Slotting tool recommendations
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 24
  1. #1
    Join Date
    Aug 2013
    Location
    IL USA
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default Slotting tool recommendations

    I'm having a heck of a time getting good tool life doing some slotting around a circular profile in thin steel plate (0.130" thick). 5" diameter circle on each part.

    I'm currently using:
    https://www.mscdirect.com/product/details/78978020
    (OSG 44700211 3/16 3fl high feed style)

    OSG recommended a similar tool with flutes that have an angle to aid in chip evac: 447200113

    But the tool life just isn't what I want, I'm fairly convinced the carbide that OSG thing is made of is some kind of mithril/vibranium but the edges are just about chowdered up and it's leaving some nasty burrs after ~45 parts.

    I've broken so many traditional endmills trying to slot the circle of these plates I really need some good advice. The only other tool I have had luck with is a 3 flute roughing endmill from lakeshore carbide--I do a reasonably steep (for me) 7 degree ramp into a short slot (3/4 long) through the plates in about 10 places per part, trying that same recipe on the larger circle was just another broken tool.

    So, if you were in my shoes and had to use a 3/16 endmill to slot circles in 0.130" thick plates, what tool would you use?

  2. #2
    Join Date
    Apr 2012
    Location
    AR, USA
    Posts
    955
    Post Thanks / Like
    Likes (Given)
    20
    Likes (Received)
    174

    Default

    Are the slots going all the way through the sheet? Are there existing holes or slots you're starting in? 3 flute end mills are not center cutting. How rigid is your setup? You have a large area considering how thin the sheet is. Is it held tightly to avoid vibration? If not, consider two sided tape or a vacuum fixture. What kind of steel are you cutting? Both of those OSG endmills look like they are for hardened steel.

  3. #3
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,512
    Post Thanks / Like
    Likes (Given)
    1191
    Likes (Received)
    2498

    Default

    What material are you Machining?

    R

  4. #4
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,249
    Post Thanks / Like
    Likes (Given)
    730
    Likes (Received)
    1784

    Default

    I"d be looking at my work-holding, this sound like chatter is wrecking your cutters.

  5. Likes TeachMePlease liked this post
  6. #5
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,280
    Post Thanks / Like
    Likes (Given)
    361
    Likes (Received)
    585

    Default

    Odd suggestion but try an endmill more suited for hard materials, the edges will have more support behind them and if you use one with corner radii those will be protected too.

  7. #6
    Join Date
    Aug 2013
    Location
    IL USA
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Quote Originally Posted by litlerob1 View Post
    What material are you Machining?

    R
    A1011 plate, it shouldn't be hardened but it's pretty tough and hot rolled. The slots go all the way through, it's held down reasonably well for plate (I probably need to buy a cheap magnet and just mill the crap out of the top) and yes the tool is a hard milling category but it's also recommended for softer stuff too in the details.

    I might just try the double sided tape.

  8. #7
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,661
    Post Thanks / Like
    Likes (Given)
    1522
    Likes (Received)
    1738

    Default

    Quote Originally Posted by robert123 View Post
    Are the slots going all the way through the sheet? Are there existing holes or slots you're starting in? 3 flute end mills are not center cutting. How rigid is your setup? You have a large area considering how thin the sheet is. Is it held tightly to avoid vibration? If not, consider two sided tape or a vacuum fixture. What kind of steel are you cutting? Both of those OSG endmills look like they are for hardened steel.
    Huh?? What are you buying/using??

    We use 3 flute endmills from .006-.500 and almost all of them are center cutting....

  9. #8
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,512
    Post Thanks / Like
    Likes (Given)
    1191
    Likes (Received)
    2498

    Default

    I agree with holding it gooder. If you can't, I'd go HSS Endmill.

    R

  10. Likes Mtndew liked this post
  11. #9
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,499
    Post Thanks / Like
    Likes (Given)
    446
    Likes (Received)
    1772

    Default

    Quote Originally Posted by meowkat View Post
    ...So, if you were in my shoes and had to use a 3/16 endmill to slot circles in 0.130" thick plates, what tool would you use?
    I don't understand why you picked a cutter with a 3/32" LOC to slot an 1/8" plate.

    I'd use something like this:

    Niagara N85590 | 3/16" Diameter x 3/16" Shank x 5/8" LOC x 2" OAL Right Hand Cut Center Cutting Single End Solid Carbide TiAlN Coating Square End Mill - All Industrial Tool Supply

    Stone a radius on the corners, or buy the version with a corner radius. Choke it up in the collet, helical toolpath, a couple times around to depth should be easy-peasy. I think they make that cutter with a 3/8" LOC which would be even better...

  12. #10
    Join Date
    Aug 2013
    Location
    IL USA
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Quote Originally Posted by litlerob1 View Post
    I agree with holding it gooder. If you can't, I'd go HSS Endmill.

