How much chip load can an end mill handle?


Results 1 to 18 of 18

Thread: How much chip load can an end mill handle?

  1. #1
    Registered
    Join Date
    Aug 2009
    Location
    US
    Posts
    235
    Downloads
    0
    Uploads
    0

    Default How much chip load can an end mill handle?

    I just, after 3 years with my mini mill, noticed that I can take a pass with an end mill at a lower rpm and get a lower spindle load. Example: I run a 5/8" solid carbide end mill 1.5" deep in alu with a .035" radial step over at 200 ipm. First pass I run 6000 rpm and get 120% load on the spindle. Second pass I run 4800 rpm and get 85% load on the spindle. My question is, how much chip load can an end mill handle before it fails? This particular end mill is an SGS s-carb 3 flute that is rated at 2000 sfm and .007 ipt, but that is with a radial step over of 40%. What about my situation? I'm only running about 5%. I would think it would have to be similar to running a feed mill, I have one that is rated at .035 ipt. I'd like to bring the rpm even lower to around 3900 rpm and get even deeper into my torque curve. Maybe even increase the step over and feed rate a little too. This is my first expensive end mill in a long time, Id prefer to hang on to it a while. Any thoughts would be appreciated. Thank you.

    Similar Threads:


  2. #2
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    "Ratings" is a misnomer. I think what you are taking about is "recommendations". Generally, I think most experienced machinists will recommend you start at 1/2 cutter diameter for your axle depth of cut and anything up to full diameter for your radial depth of cut, if your set up is rigid enough. Rough to within 0.005-0.010 and then take a finish pass at full depth (if you have the flute length to handle it and you do not get too much deflection of tool or part). For spindle speed, you will have to determine by, maximum RPM of your machine, coolant delivery, chip evacuation, chatter conditions and heat build up. Chip load is also determined by coolant delivery, chip evacuation, chatter conditions, heat, and cutter geometry. 2000 sfm sounds kind of high. I would think you would have heating problems, which in aluminum would cause material to melt and stick to your cutter. I would probably start with 800-1000 sfm and go from there. 0.007 inch per tooth sounds ok as a starting point for full diameter radial DOC. As depth of cut decreases, chip load can increase.

    Machining is as much or more of an art as it is science. There are conditions in machining that cannot be built into any formula, such as machine harmonics. Personal experience and judgment play a huge part.



  3. #3
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    Have you seen this thread? http://www.cnczone.com/forums/haas_m...rformance.html

    My opening post explains what you observe with the load reducing at a lower rpm. Also read posts 9, 14, 19, and 21 they are a bit relevant to your questions here.

    After I had posted this thread a friend at Haas sent me all the torques curves for Haas machines and I have added the one for the Mini below.

    Regarding your question about how much load an end mill can handle with a Mini and a 5/8" diameter mill you are probably going to stall the spindle first. To protect the cutter what you should do is set your spindle load limit to 120% and SETTING 84 TOOL OVERLOAD ACTION to AUTOFEED. This way the machine just backs off on the feed when the load gets too high and it will eventually stop and just sit there humming. But don't let it get this far because it is difficult to back the tool out of the cut.

    Regarding your stepover and feed rate have you read about radial chip thinning? Your 6000rpm and 200ipm give a nominal load per tooth of around 0.01 but because your stepover is so small the actual load is probably down around 0.002.

    Your feedmill may not have been the best purchase for a MiniMill because you simply do not have the horsepower and rpm, and probably not the feed, to fully utilise it. Those mills can remove a lot of material very fast but you need plenty of oomph.

    Thats is the end of my thoughts for a while. Sun is shining and I have to rototill the back garden.

    Attached Thumbnails Attached Thumbnails How much chip load can an end mill handle?-torquemini-jpg  
    An open mind is a virtue...so long as all the common sense has not leaked out.


  4. #4
    Member
    Join Date
    Sep 2010
    Location
    Canada
    Posts
    80
    Downloads
    0
    Uploads
    0

    Default

    The info TX is giving you will definitely get u going in the right direction.Emphasis
    on RIGID and ART.Rigidity is what controls your limitations.Torque down on your clamps(use more if you have to) and keep your spindle short.
    As for the "ART" this can be learned with a piece of scrap and an equivalent older endmill.This way your are more likely to push it further.KEEP PERSONAL SAFETY IN MIND.Also remember,you may be discovering your machines limitations as well.Keep an eye on your load meter if you have one installed on the machine.
    May the FORCE be with you



  5. #5
    Registered
    Join Date
    Aug 2009
    Location
    US
    Posts
    235
    Downloads
    0
    Uploads
    0

    Default

    Thanks for the quick response! My problem is spindle power. I only have 7 peak hp. At it's max rpm, 6000, it makes almost no tq. The closer I get to its 2000 rpm tq peak the better. I want to rough at a high feed rate with a low rpm. This sends the ipt through the roof.

