Chatter in Corners of Deep Pocket
Close
Login to Your Account
Page 1 of 4 123 ... LastLast
Results 1 to 20 of 74
  1. #1
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    151
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    27

    Default Chatter in Corners of Deep Pocket

    I've started a job shop in the last few months. I'm not a formally trained machinist, so I'm still learning a lot. Things are going pretty well, but I keep having issues in the corners of deep pockets. I'm getting swirl marks and the machine chatters in the corners.

    Today, it's a particularly tough one, so I'm hoping you all might have some advice. The pocket is about 2.5" deep. Corner rad is .3125. The tool I have to finish it is a 3 flute 1/2" carbide end mill with a 3" LOC. Tool holder is a hydraulic. I rough out all the material and leave .004". (6061 is the material)

    I thought to do multiple depths, so maybe 15mm deep passes. I plug this into HSM advisor and it says 10k rpm and 200 IPM. This seems crazy, so I knock it down to 4k RPM and 40 IPM. The results were awful, see picture.

    Most of the way through, I stop and reprogram taking this time 3mm deep passes. Maybe it helped, but I don't think it's going to get the part to pass.

    Can anyone help me on feed/speed for this? Should I really be going 10k RPM? [edit: machine is a 10kRPM Speedio] My instinct tells me to slow down. Thoughts?

    chatter.jpg

    tool.jpg

  2. #2
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,609
    Post Thanks / Like
    Likes (Given)
    93
    Likes (Received)
    1129

    Default

    Use a neck-relieved or reduced-shank 1/2” endmill and take depth cuts.

    You can also pre-relieve the corners by drilling and reaming 5/8”, but that adds a lot of cycle time.

    Regards.

    Mike

  3. Likes Jeremy63 liked this post
  4. #3
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,609
    Post Thanks / Like
    Likes (Given)
    93
    Likes (Received)
    1129

    Default

    Also, get whatever endmill you end up using choked way up into the holder to reduce stick out. Your hydraulic holder doesnĺt have enough depth to do this, so switch over to a collet chuck that can sink the endmill shank much farther.

    Regards.

    Mike

  5. Likes RCoburn liked this post
  6. #4
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    716
    Post Thanks / Like
    Likes (Given)
    404
    Likes (Received)
    720

    Default

    Sometimes you have to go REALLY slow on RPMs. Like maybe 1000 rpm and 6ipm.

  7. Likes Limy Sami, 706jim, wheelieking71 liked this post
  8. #5
    Join Date
    Apr 2007
    Location
    Morgantown, WV
    Posts
    807
    Post Thanks / Like
    Likes (Given)
    250
    Likes (Received)
    318

  9. Likes Bobw, Rstewart, Orange Vise liked this post
  10. #6
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    171
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    108

    Default

    There are a couple of ways to machine the corners.

    1) rough it out then plunge the corners out with a center cutting EM and leave .003-.005 stock for finishing.
    2) rough it out and use a relieved/reduced neck 1/2" em and side mill the corners out only.
    3) Semi finish the corners and try a conventional cut. Sometimes this works good.
    4) Manually change the feed to F5.- F10. when the tool enters the corner and then speed it back up when it is past the corners.
    5) Shit can the HSM advisor, there is no reason to run a long tool that fast in corners like that.

  11. #7
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    151
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    27

    Default

    I had done a deep bore in 4140 which I used a really long 3/8" 2 flute. It came out great. I think it was 2" deep and I did multiple 8mm passes. RPM was 550 and feed was 3 IPM, which I think HSM advisor did help on. I guess I'll try slowing it down. I will switch holder to a ER 32 collet and choke up on it more. I will run a test part. If I can't get it to work, I'll order a reduced shank cutter. Thanks for the help.

  12. Likes bryan_machine liked this post
  13. #8
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,039
    Post Thanks / Like
    Likes (Given)
    444
    Likes (Received)
    942

    Default

    The only way I have ever been able to get consistent results in corners of deep pockets is with a reduced shank tool, you can always cut it off to get just the reach you need so there is no more stick out then what is needed to do the job.

    For finishing, I like a ramp tool path so the tool keeps close to the same loading all the way through the pocket and lock the ramp depth to ~.200" per pass.

