584,814 active members*
5,393 visitors online*
Register for free
Login
IndustryArena Forum > Tools / Tooling Technology > CNC Tooling > 4 flute carbide end mill wear. best feed and speeds?
Results 1 to 12 of 12
  1. #1
    Join Date
    Mar 2015
    Posts
    53

    4 flute carbide end mill wear. best feed and speeds?

    Some help needed for a newbie (to CNC).

    Machine is a small gantry router. (not a bendy chinese one though!)

    12mm 4 flute solid carbide end mill.
    0.1mm finishing cut, 10mm wide, across a plate of aluminium.
    Spinle speed 8000rpm. Feed 500mm/min.
    Dry.

    The path was a simple zig zag, 350mm pass, 10mm move across return 350mm repeat 30 times to cover 300mm of the plate.

    The bit was new at the start and produced a perfect finish for approx half of the path (approx 5000mm of travel in total).

    Then the finish rapidly degraded and noise increased.

    What am i doing wrong?

    What's caused the tool wear? Lack of lube/coolant? Wrong feed or speed?

    feed and speed calculator says 6222rpm and feed of 525mm/min for a fine finish.

    Some people say that feed and speed should be mush much faster...

    Any advice welcome!

    Thanks.

  2. #2
    Join Date
    Dec 2013
    Posts
    5717

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Lack of a cutting fluid would be my best guess. A flood coolant system using a water soluble cutting fluid would be the best, but that is probably not practical for your system. A mist spray system would work well also. My next choice would be WD-40. Use a spray bottle or pressure can. The spray bottle is less costly.
    Jim Dawson
    Sandy, Oregon, USA

  3. #3
    Join Date
    Mar 2015
    Posts
    53

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Quote Originally Posted by Jim Dawson View Post
    Lack of a cutting fluid would be my best guess. A flood coolant system using a water soluble cutting fluid would be the best, but that is probably not practical for your system. A mist spray system would work well also. My next choice would be WD-40. Use a spray bottle or pressure can. The spray bottle is less costly.
    Thanks Jim.

    I will try some WD40 or a small amount of suds oil/water mix.

    The finish was great for quite a while but suddenly changed. (pics in worng order, so inital finish is on the right!)

  4. #4
    Join Date
    Nov 2013
    Posts
    4280

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Hi,
    S(m/min)=D(m)*PI* RPM
    =0.012 *PI*6222
    =234.56 m/min

    The recommended surface speed for aluminum with a coated carbide tool is in the range 200-500 m/min.
    Note that for aluminum there is considerable leeway. Your rpm setting is good.

    What appears to be happening is aluminum is 'sticking' to the tool. This is called Built Up Edge (BUE) and is very common
    with soft metals, aluminum is very prone to it. Certain grades are much worse than others, the very soft pure grades (1000 series)commonly
    used for cookware and highly extruded products is very sticky. The 5000 series has given me trouble too. 6061, 6063 are less prone to BUE.

    There are some videos that describe the process of BUE. Search some out. The essential idea is that locally the formation of the chip
    generates heat which causes the chip to adhere to the surface of the tool.

    It should be noted that the most common coatings on carbide tools are nitrides (titanium nitride, aluminum nitride etc) which are trivalent,
    aluminum is also trivalent, and so shows an 'affinity' for the coating. Consequently most carbide tools for aluminum are uncoated.
    There is a coating which is very good for aluminum, a di-boride which is quad-valent and is as slippery as hell in aluminum. Harvey Tools
    have a good range of them.

    I find that flood cooling improves my aluminum machining considerably. Partly due to keeping the tool cool, partly aiding lubrication of the
    chip on the tool surface, but largely flushing the chips away from the cutzone thereby avoiding recutting of chips. Recutting of aluminum chips
    will get you into trouble everytime.

    Craig

  5. #5
    Join Date
    Nov 2013
    Posts
    4280

    Re: 4 flute carbide end mill wear. best feed and speeds?


