how do you calculate finish passes with endmills? - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 36 of 36
  1. #21
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    177
    Likes (Received)
    1475

    Default

    Quote Originally Posted by G00 Proto View Post
    ... 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).
    I only have 16k RPM, which is the only reason I'm running that for finishing. If I had more RPM's, I think I'd still be at 100% for finishing, as long as the tool was balanced.

    Other than high L/D situations, I don't see any upside to slowing down for finishing.

    "low hum" ... I like hearing nothing when finishing, other than the coolant jets.

    Regards.

    Mike

  2. #22
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    177
    Likes (Received)
    1475

    Default

    Quote Originally Posted by Rick Finsta View Post
    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.
    For outside, lead in straight into a straight entity, go around, then roll tightly (5% radius) off of the fillet preceding that straight entity. The little cusp will be lost in the fillet. You have to have little fillets on the outside corners for this to work, at least in Mastercam:

    hide-cusp.jpg

    For inside, roll onto and off of one of the inside fillets. Again, the cusp gets lost in the transition form straight to curved entities.

    Regards.

    Mike
    Last edited by Finegrain; 09-17-2019 at 10:46 AM.

  3. #23
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    830
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    362

    Default

    Quote Originally Posted by Finegrain View Post
    I only have 16k RPM, which is the only reason I'm running that for finishing. If I had more RPM's, I think I'd still be at 100% for finishing, as long as the tool was balanced.

    Other than high L/D situations, I don't see any upside to slowing down for finishing.

    "low hum" ... I like hearing nothing when finishing, other than the coolant jets.

    Regards.

    Mike
    I guarantee you would Mike. I run 100% at 27K unless my feed rate is constrained by point to point programming/program look ahead capability to feed at the corresponding feed rates for the given rpm.

    For example if I intended to feed at 150IPM and part geometry chokes it down to 100IPM even with HSM/Look ahead in play, no sense running the spindle any faster than it has to for the desired chip load.

  4. #24
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,354
    Post Thanks / Like
    Likes (Given)
    877
    Likes (Received)
    1449

    Default

    Quote Originally Posted by lowCountryCamo View Post
    Do you use standard ipt and calculate for radial chip thinning?
    Doing it like that can give you a scalloped finish.

    Figuring out max IPT is going to be somewhat similar to finding max IPR on a lathe.

    When your IPT is maxed out, you can go faster by increasing SFM or increasing flute count.

  5. #25
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,902
    Post Thanks / Like
    Likes (Given)
    173
    Likes (Received)
    1028

    Default

    Tomorrow I'll be running a piece made from 2024, I'll rough at 12000 rpm/100ipm .1 doc .1 stepover leaving .005. ill finish at 12000 rpm/200ipm .002 stepover, both with .375 4 flute uncoated carbide. It will leave a smooth finish, I know the .002 on the finish is very close to the 0 zone on the endmill but it works pretty well.

    I do mainly one-offs so my efficiency isn't so critical.

  6. #26
    Join Date
    Apr 2008
    Location
    Calgary
    Posts
    49
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    5

    Default

    Quote Originally Posted by countryboy1966 View Post
    I guarantee you would Mike. I run 100% at 27K unless my feed rate is constrained by point to point programming/program look ahead capability to feed at the corresponding feed rates for the given rpm.

    For example if I intended to feed at 150IPM and part geometry chokes it down to 100IPM even with HSM/Look ahead in play, no sense running the spindle any faster than it has to for the desired chip load.
    27K. What is the diameter of your end mill? Why is there very little talk of surface speed in this post? My machine is limited to 10000 RPM. I mostly cut 6061. The following numbers will be what I use with 6061. I leave .002 on walls and .005 on floors with 1/2' and 3/4' two flute carbide high helix end mills. I typically run them at .0075 IPT or 150 fpm at 10000 RPM. 1/2 surface speed is 1308 FPM and 3/4 is 1963 FPM. The side wall of the valve cover in the photo was done with a 3 flute 1/2" at 10000 RPM and 150 FPM or .005 IPT.

    20190919_094510.jpg

  7. #27
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    830
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    362

    Default

    Quote Originally Posted by 1320feet View Post
    27K. What is the diameter of your end mill? Why is there very little talk of surface speed in this post? My machine is limited to 10000 RPM. I mostly cut 6061. The following numbers will be what I use with 6061. I leave .002 on walls and .005 on floors with 1/2' and 3/4' two flute carbide high helix end mills. I typically run them at .0075 IPT or 150 fpm at 10000 RPM. 1/2 surface speed is 1308 FPM and 3/4 is 1963 FPM. The side wall of the valve cover in the photo was done with a 3 flute 1/2" at 10000 RPM and 150 FPM or .005 IPT.

    20190919_094510.jpg
    A few posts back I posted 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. Accordingly for me is specified SFM/Chip load etc for the given tool tool diameter as recommended by Tooling supplier. I feel SFM is irrelevant unless referencing a specific make/model cutter as they are all different.

    Yes - in my world I'm not ripping a 1/2" EM at 27K cutting 6061Al at max speeds and feeds as reason is obvious in your post. Physics does not allow it. I use mostly 1/32"-3/8" End mills with some very small complex geometry parts that have critical finish appearance requirements.

