Enormous HSS end mills; best way to use them?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 29
  1. #1
    Join Date
    Jan 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    167
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    90

    Question Enormous HSS end mills; best way to use them?

    Hi,

    I have a few parts to make with deep side walls without step down lines. I have mainly been using 3/4 3 flute ZrN carbide endmills in side locks, and I also have a 1x3" 3 flute ZrN finisher which is now chipped mid-flute. I bought a huge HSS endmill with 6 flutes, it has a 1-1/4 shank diameter with flats and a 1.5" cutting diameter with a 6" LOC. I'll be holding it in a Maritool 1-1/4 dual contact sidelock in a CAT40 VMC. Total gauge length with be around 8.5 inches I think.

    What range of cutting speeds, feeds, WOCs and DOCs should I be looking at for a tool like this? Some of my parts have 3, 4, and 6 inch side walls that I want flat and square. If I can get these side walls done in the first operation, I can use them as reference surfaces to hold them in the vises for the remaining operations on other sides. If they aren't square they may not be stable to hold in the vises, and I don't want a part to move in the vise jaws when I'm taking heavy cuts.

    tha-biggun.jpg

  2. #2
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    3,772
    Post Thanks / Like
    Likes (Given)
    4083
    Likes (Received)
    1905

    Default

    They make pretty good paperweights and doorstops.

    Seemed really difficult to get straight anything with HSS endmills. They are like a wet noodle compared to carbide. They can remove material, but they deflect a lot. Inside corners suck.

  3. Likes Jashley73, gregormarwick liked this post
  4. #3
    Join Date
    Feb 2009
    Location
    Midwestern MN/Wi USA
    Posts
    1,295
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    350

    Default

    They were the go to choice in the 60s through the 90s for deep pockets and thin wall profiles. You know you have earned your man card when your finishing a long edge cranking one of these in an R8 adaptor on the bridgeport. It is how shit got done

  5. Likes sfriedberg liked this post
  6. #4
    Join Date
    May 2005
    Location
    CA
    Posts
    1,070
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    247

    Default

    My gut feeling is that it may be easier to get the deep wall really flat by using a reduced shank end mill and just stepping/ramping/spiraling down (depending on the type of feature and what works best to hide the lines between passes).

    PM

  7. #5
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    5,876
    Post Thanks / Like
    Likes (Given)
    1395
    Likes (Received)
    4068

    Default

    Good points already made, but in addition the relative low stiffness of the Haas mill, and the long stickout of tool and holder will just make things worse as far as cutting true and cleanly down a long sidewall.

    I'd also recommend a mostly solid necked 3/4" carbide endmill for your needs, as well as a cutting path that makes multiple finish passes at different heights to blend in each pass as best as possible, which will also minimize deflection and give truer (but not dead-true) wall perpendicularity.

    A shorty holder will also help, anything to minimize the lever arm. Just make sure it's tight, having the tool pull from the collet is annoying...

  8. #6
    Join Date
    Nov 2004
    Location
    RC, CA
    Posts
    1,935
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    360

    Default

    Enormous HSS endmill requires an enormous low speed milling machine.

  9. #7
    Join Date
    Jan 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    167
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    90

    Default

    It's a Doosan DNM 5700. I do have a 1/2" reduced shank carbide 3 flute ZrN from Maritool but the thing deflects a ton, the obvious reason being that the shank is like 12mm and the thing is sticking out of an SK16 holder over 4 inches. my normal strategy is to use the 3/4 rougher/corncob and leave a few thousandths for the 3/4 or 1" finisher. This has allowed me to get side tapers less than 0.001" over the entire length of the endmill. Bending stiffness goes up with the 4th power of diameter, so in theory a 1.5" EM should be about 81 times more rigid than a 0.5" EM.

    I figure this new huge endmill will have only a tiny amount of flex because it's 1.5" diameter, and most of the deflection will be within the holder, taper, ect.

    Speedie, I have done exactly that on an R8 bridgeport type machine. I'm hoping that by taking light cuts in 6061 I can make this work.