  6. #6
    Join Date
    Mar 2015
    Posts
    53

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Quote Originally Posted by joeavaerage View Post
    Hi,
    S(m/min)=D(m)*PI* RPM
    =0.012 *PI*6222
    =234.56 m/min

    The recommended surface speed for aluminum with a coated carbide tool is in the range 200-500 m/min.
    Note that for aluminum there is considerable leeway. Your rpm setting is good.

    What appears to be happening is aluminum is 'sticking' to the tool. This is called Built Up Edge (BUE) and is very common
    with soft metals, aluminum is very prone to it. Certain grades are much worse than others, the very soft pure grades (1000 series)commonly
    used for cookware and highly extruded products is very sticky. The 5000 series has given me trouble too. 6061, 6063 are less prone to BUE.

    There are some videos that describe the process of BUE. Search some out. The essential idea is that locally the formation of the chip
    generates heat which causes the chip to adhere to the surface of the tool.

    It should be noted that the most common coatings on carbide tools are nitrides (titanium nitride, aluminum nitride etc) which are trivalent,
    aluminum is also trivalent, and so shows an 'affinity' for the coating. Consequently most carbide tools for aluminum are uncoated.
    There is a coating which is very good for aluminum, a di-boride which is quad-valent and is as slippery as hell in aluminum. Harvey Tools
    have a good range of them.

    I find that flood cooling improves my aluminum machining considerably. Partly due to keeping the tool cool, partly aiding lubrication of the
    chip on the tool surface, but largely flushing the chips away from the cutzone thereby avoiding recutting of chips. Recutting of aluminum chips
    will get you into trouble everytime.

    Craig
    Hey thanks Craig.

    I'm guessing that your quoted speed is mm/min and not m/min!

    The video is interesting, I'd always thought that the very front edge of the tool is there to initiate splitting the chip away from the material and that once the split starts, the edge is no longer in direct contact. Maybe I got that wrong though!

    There appears to be a lot of tool wear in my case. How does BUE make that worse? I can see how it would degrade the surface finish. Does it just make for a lot of localised heating due to extra friction?

  7. #7
    Join Date
    Mar 2015
    Posts
    53

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Quote Originally Posted by joeavaerage View Post
    Hi,
    S(m/min)=D(m)*PI* RPM
    =0.012 *PI*6222
    =234.56 m/min

    The recommended surface speed for aluminum with a coated carbide tool is in the range 200-500 m/min.
    Note that for aluminum there is considerable leeway. Your rpm setting is good.

    What appears to be happening is aluminum is 'sticking' to the tool. This is called Built Up Edge (BUE) and is very common
    with soft metals, aluminum is very prone to it. Certain grades are much worse than others, the very soft pure grades (1000 series)commonly
    used for cookware and highly extruded products is very sticky. The 5000 series has given me trouble too. 6061, 6063 are less prone to BUE.

    There are some videos that describe the process of BUE. Search some out. The essential idea is that locally the formation of the chip
    generates heat which causes the chip to adhere to the surface of the tool.

    It should be noted that the most common coatings on carbide tools are nitrides (titanium nitride, aluminum nitride etc) which are trivalent,
    aluminum is also trivalent, and so shows an 'affinity' for the coating. Consequently most carbide tools for aluminum are uncoated.
    There is a coating which is very good for aluminum, a di-boride which is quad-valent and is as slippery as hell in aluminum. Harvey Tools
    have a good range of them.

    I find that flood cooling improves my aluminum machining considerably. Partly due to keeping the tool cool, partly aiding lubrication of the
    chip on the tool surface, but largely flushing the chips away from the cutzone thereby avoiding recutting of chips. Recutting of aluminum chips
    will get you into trouble everytime.

    Craig
    Hey thanks Craig.

    Does my feed speed of around 500mm/min sound right?

    The video is interesting, I'd always thought that the very front edge of the tool is there to initiate splitting the chip away from the material and that once the split starts, the edge is no longer in direct contact. Maybe I got that wrong though!

    There appears to be a lot of tool wear in my case. How does BUE make that worse? I can see how it would degrade the surface finish. Does it just make for a lot of localised heating due to extra friction?

