Announcement

Collapse
No announcement yet.

Boring Cylinders

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

  • Boring Cylinders

    I have a problem making cylinders which are very cylindrical. I am using a Bridgeport mill with boring head. I have also made some attempts on the lathe. At present I get better results with the lathe.
    If I use an inside mike on the ends, I find non circularity on both machines of up to .0015. The ends are similar with the lathe, but with the mill, the bottom can be up to .003 larger diameter. The first question is, what is an allowable run out, both for steam and for internal combustion? I have seen no figures on this. I am using cast iron piston rings.
    Second, what techniques do people use to get good cylindrical bores, and what kind of measurements to they get?
    A related question would be: What kind of cylindrical measurements are achieved in automotive cylinders?
    Finally, do people use honing to achieve a more cylindrical cylinder?
    Thanks,
    Steve

  • #2
    Steve,
    Some of your question can be answered but to really tell you why you're having trouble we would need to know much more about the accuracy of your equipment.
    First off if you're building a model steam engine you can get away with a little irregularity in your cylinder but .003 is way too much. For internal combustion engines you need dimensional tolerance plus very close concentricity. With any internal combustion engine the best way to accomplish this is by honing but the standard hones used the the home shop will generally follow the initial bore.
    The purpose of a hone is just to clean up the bore, make it concentric and take off a very small amount of material in the process.
    As to why you're getting so much runout with your machines it could be that they aren't accurate (tight) enough to hold extremely tight sizes. It could be partly your setup. It could also be the sharpness of your tooling.
    Like I stated at the beginning we would have to know a little more about your machining operation and tooling to give a good assessment of what's going on.
    gbritnell

    Comment


    • #3
      Originally posted by Stephen A. Douglass
      I have a problem making cylinders which are very cylindrical. I am using a Bridgeport mill with boring head. I have also made some attempts on the lathe. At present I get better results with the lathe.
      If I use an inside mike on the ends, I find non circularity on both machines of up to .0015. The ends are similar with the lathe, but with the mill, the bottom can be up to .003 larger diameter. The first question is, what is an allowable run out, both for steam and for internal combustion? I have seen no figures on this. I am using cast iron piston rings.
      Second, what techniques do people use to get good cylindrical bores, and what kind of measurements to they get?
      A related question would be: What kind of cylindrical measurements are achieved in automotive cylinders?
      Finally, do people use honing to achieve a more cylindrical cylinder?
      Thanks,
      Steve
      It is hard to tell what you are talking about. There is no such thing as "non-circularity". If you are talking about how round the hole is, that is circularity. It cannot be measured with an inside mike. To measure, sweep the hole or other feature with an indicator. The total movement of your indicator is "total indicator reading" (TIR). This is usually the measure of circularity. The combination of circularity and taper is "cylindricity" and that is what you should be concerned with. If you don't have a coordinate measuring machine you will have to measure the characteristics separately.
      We need a LOT more information. What is the material, clamping method, tooling. Are non moving axes locked?
      You should get a near perfectly round hole by boring, so something is wrong. Clamping is likely a part of it since it changed from lathe to mill.
      Tell us more, with proper terminology and measurement.
      Last edited by tdmidget; 08-24-2011, 01:56 AM.

      Comment


      • #4
        After getting my outboard 3 cylinder block back from being bored I had to bring all three holes up .008 to be within specs. I used My sunnen hone set starting out with I believe the j45 stones and finishing with some sort of 80-85 stones. I could not get a varying measurement anywhere in any of the bores top to bottom and all around with a bore gauge and mitsutoyo caliper to the .000".

        I was very impressed with the results and the motor has been running GREAT two years now!

        Andy

        Comment


        • #5
          Well ok not two full years but I did run it last fall and all this summer.
          Andy

          Comment


          • #6
            If you're finding that your holes are oval both on the lathe and on the mill is it possible you are clamping the part too tightly, thereby egging it up whilst you do your operation?

            Comment


            • #7
              Torque plates

              Torque plates put the same stress on the cylinders that the head do. Sometimes they are critical, other times not.

              It's hard to find the hole center.
              A combustion engine normally "eggs" out the cylinders, boring, you do it "first size" sometimes that is enough to "find the Round HOLE in the non-round bore".. other times Not..
              Look for a "shadow" as you bore, meaning you are not cutting "OUT" the previous bore size. You must go beyond the previous non-round hole.

              If you have any flex at all in your equipment, it will wander all over the place.

              Being a poor boy from Gawgia, I've bored harley jugs on the lathe. I would not know where the jig is today, but zeroing it "once " was enough, it has went back each time.
              I spun the jug.

              Does any of that make sense.. YOU can "Lose" the true centerline of a engine boring it.. especially quickway bars.. where you run it backwards to FIND HOLE Center after extending the fingers to find it. IE: why a build job changes the way a engine puts out power.. There was a local shop that said they could give me 10+ more horsepower in a bore job. Angle bore.. (offset crank center)
              Excuse me, I farted.

