316 pocket milling help
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    380
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    104

    Default 316 pocket milling help

    hey all, need some recommendations on endmills and speeds/feeds

    the job is 316 plate
    pocket depth is .277
    part is 4"x18X with some islands in the middle

    right now im running a garr vrx 4 flute stub at 2000 rpm and 15ipm

    Im only getting 4 or 5 parts from the endmill...the flutes are all chipped above the end then it finally looses a flute or two


    im ramping down at 1.5 degree angle to the full .277 depth
    any ideas?

    thanks

  2. #2
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    4,749
    Post Thanks / Like
    Likes (Given)
    1067
    Likes (Received)
    3265

    Default

    What's your stepover? And does it do a full width initial cut at the final depth? If you're using a narrow stepover but hitting the first cuts full, may want to use a small pocket program where you're stepping down until you can start the stepover cuts.

    I'm not a fan of Garr endmills, I've had a sense that their carbide is more brittle than others I've used. Not sure if that's a fair assessment, just my impression.

  3. #3
    Join Date
    Aug 2012
    Location
    Gurnee ILL. USA
    Posts
    390
    Post Thanks / Like
    Likes (Given)
    109
    Likes (Received)
    97

    Default

    Get yourself some IMCO end mills, when ordering them ask them what they recommend and I will bet you will LOVE these end mills.

  4. #4
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    4,749
    Post Thanks / Like
    Likes (Given)
    1067
    Likes (Received)
    3265

    Default

    The other thing I'd recommend is using stub length endmills, and as short a toolholder projection as you can. If using a collet holder, make sure it's in good shape, and a larger series so you can be sure it's gripping well.

    Are you using flood coolant? May want to confirm with whoever makes the endmills that it's not a thermal stress issue.

    This is presupposing that the mill is a proper 40 taper VMC in good shape, and you're not trying to do this on a converted Bridgeport...

  5. #5
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    380
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    104

    Default

    cat 40 okuma mill..very rigid machine, im using flood coolant to get the chips out of the pocket. everything is stubbed up.
    stepover is .100
    there is only about 10 inches where is doing a "full slot" everything else is peripheral

    ive tried imco...not very good imho

    i got my tool rep looking again, but it seems this company pushes garr products. everytime i need something he brings the garr rep along with him..like jeez ive gone thru the garr book a hundred times already

    I would have likes to do trochoidal cuts but i cant fit it in the memory

  6. #6
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    4,749
    Post Thanks / Like
    Likes (Given)
    1067
    Likes (Received)
    3265

    Default

    Try reprogramming the full width cut to a series of steps, maybe three. I would also consider the SGS Z-Carbs, I did a fair amount of 17-4SS and Gr2 Ti with good results.

  7. #7
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,543
    Post Thanks / Like
    Likes (Given)
    12067
    Likes (Received)
    9682

    Default

    I might be blind.. But what is the diameter of the endmill????

  8. Likes steve-l, Mtndew liked this post
  9. #8
    Join Date
    May 2005
    Location
    Republic of Arizonia
    Posts
    1,446
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    381

    Default

    A Guess based on the part size....

    Probably 3/8”.........

    more then likely rubbing the part to size, instead of making a chip...

    15 / 2000 = .0075

    .0075 / 4 = .001875 per cutting edge.....

    If I’m using a carbide End Mill in 316.

    My preference is a 3 flute AlTiN coated for a lot of materials...

    And 160 SFM as a starting point for 316....

  10. Likes Mike C. liked this post
  11. #9
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    380
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    104

    Default

    Its a 1/2 endmill..forgot to mention that,

  12. Likes Mike C. liked this post
  13. #10
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,706
    Post Thanks / Like
    Likes (Given)
    3212
    Likes (Received)
    2142

    Default

    Go with a 5 or 6 flute bullnose, lighten up the depth of cut and go with substantially higher speeds and feeds.
    316 isn't bad,but it can be a p.i.t.a. at times.

  14. #11
    Join Date
    Feb 2018
    Country
    AUSTRALIA
    Posts
    45
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    2

    Default

    Quote Originally Posted by tay2daizzo8 View Post
    hey all, need some recommendations on endmills and speeds/feeds

    the job is 316 plate
    pocket depth is .277
    part is 4"x18X with some islands in the middle

    right now im running a garr vrx 4 flute stub at 2000 rpm and 15ipm

    Im only getting 4 or 5 parts from the endmill...the flutes are all chipped above the end then it finally looses a flute or two


    im ramping down at 1.5 degree angle to the full .277 depth
    any ideas?

