How to: presize bushing with tiny inner hole concentric with OD
Close
Login to Your Account
Results 1 to 11 of 11
  1. #1
    Join Date
    Sep 2018
    Country
    RUSSIAN FEDERATION
    Posts
    24
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default How to: presize bushing with tiny inner hole concentric with OD

    Hi,

    I need some steel bushings that should have 11mm lenght, 6mm OD, 1mm ID, OD and ID centers can missmatch not more than 0.03mm.
    Which way I will get most close results?
    Using lathe and turning from rod in one setup looks most easy way, but:
    - tailstock center height is never aligned with spindle center
    - even if drill will find center on the face surface, just wonder how far from center it will exit at the back surface.
    I can also use manual mill to make hole (after OD is done with lathe). Indicating center with OD will be easy, can use smaller drill first and proper size mill to finish hole. But:
    - 1mm mills is probably more rigid than 1mm drill, but anyway it will have reasonable deflection with 11mm length.
    So, if making small hole concentric to the OD is so hard, maybe I need to reverse operations?
    Drill smaller hole, finish it with reamer, and then use tool grinder with 1mm arbor to finish OD? Does this looks realistic?

    Thanks.

  2. #2
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    18,723
    Post Thanks / Like
    Likes (Given)
    14244
    Likes (Received)
    14267

    Default

    IMO you need a better lathe of the right size for the job.

  3. #3
    Join Date
    Jun 2012
    Location
    Chicago, USA
    Posts
    1,299
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    103

    Default

    Chuck the rod in your lathe. Drill and ream the ID to finished size. Remove from the chuck. Place another piece of stock between centres and turn a mandrel to a light press fit, or a sliding fit with super glue. Then put your bushing on the mandrel and turn the ID concentric.

    Hope this helps,

    Lee

    Sent from my SM-N960U using Tapatalk

  4. #4
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    10,222
    Post Thanks / Like
    Likes (Given)
    1392
    Likes (Received)
    3674

    Default

    I'd sooner attempt the job on the mill, where at least I've got proven tooling with minimal runout, compared to a lathe tailstock's unknown reliability of position. Also have the rpms available on the mill which are quite beyond most lathes.

    Make one first and test it's concentricity. Then worry about improving it. My go to method for accurate holes is to drill first maybe .75mm in this case, then interpolate the top of the hole to 1mm to act as a guide for the reamer. Then ream it and test it.

    I guess you could grind it on a mandrel, but that sounds like a PITA to do, so I'd try anything else first.

  5. #5
    Join Date
    Jun 2012
    Location
    Chicago, USA
    Posts
    1,299
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    103

    Default

    I'm missing something here. OP needs to make an 11mm long bushing with concentric bore that deviates not more than 0.001" end to end. That's not especially close tolerance - why does it need to be ground, and why can't he use the lathe he already has? I don't think he said anything about the lathe's condition, but even a very worn lathe should be able to pull that off with some care?

    Sent from my SM-N960U using Tapatalk

  6. Likes sfriedberg liked this post
  7. #6
    Join Date
    Sep 2018
    Country
    RUSSIAN FEDERATION
    Posts
    24
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Im not familiar with watchmakers technologies, when I take 0.7mm drill it seems to deflect after each breath.
    Even if there are some ways to setup tailstock (or chuck in toolholder) with this tolerance to the spindle center, I have no ideas how drill will deflect during drilling and how far away from this perfect center it will get out.
    I dont see how smaller or more precise lathe can help. Unless you have nano boring bar that is able to bore 1mm hole.
    Turning OD hold on 1mm mandrel looks crazy for me. Even if part wont fly away, mandrel will bent and bushing will have cone shape after turning.
    So, I suppose that making ID before OD can be more easy (Im not able to bore 1mm with boring bar or boring head), but OD should be finished with lower force operation (grinding).
    So, if I have roughed OD and have made 1mm hole (with any technic), I need to use this hole as reference. Mandrel with some threadlocker/glue is one option. 60 degree chamfer (for dead center) is another option. (I can leave extra length and face this chamfers after OD is done). Which way is preferable?