              Comment


              • #8
                Ok, this is a bit of a struggle, because I have never done anything on a bulletin board before. But the two responses so far are stimulating my thinking. First of all, I am not a professional machinist. My degrees are in biology and biochemistry. But I love cutting metal.
                First, I suspect that gbritnell is George, who makes incredibly small V8s and lever action rifle, etc. I'm the guy who used to set up air lines for the modelers at the La Grange engine club show, until I moved to Seattle area to be near my daughter.
                I thought that if one used an inside mike on a cylinder, that the reading should be the same all the way around. The second person to reply is suggesting that instead I should set up a dial indicator after boring and look at runout. Okay, I can try that.
                The materials are cast iron and bronze, but I have been playing with pieces of steel pipe to work on techniques. Tools are sharp. I have clamped in v blocks in the mill vise, or placed in three jaw chuck in the lathe. I'm trying to use minimal clamping forces as I realize that that I can distort the cylinders if I clamp with too much force, and then when I take them out they will relax to a different shape than the desired cylinder.
                Thanks for the mention of what is acceptable in terms of runout. It looks like I have a way to go.
                Steve

                Comment


                • #9
                  I have no direct experience in boring cylinders in the lathe or mill but unless it is very thick walled I am sure that holding one in a 3 jaw chuck or V-blocks with enough pressure to retain it will cause more than just measurable distortion. Many, many years ago my Dad showed me how he could release an inside mike hanging in a car engine bore by squeezing the sides of the block with his hands. I thought it was a trick but learned that the bore was actually made oval enough to do that.
                  Last edited by Don Young; 08-23-2011, 11:00 PM.
                  Don Young

                  Comment


                  • #10
                    for a good tutorial on measuring round parts do a google search on centerless grinding. A part can be lobed and still measure round across two points. I have seen .32 diameter part measure round with a micrometer and be .01 out of round when measured using a V block. To tell if a part is round you need to measure across three points of contact.

                    If you are holding the part in a V block, using the V block clamp you do not have a round, nor straight hole. You need to have the maximum amount of contact on the part to reduce clamping distortion.

                    If you are boring a tube using the lathe bore the jaws to the same size as the tube and then bore the tube, it should be noted that any distortion in the roundness of the tubes OD will be passed to the ID of the tube.

                    If you are boring a block, such as an engine block, clamp from the top and put the clamping forces parallel with the bore, by clamping the part from the sides you are putting the clamping forces perpendicular to the part and automatically distorting the part.

                    Also, are you measuring the part as cut in the machine or removed and in the free state? That will also make a difference. Considering you really only care about the part in the free state.

                    Comment


                    • #11
                      What sort orf mill operation you use for boring? Do you lift the table to the cutter or feed with the quill? If the latter, I'm not suprised it shows up as bigger diameter in the bottom as the rigidity of the cutter diminishes.
                      Amount of experience is in direct proportion to the value of broken equipment.

                      Comment


                      • #12
                        Steve,
                        For the HSM types where our equipment is pretty limited and if your cylinder is small enough, Fixturing it to the lathes cross slide at the correct elevation and then using a between centers boring bar would be the best way to go. One of my prioritys when I was shopping for a new lathe was a cross slide with tee slots in it. How your lathe is built and your own ingenuity would dictate if you can do it this way. But you would get round and true cylinder bores.

                        Pete

                        Comment


                        • #13
                          Originally posted by uncle pete
                          Steve,
                          For the HSM types where our equipment is pretty limited and if your cylinder is small enough, Fixturing it to the lathes cross slide at the correct elevation and then using a between centers boring bar would be the best way to go. One of my prioritys when I was shopping for a new lathe was a cross slide with tee slots in it. How your lathe is built and your own ingenuity would dictate if you can do it this way. But you would get round and true cylinder bores.

                          Pete
                          You still have all the clamping issues as before and more. A picture of the part might net him some real suggestions on how to hold it. This sounds like a simple matter but fixturing is paramount when trying for cylindricity. He needs a way to clamp it axially, preferably exactly like it will be mounted in use.

                          Comment


                          • #14
                            Td,
                            Yeah your right about the fixturing, But since that had been already mentioned I didn't think there was much more I could add. Your also right about the need for a picture.

                            Pete

                            Comment


                            • #15
                              There's no reason that he can't get a kickass job with the equipment he's got. But not all things can be done in a vise or a chuck, especially if it's a 3 jaw. Probably no access to a real hone and even then you have to learn to use one. If he saves the bores for last, fixtures it to take into account the stresses in service, and cuts them in 2 passes, he should have a hole that a brake cylinder hone or such can finish up nicely.

                              Comment

                              Working...
                              X