  14. Likes Jeremy63 liked this post
  15. #9
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    151
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    27

    Default

    by the way, I did have some shank rubbing with my rougher for a few passes. It sounded bad and left some rub marks on the part and end mill. Should I be worried about anything being damaged from that? pull stud, holder, etc.? Thanks

  16. #10
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    2,134
    Post Thanks / Like
    Likes (Given)
    621
    Likes (Received)
    1069

    Default

    Quote Originally Posted by CosmosK View Post
    by the way, I did have some shank rubbing with my rougher for a few passes. It sounded bad and left some rub marks on the part and end mill. Should I be worried about anything being damaged from that? pull stud, holder, etc.? Thanks
    Nope. aaaaaaaaaaaaa

  17. Likes CosmosK liked this post
  18. #11
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    331
    Post Thanks / Like
    Likes (Given)
    243
    Likes (Received)
    172

    Default

    If you ain't rubbin' you ain't racin'.

  19. #12
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,537
    Post Thanks / Like
    Likes (Given)
    12048
    Likes (Received)
    9674

    Default

    You say you are new"ish" to this.. I'm going to try and not sound like
    a dick, but I'm going to fail..

    2.5" deep.. 3" flute length, plus hanging out another half of a mile.. If it
    DIDN'T chatter, I think that would be thread worthy..

    These guys have already said it.. Short flute length, necked back shank..
    You lose a LOT of rigidity in the tool when you cut the flutes out..
    But carbide is really hard and stiff... Seems that way, but its not, it still
    bends and deflects.. I've used a bunch of those type of tools (Maritool linked
    above) and I'm still flabbergasted at how far you can hang a solid shank tool
    out and still get "busy"..

    I've run 3" LOC 1/2"s before and they ALWAYS suck, they sing like Justin Beaver and
    sound just as bad..

    Reduced shank, choke it up as far as you can.. Choking up is important, short tools
    are important, you only want to be as long as you have to be, especially when you get
    into that 3:1plus range. This isn't 7th grade gym class, longer isn't better.

    Over time, you'll figure out what your machine is happy with, and what it isn't..
    You'll be able to just look at things and say "that's not gonna be good"...
    I looked at the pic of your tool and I said "that's not gonna be good"...




    Why not run a 5/8"???

  20. Likes TeachMePlease liked this post
  21. #13
    Join Date
    Dec 2011
    Location
    Whitehall, MI
    Posts
    566
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    137

    Default

    Definite on the reduced shank.

    Now, you also need to have a seperate feed command for the arc moves in the corner. The actual chipload will be way higher in the corners with 1/16 arc move.

    The formulas -
    Internal - (part ° - cutter °) / part ° x linear feed
    External - (part ° + cutter ° / part ° x liner feed

    I find that doing the internal feed calculations is very important for good results. For the 200 ipm feed you started with, you should of been doing 40 in the corners.

    As far as the rubbing, you won't damage your machine,and it's kinda of ok for roughing, but there is really no reason to be rubbing. Relieve the shank the appropriate distance. Unless you're not equipped to modify the tools easily (surface grinder and whirly gig). Then I understand.

    As a total side note, personally I don't think I would do setup in a shop that wasn't equipped to modify tool there. I programmed only at a shop the was not. Watching guys relieve shanks on a bench grinder by hand was enough for me. Lol...anwho..

    15mm is a pretty deep cut for 5xD. I would recommend backing off on that. I wouldn't do more than .100. But I've never run deep pockets in a production environment.

    I would probably start at S4000 Feed somewhere between 20 and 40 I'm thinking. Then 6 to 12 in the corners. That's how I'd approach it.

    Also, what is the tool radius? Sharper corner will help compared to having a radius.

    And are the corners of the pocket roughed with a corner slicing approach, or was like a 3/4 just jammed in there?

    The thing about deep pockets is don't get in a hurry, it's going to take some time.

  22. #14
    Join Date
    May 2005
    Location
    CA
    Posts
    938
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    163

    Default

    If you don't need a mirror finish on the walls....

    I've had amazing success on deep pockets with one of these: http://www.helicaltool.com/prod/H45A...-M-30500-R.030

    PM

  23. #15
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    151
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    27

    Default

    Quote Originally Posted by brian.pallas View Post
    Also, what is the tool radius? Sharper corner will help compared to having a radius.

    And are the corners of the pocket roughed with a corner slicing approach, or was like a 3/4 just jammed in there?
    The pocket has 8mm radius. Not sure what you're asking in the second part. I roughed it out with a 3/8 rougher (which has about 5 hours on it, mostly AL. holy cow). I was rubbing because the flute length isn't a long as the cut is deep. I finished the program, but reprogrammed it to leave a little more material as it goes deeper. Anyway, because the R4.76 it leaves, I don't think the issue is tons of material left in the corner.