  8. #7
    Join Date
    Jun 2012
    Location
    Tennessee USA
    Posts
    685
    Post Thanks / Like
    Likes (Given)
    331
    Likes (Received)
    397

    Default

    My first question would be what method/tools you're using to locate the ID hole before using a drill/end mill. If the lathe tailstock is out of alignment with the headstock then the hole will have to be put in with the mill. You will have to finish the OD on a machine that you feel will hold concentricity and that sounds like your grinder. Rough in the OD on the lathe, leaving .13mm on the OD and maybe 1.5mm on the overall length. A larger hole, for grinding arbor, can be put in on one side (4.5mm?). Put the bushing in the mill and drop the hole in. Starting the hole is critical for location, I've used a spotting drill and then an end mill depth at least 2X the cutter OD so the hole is sized/located and acts as a guide for the full sized drill. All cutting tools must be indicated for run-out in the mill spindle too. If the grinder has a tailstock for a center (dead or live) then perhaps a small chamfer can be put in on the other side to help locate/support the bushing while grinding. When the OD is ground to size and is concentric to the ID you simply toss the bushing back in the lathe and face off the extra length. Yes it's some wasted material and extra steps to go through but the conditions of your available machines and the tolerance you seek often dictate the methods used. You may have to adjust the roughing OD to leave enough material on there for the grinder to clean up. A test piece will show what needs to be done. Hope this helps.

  9. #8
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    18,723
    Post Thanks / Like
    Likes (Given)
    14244
    Likes (Received)
    14267

    Default

    Quote Originally Posted by leeko View Post
    Chuck the rod in your lathe. Drill and ream the ID to finished size. Remove from the chuck. Place another piece of stock between centres and turn a mandrel to a light press fit, or a sliding fit with super glue. Then put your bushing on the mandrel and turn the ID concentric.

    Hope this helps,

    Lee

    Sent from my SM-N960U using Tapatalk
    On a 1 mm (0.040'') diameter UNSUPPORTED mandrel / peg?

  10. #9
    Join Date
    Jun 2012
    Location
    Chicago, USA
    Posts
    1,299
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    103

    Default

    Quote Originally Posted by Limy Sami View Post
    On a 1 mm (0.040'') diameter UNSUPPORTED mandrel / peg?
    Yes, I realized after I posted that the mandrel would be tiny.

    Could the piece be turned in the chuck, and the bore created with an center cutting endmill held in the toolpost?

    Sent from my SM-N960U using Tapatalk

  11. #10
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    18,723
    Post Thanks / Like
    Likes (Given)
    14244
    Likes (Received)
    14267

    Default

    Quote Originally Posted by leeko View Post
    Yes, I realized after I posted that the mandrel would be tiny.

    Could the piece be turned in the chuck, and the bore created with an center cutting endmill held in the toolpost?

    Sent from my SM-N960U using Tapatalk
    1mm dia @ 11 x d long? ………...I'm not saying it can't be done, but I wouldn't like to try it.

  12. #11
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9,961
    Post Thanks / Like
    Likes (Given)
    3358
    Likes (Received)
    3571

    Default

    I have found that on a lathe to face and then tool bit nick the bore/hole location makes the best hold to center. Tail location and even poor drill point locating can mess up a spot-on center need. The tool bit nick will run true to the spindle, even with holding part in a poor chuck. ..the a part-off will make the other end good.

    Facing,OD,Id and parting-off in one chucking make everything run true.

    Carbide reamer might make /finish the bore..
    https://drillsandcutters.com/1-00mm-...111ab94f877d46

    Q: [ and then use tool grinder with 1mm arbor to finish OD? Does this looks realistic?}
    A very short arbor so less wheel pressure deflection.
    I have set such parts between centers to skim OD for .001 and less run out with just using the part bore... with using a point center lap to make a small center in the part.
    A AO Center Lap Mounted Point | Norton Abrasives


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •