Announcement

Collapse
No announcement yet.

precision boring on bench mill

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

  • precision boring on bench mill

    Okay, I know I've started a couple threads here but after using the search function I haven't found an answer to my question, and no, I'm not trolling trying to get the answer I want to hear LOL. Heres the back story, I have a boring job where I have to bore a small cylinder in order to install a sleeve. The fit is an interference fit of .004. So the equipment I'm using is a RF45 bench mill, an import 2"boring head with indexable 1/2" boring bar 3" long. I'm locking all axis and feeding with quill, no power feed, just turn the fine feed by hand in a slow steady fashion. I use a coax to indicate center, set the bore head up, dial in .020" running the spindle at 310 rpm. I started out with cast iron inserts and ended up with horrible tolerances, switched to hard steel insert lots of chatter and bad finish. Went back with the cast iron insert and played with speed, feed, doc, feeding with quill, feed with quill locked and using head Z axis, just could not hold a respectable tolerance over 4.5". I went through several scrap motors and on the verge of giving up, I swapped out the cast for an aluminum insert. To my surprise, it did pretty well, nice finish, no chatter but still can't nail down the tolerances. I need to hold roughly a .0005-.001 tolerance meaning but I can only get .003 top to bottom. I figured out a sharp tool is going to reduce tool pressure along with deflection and consistent doc will aid in repeatability. I had to take .120" out, so I took .020 doc removing .040 twice, one at .015 taking .030 and a finish cut of .004 taking .008 leaving about .002 to hone to size. Even at a light cut I still hear the cutter skipping you can hear it hit the high spots but just won't seem to even out. I have the block pulled tight against a 1/2 cast iron angle plate with 2 ribs, everything is locked down tight. It seems that the machine holds a tighter tolerance in the x axis vs. the y axis. I trammed the mill in the tilt and when I surface a head with a 6.5 flycutter I get a nice checker pattern which is generally a good indication the tram is spot on. As far as tilt, well that's not adjustable, but while i have the coax in I swing it in the y axis and move the quill up and down and no movement of the needle. My only thought is I need to concoct a power feed for my quill, as an inconsistent feed could cause this I assume. Is there anything I've over looked or is it just that the machine is incapable of holding such a tight tolerance? I hate to blame the machine for my lack of experience, considering I'm no machinist but hell bent in learning and becoming one even if its for my benefit only. I know the machine I have has a huge following and I'm close I just need another couple thousandths. Sorry for the long winded post just trying to be thorough.

  • #2
    Check the positioning of the hole to the quill centre after all clamping is done - re-adjust as and where nececearry.

    The machine head quill cylinder should not wear or move as quill is raised and/or lowered.

    The potential for "spring" increases as the quill projects further out from the head bore.

    I'd be more inclined to clamp the quill and raise/lower milling head on the vertical dove-tail slider - with minimum clearance.
    Last edited by oldtiffie; 07-25-2017, 10:22 PM.

    Comment


    • #3
      What sort of material is the block you're boring out? I wonder if it has hard spots or inclusions of some materials other than the intended metal?
      Chilliwack BC, Canada

      Comment


      • #4
        Try an insert with a smaller nose radius if possible. Chatter is the pitfall for smaller machines, and a smaller nose radius might help reduce tool contact.

        Sent from my XT1053 using Tapatalk

        Comment


        • #5
          What diameter bore are you shooting for?

          I always take several spring cuts before my final cut. Run it through a second and even a third time WITHOUT touching the boring bar adjustments.

          Comment


          • #6
            Thought it to be cast iron but it makes powder, chips similar to bronze and very tight 6's

            Comment


            • #7
              Originally posted by Erich View Post
              What diameter bore are you shooting for?

              I always take several spring cuts before my final cut. Run it through a second and even a third time WITHOUT touching the boring bar adjustments.
              I also tried this but it seems like it won't take that last little bit. You can hear it touch when it gets to a tight spot but it just won't take it out. But it's not squealing or chattering, and it sounds like it's taking a cut but when the bore gauge goes in, you see no difference. Like it doesn't have enough tool pressure or its just pushing off. I even spun the insert to a fresh edge and still about the same. The bore size is 3.588

              Comment


              • #8
                You are doing a 3 inch hole with 1/2 inch bar. That's 6 times the bar diameter. That's borderline for a steel boring bar. I'd use a bigger bar or switch to a solid carbide bar. A lot less flex, chatter and taper.

                Dan
                At the end of the project, there is a profound difference between spare parts and left over parts.

                Location: SF East Bay.

                Comment


                • #9
                  Sounds like it's hardening slightly, a few lite cuts with nothing, then it will jump and take 12 even though you moved it 4.
                  My guess is the spindle is looser as it goes further out, is changing the size.

                  Comment


                  • #10
                    If you're using a HSS insert, then you are probably running that spindle a bit too fast. HSS cutting annealed soft grey cast iron can run at around 100fpm. For a 3.58dia that would be around 110 rpm. For a carbide cutter you can up the numbers to around 400fpm, which would be about 450 rpm.

