Need advice milling deep slot.
Close
Login to Your Account
Results 1 to 14 of 14
  1. #1
    Join Date
    Jun 2009
    Location
    Clearwater, FL
    Posts
    121
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    14

    Default Need advice milling deep slot.

    I have a 6061 part with 2 slots, about 11mm wide and 5" deep. The slot ends up through. I am able to attack them from both sides, however there are other features next to them that require a minimum of 3.25" extension. I'm using a 3/8" endmill with a reduced neck and 1/2" for length. Not exactly the greatest set of requirements, but that's life.

    I've tried all sorts of different things. 

    Helicals MAP suggestions, HSM Advisor's suggestions, and everything in between. 1500-15000 rpm. I've held it in a lyndex SK10, and a VC13 holder. As of now I've got nothing but chatter, broken tools, and broken dreams. If anyone has any suggestions, I'd really appreciate it!!!

  2. #2
    Join Date
    Sep 2013
    Location
    PA
    Posts
    559
    Post Thanks / Like
    Likes (Given)
    271
    Likes (Received)
    435

    Default

    pre drill with as thin of a web as you can get away with. Use a tool with a corner radius to keep from blowing up your edge and finish the wall as you step down.

    I routinely mill slots 8-10X dia in 6061 and this works well for me.

    Is it a 3.25 extension or 3.25 gauge length?

  3. #3
    Join Date
    Jun 2009
    Location
    Clearwater, FL
    Posts
    121
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    14

    Default

    Quote Originally Posted by yoke View Post
    pre drill with as thin of a web as you can get away with. Use a tool with a corner radius to keep from blowing up your edge and finish the wall as you step down.

    I routinely mill slots 8-10X dia in 6061 and this works well for me.

    Is it a 3.25 extension or 3.25 gauge length?
    3.25 extended from the collet. Any suggestions on speeds/feeds and stepdown?

  4. #4
    Join Date
    Sep 2013
    Location
    PA
    Posts
    559
    Post Thanks / Like
    Likes (Given)
    271
    Likes (Received)
    435

    Default

    I use shrink fit holders which is probably a bit more rigid than your setup. Maybe?

    I would just sure the recommended feeds and depth of cut. Try to keep wall engagement as a constant so it isn't only hitting the web.

    You're around 8.6X diameter which is getting up there. You could try to plunge on the web left from pre drilling operation with your end mill to create some separation then go back and finish the wall with the endmill.

    I typically stick to .25 tools and under...

  5. Likes Vishrut liked this post
  6. #5
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    871
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    460

    Default

    What tool are you using? I have a few of these Reduced Shank 3/8 3 Flute End Mill Finisher 5.0 long X .354 Shank MariTool
    and typically use them at 2.1 or 3.1" stickout with good results. I'm only using an ER20 as well.

  7. #6
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,547
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    973

    Default

    Look at gw Shultz tools they make a cutter for ar15 mag wells that is reduce and ready to go. It works good
    Don


    Sent from my iPhone using Tapatalk Pro

  8. #7
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    3,348
    Post Thanks / Like
    Likes (Given)
    372
    Likes (Received)
    1908

    Default

    I used to mill pockets into the end of 6061 stock. The pockets were about 3.500 deep, I would drill a hole and program a bunch of plunges with an endmill...only way it could be done. Then machine the walls stepping down. Chatter is just a part of life with long thin cutters.

  9. Likes Shawnrs liked this post
  10. #8
    Join Date
    Jun 2009
    Location
    Clearwater, FL
    Posts
    121
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    14

    Default

    Quote Originally Posted by thesidetalker View Post
    What tool are you using? I have a few of these Reduced Shank 3/8 3 Flute End Mill Finisher 5.0 long X .354 Shank MariTool
    and typically use them at 2.1 or 3.1" stickout with good results. I'm only using an ER20 as well.
    It's a Helical 82480

    Helical Tool

  11. #9
    Join Date
    Jun 2009
    Location
    Clearwater, FL
    Posts
    121
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    14

    Default

    Quote Originally Posted by plastikdreams View Post
    I used to mill pockets into the end of 6061 stock. The pockets were about 3.500 deep, I would drill a hole and program a bunch of plunges with an endmill...only way it could be done. Then machine the walls stepping down. Chatter is just a part of life with long thin cutters.
    Any idea on S/F of the wall machining?

