Side lock or ER holder?
Largest Manufacturing Technology
Community On The Web
Close
Login to Your Account

Page 1 of 4 123 ... LastLast
Results 1 to 20 of 76
  1. #1
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    2,925
    Post Thanks / Like
    Likes (Given)
    429
    Likes (Received)
    889

    Default Side lock or ER holder?

    Having problems with a carbide 1/2" 3 flute x 2.0" EM slipping down when heavy profiling in 6061. The EM is only cutting to 1.6" deep so its choked up in the holder and a flat wouldn't be of use.

    Without much experience using larger ER holders with end mills, I would guess that it would provide better holding power but would like to hear from experienced users.

  2. #2
    Join Date
    Mar 2009
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    8,357
    Post Thanks / Like
    Likes (Given)
    5725
    Likes (Received)
    10067

    Default

    What about a hydraulic chuck or milling chuck?

  3. #3
    Join Date
    May 2012
    Location
    pennsylviana, usa
    Posts
    714
    Post Thanks / Like
    Likes (Given)
    159
    Likes (Received)
    185

    Default

    I don't see why a ER-32 collet would not work. Don't know of many 1/2 endmills with a flat on the side, so I would go with ER-32.

  4. #4
    Join Date
    Jan 2006
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    1,394
    Post Thanks / Like
    Likes (Given)
    470
    Likes (Received)
    606

    Default

    I would(have) grind my own locking flat and use an em holder. IME I've had less problems with pullout & chatter using solid em holders.

  5. Likes dstryr, Red eye, jdj liked this post
  6. #5
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,063
    Post Thanks / Like
    Likes (Given)
    2786
    Likes (Received)
    2100

    Default

    Quote Originally Posted by Captdave View Post
    Having problems with a carbide 1/2" 3 flute x 2.0" EM slipping down when heavy profiling in 6061. The EM is only cutting to 1.6" deep so its choked up in the holder and a flat wouldn't be of use.

    Without much experience using larger ER holders with end mills, I would guess that it would provide better holding power but would like to hear from experienced users.
    Sidelock with flat. I'd even go as far to grab a roughing endmill from either Destiny or Maritool for the job. Less side pressure. Lots of companies sell endmills with flats for aluminum.

  7. Likes jdj liked this post
  8. #6
    Join Date
    Jun 2006
    Location
    Huntsville Alabama
    Posts
    1,757
    Post Thanks / Like
    Likes (Given)
    1007
    Likes (Received)
    661

    Default

    An ER-32 takes some pretty serious tightening torque on the nut to really hold on. I do my roughing and profiling with an er-32 and 1/2 EM all the time with no problems. A side-lock holder isn't gonna give you the same low run-out as a quality ER....

    Try really bearing down on the ER nut (within spec anyways)

  9. #7
    Join Date
    Feb 2004
    Location
    Napa, CA
    Posts
    2,532
    Post Thanks / Like
    Likes (Given)
    41
    Likes (Received)
    656

    Default

    I found this article to be informative. Rego Fix invented and owns the patents on ER collets, hopefully they know. I de-grease/oil the collet ID and tool shank with some non-residue cleaner too. After pulling a 5/8 EM out of an ER-32, I started following those directions and haven't had any more trouble. Depending on the manufacturer, the torque for an ER 32 is supposed to be 80 - 100 ft lbs. That can be reasonably estimated as "as tight as I can possibly make it" with the short whimpy wrenches usually supplied.

  10. #8
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    5,103
    Post Thanks / Like
    Likes (Given)
    641
    Likes (Received)
    1008

    Default

    When using solid carbide end mills the runout is a key factor in tool wear. Using a hydraulic milling chuck or shrink fit holders minimizes runout, and holds with much higher grip than any ER collets.

  11. Likes thermite, 1cncmachinist liked this post
  12. #9
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,045
    Post Thanks / Like
    Likes (Given)
    80
    Likes (Received)
    366

    Default

    I think many people misunderstood.
    OP is using. A side setscrew holder on an endmill that is chucked deeper than it should.
    so the screw is pushing against the cylindrical portion of the tool. Hence the tool is pulling out of the holder.

    Simplest solution is to grind a new flat on the shank.

    Or use a collet.

    Sometimes i put a 3/4 3fl hi-helix end mill into a ER32.
    I acrually grease the threads and collet-nut interface to get as much grip as possible and use a propper 1foot wrench.

