Boring of a long, small tapered hole - Page 3
Close
Login to Your Account
Page 3 of 4 FirstFirst 1234 LastLast
Results 41 to 60 of 64
  1. #41
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    Quote Originally Posted by Bendak View Post
    That just so happens to be the first bar I tried machining it with, although I broke it on accident (hit the part during a rapid). The bar lost it's tip initially which I think may be due to too fast a surface speed (300SFM instead of perhaps something like 80SFM).
    Nope not Speed. Chips, Feed or depth of cut. 300 is not fast for a solid carbide bar. Solid carbide bars have very little room for error, so I always start with light feed and DOC, and watch for chips.

    R

  2. #42
    Join Date
    Mar 2011
    Country
    SWITZERLAND
    Posts
    950
    Post Thanks / Like
    Likes (Given)
    117
    Likes (Received)
    382

    Default

    Make a solid counterpart and warm form the tube onto that. A strong press is needed that has a thrower or HDD.

  3. Likes Ox liked this post
  4. #43
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9,481
    Post Thanks / Like
    Likes (Given)
    3234
    Likes (Received)
    3397

    Default

    Might you use a taper pin reamer with grinding away the section not needed to go from perhaps .230 to .205 (or what needed).
    Might a 5mm taper pin reamer work. .250 big end .193 small end.
    Straight Flute - - 5mm HSS Taper Pin Reamer

    Drill .205 through / .250 part way..perhaps .230 most of left .. and leave about 1/16,1/8 or 1/4 " for the taper pin reamer to finish the last 1/or the ID.

    *Wait with the big end .259 you need not grind the flutes away...might wrap some tape around to make the big end better fit the drill bore.

    The wood sample wont know or care there is not two ID tapers.

  5. #44
    Join Date
    Aug 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    1,269
    Post Thanks / Like
    Likes (Given)
    904
    Likes (Received)
    531

    Default

    I am surprised nobody asked how many of these you will be making. That does have an impact on how you select tooling. If you are making several it would be worthwhile to have a custom reamer ground. Using it will be more like reaming the chamber of a gun than straight reaming. Go slow. Use lots of cutting oil. I would prefer to do the reaming on a manual lathe where I could have a better feel for how the reamer is cutting.

    The D-bit suggestion has a lot of merit. It can be ground out of a drill blank. I would suggest two D-bits, one for each taper, to keep the length of cutting edge as short as possible. MSC sells half round drills. You could grind the taper onto one of them.

  6. #45
    Join Date
    Aug 2017
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    51
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    7

    Default

    Here's an image of a cross section I found on the internet:
    cross-section.jpg
    I'll consider making it as a single taper since the extractor spoon is flexible enough to modify enough to fit in a slightly undersized hole.
    From the image it seems that there are two separate straight holes drilled, the transition between the two likely formed by the chamfered end of the larger drill bit. It is then followed by a taper and terminated by a small straight section at the far left end. I was told that it is machined as one part, so I'm assuming that they drill out the pipe, first two straight sections, and final straight with different sized gun-drills, they taper probably back bored from the small end.
    If I end up helically milling or boring the hole, then I see no reason to change the geometry of what I already have. If things go sideways then I could always simplify the geometry of the hole and then use a ground reamer after step drilling many times.
    I plan on making at five or even ten of these, perhaps more in the future.

  7. Likes Ox liked this post
  8. #46
    Join Date
    Aug 2017
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    51
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    7

    Default

    Quote Originally Posted by litlerob1 View Post
    Nope not Speed. Chips, Feed or depth of cut. 300 is not fast for a solid carbide bar. Solid carbide bars have very little room for error, so I always start with light feed and DOC, and watch for chips.

    R
    Attached are some photos of the boring bars after running them at various feeds and speeds. I can't seem to run the bar without damaging it in some way. It may require some manual machining to determine the best feeds and speeds for such an operation. After than I could bring it back to CNC.
    Attached Thumbnails Attached Thumbnails heavy-damage-side-.jpg   heavy-damage-top-.jpg   slight-damage-side-.jpg   slight-damage-top-.jpg   undamaged-side-.jpg  


  9. #47
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    Like I said, it isn't Spindle Speed that hurting you. In the 4th picture it looks like DOC, but the rest look like chips not coming out of the hole. Alloyed Steel chips get hard if you're doing it right. But they need to go somewhere.