    R
    Hmm worth a try I guess. HSS to the rescue?

  13. #11
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    370
    Post Thanks / Like
    Likes (Given)
    53
    Likes (Received)
    166

    Default

    heck no...why would you go backwards in technology?

    Sounds like you are gripping that part in a a vise?

    I would drill 4 hole in the corners and bolt it down to a fixture plate for that thin material. no more warping, no chatter, plenty of support...

  14. #12
    Join Date
    Aug 2013
    Location
    IL USA
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Well I'm using it as sort of a "high feed" tool, 0.010" DOC, 45 IPM, 5,000 RPM. Low spindle speeds available on the old cnc but it is reliable and the tool life was better than all the broken ones.

    I'll give this thing a try and see how it goes: https://www.mscdirect.com/product/details/67291732

  15. Likes jancollc liked this post
  16. #13
    Join Date
    Aug 2013
    Location
    IL USA
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Quote Originally Posted by as9100d View Post
    heck no...why would you go backwards in technology?

    Sounds like you are gripping that part in a a vise?

    I would drill 4 hole in the corners and bolt it down to a fixture plate for that thin material. no more warping, no chatter, plenty of support...
    I have it screwed down with 4 5/16-18 screws to a 1/2" steel plate on top of a pierson pallet. The double sided tape should tell me if it's lifting up and breaking the tools.

  17. #14
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    370
    Post Thanks / Like
    Likes (Given)
    53
    Likes (Received)
    166

    Default

    My calculator says 5000rpm and 29.4ipm. Thats what Id try... I doubt your part is lifting up any, I think the feed is just double what it should be.

  18. #15
    Join Date
    Aug 2013
    Location
    IL USA
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Quote Originally Posted by as9100d View Post
    My calculator says 5000rpm and 29.4ipm. Thats what Id try... I doubt your part is lifting up any, I think the feed is just double what it should be.
    chip-weld-not.jpgchip-weld-not2.jpg

  19. #16
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Quote Originally Posted by meowkat View Post
    I'm having a heck of a time getting good tool life doing some slotting around a circular profile in thin steel plate (0.130" thick). 5" diameter circle on each part.

    I'm currently using:
    https://www.mscdirect.com/product/details/78978020
    (OSG 44700211 3/16 3fl high feed style)

    OSG recommended a similar tool with flutes that have an angle to aid in chip evac: 447200113

    But the tool life just isn't what I want

    So, if you were in my shoes and had to use a 3/16 endmill to slot circles in 0.130" thick plates, what tool would you use?
    I wouldn't use a 3/16 tool, I'd use a 2/16 one and spiral path it.

  20. #17
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,512
    Post Thanks / Like
    Likes (Given)
    1191
    Likes (Received)
    2498

    Default

    Quote Originally Posted by as9100d View Post
    heck no...why would you go backwards in technology?
    Kids!!!

    It's not backwards if it works. HSS is slower than Carbide. It's also tougher.

    R

  21. Likes TeachMePlease liked this post
  22. #18
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Quote Originally Posted by litlerob1 View Post
    Kids!!!

    It's not backwards if it works. HSS is slower than Carbide. It's also tougher.

    R
    Agree in a sense. If you suffer tool breakage continuously with carbide the cycle time is pointless if you spend the same time replacing tools. Expensive tools.

    If mass production on the other hand take your time figuring shit out.

  23. Likes litlerob1 liked this post
  24. #19
    Join Date
    Aug 2013
    Location
    IL USA
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Small update, tried the niagara and got lots of chatter, tried a guhring diver and got a little bit of chatter and then it exploded doing a straight plunge as advertised, tried a kennametal Harvi 1 HPHV and it took the same cut as the guhring diver did but quietly and hasn't broken yet. Should turn this job from low paid into easy money.

    I think the kennametal is a great tool so far.

  25. #20
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9,968
    Post Thanks / Like
    Likes (Given)
    3359
    Likes (Received)
    3572

    Default

    Perhaps a left helix, right hand cut end mill would tend to push down on the part to push it to have more support and less chatter..

    Could a ball nose probe/finger set just above/near and touching the part and travel about on the part as you are milling so also to reduce chatter with using your existing cutter...probe carbide/steel even nylon..

    Seems like chatter may be some/much of the short tool life.

    https://www.homedepot.com/p/Yonico-3...3-SC/306082371

    Harvey Tool - Carbide Plastic Cutting End Mills - Square Downcut Single Flute


    4 Flute Square Downcut End Mills - AlTiN Coated - MariTool

    *Agree you don't need a single flute or a plastic end mill..double or 3 flute and left helix, right hand cut would be good.

    The fixture having support (touching) just under the part and along the slot being machined..


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
  •