Announcement

Collapse
No announcement yet.

Cutting gear rumors

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

  • Cutting gear rumors

    I am in the midst of cutting several spur gears. Because of the purpose I need them to be done "by the book". The book being Machinery's Handbook or similiar. In my career there have been many discussions of making spur gears. Some say that you must cut them in a single pass, giving no reason besides "thats how I was taught". Others state that you must cut them by climb milling also giiving the same reason or stating "thats how I always do it".

    I would like any thoughts or facts that either substantiate or debunk those ideas. If you have other ideas to share that would be welcome also.

    Thanks in advance

    Pete

  • #2
    My thought is to get it done however you can to required specifications without destroying your tools.
    John M...your (un)usual basement dweller

    Comment


    • #3
      My self I will do two to three pass. If you are making a lot of gears it is faster to make one pass.
      I never climb milling, I just debur the gear. Climb milling is good for only new mills, as the mill gets old the screw wear in the center not end.

      Here is list for making 1 to 3 gears the same.
      1. do at less three pass note: lass pass cut .005"
      2. DO NOT Climb mill

      Dave
      Last edited by Gunsmithing; 12-10-2012, 11:30 AM.

      Comment


      • #4
        I share your frustration.....be wary of people who's main reasons are how long they've been doing something or it was how i was taught. If they can't justify what they're saying or haven't learned the physical why & how, you have to be suspect of the credibility.

        Advise like climb milling is usually because its expected to give a better finish but unless the machine was made for it or it is a very light cut, is a dangerous proposition. I would avoid it. So what gives a good finish? sharp cutters, a light finish cut and flood coolant/oil. That and a material that machines well.

        Do it one pass has merit from a productivity standpoint, but depending on the setup a finish cut is preferred; ie spring in the system. Other than more time/wear on the cutter, I don't know why a finish cut wouldn't be recommended from a finish/accuracy standpoint.
        .

        Comment


        • #5
          First off, let me join the chorus in saying that I cant imagine any circumstances to using climb cutting - it just dont make sense.

          Next, are you gonna use a hand ground single point cutter? If so then multiple passes are probably gonna be necessary.

          My method has evolved into - yes, its 'just the way I do it' but it works well so here it is.

          I have DRO on my mill, I have power feed on the table, and I go ahead and spring for the 50 or so dollars for a dedicated gear cutter. I determine DOC - (depth of cut) and set the blank up to meet the cutter at that depth, I get every thing locked down except the axis Im using to cut (this is critical to maintain the same depth of cut on multiple passes), I set the mill in back gear at about 150-200rpm and the PF at a slow speed, (determined by ear and how large/deep Im cutting) and start the feed. I then make one pass and on the return climb cut I listen for the cutter only making a slight ticking sound indicating Ive made a clean 'to depth' cut.
          If everything seems to be going well, you have obviously overlooked something........

          Comment


          • #6
            Originally posted by Bill Pace View Post
            First off, let me join the chorus in saying that I cant imagine any circumstances to using climb cutting - it just dont make sense.
            Rigid machine/setup. Climb milling saves your cutter and thus makes it live longer AND the surface finish is just much more better.

            People tend to advice against climb milling just because they always think the maker has only a clapped out crappy mill but don't even bother to ask. Many manual machines have ballscrews and there can always be the unusual CNC user (especially when asking if you can cut something with multiple passes).
            Amount of experience is in direct proportion to the value of broken equipment.

            Comment


            • #7
              Without doubt as in all machining you really need to rough and then finish cut to get the best results, obviously a sharp cutter and rigid set up are also necessary. I didn't know many manual mills had ballscrews but I stand to be corrected! Climb milling will give you a superior finish but if your mill has normal Acme screws don't take a full depth climb mill cut.
              Tony

              Comment


              • #8
                My manual universal mill has ball screws on all three axis as well as power feed on all three axis. I try to climb mill every chance I get as it seems to save my carbide tools. I am a novice but it seems to be working for me. I see a noticeable difference in finish when I climb mill.
                How to become a millionaire: Start out with 10 million and take up machining as a hobby!

                Comment


                • #9
                  You don't say what size tooth/gear, what size machine or material.

                  If they are large tooth sizes, it may speed the overall process considerably if you gash the teeth (gullets) first with a stagger tooth cutter and then come back and finish with the appropriate form cutter.