    R

  10. #48
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9,481
    Post Thanks / Like
    Likes (Given)
    3234
    Likes (Received)
    3397

    Default

    Cant tell much from photo,, radius seems large for a narrow boring bar and a deep bore, but that could be wear.. I am thinking a lead cutting angle perhaps 45* by about .030 for a depth of cut less than .010,(more time in the job beats the price of boring bars).. a small radius, lead clearance of perhaps 10 to 12*. small in feed rate and small. depth of cut would be good.
    I like to draw the Id circle 10x scale then draw fit the OD clearance.. this shows clearly the primary/secondary / perhaps a third secondary to fit the bore. often a boring bar can rub below the cut and fudge the operation.
    Yes often you can hold the cutter and a sample bore to eyeball the cut with the boring bar held at bore center.
    Need eyeball clearance to the smallest bore it will cut..
    looks like you have good back rake...cant tell if any side cutting edge rake.

  11. #49
    Join Date
    Aug 2017
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    51
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    7

    Default

    Quote Originally Posted by michiganbuck View Post
    Cant tell much from photo,, radius seems large for a narrow boring bar and a deep bore, but that could be wear.. I am thinking a lead cutting angle perhaps 45* by about .030 for a depth of cut less than .010,(more time in the job beats the price of boring bars).. a small radius, lead clearance of perhaps 10 to 12*. small in feed rate and small. depth of cut would be good.
    I like to draw the Id circle 10x scale then draw fit the OD clearance.. this shows clearly the primary/secondary / perhaps a third secondary to fit the bore. often a boring bar can rub below the cut and fudge the operation.
    Yes often you can hold the cutter and a sample bore to eyeball the cut with the boring bar held at bore center.
    Need eyeball clearance to the smallest bore it will cut..
    looks like you have good back rake...cant tell if any side cutting edge rake.
    The photos show wear at the cutting edge tip which originally had a 0.003” radius as shown in the final photo which has no wear. It has a 3* clearance angle at the cutting edge of an undamaged bar. Rotating the bar to negate and rubbing below the cutting edge will likely be necessary to some degree.

  12. #50
    Join Date
    Mar 2019
    Country
    ALAND ISLANDS
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    3

    Default

    Agree with the chap who said something about it being cut like a rifle cartridge chamber. Call Dave Manson at Manson Precision Reamers and send him your print. Can make it out of HSS or carbide. Maybe a couple hundred bucks. Hope you need to cut more than one. Boring of a long, small tapered hole

  13. #51
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9,481
    Post Thanks / Like
    Likes (Given)
    3234
    Likes (Received)
    3397

    Default

    Quote Originally Posted by Bendak View Post
    The photos show wear at the cutting edge tip which originally had a 0.003” radius as shown in the final photo which has no wear. It has a 3* clearance angle at the cutting edge of an undamaged bar. Rotating the bar to negate and rubbing below the cutting edge will likely be necessary to some degree.
    Possible 3* is not enough ..hold the cutter in a fished part and with a loop look to see at least 5* inside the circle of the part. Or draw the part 10x scale and draw the cutter with 3* and then 5* to see how it looks.

    Another fair to Ok method is to take one pass..then look with a loop to see the wear land..in this case the blue color is only at the top edge..not going down the side if the cutter under the cutting edge. Yes you can add clearance with a diamond wheel not green wheel.
    A boring bar should last a long time on such a job.

  14. Likes Bendak liked this post
  15. #52
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    Quote Originally Posted by gbflyer View Post
    Agree with the chap who said something about it being cut like a rifle cartridge chamber. Call Dave Manson at Manson Precision Reamers and send him your print. Can make it out of HSS or carbide. Maybe a couple hundred bucks. Hope you need to cut more than one. Boring of a long, small tapered hole
    Oh good, another gun nut from Hollands west coast.

  16. #53
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    Quote Originally Posted by Bendak View Post
    The photos show wear at the cutting edge tip which originally had a 0.003” radius as shown in the final photo which has no wear. It has a 3* clearance angle at the cutting edge of an undamaged bar. Rotating the bar to negate and rubbing below the cutting edge will likely be necessary to some degree.
    Have you tried any of the recommendations?

    You're going to have to bite the bullet and get some more Bars. The safe way to do this is probably the one Ox said about using different Bars at different depths. But whatever way you try, you need to move forward.

