Need suggestions on tooling for a part (10x small tooling)
Close
Login to Your Account
Results 1 to 11 of 11
  1. #1
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    1,674
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    671

    Default Need suggestions on tooling for a part (10x small tooling)

    Have a part I am looking at making for a customer. It's a "fun" job.

    V

    The ID of the part is a V, at the intersection of the V there is a radius, I'll use a #53 drill.

    If this were a small production job I would grind a cutter and run the part horizontal, then locate off the V cut to profile the outside.

    Cutting the rest of the V is the problem. The part is .618 thick. I would really like to cut it all in one go, flip and take the stock off.

    Maybe that is not the most economical choice. This may be a situation where flipping the part and machining it from 2 sides is best?

    Going to be making 3-5 pcs.

    38b25cd5-0b03-48af-8f2b-41207d8bec53.jpg

  2. #2
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    130
    Post Thanks / Like
    Likes (Given)
    92
    Likes (Received)
    19

    Default

    I would go through Harvey Tools and get a small end mill to do the radius unless its a loose fitment and not very critical.
    Opt 1 cut the contour about .03 pass the part depth soft jaws and face to size. Sometimes with small thin parts I go to the saw and cut along the contour close without touching the part so the face mill doesnt sling the part out of m jaws.

  3. #3
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,685
    Post Thanks / Like
    Likes (Given)
    1026
    Likes (Received)
    1059

    Default

    If you can step it down then just get a couple of mills from Harvey, you want a backup in case you break one. Their extended reach stub flute aluminum mills can feed quite aggressively, but be careful about that corner. A couple of HSM passes to clear it out may be in order.

    I would take a hard look at milling half depth and flipping to finish. The mills will be a lot more robust in the shorter length. They have a .05" x .4" doc mill that looks good to me.

  4. Likes DieselMater86 liked this post
  5. #4
    Join Date
    Dec 2014
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    359
    Post Thanks / Like
    Likes (Given)
    38
    Likes (Received)
    56

    Default

    I wouldn't call a .618" thick part a thin part. You don't say what material your cutting. I would go with the cutter or one like David Scott mentioned and flip the part doing the detail in 2 ops.

    Standing the part up vertically if that detail is open face and using a form tool would go the quickest, but for only 5.

    Just contour it with the little .05" EM in 2 ops, easy.

  6. #5
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,343
    Post Thanks / Like
    Likes (Given)
    1463
    Likes (Received)
    1583

    Default

    Material? Sorry if I missed it.

  7. #6
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    1,674
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    671

    Default

    Thanks for the input, sometimes you know the best way, but you just need to hear someone agree.

    On a minimum quantity part like this, I really hate to take the time to machine soft jaws. It is so much easier to leave a small base, saw it off, and dust the top with the surface grinder to clean up.

    Material is going to be 4340 most likely.

  8. Likes Mike1974 liked this post
  9. #7
    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 Fal Grunt View Post
    Thanks for the input, sometimes you know the best way, but you just need to hear someone agree.

    On a minimum quantity part like this, I really hate to take the time to machine soft jaws. It is so much easier to leave a small base, saw it off, and dust the top with the surface grinder to clean up.

    Material is going to be 4340 most likely.
    If it makes you feel any better, earlier this week I programmed a part that need a .01" endmill and .0115" drill, but only 1/2 hard brass.

    I would 'rough' as much as possible with an 1/8 endmill, then pick the corners with something like this -

    http://www.harveytool.com/ToolTechIn...lNumber=982160

    Then finish, in step downs with a similar tool -

    http://www.harveytool.com/ToolTechIn...lNumber=992560

    Or alternatively, ( I know you said you wanted to profile and flp) you could 3d surface the V shape with one of these (start with 1/8" or 3/16" maybe) -

    http://www.harveytool.com/ToolTechIn...umber=17747-C6

  10. #8
    Join Date
    Aug 2006
    Location
    Cape Cod, Ma
    Posts
    450
    Post Thanks / Like
    Likes (Given)
    164
    Likes (Received)
    96

    Default

    What's the inside angle? Harvey sells chamfer cutters and runner cutters in all sorts of tight angles. maybe you get lucky and they have a stock size that would work.

  11. #9
    Join Date
    May 2005
    Location
    CA
    Posts
    1,121
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    280

    Default

    Quote Originally Posted by Fal Grunt View Post
    Have a part I am looking at making for a customer. It's a "fun" job.

    V

    The ID of the part is a V, at the intersection of the V there is a radius, I'll use a #53 drill.

    If this were a small production job I would grind a cutter and run the part horizontal, then locate off the V cut to profile the outside.

    Cutting the rest of the V is the problem. The part is .618 thick. I would really like to cut it all in one go, flip and take the stock off.

    Maybe that is not the most economical choice. This may be a situation where flipping the part and machining it from 2 sides is best?

    Going to be making 3-5 pcs.


    Maybe I missed something... what does the *outside* profile look like?

    PM

  12. #10
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,493
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1849

    Default

    Hi Fal Grunt:
    I'd make this on the wire EDM but if you don't have one and can't get access to one, that's not much help.

    But you do have a surface grinder.
    So I'd just hog out what you can, dress a wheel and plunge grind the whole shape if you need it accurate and nice.

    If you don't particularly need it super nice, you could drill the apex as you suggest, mill it from one side with the smallest convenient cutter, profile the outside in the same op, buck it off to length, surface grind the sawcut end, and then lay it down and pick out the corner with a dressed wheel or even just a hand-ground flycutter

    I personally hate profiling with tiny endmills sticking out a long way...you can do it with an extended reach 1/16 cutter but I've usually been better off with a formed wheel, and if you have a good selection of skinny wheels with tapers already dressed on them, modifying one is usually quick and easy, and cheaper than endmills, especially if you can line up all 5 parts in a row and walk through them in one go on the grinder.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

  13. Likes Fal Grunt liked this post
  14. #11
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    1,674
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    671

    Default

    Quote Originally Posted by precisionmetal View Post
    Maybe I missed something... what does the *outside* profile look like?

    PM
    You did not miss anything, I did not describe the outside of the part at all.

    Quote Originally Posted by implmex View Post
    Hi Fal Grunt:
    I'd make this on the wire EDM but if you don't have one and can't get access to one, that's not much help.

    But you do have a surface grinder.
    So I'd just hog out what you can, dress a wheel and plunge grind the whole shape if you need it accurate and nice.

    If you don't particularly need it super nice, you could drill the apex as you suggest, mill it from one side with the smallest convenient cutter, profile the outside in the same op, buck it off to length, surface grind the sawcut end, and then lay it down and pick out the corner with a dressed wheel or even just a hand-ground flycutter

    I personally hate profiling with tiny endmills sticking out a long way...you can do it with an extended reach 1/16 cutter but I've usually been better off with a formed wheel, and if you have a good selection of skinny wheels with tapers already dressed on them, modifying one is usually quick and easy, and cheaper than endmills, especially if you can line up all 5 parts in a row and walk through them in one go on the grinder.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining
    Wow Marcus... That is great advice. I did not even think about using my surface grinder. Just earlier this week I picked up some 3/8" and 1/2" grinding wheels for my grinder. I could rough the part in on my mill and then clean the slot up with the surface grinder. Will have to think about that for a bit!

    Wire edm would be ideal for this part, and my preference. Unfortunately I do not have one yet.


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
  •