    In conventional machining, your numbers are perfect. That's how I used to machine. Sadly, with 7hp I had to find a different approach. I now use high feed/high speed machining. With these two techniques you are taking ether a small axial doc and large radial doc or large axial and small radial. The "actual" chip thickness is quite thin even at high feed rates "ipt". So I guess what I'm was asking is; taking into account the effects of radial chip thinning, how hard can you push an end mill? I had an iscar rep say 3 times the rated chip load in mild steel. I'm wondering if that is a little conservative when cutting aluminum. Again, thanks for any help.



  6. #6
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by double a-ron View Post
    ....So I guess what I'm was asking is; taking into account the effects of radial chip thinning, how hard can you push an end mill? I had an iscar rep say 3 times the rated chip load in mild steel. I'm wondering if that is a little conservative when cutting aluminum. Again, thanks for any help.
    It depends entirely on your stepover. At 50% stepover your chip thickness as the cutting edge enters the cut is what you have programmed. At 25% it is about 2/3, at 12-1/2% a bit less than 1/2 and at 6% about 1/3. Your 0.035 was about 6% stepover so obviously you could take your feed up threefold to get back to the nominal chip thickness, if you had the power.

    I think you are taking the correct approach for these relatively under powered machines. Wittle things away with small cuts.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  7. #7
    Member
    Join Date
    Nov 2006
    Location
    US
    Posts
    490
    Downloads
    0
    Uploads
    0

    Default

    It might depend on what you're trying to do with the particular toolpath. If it's going for a roughing movement then the feedrate can be jacked up. But naturally if it was a semi-finish or a finish cut you wouldn't want to exceed the "typical" numbers since the walls won't come out nice.

    High speed machining is great if you don't have horsepower to spare, so if I were in your position I would try to experiment with high RPMs and see how deep you can cut with them in varying conditions. The tool life may suffer when running it at low RPM and high engagement, although you won't initially be able to tell until it finally fails.
    Myself I would try to find the point where you can still be using HSM but at the same time NOT be worried about the machine's speed/torque, since you can juice the RPM as long as the tool doesn't get buried into a corner or something. I would start at say 4000 RPM ans see how well it performs, since it's possible an HSM program at 4000 RPM, full depth 0.015" stepover will finish the part quicker than 2000 RPM 0.040" and leave the tool in better condition.

    Anyway here's a great document that talks about some of the fundamental differences in material removal methods and how it affects the tool and machine. Good thing to save to the ole harddrive for future reference.
    http://www.htecnetwork.org/conferenc...f?rdm=68584670



  8. #8
    Registered
    Join Date
    Aug 2009
    Location
    US
    Posts
    235
    Downloads
    0
    Uploads
    0

    Default

    I am using volumill for gibscam. It shows actual chip thickness as well a my material removal rate. After reading your posts, I changed the roughing op to a .04 stepover at 4000 rpm and increased my mrr. I just finished running the part and the spindle stayed at a constant 100%. I tried lowering the spindle speed and increasing the feed rate, but it started to stall. I guess the maximum MRR for a mini is 12.4. The finish was rough as hell, but thats why they call it roughing. Geoff, where is that tq. curve? Couldn't find it.



  9. #9
    Registered
    Join Date
    Aug 2009
    Location
    US
    Posts
    235
    Downloads
    0
    Uploads
    0

    Default

    Ydna, funny you posting that seco brochure. I bought their feedmill. Its the smallest one they make. It's the .75" 2 flute one. At its rated feeds and speeds in steel (3500 rpm and 250 ipm) I'm pulling 70% on the spindle. Thinking of switching to iscars 3 flute 3/4 feedmill. Same rpm, but 375 ipm. Nice.



  10. #10
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by double a-ron View Post
    ...... Geoff, where is that tq. curve? Couldn't find it.
    That torque curve comes from a pdf file I was sent from Haas. It is possible the complete file is somewhere on the Haas website but I don't know how to find it.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  11. #11
    Gold Member BobWarfield's Avatar
    Join Date
    May 2005
    Location
    USA
    Posts
    2502
    Downloads
    0
    Uploads
    0

    Default

    Matching your spindle rpm to the torque peak and then trying to maximize feedrate is an interesting problem, particularly when you deal with both chip thinning and an HSM constant engagement (Volumill) toolpath.

    It's pretty easy to play with the numbers in G-Wizard. I just typed in a 2000 rpm limit which forced it to stay there or below and then ran the 5/8" cutter at the described 1.5" depth and 0.035" width of cut.

    I get 111 IPM feed at 2000 rpm for the HSM toolpath. Pretty crazy fast, but remember, the HSM path really unshrouds the cutter so it can stay cool and clear the chips. The open question is whether we can hold down the rpms that much and still have the cutter be happy--I haven't seen much real world data to say and G-Wizard is calibrated to reported successful feeds and speeds.

    Another thing to consider is that cut is showing about 1.2 HP. Even though you're at your torque peak, seems like we're scrimping a little on horsepower. In other words, it's topping out on the projected max chipload before really harnessing your torque peak.

    If we try 3000 rpm, it shows 167 IPM and 1.8 HP which is a bit better. I think I'd try more like that range. If you want to be conservating, start at
    about 85 IPM and work up to 167.