  8. #8
    Join Date
    Nov 2013
    Posts
    4280

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Hi,

    I'm guessing that your quoted speed is mm/min and not m/min!
    No, that is correct, its meters per minute. That is the surface speed not the speed of advance of the tool or cutting speed.
    The surface speed is the velocity of the tool tooth or tool surface relative to the material. So as the rpm's go up so does the
    speed of the surface of the tool that rubs the material.

    Each material has a recommended surface speed. Roughly:

    Titanium and Superalloys 20-40m/min
    Stainless 50-70m/min
    Mild Steel 100m/min
    Aluminum 200-500m/min.

    Note these surface speeds are for plain carbide. Coated carbides will tolerate more surface speed as a rule. HSS tools rather less, about 1/2 to 2/3.

    I like HSMAdvisor so much I bought it.
    https://hsmadvisor.com/

    Cutting speed is all about how big a chip you are trying to peel off.

    You are using a four flute endmill, so for each revolution it will take four chips. If each chip were 5um thick then the tool would advance:
    d=4*5um
    =20um
    or 0.02mm.
    At 6222rpm the cutting speed would be:
    CS=6222* 0.02
    =124mm/min

    The thickness of the chip, called chipload, is dependent on a number of factors including the strength of the tool, both bending AND torsion,
    the power of the spindle and the rigidty and thrust of the machine. I would suggest download HSMAdvisor (demo) and input the parameters of your
    machine and experiment a bit with it.

    What I have found is that the surface speed is the most important.....you can vary by 10-20%, but if you try to spin the tool too fast then you risk
    overheating and wrecking the tool. It does not usually hurt to spin a tool slower than the recommended surface speed would indicate, and often with small
    and very small tools your spindle can't spin as fast as you would like.

    You can reduce the cutting speed to accommodate your machine or spindle which may be a bit too light. What I do not recommend however is trying to take very
    light or slow cuts.....what happens is you just give the material a good 'rub' and workharden it WITHOUT really peeling off a chip.
    I have made that mistake......having a high speed spindle I have settled on a high rpm well exceeding the recommended surface speed and so to compensate
    tried to take very light cuts very slowly. It didn't work!

    A lot of the literature recommends NOT cooling carbide, the thermal shock of the carbide it supposed to hurt it.

    That is not my experience. With my mill whenever I use flood cooling my machining has improved VASTLY! I have had various conversations with other hobbyists
    and most use some sort of lubrication. I'm quite keen to have a go with M(inimum)Q(uantiy)L(ubrication) as a result. I'm less convinced that lubrication
    is the real point but rather using a fluid, be it cutting fluid or compressed air, to blow the chips out of the cutzone.

    Craig

  9. #9
    Join Date
    Mar 2015
    Posts
    53

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Quote Originally Posted by joeavaerage View Post
    Hi,


    No, that is correct, its meters per minute. That is the surface speed not the speed of advance of the tool or cutting speed.
    The surface speed is the velocity of the tool tooth or tool surface relative to the material. So as the rpm's go up so does the
    speed of the surface of the tool that rubs the material.

    Each material has a recommended surface speed. Roughly:

    Titanium and Superalloys 20-40m/min
    Stainless 50-70m/min
    Mild Steel 100m/min
    Aluminum 200-500m/min.

    Note these surface speeds are for plain carbide. Coated carbides will tolerate more surface speed as a rule. HSS tools rather less, about 1/2 to 2/3.

    I like HSMAdvisor so much I bought it.
    https://hsmadvisor.com/

    Cutting speed is all about how big a chip you are trying to peel off.

    You are using a four flute endmill, so for each revolution it will take four chips. If each chip were 5um thick then the tool would advance:
    d=4*5um
    =20um
    or 0.02mm.
    At 6222rpm the cutting speed would be:
    CS=6222* 0.02
    =124mm/min

    The thickness of the chip, called chipload, is dependent on a number of factors including the strength of the tool, both bending AND torsion,
    the power of the spindle and the rigidty and thrust of the machine. I would suggest download HSMAdvisor (demo) and input the parameters of your
    machine and experiment a bit with it.

    What I have found is that the surface speed is the most important.....you can vary by 10-20%, but if you try to spin the tool too fast then you risk
    overheating and wrecking the tool. It does not usually hurt to spin a tool slower than the recommended surface speed would indicate, and often with small
    and very small tools your spindle can't spin as fast as you would like.

