etc. Could cause a chip maybe. Or if you got chatter, it might have caused a chip.

    How fast are you running that?

    Comment


    • #3
      Threading 16 TPI at 70 rpm, did not have any chatter and did not see any build up on insert before it chipped.

      [This message has been edited by jpcarlin (edited 03-28-2003).]

      Comment


      • #4
        Hmmmm...70 rpm, huh? Jack that up to about 1000+ rpm and you'll be fine. Let's see...off the top of my head 70 rpm would less than 10 sfm on a 3/8-16 or 20 sfm on a 3/4-16. Way less than the minimum recommended speeds for carbide insert threading.

        I assume you're threading on a manual lathe where higher rpm's aren't possible. You might try to find a source of HSS threading inserts. That's what I've used in the past where I had rpm limitations. It's been so long ago that I don't remember where I found them, but they are out there somewhere. Possibly some advertisers in HSM.

        As to using inserts for threading....we thread on CNC lathes all the time. Everything from 4-40 stainless parts on up. Fine infeeds work well. We use a 30 degree infeed, NEVER straight in. A straight infeed gives a negative rake on the trailing side of the insert, that's bad. For repeat production jobs we use full profile inserts which "top" the thread taking care of any burrs.

        Comment


        • #5
          Vardex, Carmex, Iscar or one of the other threading insert makers has a special carbide grade for low surface speed. They advertise it for use on small diameters on CNC, where surface speed is still not high enough even at top spindle speed. I get chipping, too, on a manual lathe unless I go as fast as I can stand and take light cuts. In general cutting forces go UP as surface speed drops. It's the force that chips the insert. There's a magical point around 250-300 FPM (in steel) where cutting force really drops. The trouble is, HSS can't handle the heat generated at those speeds.

          Comment


          • #6
            OK, OK, Carbide doesn't cut well at fine feeds AND LOW SURFACE SPEED.

            You guys and your CNCs distort the picture for us poor slobs using manual machines. Different techniques altogether, depending.

            About the negative rake going straight in, though, care to explain? I assume you may be referring to the effect of thread pitch.

            It depends on diameter and TPI, OK. But I am not totally certain how the effective rake varies by which way the tool is fed in. Seems like at any instant the tool is stationary infeed-wise either way, since you set depth and then take the cut.

            The DEPTH of cut I can see varies depending, as angle-fed it is less.


            Comment


            • #7
              Oso,

              Instead of saying carbide doesn't cut well at fine feeds and low surface speed, I'd say it just isn't likely to last very long.

              .008" is not an especially fine infeed for threading. On the CNC we thread with a predefined threading cycle. One of the parameters to specify is the depth of the first pass, the machine then calculates the depth of the following passes based on some formula, one formula used makes the following passes have a calculated depth such that the volume of material removed is equal on all passes. For instance, I usually start a thread with a .015" deep first pass, by the time the tool is into the thread a bit the infeed may only be a few thousands to equal the same amount of material removed as on my first pass.

              Regarding negative rake, whenever you cut a thread with an infeed such that the tool is cutting on the side opposite the feed direction you're at or getting near negative rake. Combine that with low SFM and you're asking for short insert life.

              Comment


              • #8
                It may have escaped you that he said

                1) no MORE than 0.008, presumably he also used less.

                2) with the 29 deg angle, even 0.008 on the feed is a lot less on the trailing edge. Less is, well, less.


                Per the rake, you are saying that the longitudinal feed gives an effective negative rake? Ok, it probably does, so would the thread angle.

                I still don't see why how you get to the tool position BEFORE the cut starts would affect the rake angle.
                You said "A straight infeed gives a negative rake on the trailing side of the insert"
                But the infeed is done before you cut.

                Oh well, I think we agree on the important stuff here..the CNC end of it has no relevance to me at all, see header line at top of board...:-)

                Comment


                • #9
                  I think the material is more likely the problem. Stainless and mild steel(if it's 1018 crs) are among the nastiest materials to thread. I suggest trying your new tool holder on something easier to machine and see how it goes.

                  If the insert has a very sharp point, try stoning a small radius with a diamond hone.(available at WalMart for around $6)

                  1000+ rpm is insane on a manual lathe for threading, so don't even try that. Your carbide should work well enough at the quite reasonable speed of 70 rpm. Most of my threading is done with carbide at 40-60 rpm. Brush on a little thread cutting oil before each pass and decrease infeed gradually as the thread forms finishing up with light passes. Works for me.

                  Comment


                  • #10
                    Snorman, do you infeed using the compound,{set at 29 1/2 degree}, or the cross feed?

                    [This message has been edited by jpcarlin (edited 03-29-2003).]

                    Comment


                    • #11
                      I am new to the threading thing, but tried my first threads in some SS shafts, possibly 304/308/316. It was scrap I had around. I was making some SS leaf spring shackle pins for my 4x4. Metric fine thread, M12x1.5 or so. Ya fine thread is easier to deal with, more time. I was doing them on my 12x36 gear head using a 60 degree brazed carbide , 60 RPM. I touched the cutter ends up with a small radius using a fine green stone. I used lots of cutting fluid and was taking small cuts, of .005" or so. If I recall I had the cross feed set at 30 degrees. The threads were then touched up the wire wheel to "clean" them up. I was happy with the results and plan on making more this summer. I want to try some internal threading soon.

                      ------------------

                      Comment


                      • #12
                        I had some trouble with this using carbide inserts with a homemade holder. It turned out to be a very small space behind the insert was allowing to the carbide to rotate slightly as the load increased. Once I discovered and corrected the problem, I quit snapping the noses off those cuttters. I'm not saying that's your problem, but it is something you might look for.
                        I'm here hoping to advancify my smartitude.

                        Comment


                        • #13
                          jpcarlin, I run a fairly big lathe(16 inch) with lots of power. The threads I cut are pretty coarse, in the range of 16 to 6 tpi. I always infeed using the cross slide with the compound set to 0, ie parallel with the spindle. Some will say this is no good, but I get good results with what I do. For a small lathe at home, I suspect using the compound to feed works better but can't say for sure. I do know using the cross slide to feed is simpler and faster. For really coarse threads I actually use a combination of cross slide feed and compound feed that's easier to do than describe.

                          1144 steel is great to work with if you can get some.

                          Comment


                          • #14
                            jpcarlin:
                            I hope that you have your compound set at 29.5* and are using it to infeed and not plunging in with the crossfeed!

                            By using the compound you get a single sided chip instead of the "V" shaped one from a plunge cut. The carbide will break everytime from the "V" cut as enormous forces are placed on the tip. Plus you are infeeding a bit too much - with stainless try to maintain passes of .oo3" minimum. Figure at least 5-9 passes depending on the thread depth with a couple zero feed passes to take out and spring in the system. This will give you glass smooth thread walls even at slower speed (like your 70rpm) - use a lube or coolant.

                            This is the prefered method if you do not have canned CNC cycles and is recommended by Kennametal, Sandvik, Valenite, and other OEM of carbide. It is also recommended that larger threads be roughed out with a regular triangular insert tool to reduce wear on the expensive carbide threading inserts.

                            [This message has been edited by Thrud (edited 03-30-2003).]

                            Comment


                            • #15
                              Thrud:
                              If your method, or ANY method can give glass-smooth walls on HRS at 70 RPM, why ain't you rich?

                              I have been told by genuine experts that THEY can't expect glassy smooth walls in HRS, so I shouldn't be surprised if I can't get 'em. Leaded steels, OK, that's different.

                              Comment

                              Working...
                              X