    R

  17. Likes Bendak liked this post
  18. #54
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,725
    Post Thanks / Like
    Likes (Given)
    4855
    Likes (Received)
    7561

    Default

    I think that you must be refering to my mention of using multiple tapered drills (reamers) to break up the surface contact.
    Not bars. (I don't think?)


    Several have mentioned using a similar tool as a tapered pin reamer, and that's fine in 1018, but I don't know if I've ever tried to ream a pin hole in alloy?
    Have some of you reamed a small hole through an alloy shaft before?
    With any regularity?
    I have not. I am asking - not challenging - just to be clear.

    The drill will plunge - but I guess I should add to NOT use a manual quill machine as the helix could suck it in, but the drill will help to clear chips, while the reamer will need to go in and out umpteen times. But I guess that's good practice for a young buck?

    I have ran many tens of thousands with the drill method in 1200 series.
    Not alloy.


    ---------------------

    Think Snow Eh!
    Ox

  19. #55
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    You're right, I thought you meant Bars.

    These are my recommendations;

    1. Use Drills and get as much material out as you can. Then go in with a short Bar and deal with the large Diameter and the middle taper segment. Flip the part around and bore the rest from the .2" hole.

    2. Drill all the junk out. Bore and finish the second taper segment, change Bars. The last Bar would need to be held in a Holder that will reach into the large diameter, and finish the last taper segment.

    R

  20. #56
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,725
    Post Thanks / Like
    Likes (Given)
    4855
    Likes (Received)
    7561

    Default

    To bore from the back end, I would suggest that you kick your bar over to prox same angle that you want to bore.
    Otherwise you will need an even smaller shank for Clarence.


    ------------------

    Think Snow Eh!
    Ox

  21. #57
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9,481
    Post Thanks / Like
    Likes (Given)
    3234
    Likes (Received)
    3397

    Default

    Does the wood core sample know or care there is a straight portion of .259 for .926 deep / then a tapering for .720 depth from .926 to .234/ then a second tapering from .234 to .205.
    You are trying to master-match sizes likely a turkey shoot at the first part.
    Likely exact size means a hill of beens.
    Perhaps:
    Drill through with a 13/64 (.203)
    Then drill .726 deep with a G drill (.261)
    Then almost all the remaining with a 15/64 (.234) leaving only 1/8 of the 13/64 (.203)
    Then ream the 1/8” remaining of the 13/64 with the $10 5MM straight flute taper pin reamer.

    Yes best to draw this ID 10x scale to see it works for the taper reamer to finish the small end.

    But yes most any Tool and Cutter grinding shop would make an altered standard reamer into a straight / taper/taper reamer if you are sensible about the size and asking for +- .005 Dia. and +- .030 in taper length or so. like I said most of the ID size does not matter. The special reamer could be made from a $20 17/64 reamer (.265)

    And the same Tool Cutter shop can alter the 5MM taper reamer if you would like a different taper.( I have not figured out that reamers taper. perhaps 1 degree is good for the small end ID.

    If you don't get 5 or more out of a $20(or so) boring bar it is a dead job (not worth the time and cost)

  22. #58
    Join Date
    Aug 2017
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    51
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    7

    Default

    Thanks for all the ideas. I’ll let you know what works when I get the chance to machine it.

  23. #59
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,725
    Post Thanks / Like
    Likes (Given)
    4855
    Likes (Received)
    7561

    Default

    He could try rolling his own straight flute reamer.

    If you don't havea T&C grinder available to you, you can chuck up the reamer in your 5C collet spin fixture.
    Set it on your sine plate.
    Leave it hang out a ways if it doesn't chatter too much.

    Grind the taper.

    Now spin your sine plate and all 90*.
    Put the smallest wheel that you have on the grinder.
    Now try to grind the relief on the back side of the flutes.

    You need good light, and a black marker and bright flashlight to check will help.

    You can knock a few of these out in the time that you are trying to order a special somewhere with 6 weeks delivery.
    .. and again - VERY good experience!
    Anyone can dial (is that still an applicable term?) the phone.


    -------------------

    Think Snow Eh!
    Ox

  24. #60
    Join Date
    Mar 2019
    Country
    ALAND ISLANDS
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    3

    Default

    Quote Originally Posted by litlerob1 View Post
    Oh good, another gun nut from Hollands west coast.
    Actually no, from the part of what should have been Canada’s west coast that Seward bought (stole) from the Russians. Boring of a long, small tapered hole

    Gun nut? Probably...my wife thinks so.


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
  •