    You can reduce the cutting speed to accommodate your machine or spindle which may be a bit too light. What I do not recommend however is trying to take very
    light or slow cuts.....what happens is you just give the material a good 'rub' and workharden it WITHOUT really peeling off a chip.
    I have made that mistake......having a high speed spindle I have settled on a high rpm well exceeding the recommended surface speed and so to compensate
    tried to take very light cuts very slowly. It didn't work!

    A lot of the literature recommends NOT cooling carbide, the thermal shock of the carbide it supposed to hurt it.

    That is not my experience. With my mill whenever I use flood cooling my machining has improved VASTLY! I have had various conversations with other hobbyists
    and most use some sort of lubrication. I'm quite keen to have a go with M(inimum)Q(uantiy)L(ubrication) as a result. I'm less convinced that lubrication
    is the real point but rather using a fluid, be it cutting fluid or compressed air, to blow the chips out of the cutzone.

    Craig
    Thanks again Craig, yes I mis-read confused surface speed with feed!

    I have a demo of G-Wizard and it's showing me a surface speed of 274m/min, rpm 6400rpm.

    If the 'finish' slider is on finest, then feed is 540mm/min. Conversley if it's set to coursest, 2700mm/min which seems scary fast!

    Now the bed is flat and square, I'll have a play with some spare ali plate and see what different lube setups give me. I will pay close attention to build up on the tool this time too....

  10. #10
    Join Date
    Nov 2013
    Posts
    4280

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Hi,
    to be honest I think those feed rates are way to high. They might be appropriate for a high power production mill but for a hobbyists machine
    way too much.

    I use some very small (0.5mm two flute) endmills for copper circuit boards. Because they are so small an fragile I use a chipload of 1% of tool diameter per tooth.
    Thus 1% of 0.5mm =.005mm or 5um. Because there are two teeth (flutes) that's 10um tool advance per revolution.
    At 24000 rpm (24000* .01)=240mm/min

    For larger and stronger tool you can tolerate a bigger chipload without breaking the tool. About 2% of diameter is a good place to start.
    For your 12mm 4 flute tool:
    2% of 12mm =0.24mm at 6222rpm means the feed rate is 6222*0.24*4=5973mm/min!!!
    The only question is can your machine and spindle handle it?

    I would be tempted to reduce the feed rate to about 10% of the calculation and try it, ie 590mm/min. You can always increase it if your machine
    is just coasting. It will result in a fairly thin chip but it won't be just giving it a 'rub' either.

    I will pay close attention to build up on the tool this time too....
    Yes, this is vital. Just about everyone who has done any milling has encountered BUE.....and you absolutely HAVE TO DEVISE a strategy for avoiding
    it.

    Craig

  11. #11
    Join Date
    Jun 2010
    Posts
    4252

    Re: 4 flute carbide end mill wear. best feed and speeds?

    BUE is a serious problem with aluminium. You simply have to keep the cutter 'wet' to avoid it. For this one used to use flood coolant, but these days pulsed misting and MQL are a better (cheaper, cleaner, more effective) choice. Pulsed misting works fine (my experience) on aluminium, steel and titanium.

    But BUE is not the only problem. Many aluminium alloys contain residual aluminium oxide particles, and AlOx is a well-know abrasive. Carbide is a good choice here, although aluminium-specific HSS cutters can also work fine - but both need to be lubricated or kept 'wet', as above.

    Some tuning of feed and speed will still be needed.

    Cheers
    Roger

  12. #12
    Join Date
    Mar 2015
    Posts
    53

    Re: 4 flute carbide end mill wear. best feed and speeds?

    Thanks guys.

    I am setting up for flood cooling at the moment.

Similar Threads

  1. Single flute end mill wear
    By Joe2014 in forum CNC Tooling
    Replies: 14
    Last Post: 03-27-2016, 09:11 PM
  2. Countersink Speeds and Feeds, 6061, 6-flute carbide
    By sanddrag in forum Uncategorised MetalWorking Machines
    Replies: 10
    Last Post: 01-14-2013, 04:45 AM

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
  •