Need advice milling aluminum, broke endmill after 2 hours of milling

Results 1 to 19 of 19

Thread: Need advice milling aluminum, broke endmill after 2 hours of milling

  1. #1
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Need advice milling aluminum, broke endmill after 2 hours of milling

    Hi guys,

    I've been self educating myself on CNC milling for the last year or so. Up to now I have milled mainly Plywood and MDF. Started experimenting with aluminum just recently. Today I started my first big cut. This one should take somewhere about 70+ hours. Started my first operation, that should last for about 7:30 hours. At exactly 2 hours and 10 mins the endmill broke. I believe I used moderately light feedrate, stepover and depth, so I am curious to find out what caused the breakage.
    There 3 possible reasons that I can think of:
    1. Overheating of both the stock and the endmill
    2. ****ty chinese endmills
    3. I am mistaken and I need to further reduce the feedrate and stepover.

    So here is some info on the machine and settings I am using.
    CNC router equipped with a 2.2 kW ER20 chinese spindle. Max feedrate 1200 mm/min min/max RPM 3000/21800. Since those spindles have very low torque at low rpm, I prefer faster cuts with higher rpm.
    The cut is done with a 6mm, 2 flute, flat HSS endmill (from Aliexpress), which is sticking out 33mm. Feedrate is 750 mm/min, rpm ~15100. I have equipped DIY mist cooling. It is powered by an 8bar compressor (limited to 2.5-3 bar for this operation). For coolant I use hydraulic oil (VG32).

    The stock I am working on is 6082 T6 aluminum slab with dimensions 500x330x40 mm. This first cut goes down 19mm deep, at 2mm stepdown increments, and 1.8mm stepover.

    I have came up with those settings using GWizzard. Any more feedrate/stepdown/stepover increases the tool deflection to "red" numbers. For those 2 hours everything seemed and sounded fine, until suddenly the endmill broke. Examining the broken piece I didn;t notice any wear on the cutter, so that shouldn;t be the problem.

    One thing that I noticed. About 10 minutes after the endmill broke, I touched the stock it was roughly 50 degrees celsius to the touch. Which means it was even hotter at the time of breakage, and at the place of the cut the temp was probably even higher (maybe well over 100 degress). Could the temp of the stock have affected the properties of the aluminum?
    If this is the case, maybe I should spray some water on the stock from time to time, hoping that evaporation will cool it. And maybe a short break after each hour of milling? I'm even thinking about switching the oil with water, but I am not sure how good of an idea that is.

    I need to improve the rate of breakage. I have at least 10 more hours of milling with a 6mm endmill, and I have about 5 more such endmills. If these rates keep up I might need more endmills

    Attached you can see my G-Wizzard screen, and the piece of stock right after the breakage.

    Edit: Forgot to mention. This was a brand new endmill, so those were the first 2 hours and 10 minutes of its usage.
    And one more question. See those circles on the stock? Those are eventually going to be the mounting place for a COB LED, I need them perfectly flat. But after the current operation they are not perfectly flat. They are actually perfectly flat almost all over, except for a small notch at the exact center of the circle. It is obvious I need to do a second operation to fix this, but if I use the same cutting strategy, I'll probably get the same notch. I am thinking about using parallel passes instead of a spiral. Sure that might leave some bumps near the circle's boundary, but the center part should be fine, and that is what matter to me.
    Would love to hear your thought on that.

    Similar Threads:
    Attached Thumbnails Attached Thumbnails Need advice milling aluminum, broke endmill after 2 hours of milling-gwiz-jpg   Need advice milling aluminum, broke endmill after 2 hours of milling-mill-jpg  
    Last edited by zeox; 06-15-2017 at 07:48 PM.


  2. #2
    Member awerby's Avatar
    Join Date
    Apr 2004
    Posts
    5728
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    I don't think making hydraulic oil into a mist is really recommended; it's not healthy to breathe. And it doesn't seem to have kept your stock cool either. Most coolant/lubes are a water-oil emulsion that combine the best features of both substances.

