Narrow slot roughing tactics
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,471
    Post Thanks / Like
    Likes (Given)
    770
    Likes (Received)
    1848

    Default Narrow slot roughing tactics

    I need to create a .375" deep, .125"( +.01, - 00) slot in 304ss. It's a 16.5" diameter circle in the face of a tube sheet for seating filter elements. Unfortunately I can't turn the part, lathe is a smidge too small so it's going on the VMC.

    Would you guys HEM this with an undersized tool, run it traditionally with an 1/8" rougher, or something else?

    The job was priced with a traditional slow movin path in mind so if that's the best way Im covered but I feel like there's a more efficient method.

    Thanks, Cole

    Sent from my SM-G973U using Tapatalk

  2. #2
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,494
    Post Thanks / Like
    Likes (Given)
    572
    Likes (Received)
    812

    Default

    What about drilling the bulk of material out with a drill about .010 under then come back with a 3MM make a roughing then finish pass?

    I hate those small deep slots, Not so much they are difficult they just take too long.

  3. #3
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    2,287
    Post Thanks / Like
    Likes (Given)
    202
    Likes (Received)
    1255

    Default

    Carbide .09375 4 flute altin coated run it in a shallow ramp.

  4. Likes Red James, mmurray70 liked this post
  5. #4
    Join Date
    Jun 2006
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    1,883
    Post Thanks / Like
    Likes (Given)
    1089
    Likes (Received)
    738

    Default

    Quote Originally Posted by plastikdreams View Post
    Carbide .09375 4 flute altin coated run it in a shallow ramp.
    With coolant blasting!

  6. Likes Red James liked this post
  7. #5
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,863
    Post Thanks / Like
    Likes (Given)
    755
    Likes (Received)
    2199

    Default

    Quote Originally Posted by Cole2534 View Post
    I need to create a .375" deep, .125"( +.01, - 00) slot in 304ss. It's a 16.5" diameter circle in the face of a tube sheet for seating filter elements. Unfortunately I can't turn the part, lathe is a smidge too small so it's going on the VMC.
    Not much of a 304 machinist, but I have a project with a 1" diameter, .125" wide, .125" deep slot in 17-4PH. The bigger challenge is that I need .5" of tool stick-out to get to the top of the feature.

    Went with the Helical HEV-C, a 5 flute chipbreak rougher and it worked amazingly well. Plugged my cut into the Helical Milling Advisor and ran the book numbers (4k something RPM, 8IPM). Worked beautifully! The chip breakers really make keeping the slot clear, which is just about the most critical thing to all this.

    Same Milling Advisor says your parameters would be 7460rpm at 24IPM taking that slot in .125" deep passes. I would pre-drill and plunge between levels (my setup chattered like the dickens on helical entry, so I drilled a hair undersize and plunged slowly between passes).

    The Harvey is a great tool!

  8. Likes vegard liked this post
  9. #6
    Join Date
    May 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    192
    Post Thanks / Like
    Likes (Given)
    115
    Likes (Received)
    78

    Default

    At +.01" tolerance I would use a .125" tool, with 3/8 LOC and a TiAlN coating or similar, and a slight corner radius ideally (.01 to .015"). Drill a start hole, then enter that and go around .021" at a time. Make sure you slowly plunge into the last couple of depth to cut your way in. Make darn sure you are getting the chips out. If my math's right this would end up being around 20 minutes of cutting.

    I'd be afraid of breaking drills off in the part and being screwed so I wouldn't feel great about chain-drilling, personally.

    If you have the power and rigidity, I wonder how a shop-made trepanning tool might do.

  10. #7
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,471
    Post Thanks / Like
    Likes (Given)
    770
    Likes (Received)
    1848

    Default

    I don't like chain drilling, but a 3mm cutter followed by a 1/8" is a good idea.

    I spoke with Helical and they suggested the HEV series. I think that's what I'll try.

    As for coolant, I'll be using Trim 690xt at about 10% concentration and doing whatever I can to clear the chips. Now I understand the desire for servo driven coolant nozzles.

    Sent from my SM-G973U using Tapatalk

  11. #8
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Iscar EC-E7 2 millimeter seven flute end mill, you will not find a better tool, go for a trochoidal path and chances you break it are slim to none. You'll save time with predrilling yes.

  12. #9
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,219
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2654

    Default

    Quote Originally Posted by Cole2534 View Post
    I need to create a .375" deep, .125"( +.01, - 00) slot in 304ss. It's a 16.5" diameter circle in the face of a tube sheet for seating filter elements. Unfortunately I can't turn the part, lathe is a smidge too small so it's going on the VMC.

    Would you guys HEM this with an undersized tool, run it traditionally with an 1/8" rougher, or something else?

    The job was priced with a traditional slow movin path in mind so if that's the best way Im covered but I feel like there's a more efficient method.

