Cutting narrow slots (.005"W X .0045"D) across fins (.012") of 303/304 SST
Close
Login to Your Account
Results 1 to 9 of 9
  1. #1
    Join Date
    Jul 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Cutting narrow slots (.005"W X .0045"D) across fins (.012") of 303/304 SST

    Hello,

    A machining question for folks on this forum.

    I'm trying to make a small slot across the top of some fins of our fixture. (See Pix) Our Fixture has a 40,80, and 120 mm version.
    strip-holder-wide-view.jpgstrip-holder-slot.jpg

    The slot is going to be .005" W X .0045"D. The fins are .012" thick. Material is to be 303 or 304 SST.

    We need the slots to be uniform all the way up the length of all the fins. They need to be as close to those dimensions as possible. We need the bottom of the slot to be even and flat as possible. NOTE: Some radius on the inside corner of the slot is ok but not more than .001".

    Does anyone have suggestions on how to make this slot?


    Conventional CNC machining - tried already with small .006 or .007 diameter end mills. Bottom of milling was very rough (not flat). Machinist couldn't hold tolerances.

    Wire EDM - might be possible but would need something like 0.002" diameter wire (Tungsten?). Not sure if wire EDM could do this in a line or not. Radius on the bottom would be ok but we need the middle .003" of the slot to be flat(ish).

    Sink EDM - not sure if this is practical or not.

    Electrochemical Machining?

    Etching?

    Laser / water cutting? Probably too much radius needed for the more exotic processes. I assume they wouldn't be able to whole slot length.

    Please help.

    Any advice would be appreciated.

    Thanks,
    Zenbot01

  2. #2
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    6,767
    Post Thanks / Like
    Likes (Given)
    1607
    Likes (Received)
    4725

    Default

    A fine toothed carbide saw, ideally thinned from a thicker blank with just enough tooth depth for the needed cut. So start with a 1.5" OD x 1/8" thick x 3/4" bore blank, grind the periphery to a .005" thin rim about .010" deep, saw teeth about .040" - .050" pitch. Get enough to last the job, cheaper than multiple orders.

    Cut at the max speed that gives decent life, make sure you have plenty of flushing coolant. Need good fixturing, both concentric arbor and laydown clamp to locate parts.

    Talk to member Frank Mari about a quote for the cutters.

    https://www.practicalmachinist.com/v...=newpm&u=74846

  3. Likes Illinoyance liked this post
  4. #3
    Join Date
    Dec 2014
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    351
    Post Thanks / Like
    Likes (Given)
    37
    Likes (Received)
    54

    Default

    Yep that works good, beats the hell out of those -.01" EM. Scraping would probably work fine too.

  5. #4
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,255
    Post Thanks / Like
    Likes (Given)
    1152
    Likes (Received)
    2323

    Default

    WEDM is the answer. But this is (sort of) the Manual Machining sub forum. I would post in the CNC sub, if you want super technical answers. Because this is a very technical part.

    R

  6. #5
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,245
    Post Thanks / Like
    Likes (Given)
    406
    Likes (Received)
    1630

    Default

    I've used dental slitting disks to make witness marks on stainless parts.

    Like these:

    Small Diamond Slitting Discs

  7. #6
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,255
    Post Thanks / Like
    Likes (Given)
    1152
    Likes (Received)
    2323

    Default

    Quote Originally Posted by jancollc View Post
    I've used dental slitting disks to make witness marks on stainless parts.

    Like these:

    Small Diamond Slitting Discs
    I can't tell if you are serious or not

    Those are .5mm (.02"). Plus unless I am misinterpreting the drawing you would have to be able to reach that thing down 4". And cut into the part .003". In my experience those things are not very Round and the Runout is horrifying.

    R

  8. #7
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,245
    Post Thanks / Like
    Likes (Given)
    406
    Likes (Received)
    1630

    Default

    Quote Originally Posted by litlerob1 View Post
    I can't tell if you are serious or not

    Those are .5mm (.02"). Plus unless I am misinterpreting the drawing you would have to be able to reach that thing down 4". And cut into the part .003". In my experience those things are not very Round and the Runout is horrifying.

    R
    .17mm is .0066". Maybe I'm the one misinterpreting the drawing. I see the little slot in detail C, which is right on the top of the part. Lay it flat on table, partt's only 1/4" thick. You only need 1/8" sticking out to get to the center of the part where the slot is. The arbor has more than that, so it can be chucked all the way up in the collet. I don't see any feature on that drawing that requires a 4" anything.

    I make a 303 turnbuckle body that gets a slot on the left hand thread end. It's not a critical tolerance, but it's a lot deeper than .003". I don't use that skinny of a saw, I use an .020" but I'm grinding about .015" deep.

    I think the scraping idea is good too, probably easier to hold the tolerance if the tool is made right. Same with the carbide slit saw if you can keep it from blowing to pieces when it hits the part...

    I have no experience with EDM so I can't express an opinion there- I'll take the word of you guys that do.

    edit to add: Another possibility- Thinbit makes grooving inserts .004" and up in .001" increments. Wouldn't be difficult to rig up a setup to scrape the groove with a grooving insert, the feature isn't much more than a scratch.

  9. Likes litlerob1, camscan liked this post
  10. #8
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,470
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1821

    Default

    Hi All:
    Wire cutting these is a possible solution but you need to find a fine wire shop and there are relatively few around.
    If the longest of these parts are only around 4" and change, you can stand them up in the worktank and cut them relatively simply; you just have to fixture them accurately so they sit in the proper orientation.
    Your cut volume is small enough to allow you to cut them relatively uneventfully with moly or tungsten wire down to 0.00078" diameter. (the 4" of length does not all need to be cut, only 0.012" x the number of ribs actually sees the wire and the slot is shallow so the flushing is good).

    One BIG benefit not touched on yet is that EDM cutting is bur-free,,,trying to saw or shape these will force you to deal with some pretty nasty burs that might be bigger than the features, assuming the super thin sections don't strip the teeth off the saw, or fold over from the force of the cut.

    Sinker EDM I would be doubtful of; by the time you account for the overburn, you have to make the electrode paper thin.
    At 0.001" per side overburn your trode is only 0.003" thick, and you have to give it enough height to allow flushing jets alongside it.

    There are a few tricks you can use like tapering the trode to make it a bit stronger and wire cutting the trode from something like copper tungsten or grinding it from POCO Angstrofine graphite, but I'd still promise only to try and see what can be accomplished; I'd never promise guaranteed success on a part like this.
    My experience on my old Hansvedt sinker has been that I cannot do it reliably...now someone with a nice new Makino may have a totally different take on it and see it as an easy job...the technology has come a long long way since my machine was built (1996).

    But EDM of either kind does have some significant advantages.

    Cheers

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

  11. #9
    Join Date
    May 2005
    Location
    AZ
    Posts
    2,319
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    789

    Default

    I think WEDM is probably a good bet for this, which would make my following comment somewhat moot, BUT if I were to choose a machining path that involves cutting the material with a toothed cutter of some sort, I would eliminate the use of 304 alloy right off the bat. 303 will be a more friendly material, and more forgiving in speed/feeds than 304.

  12. Likes camscan 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
  •