                  An involute gear tooth milling cutter has about the worst chip flow characteristics that can be imagined, especially when cutting from solid. This is in contrast to the stagger tooth cutter which can easily operate at depths of cut and feed rates that would quickly destroy an involute cutter. This is accentuated when working in steel, not so much in the short chipping materials.

                  Dave

                  Comment


                  • #10
                    Well every one has had their say .So here is mine. If you have a big horizontal mill B&S ,Cincinnati are what ever you can climb mill . If you in a Bridgeport are small mill I would not .As far as depth of cut . I cut 32 pitch gears in one pass they only about .078 deep if I was cutting a 14 DP gear may be 1 pass if soft material something less than 4140 PH. A big gear 6 DP are larger 2-3 passes depending on what Dp. so go from their. Listen to the machine and just watch the cut . Don`t push it just pay attention to what the machine and the set up is telling you . If you need ear plugs something is not right.
                    Every Mans Work Is A Portrait of Him Self
                    http://sites.google.com/site/machinistsite/TWO-BUDDIES
                    http://s178.photobucket.com/user/lan...?sort=3&page=1

                    Comment


                    • #11
                      Textbook Approach

                      Always try to cut to the correct depth with one cut; nibbling away with a succession of small cuts is not recommended. Commercial gear cutters are expensive items and naturally the amateur wants them to last as long as possible between re-grinds. It is a fallacy to think that you are being kind to the cutters by making numerous light passes. Set the cutter to the correct depth and regulate the feed to suit the machine, naturally a heavy robust machine will be capable of a faster feed rate than a small lighter one. When cutting large teeth such as those found on traction engine models, the equipment available may not be man enough to produce the tooth at one pass in which case it may be an advantage to 'gash' the teeth first with either a slitting saw or a side-and-face cutter. This will remove the bulk of the material and lighten the load on the machine when the form cutter is used. Gears and Gear Cutting, Ivan Law. pp. 66-67

                      If the gear teeth are of fairly coarse pitch, it may be desirable to take roughing and finishing cuts. This is often done in cutting gears coarser than 6 or 7 diametral pitch, although a definite dividing line cannot be drawn owing to variations both in regard to the cutting capacity of the machine itself and the cutting qualities of the stock. When roughing cuts are considered desirable, special stocking cutters are often used for the roughing operations, as they are more efficient for removing stock rapidly than the regular formed cutters. When a second cut is taken for finishing, it is important to have the roughed-out tooth spaces central with the cutter to avoid removing unequal amounts of metal on the sides, since this tends to wear the cutting edges unevenly and produce inaccurate teeth. If roughing cuts are taken, the "stocking" cutter should be set to mill the teeth the full depth, the allowance for finishing being on the sides. Machine Shop Training Course Vol. 2, Franklin D. Jones. pp.226-227

                      Depth of Cut. On most work no more than two cuts are required---a roughing cut and a finishing cut. If it happens that two or more cuts are necessary, the rule is to take, for the roughing cuts, a coarse feed and about all the depth of cut the machine, cutter, and work will stand...
                      Finishing Cut. Remember that attention to the slogan "keep cutters sharp" is one of the main factors in good milling; bear in mind that a surface that has been milled with a good sharp cutter is as accurate as a filed and polished surface. Also it is easier and quicker, and therefore cheaper, to mill to size than to finish by filing and polishing.
                      When it is advisable to make two cuts, a roughing cut and a finishing cut, leave at least 1/64 in. for the finishing cut. In any machine a cutting tool will do better work and last longer if the edge has a chance to get under the chip, where it has less tendency to rub.
                      There is always spring in every milling operation. If the feed is stopped while the cutter revolves on the work, the surface will be defaced by an undercut. Do not throw out the feed on a finishing cut.
                      For the same reason as above, if a cut just made is run back under a revolving cutter, the work will be marked each revolution of the cutter. Stop the cutter before running back or else lower the work a trifle. Machine Tool Operation Part II, Burghardt and Axelrod. pp.210-211