    You might think about using a larger cutter to rough out with and coming back with the smaller one to do a finish cut. That would be less stressful for the 6mm cutter.

    What CAM software were you using? It doesn't seem to have been very sophisticated if it left prongs standing up in the middle of your pockets. Running a tool into a sharp corner can often break it, if the software doesn't recognize that condition and treat it as a special case.

    [FONT=Verdana]Andrew Werby[/FONT]
    [URL="http://www.computersculpture.com/"]Website[/URL]


  3. #3
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    I am using Inventor Professional 2015, but I am using standard pocket clearing, as the Adaptive option takes too long to compute and too long to cut. I know the Adaptive strategy will increase the tool life maybe I'll use it for the next cut.

    As for the coolant I will try to find some specialized fluid for this.

    As for larger endmills. Both the model that I am working on and the CNC router itself do not allow me to use a larger endmill on aluminum. This chinese spindle is not performing well at low rpm, actually anything below 7000 is useless (even though I can go down to 3000), it just doesn't have enough torque. And larger bits require lower rpm. I have 12mm and 16mm endmills but I use those only on MDF and Plywood. Anything over 8mm is useless for aluminum on this particular router.
    After the 6mm endmill operation, I will start cutting the finer detail for a 3mm endmill.

    I did about an hour and 20 mins of cutting today. I stopped because the stock was getting hot. There wasn't any breakage this time. I hope that changing the coolant will allow me to cut for longer.

    Attached a picture of todays progress

    Attached Thumbnails Attached Thumbnails Need advice milling aluminum, broke endmill after 2 hours of milling-wp_20170616_20_05_03_pro-jpg  


  4. #4
    Member dharmic's Avatar
    Join Date
    May 2015
    Location
    Australia
    Posts
    1422
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    I had the same issue yesterday, very similar feed/speeds etc. I use a 20/80 mix of methylated spirits and water through a mister. A couple of hours in and the spindle suddenly started slowing down, about two seconds later the tool sheared.

    I suspect, from the way it slowed down and bogged in first, that I fell victim to the edge welding phenomenon. Again, suspicion only at this point, but I think it likely caused by having only a single mister nozzle working at the time and the workpiece blocking the spray from the cutter over a run leading up to the failure.

    I'll try again this weekend with a higher coolant flow and paying a bit more attention to the nozzle placement



  5. #5
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    I am using a single nozzle too. I was thinking about adding a second one (I had ordered a second one as spare) with just air no coolant fluid.

    And yes, whenever the end mill goes deeper, the stock is actually blocking the air flow. That is why I am sitting next to the thing and blowing manually with a standard blow nozzle.

    Regarding your cooling fluid, how well does it handle aluminum? I can easily obtain methylated spirits, but I am unsure if it provides any lubrication. Would love to hear your experience with this coolant.

    Anyways I already found some oil for making an emulsion online. It is marketed for usage in turning, milling, polishing and other operations, has to be mixed in a 1:20 ratio with water. It's a local brand, fairly cheap, so I will give it a try probably on Wednesday (Since it is already Friday night here, my order will be processed on Monday, and I'll probably get it on Wednesday).



  6. #6
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Kerosene, also known as lamp oil or paraffin depending on where you are at, is my coolant of choice for aluminum. Seems to prevent welding, even when applied in very small amounts. I normally use about 120mL / hr (about 1/2 cup/hr) on the mill, applied with a mist system. Might require a higher flow with a router spindle. I also use solid carbide, 2 or 3 flute bits, normally in the 6 to 10 mm range.



