how do you calculate finish passes with endmills?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 36
  1. #1
    Join Date
    Jan 2012
    Location
    Savannah, Georgia, USA
    Posts
    1,649
    Post Thanks / Like
    Likes (Given)
    2624
    Likes (Received)
    628

    Default how do you calculate finish passes with endmills?

    how do you calculate finish passes with endmills? Of coarse different for different materials. Do you use standard ipt and calculate for radial chip thinning? I feel like I could increase feed of my finishes passes. How about rpms? Slower or faster?

    Thanks,

    steve Austin

  2. #2
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    264
    Post Thanks / Like
    Likes (Given)
    312
    Likes (Received)
    110

    Default

    add or subtract feed/rpm as needed!

    jk, i'm also interested in the science behind deciding finish pass parameters.

  3. #3
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    141
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    23

    Default

    I'm sure you will get any number of answers. personally I leave between .01 and .02 for cleanup on both walls and floors. I generally run a rpm of 6800 in aluminum. if it's a long cutter I may drop it to below 4000. 1 thing you dont want is squalling in the corners. I generally run a .002 or less chip per flute in aluminum as my finish pass. play with it and see what works for you. In hard metals like 17-4 I run that at about a 1/4 of aluminum.

  4. #4
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    177
    Likes (Received)
    1475

    Default

    I run 16k RPM for finishing unless I have a L/D challenge, then slower to avoid chattter.

    .002" IPT for workaday parts in Al with 3/8" & 1/2" endmills, and .001" for smaller. At higher IPT's, I can start to see the scallops.

    If it's something precious or high-precision I might cut the IPT in half.

    Regards.

    Mike

  5. #5
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,923
    Post Thanks / Like
    Likes (Given)
    173
    Likes (Received)
    1043

    Default

    For aluminum and steel I tend to leave .01 - .005 to clean up. On plastic I usually go .02...when surpacincg steel I leave .01 and aluminum and plastic usuly .005.

    I run most of my finishing passes at 100 or more ipm using ramps on 2d stuff steel around 5000-7000 rpm and aluminum and plastic 12k.

  6. #6
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    930
    Post Thanks / Like
    Likes (Given)
    1103
    Likes (Received)
    573

    Default

    I use the recommendation from HSMAdvisor or the Helical Machining Advisor. Beats the heck out of spreadsheets or calculating it yourself.

  7. #7
    Join Date
    Jan 2012
    Location
    Savannah, Georgia, USA
    Posts
    1,649
    Post Thanks / Like
    Likes (Given)
    2624
    Likes (Received)
    628

    Default

    Quote Originally Posted by mhajicek View Post
    I use the recommendation from HSMAdvisor or the Helical Machining Advisor. Beats the heck out of spreadsheets or calculating it yourself.
    I is HSM for roughing. Does it have a setting for finish passes? I have feel like a spend more time finishing parts than I should.

  8. #8
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,032
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2609

    Default

    the most important factors are
    .
    1) stickout length to diameter ratio
    2) tool holder length
    3) machine rigidity
    4) part rigidity
    5) work holding rigidity
    6)if circular milling a bore, the cutter dia to bore dia ratio. for example 3" dia cutter on a 3.100" dia bore
    .
    obviously there are cutting parameters specific to tool stickout lengths and tool holder length. if depths are 0.5" its different than 5" or 15" depths
    .
    obviously finish is not good til you can see reflection like its a mirror in finish. end mills in general dont give as good a finish as facemills
    Attached Thumbnails Attached Thumbnails shinymilling_cropped.jpg  

  9. #9
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,121
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    431

    Default

    Quote Originally Posted by lowCountryCamo View Post
    I is HSM for roughing. Does it have a setting for finish passes? I have feel like a spend more time finishing parts than I should.
    In HSMAdvisor you can just enable the HSM, disable Chip Thinning and set the feed override to 50%
    Seems to work fine for most cases.
    Attached Thumbnails Attached Thumbnails hsma_finishing.jpg  

  10. Likes lowCountryCamo liked this post
  11. #10
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    1,560
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    183