    Best,

    BW

    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html


  12. #12
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    I did not try to calculate the horsepower. But...

    1.500 ADOC X 0.035 RDOC X 111 IPM (@2000 RPM) = 5.8275 cubic inches per minute material removal

    0.625 ADOC X 0.25 RDOC X 49 IPM (@4889 RPM) = 7.6563 cubic inches per minute material removal

    I am betting you will find a happy medium somewhere between. Yes?



  13. #13
    Registered
    Join Date
    Aug 2008
    Location
    USA
    Posts
    292
    Downloads
    0
    Uploads
    0

    Default parameters

    hp load an end mill can take is based on how long it is. In general a shorter end mill can take a much higher load, 1/2 length can take 2x2x2 or 8 times more.
    ....... also if flutes get clogged or chips stick to flutes you can overload these estimates by 10 - 100 times

    parameters at 100% max load based on Machinabilty rating of 4.0 cubic inches per hp per minute...... assuming I have not made an error in calculations

    5/8 diam, 3 flute, carbide end mill
    SFPM 2025
    Coolant used but minimal (not flood)
    Stickout from collet 2.0
    DOC 1.500
    WOC 0.138
    chip thickness with thinning 0.0041
    Feed 210 ipm
    RPM 14,000
    Hp 10.85
    Load on end of End Mill 478 lbs
    MRR 43.4 cubic inches per minute

    at
    Stickout from collet 2.5
    DOC 1.500
    WOC 0.088
    Feed 168 ipm
    chip thickness 0.0029
    Hp 5.56
    Load on end of End Mill 245 lbs
    MRR 22.2 cubic inches per minute



  14. #14
    Registered
    Join Date
    Aug 2009
    Location
    US
    Posts
    235
    Downloads
    0
    Uploads
    0

    Default

    Thanks all. I got an email back from SGS. Took them one day to respond. Nice. They basically said the same thing Geoff said. After reducing to 4000 and increasing the stepover to .04 I was able to cut 2 min from the cycle while staying at 100% load. My poor machine, it's always at 100%. I don't think its seen anything lower than 50% in 2 years. Take that Haas haters.

    BobWarfield, What is this program your talking about? It sounds cool as hell. Same with DMF_TomB. What program are you using that gives all this useful info? Why isn't this data given in my expensive cam software?

    I wish you all could see the volume of material I'm removing with this little machine. It's truly breathtaking to watch a volumill toolpath hog out a 3x5x9 piece of billet. It's like it doubled the horsepower of the mill. I've even given up on the chip auger and started using a snow shovel to empty the chips.

    Again thanks for all the input. Happy cutting!



  15. #15
    Gold Member BobWarfield's Avatar
    Join Date
    May 2005
    Location
    USA
    Posts
    2502
    Downloads
    0
    Uploads
    0

    Default

    Constant engagement angle toolpaths are the next best thing to magic, LOL.

    The software I refer to is G-Wizard, a feeds and speeds (and many other things) calculator I wrote for machinists:

    GWizard: A CNC Machinist's Calculator for Feeds and Speeds

    What's really needed is some way to cross optimize all these factors so we find the point of maximum MRR within the limits of what the tool can put out and within the limits of the power your machine can deliver. G-Wizard will optimize for max feeds and speeds within a tool deflection limit, but I'll have to think about how to do this sort of optimization.

    Best,

    BW

    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html


  16. #16
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by double a-ron View Post
    .....My poor machine, it's always at 100%. I don't think its seen anything lower than 50% in 2 years....
    Don't worry they can take it.

    Because we do production work it was worth my while to refine programs to get the maximum productivity out of the machines so our machines often run between 100 and 120%.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  17. #17
    Registered
    Join Date
    Aug 2008
    Location
    USA
    Posts
    292
    Downloads
    0
    Uploads
    0

    Default free Excel file for calculating Speed Feed DOC

    latest free Excel file for calculating speed, feed, depth of cut. it can be opened with the free Open Office Calc program. it will figure DOC, horsepower, force on the end of the end mill
    ..... experimental it needs data like
    1) diameter of end mill
    2) length it is sticking out
    3) SFPM you want to run at
    4) MR or machinabilty rating of metal being cut with a chart of common metal alloys. MR is how many cubic inches per hp per minute you get machining a particular alloy.
    .
    has areas to help calculate what load setting you need to enter to get a particular DOC, or hp load, or force on end mill in pounds. has rows for side milling too, high DOC low WOC. and has row for ball end mill with rpm based on width of cut which is less with shallow depths with a ball end mill
    .... it is experimental

    Attached Files Attached Files


  18. #18
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    @TomB - Thanks. Maybe something like this is what these guys need.

    I would like to suggest that you just put all the fill-in-the-blanks with an answer box on the first sheet and then bury all the data in the follow up sheets. Be sure to lock cells and protect sheets as needed so that data or formulas are not accidentally changed.



Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

How much chip load can an end mill handle?

How much chip load can an end mill handle?