  10. #8
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    13,182
    Post Thanks / Like
    Likes (Given)
    1980
    Likes (Received)
    3165

    Default

    I didn't see material specified, did I miss it? For mild steel, 50 FPM, for 6061, 300 FPM. For tougher material, look for another way. Feed will be controlled by machine stability. Getting a straight and parallel finished wall will be a challenge as described above.

    Edit - took too long to type.

  11. #9
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,066
    Post Thanks / Like
    Likes (Given)
    371
    Likes (Received)
    1429

    Default

    I've run a lot of 1-1/2x6 and 2x8 endmills in steel and 15-5/Ti.

    But never in a 40 taper machine! I'd call that pushing the envelope a bit.

    For roughing steel, I always used the TIN coated fine tooth corncobs, if it's PH or Ti I like Crescutters.

    SFM is just the normal SFM. Chipload is gonna depend on the cut. Roughing out a deep pocket, you have a chip problem- you gotta blast them out of there somehow. I usually like to break in the cutter with a reduced feedrate when it's new, they can be pretty chirpy when they are sharp. After a few minutes, I'll bump it up gently till I'm at 100%.

    I'd look at something like a coromill for roughing- something that can ramp and race around the part with higher speed and lower tool pressure. Then a finish and spring pass with the end mill.

    Rigidity with a 1-1/2x6 is like a 1/2x2- not great, and worse with a reduced shank cutter. If I'm gonna run a long 1-1/2" end mill, I want it to have a 1-1/2" shank...

  12. Likes sfriedberg liked this post
  13. #10
    Join Date
    Jan 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    167
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    90

    Default

    I should clarify that this long end mill only has one purpose; final skim cuts on square perimeters with rounded corners. There are no inside corners or pockets (although I may try it on a large ID bore). I'll be doing most metal removal with a shear hog T slot cutter and/or the carbide end mills mentioned before.

    This tool is strictly for getting flat walls on the perimeter of the parts without having step down marks. I suppose the best way would be a dual column mill with HSK-125 spindle holding a 1.5" carbide endmill in a shrink fit holder, but I don't have that.

    EDIT: I'm sort of hoping the small amount of TIR from the side-lock holder against the HSS set screw shaft will cancel out the deflection taper a little. Like, the end of the mill will have enough runout that it will effectively be a larger diameter than the top, and this larger diameter will over cut the side wall. I'll post back with results when I have them.

  14. #11
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,066
    Post Thanks / Like
    Likes (Given)
    371
    Likes (Received)
    1429

    Default

    Quote Originally Posted by Generic Default View Post
    This tool is strictly for getting flat walls on the perimeter of the parts without having step down marks.
    You're talking about aluminum, maybe .005" finish allowance- once around and a spring pass if needed. That's not really pushing things that hard, just check your runout before you start.

    I don't think you're gaining anything by the 1-1/2" diameter though. It's not much stiffer than a 1-1/4" and the tool pressure is higher. A little more core cross-section with the 1-1/2 I guess...

    But overall I don't really see a problem- it's just a finish cut.

  15. #12
    Join Date
    Feb 2014
    Location
    United States
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    4

    Default

    A 2 or 3 inch indexable shoulder mill with a long holder is tough to beat for squareness and surface finish when you're sticking it out that far in a 40-taper machine.

    It takes a fair number of step-downs to finish a surface, but they can be done at a fairly high feed rate (thanks to chip thinning), and it doesn't leave steps that you can feel, like a relieved solid endmil tends to.

    Sent from my SM-G965U1 using Tapatalk

  16. Likes jancollc liked this post
  17. #13
    Join Date
    Feb 2008
    Location
    Mishawaka, IN
    Posts
    302
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    67

    Default

    I only use mills like that in a Cat 50 machine; but I suppose a final skim pass application may be feasible. I definitely would not be pushing it in Cat 40 or less.

    Post again once you have done this.

  18. #14
    Join Date
    Nov 2011
    Location
    CANADA
    Posts
    526
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    163

    Default

    Funny everyone suggests another way to do it when the guy just wants help to use the cutters he has.... It's been a real long time but we used to clean insert pockets up with similar end mills. Usually a cat 50 machine, but as long as it runs true a cat 40 would get by most likely. I'm guessing to leave .005" for a final pass and maybe in the 300rpm range and 10in/min..

