Help slotting ar400
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 41
  1. #1
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    536
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    291

    Default Help slotting ar400

    I had a little job today where I needed to slot some ar400 plate. It is basically a rectangular plate with 27 slots 3/8" wide by 2 1/2" long. It resembles a floor drain plate but I'm sure that is not what its for. The plate is 3/4" thick and the slots go all the way through. I thought the endmill would have trouble plunging this ar400 so I drilled the end of all the slots. Then I tried to mill the slots with a 5/16 carbide endmill and then I was going to finish with a 3/8" endmill. I tried a .100" depth of cut at 12 in/min and 3000 rpms. That quickly broke a cutter. Then I tried .075" depth of cut and slower feed. Still broke a cutter after about 2 slots. I had the best luck with 1400 rpm and 3 in/min feed. I still can only get about 3 slots before the cutter breaks. I gave up and need help. Lol What seems to be the problem is that the edges of the holes that I drilled are work hardened. I plunge into the drilled hole and it makes noise when it starts to mill longitudinally until it gets through the hardened edge of the hole. I drilled the holes with a 11/32 high speed drill but for some reason it work hardened the edges of the hole. By the time I get one slot milled out the last .100 of the endmill is about toast. Any help would be appreciated. We might end up getting the slots water jetted.

  2. #2
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    103
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    17

    Default

    water jet would be the way to go without a doubt. if you had to cut it with a endmill I'd be more conservative like .05 dept and 1 inch a min and 900 to 1000 rpm. I'd also consider doing volume mill type pass where you are side cutting about. 02 a pass with increased depth like .1, as well as feed and speed.

  3. Likes lumley32 liked this post
  4. #3
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    536
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    291

    Default

    I forgot I also tried to plunge mill a few slots. I stepped over .100 for each plunge and ran 2.5 in/min feed and 1400 rpm but this also only produced about 3 slots before the cutter gave up the ghost.

  5. #4
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    7,004
    Post Thanks / Like
    Likes (Given)
    1651
    Likes (Received)
    4826

    Default

    If you want to avoid having to waterjet, then try using a good, sharp carbide drill to drill a new start hole just inside one of the previous end holes (just one end), then use a 1/4 x 1/2 stub endmill to troicoidal the rough slot width at 1/2 depth. Watch the cut, if the endmill shows excessive signs of wear swap to a fresh one.

    Slow feed/speed when you get to the previous drilled areas to lessen the damage against the WH surfaces. Use a quality AlTiN or similar coated tool, and check with the manufacturer about whether to use an air blast rather than coolant.

    When you get one side done, flip and finish the second side through. For finishing, I'd want to use an undersize endmill at full depth so that you're not rubbing on the "conventional" side, and maybe use a six flute tool meant for die finishing so you can get a rigid core. Anyone make a 9mm six fluter?

    Did you check the condition of the HSS drill you used for the pilot holes? Did one drill do them all?

  6. #5
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    536
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    291

    Default

    I sharpened the drill before I started and it drilled all the holes without sharpening. Whats weird is the first hole was just as worked hardened as the last one. I actually plunged a 3/8 carbide endmill in all the holes to try and get rid of the hard edge but the hard edge extends out past the reach of the 3/8 endmill. I could step over .100 on all the holes and plunge mill to get rid of the hard edge and then try to mill the slots after that. I could flip it over after going going half way through but it would be hard to get set up since the plate is only burned out on the outside edges. I could indicate one of the holes though and keep the same side against the solid jaw of the vise.

  7. #6
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,299
    Post Thanks / Like
    Likes (Given)
    1158
    Likes (Received)
    2340

    Default

    Quote Originally Posted by cuttergrinder View Post
    I had a little job today where I needed to slot some ar400 plate. It is basically a rectangular plate with 27 slots 3/8" wide by 2 1/2" long. It resembles a floor drain plate but I'm sure that is not what its for. The plate is 3/4" thick and the slots go all the way through. I thought the endmill would have trouble plunging this ar400 so I drilled the end of all the slots. Then I tried to mill the slots with a 5/16 carbide endmill and then I was going to finish with a 3/8" endmill. I tried a .100" depth of cut at 12 in/min and 3000 rpms. That quickly broke a cutter. Then I tried .075" depth of cut and slower feed. Still broke a cutter after about 2 slots. I had the best luck with 1400 rpm and 3 in/min feed. I still can only get about 3 slots before the cutter breaks. I gave up and need help. Lol What seems to be the problem is that the edges of the holes that I drilled are work hardened. I plunge into the drilled hole and it makes noise when it starts to mill longitudinally until it gets through the hardened edge of the hole. I drilled the holes with a 11/32 high speed drill but for some reason it work hardened the edges of the hole. By the time I get one slot milled out the last .100 of the endmill is about toast. Any help would be appreciated. We might end up getting the slots water jetted.
    In the Green part you are running 225 SFM, then you slowed down to 1400 RPM which is still 114 SFM. I would run around 45 SFM with a carbide Endmill....so 550 RPM with a .3125" Endmill, similar chipload though, so the change would be about 2 IPM at 550 RPM. AR400 is a nightmare to work with. If you can generate the holes you're doing okay, but Drills are tough tools, Endmills aren't.

    R

  8. #7
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    142
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    28

    Default

    I often work with AR500 and 46100E (hence the name hardplates). Troicoidal, adaptive, profit milling, high speed machining or whatever you want to call it is your friend here. I am rather conservative with my radial engagement and would start around .005-.010" and take the depth in 2 separate wacks. But I would run 300-500 fpm and start around a .001" per tooth feed. 400 is a good bit softer than 500, no fancy endmills needed, just quality carbide works for me. Also if your predrilled hole are still giving you trouble you can take 1 pass around them conventional milling to help get under the work hardening.