    Never had anything slip out of that.

  13. Likes John_B liked this post
  14. #10
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    9,682
    Post Thanks / Like
    Likes (Given)
    29
    Likes (Received)
    7164

    Default

    I can't believe this works at all...

    Most carbide end mills made for aluminum do not have flats. This is because they run at high RPMs and balance is key. You should be at 8000 RPM or more for a .5" end mill. I've never had much luck running Weldon holders over about 6000 RPM.

    If this is HSS, I suppose you can grind in a flat.

    Get an ER32 collet chuck. I've never had a tool move in one when properly torqued. I use tap collets, but even taps never spin in regular collets in my experience.

  15. Likes BobWarfield liked this post
  16. #11
    Join Date
    Nov 2004
    Location
    Sutter Buttes / California
    Posts
    418
    Post Thanks / Like
    Likes (Given)
    245
    Likes (Received)
    32

    Default

    Collet and holder quality play a big role in gripping your tools properly. Which ever route you choose make damn sure it's quality tooling, hence "QUALITY"

  17. #12
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,063
    Post Thanks / Like
    Likes (Given)
    2786
    Likes (Received)
    2100

    Default

    Quote Originally Posted by ewlsey View Post
    I can't believe this works at all...

    Most carbide end mills made for aluminum do not have flats. This is because they run at high RPMs and balance is key. You should be at 8000 RPM or more for a .5" end mill. I've never had much luck running Weldon holders over about 6000 RPM.

    If this is HSS, I suppose you can grind in a flat.

    Get an ER32 collet chuck. I've never had a tool move in one when properly torqued. I use tap collets, but even taps never spin in regular collets in my experience.
    Good endmill holders get the run out down to less than .0003-.0004. Good enough for roughing IMHO.

  18. Likes jdj liked this post
  19. #13
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,045
    Post Thanks / Like
    Likes (Given)
    80
    Likes (Received)
    366

    Default

    Quote Originally Posted by dstryr View Post
    Good endmill holders get the run out down to less than .0003-.0004. Good enough for roughing IMHO.
    Oh yeah a 2" long 1/2 hi-helix EM will deflect 5 thou no problem.. so even a 1 thou runout will not screw things up too much...
    I personally like to use weldon holders for roughing- they have smaller nose dia on the end and also there is usually a 1/2" 45deg champfer that lets you chuck deeper and gives better clearance than said ER32

  20. #14
    Join Date
    Jun 2006
    Location
    Munich / Germany
    Posts
    2,338
    Post Thanks / Like
    Likes (Given)
    342
    Likes (Received)
    1062

    Default

    I find this article very interesting.
    Along with the torques, it talks about static and dynamic stiffness.


    Nick

  21. #15
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    2,925
    Post Thanks / Like
    Likes (Given)
    429
    Likes (Received)
    889

    Default

    I'm using a 1/2" x 2" 3 flt rough/finish EM from Lakeshore at 8,000 RPM (the sweet spot for torque) at 125 IPM 25% step over and 1.6" LOC with the tool as far up in the holder as possible.

    I'll be running this job again next week so I'll try a few of the suggestions.

  22. #16
    Join Date
    Mar 2006
    Location
    Northern California
    Posts
    529
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    12

    Default

    Quote Originally Posted by zero_divide View Post
    Oh yeah a 2" long 1/2 hi-helix EM will deflect 5 thou no problem.. so even a 1 thou runout will not screw things up too much...
    Yeah, it is possible to run it so it deflects 5 thou, that's no problem. But doing so leads to two major sources of problems:

    First, it is heck on the tool life. It isn't hard to see that applying the repetitive stress hammer to the tool enough to make it bend 5 thou thousands of times a second can't be helpful for the tool life. But hey, forget that visual. With tooling manufacturer's saying you can lose 10% of tool life for every tenth of runout, viewing a thousandth as no big deal is one thing but adding another 5 thou to that is asking for trouble.

    Second, it is an open invitation to chatter. Tool deflection is a major cause of chatter. When the tool deflects, that leaves a "bump" that subsequent flutes travel over creating a periodic change in cutting force and depth of cut. That is the resonant vibration that is chatter.

    Tooling manufacturers recommend keeping deflection under 0.001" to avoid chatter, and that's why that limit was chosen in G-Wizard. Above 0.001" of deflection, it's only a question of whether you're running at a spindle rpm that happens to be resonant with the chatter.