  19. #15
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,113
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    422

    Default

    Do a couple of cuts at final depth to see what kind of WOC and cutting direction will yield acceptable finish and straightness.

  20. #16
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    13
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    2

    Default

    Fine cut in aluminum with big uncoated HSS end mill, 38mm tool, 150mm length? I use similar tools for plastic and aluminum at my job.

    Lots of coolant, of course.

    I'm Swede so I use metric. As a starting value I'd use Vc70 and F0.025-0.035; WOC in the ballpark of 1mm (0.04in), smaller for better finish but no lower than 0.5.

    So: Full depth of cut. 600rpm F90-120mm/min. (3.5-4.7ipm.)

    This would count as very conservative but should get the job done. Remember the tool must not scream. Go from here and see what you can get away with. You could go faster for sure but it depends on your machine, your vise, your...

  21. #17
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,670
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2508

    Default

    Quote Originally Posted by Generic Default View Post
    Hi,

    I have a few parts to make with deep side walls without step down lines. I have mainly been using 3/4 3 flute ZrN carbide endmills in side locks, and I also have a 1x3" 3 flute ZrN finisher which is now chipped mid-flute. I bought a huge HSS endmill with 6 flutes, it has a 1-1/4 shank diameter with flats and a 1.5" cutting diameter with a 6" LOC. I'll be holding it in a Maritool 1-1/4 dual contact sidelock in a CAT40 VMC. Total gauge length with be around 8.5 inches I think.

    What range of cutting speeds, feeds, WOCs and DOCs should I be looking at for a tool like this? Some of my parts have 3, 4, and 6 inch side walls that I want flat and square. If I can get these side walls done in the first operation, I can use them as reference surfaces to hold them in the vises for the remaining operations on other sides. If they aren't square they may not be stable to hold in the vises, and I don't want a part to move in the vise jaws when I'm taking heavy cuts.

    tha-biggun.jpg
    .
    1) length to dia ratio is the most important factor. a 2" dia endmill with 12" of flute deflects 2x2x2= 8x more than a 6" long flute end mill.
    .
    2) runout can be a lot not unusual to see .020" dia difference runout.
    .
    3) usually manufacturer has a chart for slotting and for side milling giving sfpm and ipt. often the depth and or width of cut is adjusted. if end mill making a clicking noise it aint good. not unusual to have 12" long flute 2" dia end mills cost $800. to $1600. usually i dont push the longer mills hard as they are expensive when they break.
    .
    4) if spindle out of tram alignment or leaning obviously it will effect perpendicularity. as well a deflection effect perpendicularity.

  22. #18
    Join Date
    Aug 2006
    Location
    Wisconsin
    Posts
    1,570
    Post Thanks / Like
    Likes (Given)
    687
    Likes (Received)
    654

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    2) runout can be a lot not unusual to see .020" dia difference runout.
    Please tell me you missed a zero in there.

  23. Likes mhajicek liked this post
  24. #19
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,670
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2508

    Default

    Quote Originally Posted by 5 axis Fidia guy View Post
    Please tell me you missed a zero in there.
    .
    and how many thousands of tools in tool holders 12 to 22 inch long have you measured for actual assembled together runout ?? with a optic tool setter the tool is checked everytime and all the flutes are checked to get the max diameter.
    .
    sure i send the worst tool holders out to get the taper reground. to determine a tolerance you need to establish a average of many thousands of tools and need to establish what limit causes actual tooling problems.
    .
    and of course not all mills are sharpened with low runout. you can have perfect tool holder and still get runout cause its coming from the tool

  25. #20
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    594
    Post Thanks / Like
    Likes (Given)
    473
    Likes (Received)
    304

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    and how many thousands of tools in tool holders 12 to 22 inch long have you measured for actual assembled together runout ??
    OPs tool is 8.5" gauge length, not 22". I might expect to see up to .005" in a cheap or reground endmill in a beat up holder. For my stuff if there's more than a couple tenths that raises a red flag.


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
  •  
2