    Take a look at some hardmilling speeds and feeds online. This isn't what "I" would call hardmilling but it can help to show you what direction to head it with speeds and feeds.


    Paul

  9. #8
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    536
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    291

    Default

    Thanks guys for all the help. Does anyone know roughly how much it would cost to water jet these slots. I have no idea if it would take an hour or 24 hours.

  10. #9
    Join Date
    Jan 2013
    Location
    Plainfield, Indiana, USA
    Posts
    1,714
    Post Thanks / Like
    Likes (Given)
    1289
    Likes (Received)
    914

    Default

    Quote Originally Posted by Hardplates View Post
    I often work with AR500 and 46100E (hence the name hardplates). Troicoidal, adaptive, profit milling, high speed machining or whatever you want to call it is your friend here. I am rather conservative with my radial engagement and would start around .005-.010" and take the depth in 2 separate wacks. But I would run 300-500 fpm and start around a .001" per tooth feed. 400 is a good bit softer than 500, no fancy endmills needed, just quality carbide works for me. Also if your predrilled hole are still giving you trouble you can take 1 pass around them conventional milling to help get under the work hardening.

    Take a look at some hardmilling speeds and feeds online. This isn't what "I" would call hardmilling but it can help to show you what direction to head it with speeds and feeds.


    Paul
    I don't understand your description, please elaborate. 5 to 10 thou radial cuts, in a slot, depth 3/8".

  11. #10
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,608
    Post Thanks / Like
    Likes (Given)
    10188
    Likes (Received)
    3049

    Default

    Quote Originally Posted by Red James View Post
    I don't understand your description, please elaborate. 5 to 10 thou radial cuts, in a slot, depth 3/8".

    Trochoidal slotting... Low radial engagement, higher SFM, higher feedrates... Death by a thousand cuts, basically.. Like this:

    YouTube

  12. #11
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    142
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    28

    Default

    Quote Originally Posted by TeachMePlease View Post
    Trochoidal slotting... Low radial engagement, higher SFM, higher feedrates... Death by a thousand cuts, basically.. Like this:

    YouTube

    Exactly

    Goes without says you need to use a cutter smaller than the slot.



    I don't know about waterjet but on my plasma table I would charge $0.20 a pierce and $0.15 an inch. Waterjets have a higher operating cost and are much much slower so maybe that might help you guess pricing....

  13. #12
    Join Date
    Dec 2012
    Location
    OHIO
    Posts
    249
    Post Thanks / Like
    Likes (Given)
    232
    Likes (Received)
    203

    Default

    What are you machining these on? Try something similar to garr vrx , 9/32 x 7/16 LOC to rough with. Machine slot using a trochoidal type path in 2 passes at about .4 doc, offset second pass about .01 from first to avoid shanking out. Finish slot with 9/32 or 5/16 x 13/16 loc.

  14. Likes Hardplates liked this post
  15. #13
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    536
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    291

    Default

    Im running this on a mazak vtc 16. Unfortunately i have no way to generate code for a trochoidal tool path.

  16. #14
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    7,004
    Post Thanks / Like
    Likes (Given)
    1651
    Likes (Received)
    4826

    Default

    Quote Originally Posted by cuttergrinder View Post
    Im running this on a mazak vtc 16. Unfortunately i have no way to generate code for a trochoidal tool path.
    No CAM? Time to download and try out Fusion...

    Can you draw in CAD? Try a repeated "C" shape, with the curve of the C in the direction of travel, and spaced about .007-.010 one to the next. Then map out coordinates with whatever offset needed for the tool diameter you're using.

  17. #15
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    142
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    28

    Default

    Quote Originally Posted by Milland View Post
    No CAM? Time to download and try out Fusion...

    Can you draw in CAD? Try a repeated "C" shape, with the curve of the C in the direction of travel, and spaced about .007-.010 one to the next. Then map out coordinates with whatever offset needed for the tool diameter you're using.

    I was thinking the exact same thing! A small straight slot shouldn't be to difficult to hand write trochoidal(ish) G-code, a pain yes but can definitely be done. Probably quicker and easier to just try Fusion though.

  18. #16
    Join Date
    Jun 2012
    Location
    Davis Junction, Illinois
    Posts
    149
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    22

    Default

    Are you getting the chips evacuated and out of the way? Cutting dry with air blast is preferred. I would straight slot it with the 3/8 end mill. Depth of cut will be limited, as the slot depth is twice the cutter diameter. 90% of my work is 400-500 wear steels. 400 should machine well at 300+SFM. Make sure you are not pausing in the cut anywhere, especially if you are manually programming. Is this a quality brand name tool, or some MSC garbage?

  19. #17
    Join Date
    Dec 2007
    Location
    Idaho Falls
    Posts
    59
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    10

    Default

    I am going out on a limb here but a good solid carbide roughing corncob style endmill with moderate helix with enough cut length is what I would use for roughing. Many companies make them Niagara SR420 style are pretty good.

    Drop in your predrilled hole and cut adjust your feed to not just break off the endmill cutting full depth.

    An advantage of going all the way through on the first cut is a place for the chips to go.

  20. #18
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    536
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    291

    Default

    I do have an old version of bobcad but it doesnt do any high speed tool paths. I could draw c shapes but that would be a pain.

  21. #19
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    130
    Post Thanks / Like
    Likes (Given)
    92
    Likes (Received)
    19

    Default

    http://protoolkft.hu/sgs/katalog/4.pdf

    Page 13 SGS Z-CARB HTA™ SERIES ZH1CR

    Page 17 has the recommend feeds and speeds for different methods of milling

  22. #20
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,509
    Post Thanks / Like
    Likes (Given)
    4108
    Likes (Received)
    2670

    Default

    AR is a tough material.. speed is NOT your friend with this stuff.


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
  •