Turning small long shafts on big lathe?

Discussion in 'General Engine Discussion' started by jtrout13, Jun 29, 2011.

Help Support HMEM by donating using the link above.
  1. Jun 29, 2011 #1

    jtrout13

    jtrout13

    jtrout13

    Well-Known Member

    Joined:
    Mar 3, 2010
    Messages:
    93
    Likes Received:
    9
    I recently built Elmer's Fancy engine and while it performed well, I was unhappy with the piston. I am having trouble turning the connecting rod for this piston (it is a 0.25 inch OD rod, with a section turned down to 0.125 inch diameter, 1.25 inches long).

    My lathe is large Romi 13-10. I keep having trouble with one end of the turned-down section being a larger diameter than the other end, and I can't seem to get a constant OD all the way down the turned section. I have tried doing it between centers (difficult) and also tried turning it in small steps of length (only neck down about 0.25 inch at a time) to reduce the cutting force deflecting my workpiece. However, I am still having no luck. (have tried using both HSS and indexable tooling).

    Would anyone be so kind as to provide some advice?
     
  2. Jun 29, 2011 #2

    steamer

    steamer

    steamer

    Well-Known Member

    Joined:
    Nov 30, 2007
    Messages:
    5,406
    Likes Received:
    26
    What is occuring? Taper?, chatter?

    Have you leveled your lathe?

    Dave
     
  3. Jun 29, 2011 #3

    Rayanth

    Rayanth

    Rayanth

    Well-Known Member

    Joined:
    Jun 7, 2011
    Messages:
    338
    Likes Received:
    7
    Also, what's the material? Aluminum, steel?

    Have you tried taking more, shallower cuts and gradually approaching the target diameter? I have heard on steel that swelling from heat can cause this issue.

    - Ryan
     
  4. Jun 29, 2011 #4

    jtrout13

    jtrout13

    jtrout13

    Well-Known Member

    Joined:
    Mar 3, 2010
    Messages:
    93
    Likes Received:
    9
    Sorry for the poor description. I am using drill rod O-1, and the problem I am having is taper. Chatter isn't a problem, and surface finish is great, but I'm getting the taper and having problems zeroing in on the final dimension.

    Also, it's tough to take small cuts on this lathe due to deflection of the workpiece (the tool just bends the shaft instead of cutting into it), so I am doing a minimum of 0.030in depth of cut (0.060 reduction in diameter).

    I have always had great accuracy and never had taper occur with this lathe, but I usually don't turn any diameters smaller than 1/4 inch. This is the first part I've had this problem on, so I'm totally confused.
     
  5. Jun 29, 2011 #5

    websterz

    websterz

    websterz

    Well-Known Member

    Joined:
    Mar 3, 2009
    Messages:
    344
    Likes Received:
    6
  6. Jun 29, 2011 #6

    Rayanth

    Rayanth

    Rayanth

    Well-Known Member

    Joined:
    Jun 7, 2011
    Messages:
    338
    Likes Received:
    7
    A follower rest is a good idea, but I would still look into the possibility of heat expansion. It's possible you're still cutting true, but as the stock heats it expands, so you're cutting deeper relative to the stock. When it cools and shrinks it shows as a taper. Smaller stock has less mass to soak up the heat and less surface area to shed it, so it gets hotter, quicker.

    The follower rest will prevent deflection, allowing you to make lighter cuts, which will both cause less friction so less heat, and give the stock time to cool between cuts.

    Of course, your mileage may vary, and i'm approaching it all from the theory angle .... I could be way off base ;D

    - Ryan

     
  7. Jun 29, 2011 #7

    bentprop

    bentprop

    bentprop

    Well-Known Member

    Joined:
    Mar 1, 2008
    Messages:
    503
    Likes Received:
    3
    I believe what you need is a box tool.This feeds the rod to be cut through a sized bush with a cutter being placed after the bush.This allows thin rod to be reduced in size without bending the rod.Of course,you need a bush for every size rod.F.i.,if you want to cut a 1/4" rod to 3/16",you will need a 1/4",and possibly a 11/16" bush.
    There have been various designs mentioned on forum boards,but goshdurnit,I can't find a single one at the moment :(.
    I seem to remember Tel had a nice simple one you could copy.
     
  8. Jun 29, 2011 #8

    prof65

    prof65

    prof65

    Well-Known Member

    Joined:
    Nov 14, 2008
    Messages:
    82
    Likes Received:
    7
    I think this is the tool bentprop is talking about.

    smalldial.jpg
     
  9. Jun 29, 2011 #9

    tel

    tel

    tel

    Well-Known Member

    Joined:
    Feb 8, 2008
    Messages:
    3,303
    Likes Received:
    40
    Indeed I dew!