    I ran a test part after lunch. RPMs between 500 and 1000 worked. Chipload didn't seem to make much difference (in happiness sound). .005" is where I left it. Stepped down every 4mm. Surface looked acceptable. I reran a replacement part up to this point and will try the finish them in morning. I put the tool in a collet and choked up more. I think I'll go with 700 RPM, 12 IPM, 3mm steps.

    Thanks for the info. I don't believe I can have separate corner feeds in the CAM I'm using (inventor/hsm express).

    Also thanks for the info on the reduced shank rougher. That looks cool. I was scoping this one out: link

  24. #16
    Join Date
    Jan 2018
    Country
    UNITED KINGDOM
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Feedrate has to be slowed down in corners.

    The feedrate you program is the feedrate for centre of tool. The cutting point travels at a much faster feedrate on internal corners. If you want to do it properly you need some high end software, Vericut Optipath can sort out but is megabucks.

    Before you do your finish pass mill out the corners with whatever feed you have to. I would drill the corners out first then mill the rads with a small straight lead. After that do the roughing you do and on the finishing pass use a bigger rad to avoid touching the corners all together.

  25. #17
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    91
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    35

    Default

    Quote Originally Posted by CosmosK View Post
    The pocket has 8mm radius. Not sure what you're asking in the second part. I roughed it out with a 3/8 rougher (which has about 5 hours on it, mostly AL. holy cow). I was rubbing because the flute length isn't a long as the cut is deep. I finished the program, but reprogrammed it to leave a little more material as it goes deeper. Anyway, because the R4.76 it leaves, I don't think the issue is tons of material left in the corner.

    I ran a test part after lunch. RPMs between 500 and 1000 worked. Chipload didn't seem to make much difference (in happiness sound). .005" is where I left it. Stepped down every 4mm. Surface looked acceptable. I reran a replacement part up to this point and will try the finish them in morning. I put the tool in a collet and choked up more. I think I'll go with 700 RPM, 12 IPM, 3mm steps.

    Thanks for the info. I don't believe I can have separate corner feeds in the CAM I'm using (inventor/hsm express).

    Also thanks for the info on the reduced shank rougher. That looks cool. I was scoping this one out: link
    Look for "feed optimization" in Inventor to change feed rate.

  26. #18
    Join Date
    Aug 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    35
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    13

    Default

    There's a lot of good advice on here! A few have said this but whenever you run into corners of pockets you are increasing the engagement on your end mill and need to cut the feed rate in half. I'd run it at around 4,000 RPM at 12 IPM in the corners.

    Also, even though you are deep pocketing into the corners of the part .005" isn't enough material to leave on the walls for the finish pass, you generally want to leave about 2%-4% of the tool diameter when finishing otherwise I have found you aren't cutting and the end mill wants to deflect leaving chatter marks. So leaving anywhere from .010"-.020" to finish will help as well.

    As others have mentioned a Necked End Mill will help a ton and Helical has a 40 degree variable pitch necked end mill for aluminum that has worked well for us in similar applications and would be a great option.

  27. Likes Jeremy63 liked this post
  28. #19
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    151
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    27

    Default

    Quote Originally Posted by Wsurfer View Post
    Look for "feed optimization" in Inventor to change feed rate.
    I see it, thanks. My tiny amount of testing seemed to indicate rpm was a bigger factor, but I will knock it down in the corners and see how it goes.

    Seeing lots of .005" and .010" here: thread

    I've been leaving .004-.006 on lots and lots of parts and have had no issues, granted this deep stuff is kicking my ass. My AL finisher has lasted a really really long time too. Both are from maritool, but case on some say HTC. Not sure if they supply for HTC or resell, but either way, I've been getting some really good mileage out of them.

  29. #20
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    1,135
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    295

    Default

    You should be able to slow the feed rate just for the corners in your CAM software.

    I have always found reducing rpm and increasing feed works better for chatter, especially in aluminum.

    I would choke your endmill WAAAAAAYYYYY up into an ER holder, until the face of the nut is almost rubbing on your part. Then slow your RPM down, WAY down, and increase your feed.

    Only on your last skim pass would I slow down the cutter to a crawl.

    I do a lot of work with 1/2" long reach 2"LOC and 3" LOC cutters. Almost all of it is in Steel. Fixturing has a lot to do with it too. Are you holding on the bottom 1/8" of the part? That allows the part to ring like a tuning fork.

  30. Likes Greg White, 5 axis Fidia guy liked this post

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
  •