    Default

    Quote Originally Posted by zero_divide View Post
    In HSMAdvisor you can just enable the HSM, disable Chip Thinning and set the feed override to 50%
    Seems to work fine for most cases.
    Not using HSMAdvisor, but this is basically what I do. I will utilize bonus SFM when good tooling and working setups are available. Typically when finishing from a dynamic path in Ti I will take a .025" semi-finish with chip thinning, then .005" finish pass without chip thinning, usually somewhere between .001-.002" per tooth feed for the finish path, tool size dependent. If the semi-finish is with the finish tool, I won't typically exceed the book recommended feed per tooth after chip thinning, if it starts to chip the flutes, I will increase up to 40% more on the ipt until the condition goes away, if it doesn't go away, then typically an increase in surface footage is needed. This of course is in stable conditions. Unstable parts, machine, or whatnot, you can throw all this out the window, and just have to play with it to find the best tool life or finish. Typically they will coincide with each other. Also, in these cases it never hurts to throw anti-logical solutions at the problem. Sometimes you get lucky and they just work better than what you would consider to be the best practice. The key is to figure why it worked and capitalize on it.

  12. #11
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    654
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    711

    Default

    I generally leave between .020" and .005". This depends on how aggressively I am roughing (surface tolerance, roughing tool, corner chatter etc). Then I try and take a full depth finish pass when possible. I generally slow my rpms down to about 6k and a federate of about .002" IPT. This seems to give me the best cosmetic finish on my machines. I'm sure I could run the RPMs higher and the feed higher, but the above conditions coupled with my tumbling and anodizing processes yields very consistent and appealing results.

    I also strive for absolutely consistent radial depth of cut on my finish passes. If I leave .005" on the wall, I want that exact amount all the way around, and I also want the cutter contact angle to stay consistent. This means that on some internal radii, I will do a quick high speed toolpath with the finish cutter to ensure that there is .005" all the way around, especially if I roughed with a larger cutter or had my max internal radius set high for roughing speed. I like the end result to be an absolutely consistent sounding smooth cut all the way around the finish cut. Any change in sound will show up in the finished product.

  13. Likes huskermcdoogle, Jrill liked this post
  14. #12
    Join Date
    Feb 2013
    Location
    Northeast USA
    Posts
    145
    Post Thanks / Like
    Likes (Given)
    63
    Likes (Received)
    14

    Default

    I don't think there's a good way to calculate a finishing pass. Finishing passes are inefficient because they're driven by the result and not the tool. You just have to use whatever ipt gets the finish you need at whatever the highest reasonable sfpm is, which will probably be determined by tool life.

    For aluminum I leave 0.005-0.020 for the finishing passes, I take two identical finishing passes to reduce deflection, I use max rpm and ~0.005ipt (depends on cutter size and desired finish but I don't use more than 0.005 and I've been trending towards 0.004 and less lately, even with larger cutters, because it looks a lot better).

  15. Likes lowCountryCamo liked this post
  16. #13
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    154
    Post Thanks / Like
    Likes (Given)
    52
    Likes (Received)
    17

    Default

    I'm a simpleton so generally I just leave 0.3mm and double the RPM.

  17. #14
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    654
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    711

    Default

    I'm surprised you guys are increasing your spindle speed for finish passes. I assume you are machining hard materials (steel, titanium, stainless...). In aluminum I generally slow down the spindle rpms and try and load up the cutter and get that low hum sound (scientific, I know). In hard materials I usually increase my RPMs by about 25%.

    I guess it is still better than lathes... slow it down, take a big depth of cut, do some witch doctor dance and get a good surface finish

  18. #15
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    830
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    362

    Default

    Using high helix end mills.

    20-27K RPM depending on a few things generally part geometry related. .002"-.005" Finish pass. Feeds set accordingly for low side of chip load. 200 block look ahead.