  7. #7
    Member dharmic's Avatar
    Join Date
    May 2015
    Location
    Australia
    Posts
    1422
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Ethanol/Water is what the Datron machines use - and they are built to do high speed, high definition aluminium work. It lubricates ok, cools well and leaves zero mess on the job or the machine. The metho helps the water evaporate before it has a chance to cause corrosion issues. It's a winner IMO - just make sure the workcell is well ventilated if you plan on driving home afterwards

    Kerosene or the WD-40/CRC 556 branded sprays make a fantastic lubricant for aluminium but you end up with oily crap everywhere at the end of the job.

    The thing with blocking flow: in a mister, it means you're also blocking the lubricant from the tip so you might as well be cutting dry. Just blasting with an air nozzle helps clear chips away but it does nothing for keeping the cutting edges wet.



  8. #8
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Well, seems like I'll do some testing these days. I'll get some ethanol from the pharmacy tomorrow for the test. On Monday I'll obtain both lamp oil and methylated spirits and I'll mess around with those until Wednesday. I might even try to emulsify some of the hydraulic oil I am currently using for tomorrow's cut.

    @Dharmic, as you mentioned, using oil based substances really leaves an oily mess at the end. So in a way, when I blow manually on the endmill, the cut is not dry, there's oil everywhere If you look at the picture those triangular shapes become sort of pools of oil

    @Jim Dawson, do you use pure Kerosene or do you mix it with water? If mixed, at what ratio? Thanks.



  9. #9
    Member dharmic's Avatar
    Join Date
    May 2015
    Location
    Australia
    Posts
    1422
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    I wouldn't bother with pure ethanol, if Bulgaria is anything like Oz it costs a fortune compared to the methylated spirits which works just as well.

    I know that the fluid pools (so does my mix) but a fast spinning cutter is gonna throw it off the cutting edge pretty fast.



  10. #10
    Member
    Join Date
    May 2011
    Location
    Canada
    Posts
    790
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Quote Originally Posted by zeox View Post
    Max feedrate 1200 mm/min
    That's only 47 IPM. Is this accurate?
    Quote Originally Posted by zeox View Post
    I have came up with those settings using GWizzard. Any more feedrate/stepdown/stepover increases the tool deflection to "red" numbers.
    You can't use conventional feed and speed calculators on a DIY machine and expect good results. The numbers they give you assume a certain stiffness in your machine design. That isn't a bridgeport mill you have there! No amount of misting or other coolant will fix this.

    Quote Originally Posted by zeox View Post
    The cut is done with a 6mm, 2 flute, flat HSS endmill (from Aliexpress), which is sticking out 33mm. Feedrate is 750 mm/min, rpm ~15100.

    This first cut goes down 19mm deep, at 2mm stepdown increments, and 1.8mm stepover.
    I'd try tripling the feed rate (if you can on your machine) and reduce your depth of cut to 0.5mm or less. Try that and see what happens. Also consider using extremely sharp solid carbide bits. If the bit gets dull, you're done. IMO, you can run shallow and fast with a sharp carbide bit on a DIY machine without any coolant. Try some different RPM settings as well.

    I can't see your machine frame in the picture so I can't guess how stiff it might be. I think it is safe to say that you can not expect a conventional feeds and speeds calculator to do much for you on your DIY machine. You have to try a few things out to see what you can get to work reasonably well on your machine.



  11. #11
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    @Dharmic, yes Ethanol is much more expensive. But I'm going to get only a small bottle of it just for the test. When mixed 1:20 with water it should give me plenty of fluid until Monday. The places where I can buy Methylated spirirts do not work on the weekends.

    @NIC 77. Sadly there is no error, and that is the max feedrate of this machine, it's crap, I know. The gantry is moved by screws, its original application was stone carving.
    When I was buying this machine I had absolutely no idea about milling, but being one of the cheapest out there it was a good option for a learner. I will be upgrading this autumn hopefully.
    I don't have a good picture of my machine, but here is a pic from the site of the guy who makes them.


    I am really pushing this thing to it's limit, am I?
    I've been also thinking about lighter cuts, but this takes way too long on this machine. I have ordered some carbide roughing mills and am currently waiting for them. That should allow me to increase the rpm and feedrate even further. Then I might consider shallower cuts.