                    Double check the position of the boring bar to be sure that the cutting edge is in line with the boring head line of travel. This is the equivalent to making sure a lathe tool cutting edge is at the correct center height. This affects accuracy and the tool geometry angles.

                    Also, with most boring heads there is a friction screw on the side that adjusts the amount of tension on the dovetail's gib, and thus controls the amount of torque required to turn the slide screw. If the gib is too tight the tool will not advance uniformly from one cut to the next. Too loose and the boring head will chatter and not repeat, in addition to leaving a poor finish.

                    Comment


                    • #11
                      Any chance you can mount the bar in the horizontal hole? That would make it much stiffer.

                      Sent from my Nexus 5 using Tapatalk

                      Comment


                      • #12
                        Originally posted by 754 View Post
                        Sounds like it's hardening slightly, a few lite cuts with nothing, then it will jump and take 12 even though you moved it 4.
                        Yep. I used to play around with boring single cylinder go-kart engines on my crappy Smithy 3-in-1 when I was just starting out. The cast aluminum blocks wound up being the worst, but even the cast iron blocks would also cause problems. I'm not sure if it was work hardening from my cutting or if was just a result of the abuse the cylinder sees during normal operation, but it was all but impossible to cut a good bore. The boring bar would deflect on the hard spots but then cut in the soft spots. And, as 754 noted, there would be situations where moving the bar out 5 thou would result in no change, so I'd adjust another 5 thou and it might take 1 thou off, so I'd adjust another 5 though and then it would take 15 thou off. Essentially I was loading the boring bar until there was enough "spring pressure" to actually cut and then it would dig in and cut the full 15 thou.

                        How did I address these problems? I bought a bigger mill

                        To summarize what others have said, you have 2 avenues to explore:
                        1) Investigate quill and make sure it is snug and perpendicular to the work so that, as you extend the quill, you don't run into unexpected problems. Limit the amount you have to extend the quill to maintain as much rigidity as possible
                        2) Improve your boring bar setup: larger diameter bar, solid carbide bar, etc. to improve rigidity and use sharp inserts (like the aluminum ones) to reduce load on the bar. Mounting the bar horizontal (Kotyara's tip) is a good suggestion, too. Playing with speed/feed and using lots of cutting oil to keep things cool and well lubricated will also help.

                        It's tough with a small machine.

                        Comment


                        • #13
                          Originally posted by Kotyara View Post
                          Any chance you can mount the bar in the horizontal hole? That would make it much stiffer.

                          Sent from my Nexus 5 using Tapatalk
                          Yes that is the method I've been using from the start, I meant to include that in the beginning but I was tired and couldn't think of a proper way to say it. Fatigue is a awful thing, get tired and forget how to speak.

                          Comment


                          • #14
                            Originally posted by Fasttrack View Post
                            Yep. I used to play around with boring single cylinder go-kart engines on my crappy Smithy 3-in-1 when I was just starting out. The cast aluminum blocks wound up being the worst, but even the cast iron blocks would also cause problems. I'm not sure if it was work hardening from my cutting or if was just a result of the abuse the cylinder sees during normal operation, but it was all but impossible to cut a good bore. The boring bar would deflect on the hard spots but then cut in the soft spots. And, as 754 noted, there would be situations where moving the bar out 5 thou would result in no change, so I'd adjust another 5 thou and it might take 1 thou off, so I'd adjust another 5 though and then it would take 15 thou off. Essentially I was loading the boring bar until there was enough "spring pressure" to actually cut and then it would dig in and cut the full 15 thou.

                            How did I address these problems? I bought a bigger mill

                            To summarize what others have said, you have 2 avenues to explore:
                            1) Investigate quill and make sure it is snug and perpendicular to the work so that, as you extend the quill, you don't run into unexpected problems. Limit the amount you have to extend the quill to maintain as much rigidity as possible
                            2) Improve your boring bar setup: larger diameter bar, solid carbide bar, etc. to improve rigidity and use sharp inserts (like the aluminum ones) to reduce load on the bar. Mounting the bar horizontal (Kotyara's tip) is a good suggestion, too. Playing with speed/feed and using lots of cutting oil to keep things cool and well lubricated will also help.

                            It's tough with a small machine.
                            Yes the mill I have is a 9x32 claimed weight is 800 lbs. A machinist friend was talking to me and said that a sharp tool and even cuts through out the process yield the best results, although he is using a Kwik way boring machine. I realized my best chance was to use a sharp insert and that helped tremendously. I'm cutting dry but even on a .020-.030 cut the bore stays cool, the insert is cool enough to hold your finger on so didn't think of work hardening the bore.
                            As some pointed out, I may need to find a smaller nose radius insert to further reduce cutting pressure and I'm sure a power feed would help to a point, may look at carbide boring bar if I can't get it with a few more tries.

                            Comment


                            • #15
                              You are using an indexable bar. Most inserts for cast iron or steel have a hone on the cutting edge. Those inserts don't do well on small depths of cut like when you are sneaking up on a diameter. Inserts intended for aluminum have a sharp cutting edge and work much better. I prefer high speed steel for boring. Brazed carbide works well also as long as the edge is sharp.

                              Comment

                              Working...
                              X