                      It is always tempting to reduce the feed rate if the cutter exhibits distress, but though a slight reduction does no harm this is, in general, a mistake. The depth of cut should be reduced and the feed rate maintained... Very slow feed rates cause the tooth to rub at the beginning of the cut, and this causes poor finish... DEPTHS OF CUT. The rule here is simple: the depth of cut should be as large as the available power will permit up to the limit prescribed for the type of cutter... it will be realised that the thickness of the chip is unaffected by the depth "D" -- it depends only on the feed rate. A full depth cut produces a long, but thin, chip.
                      ...To sum up. The cutting speed is the main factor determining tool life. The figures suggested above are not critical, but when in doubt, use a lower speed. Feed rate is goverened by the tooth load. Too high a tooth load will result in poor finish and may cause "interference" on the primary clearance. Too low a feed rate will cause rubbing, especially if the cutter is a bit worn. Again, the rates derived from Fig. 43 are not critical. The depth and width of cut which can be used depends more on the rigidity of the machine and the power available than on anything else, and should be as high as can be managed with comfort. Very light cuts should be avoided, especially if the cutter is not dead sharp. Milling Operations in the Lathe, Tubal Cain. pp.27-28

                      Remember to bear the above quote in mind when reading the following comment later in the same book---especially his use of the term "moderate cut." It is obviously reflective of a set-up lacking rigidity when cutting gears on a small (3-1/2" English designation) lathe. A compromise between depth of cut and chatter must be realized while maintaining sufficient feed for the best result.

                      Even small wheels in brass will benefit from a finishing cut, and any wheel of any size should be given a series of moderate successive cuts. The setup is inherently "whippy" and there is always risk of chatter if too much is taken off at one cut. Once chatter develops it may be very difficult to get rid of it. Cain. pg.104

                      The size of the cut is made up of the feed per revolution (or per tooth on milling work) and the depth of cut... The amount of feed largely determines the point of initial chip contact and the unit pressure against each unit length of cutting edge. The depth of cut does not change the unit edge pressure but only varies the total pressure against the tool which in turn controls the amount of shank deflection. Design and Use of Cutting Tools, Leo St.Clair. pg.249

                      Analysis of Cutting-feed Conditions. First, it will be understood that in any operation of cutting metal a considerable force is exerted against the piece being cut and equally against the cutter itself; and that the amount of metal removed (feed and depth of cut) is in proportion to this force. Therefore, the proper depth of the cut and the proper amount of feed depend to a certain extent upon each other and, in addition, both depend on the power and rigidity of the machine itself.
                      Second, the correct depth of cut and feed depend on the strength of the cutter and the rigidity with which it is held, and the strength of the work and the manner in which it is held. For example, a slender end mill or a thin slitting cutter cannot be given heavy duty; neither should a frail piece of work or a piece held in such a manner that it may spring or bend be given a heavy cut or feed.
                      Third, the teeth of the coarse-tooth cutter are proportionately stronger than the finer teeth, the chips wash out more readily, and the cutting fluid keeps the cutting edge cooler. For these reasons a heavier chip may be taken with a coarse-tooth cutter.
                      Fourth, while the coarse feed removes metal faster, the appearance and accuracy of the surface are not as good as is desirable for finished work; therefore, a finer feed is used for finishing...
                      The general tendency is to overspeed and underfeed a milling cutter. The reason for most of the too quickly dulled cutters is too much speed, and rarely if ever too much feed. It will be well for the beginner to go fairly slowly at the start and avoid spoiling the cutter, the work, or possibly both, but to keep right on the job with the idea of advancing the speed or the feed as much as possible with due regard to the time it takes to sharpen the cutter. Machine Tool Operation Part II, Burghardt and Axelrod. pp.209-210
                      Last edited by Arthur.Marks; 12-10-2012, 10:12 PM.

                      Comment


                      • #12
                        Once you are "in" the cut, milling involves a gradual transition from "zero chip depth" to maximum, so I don't know that feed adjustment is any worse than setting depth of cut..... The less the depth of cut, the longer the shallow portion of the cut as a percentage of the total cutting distance, very much the same effect as for a slower feed.

                        Since they both have similar effects, I prefer to adjust feed and have a deeper depth of cut. That tends to have more "teeth in the cut" at once, making the load more even.

                        Originally posted by Jaakko Fagerlund View Post
                        Rigid machine/setup. Climb milling saves your cutter and thus makes it live longer AND the surface finish is just much more better.