  19. #16
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    553
    Post Thanks / Like
    Likes (Given)
    58
    Likes (Received)
    272

    Default

    To add to (or siphon from LOL) this discussion; the programmer I have been working with and learning from lately always repeats the finish pass. I understand why, as there is always a chip being taken the second go around due to deflection. Is this very common? It seems to me that tool life could decrease greatly in some materials if you aren't taking enough chip load? In the low volume production environment it did save us from having to lose a part or two developing the cutter comp to hit tight tolerances. Maybe that was the intention more than the finish quality.

    I always hated to see a finish pass repeated since it was always the slowest part of the cycle. I could rough a part in 30 seconds, and then it could take three times that to finish and chamfer. I might save 20-30% total cycle time by skipping the repeat passes on some parts.

    My biggest problem getting great side wall finishes has always been the radial moves in and out - I usually run a small bit over overlap to ensure there is no cusp but that means you can see much more of a blend line. I always just tried to get the CAM to move it to where it was the least innocuous.

    One thing I found is finishing size on size inside corners, I leave as little stock for the finish pass as I can without over cutting during roughing (Like <0.005" if I can). The lower the rpm and less total radial cut in those corners seemed to do a good job at avoiding chatter.

  20. #17
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    154
    Post Thanks / Like
    Likes (Given)
    52
    Likes (Received)
    17

    Default

    Quote Originally Posted by G00 Proto View Post
    I'm surprised you guys are increasing your spindle speed for finish passes. I assume you are machining hard materials (steel, titanium, stainless...). In aluminum I generally slow down the spindle rpms and try and load up the cutter and get that low hum sound (scientific, I know). In hard materials I usually increase my RPMs by about 25%.

    I guess it is still better than lathes... slow it down, take a big depth of cut, do some witch doctor dance and get a good surface finish
    Well, this is how I finish-face-mill. Super scientific too.


  21. #18
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,923
    Post Thanks / Like
    Likes (Given)
    173
    Likes (Received)
    1043

    Default

    So today I inadvertently did something different on my finish path...I left cutter comp off by accident. Took a bit more than the .005 I left from roughing...I don't suggest doing that

  22. Likes TeachMePlease liked this post
  23. #19
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    654
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    711

    Default

    Quote Originally Posted by Rick Finsta View Post
    To add to (or siphon from LOL) this discussion; the programmer I have been working with and learning from lately always repeats the finish pass. I understand why, as there is always a chip being taken the second go around due to deflection. Is this very common? It seems to me that tool life could decrease greatly in some materials if you aren't taking enough chip load? In the low volume production environment it did save us from having to lose a part or two developing the cutter comp to hit tight tolerances. Maybe that was the intention more than the finish quality.

    I always hated to see a finish pass repeated since it was always the slowest part of the cycle. I could rough a part in 30 seconds, and then it could take three times that to finish and chamfer. I might save 20-30% total cycle time by skipping the repeat passes on some parts.

    My biggest problem getting great side wall finishes has always been the radial moves in and out - I usually run a small bit over overlap to ensure there is no cusp but that means you can see much more of a blend line. I always just tried to get the CAM to move it to where it was the least innocuous.

    One thing I found is finishing size on size inside corners, I leave as little stock for the finish pass as I can without over cutting during roughing (Like <0.005" if I can). The lower the rpm and less total radial cut in those corners seemed to do a good job at avoiding chatter.

    I try and never do a spring pass. Sometimes you get a better finish, sometimes it does nothing but weld chips to the part. I never have felt that it is healthy for tool life.

    I used to work with a guy that was in the habit of taking a conventional spring pass. He claimed that it "squared up" the part. He was a pretty smart guy, but I always found that it left a shitty surface finish.

    I also worked with a guy that would run the cutter backwards on the spring pass to "burnish" the surface... he was an idiot and decided that machining wasn't his cup of tea.

  24. #20
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,725
    Post Thanks / Like
    Likes (Given)
    708
    Likes (Received)
    1985

    Default

    Quote Originally Posted by zero_divide View Post
    In HSMAdvisor you can just enable the HSM, disable Chip Thinning and set the feed override to 50%
    Seems to work fine for most cases.
    I've always thought a "Finishing" checkbox in HSM Advisor would be cool, sorta does it all for you in one click.


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
  •