Need Help trying to attain an 8 RA surface finish on a VMC.
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 26
  1. #1
    Join Date
    Jul 2019
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default Need Help trying to attain an 8 RA surface finish on a VMC.

    Hey all, first post here, but need a bit of advice. My shop recently quoted a part that should really be on a cylindrical grinder (Tight tolerance bores, concentricity, and true positions) as a mill job, simply because they could only find the stock in plate form. So now I've got these parts to make, and I'm racking my brain as to how to do it. I've only been in Machining for 2-3 years and could really use some tips. Here's what I know-

    my parts are shaped like bushings with hats, (Probably not allowed to share details and specs, you know- Top secret stuff) .228 thick, about 1.750 in diameter. My stock is some 4340 aircraft grade steel, arriving in plate form, 12x6x.25. My only forms of workholding are a 6 inch vise and some clamps, but I have no subplate.

    I was originally planning to cut the stock into 2x6 inch strips and roughing the bottom hat, then holding them in softjaws in the second op.

    The biggest issue I'm having, however, is figuing out how to get an 8 RA surface finish on the part. I've never seen an 8 RA finish on a VMC, let alone on an Okuma Genos m560, in steel, no less. I've only got 50 parts to do, but I feel like my tooling costs are going to be at least 2k or something. I have a lot of ER32 collet holders and a few nominal set screw holders for weldon shanks, along with two .75 milling chucks.

    It's a lot to ask, but please help a new guy out. I've looked into some grinding bits for the mill, but most can only get a max of 12 RA from what I've seen.

  2. #2
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,000
    Post Thanks / Like
    Likes (Given)
    13597
    Likes (Received)
    10612

    Default

    So a really short flanged bushing??

    What kind of tolerances are we looking at here? And are
    there any loose tolerances (those areas give you something to
    grab in some soft jaws)

  3. #3
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,950
    Post Thanks / Like
    Likes (Given)
    5194
    Likes (Received)
    7716

    Default

    An 8 in a mill with soft steel?

    "That's a Tuffy"

    This is the bore that needs to be so smoooooth - right?

    I would leave a bit of stock and send it to your neighborhood honing shop.
    Check with them as to amount of stock to leave.
    And hopefully they can finish that low in soft material.
    They would likely need to 2 or 3 stage them with different grits to hit your target.

    We use'ta run some small shafts that got ground to either and 8 or a 6.
    They were like a mirror (prolly the 6), but 8 wouldn't be too far from that.


    What I find more concerning is that you are wanting to run a bushing in a vice.
    Hopefully you make some full profile soft jaws to keep from oblonging the hole.
    I guess the hone guy would straighten that out for the most part, but he's not going to like dealing with it.


    If your nice surface is anywhere other than the bore, have fun!


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

    Think Snow Eh!
    Ox

  4. #4
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    2,924
    Post Thanks / Like
    Likes (Given)
    212
    Likes (Received)
    2039

    Default

    yeah, you need a second op, really cannot machine an 8

    would have to know more about dimensions and tolerances to get better advice on any way you can automate the finishing yourself

  5. #5
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    12
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4

    Default

    For getting a nice finish in a bore, you could check out roller burnishing. I've been able to achieve 4-6 Ra finishes in 316 SS using burnishers. Not sure about 4340. You'd want to have a nice reamed hole first.

    For the rest of the part, hand polishing?

  6. Likes Dan from Oakland, dstryr liked this post
  7. #6
    Join Date
    Jul 2019
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    So my ID Bores on two sides are both .875 +/- .0005, and all of my outside surfaces are +/- .005 or .001.

    I've considered hand polishing or grinding as many surfaces as possible on the surface grinder, but I still have the ID work to consider.
    Material is also being heat treated and coated afterwards, and the dimensions are after coating.

  8. #7
    Join Date
    Jul 2019
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Yeah, the engineers and top brass refuse to let our machinists look at parts before they bid them. They usually pick weird stuff and assume we can do it, but don't like when we tell them we can't do it with what they have.

    It's a pain, and I want to usually rip my hair out over it. Will see if they're willing to export to another shop for honing, not sure if that's in the profit margin at all (They like to underquote for some god awful reason.)

  9. Likes Bobw liked this post
  10. #8
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    12
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4

    Default

    If you experiment with the feeds and speeds, you can usually attain a nice finish by boring those .875 IDs. Assuming you have a nice boring head.

  11. #9
    Join Date
    Jul 2019
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Quote Originally Posted by Buttpoop View Post
    If you experiment with the feeds and speeds, you can usually attain a nice finish by boring those .875 IDs. Assuming you have a nice boring head.
    No boring head, just some accupro endmills and Mastercam.

  12. #10
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,343
    Post Thanks / Like
    Likes (Given)
    1463
    Likes (Received)
    1583

    Default

    Quote Originally Posted by jrk190 View Post
    No boring head, just some accupro endmills and Mastercam.
    Not going to happen, sorry. I have no problem with Accupro, we use them everyday... on aluminum. At the very least you are going to need a better endmill, like a Garr, MA Ford or something. You could probably mill +/-.0005", but if there are any other tolerances like roundness you are going to be in trouble IMO.