  8. #28
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,667
    Post Thanks / Like
    Likes (Given)
    10268
    Likes (Received)
    3101

    Default

    Quote Originally Posted by countryboy1966 View Post
    I feel SFM is irrelevant unless referencing a specific make/model cutter as they are all different.
    Interesting... I take the opposite approach... I don't care what the cutter is, I don't care what diameter it is, I (and this is not a complaint, just my personal feeling) HATE it when people talk RPM and IPM when (to me) SFM and CLPT/FPT are the real, relevant numbers.

    Just one of those "Ask 10 machinists a question and get 12 answers" kinda things, I guess

  9. Likes CarbideBob, Matt_Maguire liked this post
  10. #29
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,902
    Post Thanks / Like
    Likes (Given)
    173
    Likes (Received)
    1028

    Default

    Quote Originally Posted by TeachMePlease View Post
    Interesting... I take the opposite approach... I don't care what the cutter is, I don't care what diameter it is, I (and this is not a complaint, just my personal feeling) HATE it when people talk RPM and IPM when (to me) SFM and CLPT/FPT are the real, relevant numbers.

    Just one of those "Ask 10 machinists a question and get 12 answers" kinda things, I guess
    It's funny you mention it like that, I've never worked anywhere that people talked about sfm and ipt, its always been ipm and rpm lol

  11. #30
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    177
    Likes (Received)
    1475

    Default

    Quote Originally Posted by TeachMePlease View Post
    Interesting... I take the opposite approach... I don't care what the cutter is, I don't care what diameter it is, I (and this is not a complaint, just my personal feeling) HATE it when people talk RPM and IPM when (to me) SFM and CLPT/FPT are the real, relevant numbers.

    Just one of those "Ask 10 machinists a question and get 12 answers" kinda things, I guess
    For me, in Al, I don't actually care what the SFM is. I run >8,000 SFM in some cuts. I'm much more concerned about respecting the geometry, scallop height, chip evacuation, and chatter. As such, in Al, I am at 16k RPM all the time, except drilling where chip evacuation is a concern, facing because it is risky to run a 2-1/2" or 3" facemill that fast, and tapping since my rigid tapping is 6k RPM max. Also high L/D ratio cuts I slow down if chatter is happening.

    Regards.

  12. Likes countryboy1966 liked this post
  13. #31
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    830
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    362

    Default

    Quote Originally Posted by TeachMePlease View Post
    Interesting... I take the opposite approach... I don't care what the cutter is, I don't care what diameter it is, I (and this is not a complaint, just my personal feeling) HATE it when people talk RPM and IPM when (to me) SFM and CLPT/FPT are the real, relevant numbers.

    Just one of those "Ask 10 machinists a question and get 12 answers" kinda things, I guess
    I wasn't saying SFM was irrelevant in terms of calculating SFM, CLPT and FPT, but in general discussion where are not talking specific tooling. If a tooling manufacturer stats certain SFM, CLPT and FPT, another tooling manufacturer may specify it differently. RPM, FPT, CLPT, FPT, SFM are all relavant because they are all factors in the same calculations for speeds and feeds.

    So if I was talking about TITAN high helix carbide coated endmills I would talk specifics but we weren't. The speeds and feeds for it are different than a standard helix uncoated endmill from say harvey.

    With that said, like Finegrain eludes to, when working with aluminum, it is very forgiving and you can drive it like you stole it.
    Last edited by countryboy1966; 09-22-2019 at 03:42 PM.

  14. #32
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    167
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    96

    Default

    In Aluminum, I run my max 10000 rpm except drilling and tapping. I have a 2" ripper 4 flute that moves 44 cubes/min in my little 10hp Brother and leaves a nice finish.

    According to the Destiny tool website, there really is no SFM limit in Aluminum.

  15. #33
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    167
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    96

    Default

    Quote Originally Posted by plastikdreams View Post
    Tomorrow I'll be running a piece made from 2024, I'll rough at 12000 rpm/100ipm .1 doc .1 stepover leaving .005. ill finish at 12000 rpm/200ipm .002 stepover, both with .375 4 flute uncoated carbide. It will leave a smooth finish, I know the .002 on the finish is very close to the 0 zone on the endmill but it works pretty well.

    I do mainly one-offs so my efficiency isn't so critical.
    I learned with the yg-1 alupower to leave .01" of stock using HSM roughing. I tried .005, but violated the model. They are a tad flexy I guess.

  16. #34
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    539
    Post Thanks / Like
    Likes (Given)
    55
    Likes (Received)
    272

    Default

    On a Speedio without high speed modes enabled I would have to leave up to 0.050" to not violate the model on a few parts! If you tell them 700ipm, they will hit it and then do their damnedest to stay there even if it over/under cuts LOL. I wish I had time to go in and tweak the code but all short run parts (</=100 parts).

    I think stock to leave can be very part, machine, tool, and workholding specific.

  17. #35
    Join Date
    Nov 2012
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    91
    Post Thanks / Like
    Likes (Given)
    245
    Likes (Received)
    13

    Default

    Quote Originally Posted by huskermcdoogle View Post
    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.
    How many does it take you to get a good one?

  18. #36
    Join Date
    Sep 2019
    Country
    UNITED STATES
    State/Province
    Alaska
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Actually I do not so strong in math so I use electronic calculator for it. I have Texas Instruments Ti-84 CE like https://bestcalculators.net/ti84-vs-ti83-vs-ti89/ which is powerful device for calculate different hard tasks.
    Last edited by darui; 09-26-2019 at 01:01 AM.


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
  •