No announcement yet.

rotary broach d o c ??

  • Filter
  • Time
  • Show
Clear All
new posts

  • rotary broach d o c ??

    Hey All,

    I made up a rotary broach, hope to cut a T-40 Torqx socket in 4140 annealed steel (will be retaining bolt - shell mill arbor).

    This is about 27 thou doc on each spline, much more than for a hex. Am I likey to get away with this in one pass, or will I need to grind a smaller dia "starter broach" & attempt it in 2 passes?

    If so, will final broach follow the starter, or do I neet to file a "chute" (guide chamfer) at stater splines to keep final tool in register?


  • #2
    T-40 is a large size for rotary broaching, but can be done.
    1. Try to make your pilot hole oversize by about 3-10%, this creates separated chips while broaching.
    2. Leave enough room in the bottom of the hole for chips. (I've seen alot of broken tooling result from 'looks deep enough'.)
    3. The chamfer should go all the way out to the major diameter.
    4. Try low feed rate to start .001-.002 IPR.
    5. If you use a rougher and finisher broach, they can be aligned by hand for a small quantity. For larger quantities you could make or use a rotary broaching brake.

    Bonus - Most rotary broach manufacturers (including mine) will tell you to set your feed and speed and then run the broach into the hole to the desired depth. However, contact at the workpiece with a staionary part this size often results in severe skidding on the part or chipped broach teeth. A better technique is to bring the broach into the part, maybe .005" deep at low RPM (50-100?). After contact is made ramp up to full speed.

    Hope that helps.


    • #3
      Thank you, Polygon. Just the type of info I wanted before attempting this first time.

      Looks like you guys make some slick tooling. I hope this project wil be just a one-off, so I'll "run 'er slow & see how she goes"!

      I'll try to remember to post an update & thanks again.



      • #4
        I wonder if it would help improve the depth of the plunge by boring out the center of the broach to give chips somewhere to go. I don't have one yet so don't know if this is even a problem.


        • #5
          good idea dp. For example, all of our hex broaches have a hole through the center of the broach. This allows fluid and air to escape if broaching a blind hole. The idea is to eliminate the risk of hydraulic pressure build up. We've put a larger hole at the end of some broaches as you suggest, but the trade off is a weaker broach.


          • #6
            Polygon, Thanks, I have learned something new today from your link about broaching. rotatory broaching sounds like a very cool way of making some very interesting screws and other hardware and it looks like sockets too. Just a question about tamper resistant screws does the hex type or torx type with the pin in the middle come from the same process?

            TX Mr. fixit for the family


            • #7
              Mr. Fixit, I too have always wondered about that. I've quoted some custom tools with the hole in it for that purpose, however I've also had to reject quite a few torx type because the wall of the broach was too thin. I suspect those must be made by cold heading or some other process.


              • #8
                Originally posted by Mr Fixit View Post
                Polygon, Thanks, I have learned something new today from your link about broaching.
                For those interested, there are number of shop-made rotary broach ideas out there. Here's one I'm adapting:


                • #9
                  Yep dp, Mike's is the basic design I worked off of. I made the outer cylinder to fit in boring bar holder of QCTP. Don't spin it too fast, and it seems to work fine (don't ask how I know).

                  I did have to broach T-40 hole in 2 passes (2 broaches), so now I have to get another bit to test the hole. Even then, had to break the chips w/ pilot drill a couple times.

                  I turned the whole assemble concentric in chuck, then set over compound 1* in use. If one were to machine the cylinder in boring bar block w/ the 1* built in (& mark orentation), you could lock cariage & feed w/ compound - may get more cutting force for the deep cut. There was some deflection w/ the broach so far off center (out in boring bar tool block).

                  It should cut hex sockets easily.


                  • #10
                    Originally posted by uute View Post
                    Yep dp, Mike's is the basic design I worked off of. I made the outer cylinder to fit in boring bar holder of QCTP. Don't spin it too fast, and it seems to work fine (don't ask how I know).
                    No surprise to me as that is exactly how I'm building mine, too. Was going to machine up a block then realized I have a boring bar QCTP lump so decided that would be my cutter holder.

                    I'm curious how rotary broachers align the cutter with the hole to be broached. Eyeball? Hyperbolic trig? BSL? "And here a miracle occurs"?


                    • #11
                      I lined up by eye, but had just carefully set hight to center for a previous project. A cone center to fit broach bit hole might be a good idea, or pop in a countersink.



                      • #12
                        Just a thought. You should consider making two or more whilst you have that set-up. Never hurts to have an extra screw like that.

                        Mentally confused and prone to wandering!


                        • #13
                          Krutch - luv the tagline - I'm more that way ever day. lol

                          That is a good thought, I've been debating about heat treating it. Harder to hold the broached slines, but will I just end up breaking the 1/4" threaded post off??

                          Prolly no need, that's why I went t-40 - fear of stripping out a hex.

                          Anyway, pics are more fun, so:

                          Rotary Broach:

                          Shell Mill Arbor:



                          • #14
                            Nice work, I love the pics.


                            • #15
                              In years past I rotary broached thousands of parts. They were done in bar fed lathes. The machines used 5C collets, a common problem was the work pushing back in the collet because of force needed to drive the broach in. Never found a good solution to that, except to switch over to a hydraulic press for the harder to broach jobs. BTW, when I bought my rotary broach heads I called Slater and explained what machines I was going to use (Hardinge), the guy told me to call back when I got a "real" machine, so I bought Somma heads.

                              For onesy-twosy broaching I recommend the press. But, rotary broaching is so cool it seems lots of guys want to do it just for the coolness factor. It can be done without the head. Make the broach out of an old end mill with a center point in the shank end. Offset your lathe tailstock to give the 2 degree offset (I forgot, is it 2 or 3 degrees that's commonly used?) Use a bearing type tailstock center to hand crank the offset broach in. You may have to figure a way to extract the broach though, still easier than building a head for the limited use most guys have for the process.

                              I wish the commercially made heads used inch size broach shanks rather than metric. Finding hardened drill blanks to make broaches from is a pain sometimes.