                        People tend to advice against climb milling just because they always think the maker has only a clapped out crappy mill but don't even bother to ask. Many manual machines have ballscrews and there can always be the unusual CNC user (especially when asking if you can cut something with multiple passes).
                        Not just about rigidity...... the real reason for NOT climb milling is if the machine has any slop at all in the feed.

                        Climb milling is "self feeding", in the sense that the cut is taken in the direction to make the cutter "draw the work in", so there must not be any slop in the feed that allows the table to pull towards the cutter. If it CAN, it WILL, and the "draw-in" will cause an uncontrolled increase in the chipload per tooth.

                        Ballscrews are about the only feed that won't do that, other than an adjustable double nut on the feed which can be tightened so as to have no slop. But wear on the screw can cause the double nut to lock up when the nut reaches a less-worn part. The screw must be 100% in control of the table movement.. ANY slop will result in the work being repeatedly "drawn in" by the amount of the slop.

                        Chances are that is enough to break something, or cause the cutter to "walk over" the work, maybe bending the arbor. If the machine is not rigid, it may "give" enough not to bend anything.

                        If the machine is non-rigid enough, I suppose it could have the same effect as slop, but most such machines will probably have a slop problem that is worse than the rigidity problem.

                        if your machine CAN take it, climb milling gives a very nice finish, though.

                        Sometimes, if you can set for a light depth of cut, and put drag on the table with the axis lock, you can make the feed friction more than the "pull-in" force, and then you can get away with it. You then have to "push" the table with the feedscrew. I think that is best left for rare instances of real necessity.... it involves a good deal of force on the feedscrew, and extra wear on the machine in general.
                        Last edited by J Tiers; 12-11-2012, 12:04 AM.
                        1601

                        Keep eye on ball.
                        Hashim Khan

                        Comment


                        • #13
                          Originally posted by Stepside View Post
                          I am in the midst of cutting several spur gears. Because of the purpose I need them to be done "by the book". The book being Machinery's Handbook or similiar. In my career there have been many discussions of making spur gears. Some say that you must cut them in a single pass, giving no reason besides "thats how I was taught". Others state that you must cut them by climb milling also giiving the same reason or stating "thats how I always do it".

                          I would like any thoughts or facts that either substantiate or debunk those ideas. If you have other ideas to share that would be welcome also.

                          Thanks in advance

                          Pete
                          The gear outside diameter (OD) is not important within reason - most who consider it imporatant only do so to "scratch" (ie "witness") to set depth of cut to zero.

                          The Pitch Diameter is not too important either as it can be varied to suit the gear tooth width and "back-lash" ie "Clearance" which is set by increasing or (decreasing) the depth of cut to get the correct gear tooth width.

                          Gear tooth width/thichness can be measured with common shop vernier ir digital calipers. Gear calipers are not needed.

                          http://i200.photobucket.com/albums/a...r-measure1.jpg

                          The centre/axis of the gear cutter and the centre axis of the job must be in the same vertical plane (assuming a horizontal mill is used). Rotate into the horizontal plane when using a vertical spindle/arbor.

                          Common tables while in accordance with "Machinery's Hand Book" are nominal only and if used would result in gears with no clearance.

                          http://i200.photobucket.com/albums/a...k/BB_50-51.jpg

                          http://i200.photobucket.com/albums/a...book/BB_52.jpg

                          I will enlarge on this later if I have time and if it is necessary.
                          Last edited by oldtiffie; 12-11-2012, 02:11 AM.

                          Comment


                          • #14
                            Originally posted by J Tiers View Post
                            Not just about rigidity...... the real reason for NOT climb milling is if the machine has any slop at all in the feed.
                            That's what I said.
                            Amount of experience is in direct proportion to the value of broken equipment.

                            Comment


                            • #15
                              Not quite.

                              I was taught in at least one shop (many years ago) that climb milling is OK- if the cut it light - to "brake" the lead-screw hand-wheel with your (right) hand (light cuts only) which takes a bit of skill to aquire it - but it can work very well.

                              I use it on the lathe the "scrape" the trailing/rear thread face when screw-cutting - that works well too - but learn that skill first before you try it on something you might wish you hadn't if you get it wrong.

                              Comment

                              Working...
                              X