    [​IMG]

    [​IMG]

    [​IMG]
     
  10. Jun 29, 2011 #10

    GRAYHIL

    GRAYHIL

    GRAYHIL

    Well-Known Member

    Joined:
    Jul 22, 2010
    Messages:
    62
    Likes Received:
    5
    Hi All
    .030" is not a small finishing cut! when not supported especially with HSS.
    You may need to try several "spring cuts" to try and stop deflection.
    Other than that all the metods described are worth a try.
    Graham
     
  11. Jun 29, 2011 #11

    steamer

    steamer

    steamer

    Well-Known Member

    Joined:
    Nov 30, 2007
    Messages:
    5,406
    Likes Received:
    26
    Grayhill beat me to it

    .03 on a .125 shaft is FAR from a finishing cut...Suggest the following

    the last three passes should be no more than .005" DOC preferably less! like .001"

    Let the last pass be a spring pass. No additional feed

    Slow your feed down to like around .002"/rev

    Make sure you speed is up where it's supposed to be. ( I would bet about 1500 rpm for 0-1)

    Make sure your tool has about a .005" radius on it..and NO more, and stone it. You want the radius of this to be bigger than your feed rate...twice the size is about right. Any bigger causes more tool area in contact with the cut and creates higher radial cutting forces....that causes springing.

    Make sure the tool is on center.

    The good quality HSS tool has the right rake and clearance angles on it ...right? NO NEGATIVE RAKE TOOLS!
    I think 8 degrees all around would work fine here. Splurg for the Cobalt or M42


    Leave carbide in the draw. It has no place here. Especially negative rake tools as the radial cutting force is much higher than positive rake tools. This will tend to spring the work, and that will cause taper

    Actually violating any of the above will cause taper!

    Use some cutting fluid

    Ideally back up the shaft with the tailstock center or a follower rest.

    or

    with a box tool as described by Tel. Those work nice, but it can be hard to get to a shoulder with it sometimes.

    Try that and report back.

    Dave
     
  12. Jun 29, 2011 #12

    jtrout13

    jtrout13

    jtrout13

    Well-Known Member

    Joined:
    Mar 3, 2010
    Messages:
    93
    Likes Received:
    9
    I really like the box tool you guys are suggesting. I will give that a try, and will experiment with smaller cuts I suppose. Thanks for the replies!
     
  13. Jun 30, 2011 #13

    MachineTom

    MachineTom

    MachineTom

    Senior Member

    Joined:
    Oct 20, 2010
    Messages:
    851
    Likes Received:
    114
    I have just finished 2 shafts similar to yours. As already stated you need to sneak up on that final size with small cut the last .015" or so. The piece shown was 5/16 O-1 material, distance from chuck to tailstock center was 4.25" final D was aimed at .155 with taper its .1545- .1555 that more than good for the application, swing arm for a flyball governor. The tailstock end was done first, a distance of 2.6", final cuts were cut forward and backward, not feed advance on the return cuts. The cutter was a TNMG 322 in a 15/45 tool holder, rpm 1200, feed .0015 per rev, doc .002.
    the diameter closest to the chuck was then done.

    [​IMG]

    A bit closer

    [​IMG]


    This is a box turning tool, the wheels adjust as well as the tool bit. I did not use this tool to make the shaft.

    [​IMG]

    and a bit more detail

    [​IMG]

     
  14. Jun 30, 2011 #14

    jtrout13

    jtrout13

    jtrout13

    Well-Known Member

    Joined:
    Mar 3, 2010
    Messages:
    93
    Likes Received:
    9
    MachineTom, so did you turn that piece between centers?
     
  15. Jun 30, 2011 #15

    steamer

    steamer

    steamer

    Well-Known Member

    Joined:
    Nov 30, 2007
    Messages:
    5,406
    Likes Received:
    26
    Oh and 1 2 more rules of thumb

    Anything more than 5X the diameter sticking out of the chuck? Bring up the tailstock and support it or use a fixed steady. That's just good practice.

    A polished tool will cut a polished surface....if you leave it ragged from the grinder, you won't get good finish on the part. Get a small slip stone and polish the surface.


    Dave
     
  16. Jun 30, 2011 #16

    MachineTom

    MachineTom

    MachineTom

    Senior Member

    Joined:
    Oct 20, 2010
    Messages:
    851
    Likes Received:
    114
    Yes, the part was between centers. The light final cuts are what is needed to reduce the taper. The large end on the right has not been cut off in the photo's, that was for the center. The spring cut on return of the carriage is also important in reducing taper.
     
  17. Nov 26, 2014 #17

    doug9694

    doug9694

    doug9694

    New Member

    Joined:
    Nov 26, 2014
    Messages:
    2
    Likes Received:
    0
    I have used a sharp file and emery cloth on tapers.
     

Share This Page