    thanks
    I cut 316 plate which is 3mm in depth with either 3 or 4mm end mills quite often. (mostly 3mm)
    I profile out the parts, and only go as wide around it as the end mill itself.
    I bought some of the 3mm Imco M924 bits some time back for approx $20 USD each and ran them at speeds recommended by Imco on their site. So a 3mm end mill and 7000 rpm or so and 220mm per minute ramping down at 0.2mm max ,at a 2 degree angle to 3.01mm depth with a little tab to keep it in place with full flood coolant.
    My parts are approx 24mm long and 5mm high, so that cutter needs to cut 58mm in length or so to get around it each step.
    I am not in a job shop, so no hurry, but I got from those Imco mills 400 parts cut before the coating started to wear with very minimal wear on the diameter. Those mills are still usable though, for cutting with the full length on other parts and ROI on those plates was great.
    I do these parts all the time and I do not get chipped flutes at those speeds on any cutters I use, but those Imco M924 cutters are worth every cent.
    I have found that I no longer run it by ear, but start with the manufacturer recommended feeds and speeds in 316 every time. I did have a lot of mis drilled holes and drills breaking on those parts ( they have drilled holes as well) until I used the Sutton Tools feeds and speeds for their 1.8mm bits.
    They plunge in 225mm at 7500 rpm and I now get 800 holes a bit since I used that, where I was lucky to get 50 before one broke previously and that was plunging at 25mm! and with a spot drill to each hole, I no longer have any scrap as everything drills true.

    I ran Sandvick cutters in the same material and the results were the same, if I followed their recommended speeds and feeds, though their site is more complicated to get those and of course their cutters are quite a bit more to buy

    I would suggest buying one of those Imco cutters , as their prices are good and they have the correct info right there on their site.

  15. #12
    Join Date
    Dec 2009
    Location
    Louisiana
    Posts
    409
    Post Thanks / Like
    Likes (Given)
    136
    Likes (Received)
    217

    Default

    Abandon the ramp. You'll need 3 tools instead of one. First drill a hole at least 25% larger than the diameter if your endmill, .01 above the depth of your pocket. Drop into your drilled hole with a center cutting 3 flute end mill (slowly) .002 above the floor depth of your pocket and open up that drilled hole just enough to cut out the angle left by the drill point. The finally get in there with your standard 4 to 7 flute endmill to finish the job. I find with 316 all the damage is done when your tool gets into non-ideal cutting situations, 316 is very unforgiving.

  16. #13
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    380
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    104

    Default

    thanks everyone, i think im going to do what kingbob said, drill and plunge, should save my endmill some.
    3 flute in 316 tho? i got some new alumapower bright and shiny 3 fluters i guess i could give a try, but my feed would be reduced 25 percent.
    i am a job shop and right now im looking at a 3hr cycle(most of that is 44" of dovetail oring groove, which is another diaster all in itself)

  17. #14
    Join Date
    May 2005
    Location
    Republic of Arizonia
    Posts
    1,446
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    381

    Default

    So your still going with hardly any chip load at all?

  18. #15
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    380
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    104

    Default

    what do you suggest

  19. #16
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,543
    Post Thanks / Like
    Likes (Given)
    12067
    Likes (Received)
    9682

    Default

    Quote Originally Posted by JS View Post
    So your still going with hardly any chip load at all?
    I'm going to disagree with that... I know the "consensus" in Stainless is to FEED IT!!! FEED IT HARD!!
    or it'll work harden on you..

    Though if you go and look at ANY manufacturers feed and speed #'s, the stainless #'s are always the lightest feeds.

    Quite a few years ago, I had to mess with some A286, and for some reason I decided to call IMCO's tech line.. And he
    gave me some #s (lower feed per tooth than I thought) and we got talking about some other stuff I was working on..
    TONS of 13-8.. I was running a lot of 1/2" endmills.. .003 per tooth.. 100sfm would give me very good tool life,
    120 was the absolute tops, hit 130 and I might as well have just hit them with a hammer and tossed them in the scrap
    bucket..

    So, the recommendation was 200sfm... BUT only .0015 per tooth, on a 1/2".... Really??? REALLY!!! I ran out the rest of
    that 13-8, I had 2 1/2" endmills in there.. When the job was done, one had 24 hours on it, and one had 26.. And I could
    have put them back in the container and sold them as new... I was also able to run deeper, wider, and eliminate finish
    passes.. Lighter chip load, less tool pressure, I could dig much deeper and much wider, and double my surface speed.
    It sounded a LOT better too..

    When pulling a BIG THICK chip on a work hardening material.. You are trying to curl that chip, and it gets Freeken HARD..
    Its not the material you are going to be cutting you have to worry about, its the material you are trying to curl into the
    flute..

    Years ago there was an ad on the back MMS, I don't remember the brand, but it was a 304 cutting comparison.. If
    you actually looked at the #'s.. 1/2" endmill, in 304.. They had some competitor #'s and "their" #'s..
    The "WOO-HOO awesome" endmill was able to run deeper and faster, the difference?? they backed the
    feed WAY down to .0014 per tooth...

    I'm completely cool with less than .002" a tooth on a 1/2"er.

  20. #17
    Join Date
    May 2005
    Location
    Republic of Arizonia
    Posts
    1,446
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    381

    Default

    I would experiment and see how hard I could push the cutter.

    316ss less then 28 RHc

    full slot 190 sfm .0018 fpt

    heavy roughing 235 sfm .0023 fpt

    light roughing 305 sfm .0028 fpt

    finishing 390 sfm .0052 fpt


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
  •