  12. #10
    Join Date
    Dec 2013
    Location
    India
    Posts
    215
    Post Thanks / Like
    Likes (Given)
    128
    Likes (Received)
    18

    Default

    As said earlier,
    1. Remove maximum stock with drilling.
    2. Plunge thin webs -- ask your tooling supplier for special "Plunging" geometry endmills.
    3. Finish the walls with reduced shank endmills.

  13. #11
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    3,348
    Post Thanks / Like
    Likes (Given)
    372
    Likes (Received)
    1908

    Default

    Quote Originally Posted by JBethell View Post
    Any idea on S/F of the wall machining?
    Not very good lol

  14. Likes Vishrut liked this post
  15. #12
    Join Date
    Jun 2009
    Location
    Clearwater, FL
    Posts
    121
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    14

    Default

    Quote Originally Posted by plastikdreams View Post
    Not very good lol
    Speeds/feeds, lol, not surface finish.

  16. #13
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,796
    Post Thanks / Like
    Likes (Given)
    16796
    Likes (Received)
    11993

    Default

    It has a 3/8" shank. Grind a little flat on it and stick it in a set screw holder.

    What machine are you doing this on.. Maybe its just a floppy POS to begin with..

    Here is some of my chatter stopping methods when working with long endmills.

    Looks like your endmill is a square corner, try something with a radius or a chamfer.
    Feel free to chamfer it yourself. Its not that hard, and if you have some practice,
    you can even put your own radiuses on. Sharp square corners on long endmills can
    get really grabby.

    Make the tool "MORE VARIABLE".. Seriously.. Just grind a big honking chamfer on one
    flute. It works, I've done it a bunch of times. I had one machine quite a while ago
    that would do it for me.. Shake, rattle, noisy.. Until a corner broke off, and then it
    cut clean.. Occasionally taking the cutter with it, so I started just taking new endmills,
    Vari flutes, with corner rads and just grinding a big chamfer on one flute. Floppy machine,
    FLOPPY!!! The X-Y was pretty stout, the spindle was the problem, and tool interface was
    shit. A series 10 Acroloc..

    RAMP!!! It puts pressure straight back up through your spindle. Sort of like how a high feed
    mill works, and why they can hang out a mile. You're taking that little bit of flex out of the
    Z axis.. You're making your machine and tool more rigid than it actually is.

    Those are my little tricks. Though one more thing. In my experience using long endmills,
    chatter happens when the tool doesn't have much to do. If it doesn't have much to do it
    bounces around and makes a lot of noise. Like an employee with a cell phone.. Keep it
    busy and it tends to be calmer and less noisy... Almost like a little kid.

    I've roughed out a pocket or an outside wall, and left a little more on the last step down.
    Keep the bottom of the tool busy on the finish, and the tool calmed right down.. Ran it
    faster and ran it harder..

    Lots of a little tricks, and essentially none of them have to do with slowing down
    the speed, or feeding it lighter. Occasionally that is the only answer, but what you
    are doing isn't that crazy.

    One last though. Only use the long tools when you need them. Go as deep as you can with
    a short one. Go deeper with a little longer one, and then waste the time with the long
    expensive endmill, only where you actually need it.

  17. Likes Vishrut liked this post
  18. #14
    Join Date
    Jun 2009
    Location
    Clearwater, FL
    Posts
    121
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    14

    Default

    Quote Originally Posted by Bobw View Post
    It has a 3/8" shank. Grind a little flat on it and stick it in a set screw holder.

    What machine are you doing this on.. Maybe its just a floppy POS to begin with..
    Thank you for the suggestions. The machine is a 2 year old Matsuura H.Plus-500, so I think the machine is fine. As far as the holder, I have a set screw holder on the way. Originally, I wasnt able to find one. It's a Cat50, in which we run all dual contact to keep the spindle face clean. We stick to lyndex and big kaiser if we can. However lyndex doesn't make a 3/8, and big kaiser's shortest is 6" gage length. Ended up finding a YG-1 holder which should be here tomorrow.

    Regarding the concept of cutting harder to get rid of chatter, generally, I agree that it's the way things go, although on these long reach tools, it always seems to make it worse when. I try it. Helical suggests something like a 7° ramp angle at max RPM which absolutely did not work. I'd love to see it done successfully, because I usually end up having to drop the SFM way down and keeping the chip load up when using long tools.

    As far as the radius, I couldn't find one with a radiused corner and enough of a reduced neck, and due to the production nature of the part, we try to keep tools "off the shelf" whenever possible for our automated ordering system. I only looked briefly for a radiused tool though since I got through the slot and need to get the first part out. Once that's done, I'll definitely be trying a radiused tool if I can find one.

    Thanks again!


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
  •