  13. #11
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,950
    Post Thanks / Like
    Likes (Given)
    5194
    Likes (Received)
    7716

    Default

    Well, doo the H/T before the grind/hone opps for sure!

    Harder material produces finer finishes much easier.


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

    Think Snow Eh!
    Ox

  14. #12
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    12
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4

    Default

    Quote Originally Posted by jrk190 View Post
    No boring head, just some accupro endmills and Mastercam.
    Bummer.

    If thats all you have to work with, try interpolating @ 75-100 SFM @ .0005-.001 IPT with 2 spring passes. I know it looks slow, but the lower SFM will not cause as much deflection/harmonics resulting in better surface quality.

  15. #13
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,255
    Post Thanks / Like
    Likes (Given)
    354
    Likes (Received)
    579

    Default

    Quote Originally Posted by jrk190 View Post
    Yeah, the engineers and top brass refuse to let our machinists look at parts before they bid them. They usually pick weird stuff and assume we can do it, but don't like when we tell them we can't do it with what they have.

    It's a pain, and I want to usually rip my hair out over it. Will see if they're willing to export to another shop for honing, not sure if that's in the profit margin at all (They like to underquote for some god awful reason.)
    “We, the unwilling, led by the unknowing, are doing the impossible for the ungrateful. We have done so much, for so long, with so little, we are now qualified to do anything with nothing.”

    Good luck

  16. Likes mhajicek, Bobw, jz79, chip_maker, Mike1974 liked this post
  17. #14
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    768
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    289

    Default

    Quote Originally Posted by jrk190 View Post
    Hey all, first post here, but need a bit of advice. My shop recently quoted a part that should really be on a cylindrical grinder (Tight tolerance bores, concentricity, and true positions) as a mill job, simply because they could only find the stock in plate form. So now I've got these parts to make, and I'm racking my brain as to how to do it.
    Cut round blanks out of plate (laser, water jet, or simply mill them. Hougen drill even?) and send them over to the lathe.

    Let me ask you: do you even have the means to measure surface finish?

    I only ask because if you are told to hold an 8 in a mill, someone (production manager or other blameable person) doesn't know what they are doing there. And as a parallel thought, probably doesn't know what an 8 is, looks like, or how to check it. It sure isn't "shiny"


    You will want to HT the part first, btw. Do not do HT afterward.

    Where is the 8RA called out at? OD, ID, and face?

  18. #15
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    2,924
    Post Thanks / Like
    Likes (Given)
    212
    Likes (Received)
    2039

    Default

    1.75 dia 4340 from mcmaster 85 bucks for 3 feet

    that's the real sin in all this

    If I had to make them on a mill I would turn them in the spindle

  19. Likes Ox, Bobw, dstryr liked this post
  20. #16
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    768
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    289

    Default

    Quote Originally Posted by gustafson View Post
    1.75 dia 4340 from mcmaster 85 bucks for 3 feet

    that's the real sin in all this
    I agree with that. However, I wonder if this job is military work and the material needs to be DFAR compliant. I know I have had to make plate stock round in the past. I have no idea if the mcmaster material is; you could probably call to find out.

  21. #17
    Join Date
    Jul 2019
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Quote Originally Posted by dandrummerman21 View Post
    Cut round blanks out of plate (laser, water jet, or simply mill them. Hougen drill even?) and send them over to the lathe.

    Let me ask you: do you even have the means to measure surface finish?

    I only ask because if you are told to hold an 8 in a mill, someone (production manager or other blameable person) doesn't know what they are doing there. And as a parallel thought, probably doesn't know what an 8 is, looks like, or how to check it. It sure isn't "shiny"


    You will want to HT the part first, btw. Do not do HT afterward.

    Where is the 8RA called out at? OD, ID, and face?
    ID and OD. We really don't have the capabilities for it. Only grinder we have is a crappy secondhand surface grinder I just made a wheel guard for on the bandsaw and need to grind the chuck in on.

    They claim they couldn't find the right mil spec. material or something in anything other than plate which I find awful hard to believe. Our one chance for this part would've been on the lathe but can't do it out of plate on the lathe.

    Another case of making chicken soup from chicken scat.

  22. #18
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    2,924
    Post Thanks / Like
    Likes (Given)
    212
    Likes (Received)
    2039

    Default

    then rough the blanks on the mill and finish on the lathe

  23. Likes 5 axis Fidia guy, J Gilles, Ox liked this post
  24. #19
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    462
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    241

    Default

    I think the only way you're getting that finish on a mill is if the print is in metric LOL.

    We just had to roll burnish some 48Rc nodular iron to get an internal bore to a 12 microinch finish and it was a huge pain.

    I've cut 9-11 microinches in the Swiss but I don't think I'd try it on a VMC. Best bet for an endmill might be a helical boring operation?

  25. Likes Ox liked this post
  26. #20
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    49
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    10

    Default

    Nothing is impossible to the person that doesn't have to make it work. :-)

    I've heard of shops normalizing 4xxx steels before machining.
    Laser cut does not sound like a good idea, 4340 is 'almost' air hardening.
    Round stock sounds nice but you may lose more than you want cutting wafers.
    All I can do is wish you luck.

  27. Likes jrk190 liked this post

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
  •