    Thanks, Cole

    Sent from my SM-G973U using Tapatalk
    .
    1) usually dont use same size end mill as the slot that is usually rough slot leave material on sides and bottom then take finish cut to improve surface finish and slot size consistency
    .
    2) 304 usually have short tool life and sudden tool failure rate is higher. usually have to be cautious about not damaging the part. little end mills in 304SS often dont finish long slot like that. i wouldn't be going 24ipm feed either. going by tool history data on 1000's of previous jobs. obviously part cost and risk of part damage from sudden tool failure need to be considered
    .
    3) often roughing end mill has chamfered corners for longer tool life and the finish end mill has smaller corner chamfers to make a more square corner slot. usually square corner end mill dont last very long roughing in 304SS
    .
    4) tool stick out length problem most important factor. usually stickout length over 3 dia and especially over 4 dia tool flex can be a problem. .125 dia that 0.5 stickout is very long length. .093dia end mill thats .36 stickout is long

  13. #10
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,418
    Post Thanks / Like
    Likes (Given)
    5677
    Likes (Received)
    8093

    Default

    I might consider plunge cutting with the 3mm, or even a 3/32 mill.
    Drill a start hole, and then switch to the mill and just program a "bolt hole pattern" with like 100 or whatnot holes in it - so that you are only taking .06 (?) at a time.
    That would seem to be the strongest use of the tool and the programming would be almost a one liner!


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

    Think Snow Eh!
    Ox

  14. #11
    Join Date
    Dec 2002
    Location
    Granville,NY,USA
    Posts
    3,934
    Post Thanks / Like
    Likes (Given)
    333
    Likes (Received)
    427

    Default

    I would also stay away from chain drilling. I rode that wild bull once. Thought I could get a 8 second ride and ended up on the arena floor spitting poop out of my mouth.

    Ox's idea has some good legs with a tool that is happy end cutting. Do you have TSC? Not sure if the Guhring Diver is available in 3mm but with TSC that could be mint.

    I would also be keen to go with a ramp down play



    I have no earthly idea why I made a rodeo themed post.
    Last edited by ARB; 11-16-2019 at 10:52 PM.

  15. Likes Ox, Mike1974, kineticmx, CBlair liked this post
  16. #12
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,471
    Post Thanks / Like
    Likes (Given)
    770
    Likes (Received)
    1848

    Default

    Quote Originally Posted by ARB View Post
    I would also stay away from chain drilling. I rode that wild bull once. Thought I could get a 8 second ride and ended up on the area floor spitting poop out of my mouth.

    Ox's idea has some good legs with a tool that is happy end cutting. Do you have TSC? Not sure if the Guhring Diver is available in 3mm but with TSC that could be mint.

    I would also be keen to go with a ramp down play



    I have no earthly idea why I made a rodeo themed post.
    Me neither, but yee haw.

    Sent from my SM-G973U using Tapatalk

  17. #13
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Quote Originally Posted by Ox View Post
    I might consider plunge cutting with the 3mm, or even a 3/32 mill.
    Drill a start hole, and then switch to the mill and just program a "bolt hole pattern" with like 100 or whatnot holes in it - so that you are only taking .06 (?) at a time.
    That would seem to be the strongest use of the tool and the programming would be almost a one liner!


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

    Think Snow Eh!
    Ox
    Yeah, that idea could be meritable. And yes the code would be only one line if you wanted (G16 G91 Y3.6 K100)

  18. #14
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,949
    Post Thanks / Like
    Likes (Given)
    1590
    Likes (Received)
    1841

    Default

    I have nothing of value to add....

    Buuutt... 1/8" is a big tool at current job! Now 'roughing' a .010"x.030" deep slot with an .007" endmill is where it's at LoL

    aluminum though...
    I'll see myself out hehe

  19. #15
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,029
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    672

    Default

    I'd pocket out a starting point and use a trochoidal tool path.

  20. #16
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,471
    Post Thanks / Like
    Likes (Given)
    770
    Likes (Received)
    1848

    Default

    Quote Originally Posted by AARONT View Post
    I'd pocket out a starting point and use a trochoidal tool path.
    I think this is my path.

    Carefully pocket out a small arc to start then trochoidal path with a 3mm e/m. 2 depth passes would be good, but I think 3 it going to be minimum.

  21. #17
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    119
    Likes (Received)
    158

    Default

    High Feed Mill

    I would ramp in quickly with a high feed endmill like above, may need to relieve the shank a little to get that deep.

  22. #18
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    689
    Post Thanks / Like
    Likes (Given)
    141
    Likes (Received)
    740

    Default

    Build a 8.25" Trepanning tool with a carbide parting tool. Turn the spindle at 500 RPM and plunge cut it...

    I'm kidding, but it sure would look cool.

  23. #19
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,471
    Post Thanks / Like
    Likes (Given)
    770
    Likes (Received)
    1848

    Default

    Quote Originally Posted by Hardplates View Post
    High Feed Mill

    I would ramp in quickly with a high feed endmill like above, may need to relieve the shank a little to get that deep.
    Hardplates, you're my man. I like this approach a LOT. It keeps the coding simple for my old VMC and with its .120" diameter it's a perfect roughing tool.

    Thank you!

    I emailed Carl at Lakeshore to see what he recommends for speed/feed/DOC, I'll reply with his suggestions.

  24. #20
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    119
    Likes (Received)
    158

    Default

    Quote Originally Posted by Cole2534 View Post
    Hardplates, you're my man. I like this approach a LOT. It keeps the coding simple for my old VMC and with its .120" diameter it's a perfect roughing tool.

    Thank you!

    I emailed Carl at Lakeshore to see what he recommends for speed/feed/DOC, I'll reply with his suggestions.

    Thread Mill Speed Charts | Feed & Variable Flute Speed Chart

    click on high feed


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
  •