    Cheers,

    BW
    CNC Machinist Cookbook: Software and Information

  23. #17
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,045
    Post Thanks / Like
    Likes (Given)
    80
    Likes (Received)
    366

    Default

    Quote Originally Posted by BobWarfield View Post
    Yeah, it is possible to run it so it deflects 5 thou, that's no problem. But doing so leads to two major sources of problems:

    First, it is heck on the tool life. It isn't hard to see that applying the repetitive stress hammer to the tool enough to make it bend 5 thou thousands of times a second can't be helpful for the tool life. But hey, forget that visual. With tooling manufacturer's saying you can lose 10% of tool life for every tenth of runout, viewing a thousandth as no big deal is one thing but adding another 5 thou to that is asking for trouble.

    Second, it is an open invitation to chatter. Tool deflection is a major cause of chatter. When the tool deflects, that leaves a "bump" that subsequent flutes travel over creating a periodic change in cutting force and depth of cut. That is the resonant vibration that is chatter.

    Tooling manufacturers recommend keeping deflection under 0.001" to avoid chatter, and that's why that limit was chosen in G-Wizard. Above 0.001" of deflection, it's only a question of whether you're running at a spindle rpm that happens to be resonant with the chatter.

    Cheers,

    BW
    CNC Machinist Cookbook: Software and Information
    Well. Tool deflection is a part of machining process.
    The guy is running his EM at 8000RPM and 120 IPM daking 1.6DOC and .125 WOC.

    I would bet that 1/2" 3Fl 2" long EM is gonna deflect ATLEAST 5 thou anyway.
    Yesterday i ran Niagara HPEM with same parameters but 1.375" DOC, 0.05" WOC at 10000 RPM and 280IPM, here is a link if anyone is interested.
    So at the bottom pocket ended up being around 3 thou per side smaller than on top.
    Keeping deflection under 1 thou is nice but this means keeping your cuts waay below what your tool and machine can handle (talking about production equipment here)

    EDIT:
    Captdave,
    You got nice MRR- 26 in^3, mine was slightly lower only 20

  24. Likes NTM liked this post
  25. #18
    Join Date
    Jul 2006
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    4,323
    Post Thanks / Like
    Likes (Given)
    17118
    Likes (Received)
    3994

    Default

    Quote Originally Posted by John Welden View Post
    What about a hydraulic chuck or milling chuck?
    Very sturdy indeed.

    Nobody has mentioned the TG (tremendous grip) series collets yet. They are the middle ground between an ER (extended range) collet and the hydraulic chuck, milling chuck, or shrink fit holders.

    The shallower taper of the TG collets gives then much more clamping force than an ER collet, but have limited clamping diameter range on each collet size.

  26. Likes cnctoolcat liked this post
  27. #19
    Join Date
    Dec 2008
    Location
    W V USA
    Posts
    450
    Post Thanks / Like
    Likes (Given)
    329
    Likes (Received)
    120

    Default

    Quote Originally Posted by swarf_rat View Post
    I found this article to be informative. Rego Fix invented and owns the patents on ER collets, hopefully they know. I de-grease/oil the collet ID and tool shank with some non-residue cleaner too. After pulling a 5/8 EM out of an ER-32, I started following those directions and haven't had any more trouble. Depending on the manufacturer, the torque for an ER 32 is supposed to be 80 - 100 ft lbs. That can be reasonably estimated as "as tight as I can possibly make it" with the short whimpy wrenches usually supplied.

    80 to 100 ft lbs as i remember is quite a good pull on a 2ft long 1/2 drive Mac torque wrench, not sure if
    the short wrenches will get you near it but it might be interesting to check just how much the factory wrench
    can put on it with a normal pull.

  28. #20
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    2,925
    Post Thanks / Like
    Likes (Given)
    429
    Likes (Received)
    889

    Default

    Its milling some really deep lobes with a HSM pocking op so its not a constant engagement where the spindle load settles down at a given point but I'll bet its near or at 100% power maybe slightly over.

    The lobes get a dedicated finish tool afterwards so any deflection is removed, just need to get them roughed quickly. I do like Lake shores rough/finish tools as they break up the chips well so less change of re-cutting a big thick chip and breaking the tool and fewer time cleaning the machine out.

  29. Likes jdj liked this post

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
  •