    I am planning to upgrade to a modified version of this machine


    It is way too big. I'll order it with the size of my current one. Maybe even make it narrower, to increase the stiffness of the gantry. This machine can go up to 18 000 mm min, so with such higher feedrates I can really afford much lighter cuts. It is still an amateur design, but that is what I can afford.

    For comparison, here is a higher class machine, produced by another local manufacturer


    Now I am sure this will perform much better, but I can not yet afford it.
    My current machine costs about 3000 EUR, The one that I'm thinking about upgrading to is about 4000 EUR (the upgrade will cost me ~1500 EUR), and that last one costs 10 000 EUR

    Edit: I am also considering the purchase of a second hand vertical machining centre, tha will handle all cuts with mills over 6mm, and using the router only for operations with smaller bits, that require high rpm and moderate feedrates.

    Attached Thumbnails Attached Thumbnails Need advice milling aluminum, broke endmill after 2 hours of milling-cnc1-jpg   Need advice milling aluminum, broke endmill after 2 hours of milling-cnc2-jpg   Need advice milling aluminum, broke endmill after 2 hours of milling-cnc-3-jpg  
    Last edited by zeox; 06-17-2017 at 09:40 AM.


  12. #12
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Quote Originally Posted by zeox View Post

    @Jim Dawson, do you use pure Kerosene or do you mix it with water? If mixed, at what ratio? Thanks.
    Pure Kerosene. I use so little that it pretty much evaporates in use and does not leave a mess.



  13. #13
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Well guys, I found the problem. It is tool deflection, but it was hard to notice it initially
    Today I started cutting and broke the mill on the 8th minute. Changed it, continued cutting for another hour and a half and broke another one.
    While the first breakage occurred in the shallow circular parts, those next two happened in the deep triangular cuts in the same place of the cut. I guess the first time the endmill lickily survived this part and broke just after that on the easy place. Anyways I blew away all chips and coolant and started examining, what I found was both obvious and very strange.
    On the base two corners of the "triangle" the mill engages with its full diameter for a short time, I was worried about this at the start but all seemed fine.
    After I examined the cut thoroughly I found out that the cut is fine on one side (the one that is farther from me) and like a stairway on the other (The one closer to me). In the places where the triangle's base was less or more than 90 degrees to the X axis there was a very slight stairway pattern. It was only the places where the tool was moving entirely by the Y axis that this occurred. Here are some pics.

    First this is the toolpath:

    The problematic part is on the bottom left and right. However when viewed from the front I usually only see the farther corners, and here is what I see:

    Looks like a clean cut no different than the rest. Actually part of the stairway pattern is seen in the opposite corner, but that is due to the cameras angle and closeup, and the fact that I cleaned everything. From my normal position this is invisible. Anyways, now looking at the opposite sides, where the pattern shows:


    This I believe is a sign of severe tool deflection, but I can not understand why it occurs on just one side, given the fact that the toolpath is symetrical. If you look closely, it seems that the tool has gone a bit further than in the opposite corner. The two corners are not the same, but they should be.
    And the pattern is more visible when this corner is pointed towards me (the tool moves on the (-)Y direction).
    I should first examine the G-Code and see if the problem is not within it, before I blame this on the machine, but the fact that this occurs mostly in one particular direction, makes me think that the machine indeed has something to do with this problem.

    Anyways, in order to be able to finish this thing I will alter the toolpath to avoid working in those corners with the 6mm endmill.
    Something like this


    Or maybe try it even safer (and slower) like this


    Edit: Just thought of something. The direction towards me is the direction from which the mist cooling is blowing on the mill. Could it be that it is not able to blow away the chips in this direction, and this leads to the deflection?

    Attached Thumbnails Attached Thumbnails Need advice milling aluminum, broke endmill after 2 hours of milling-path-jpg   Need advice milling aluminum, broke endmill after 2 hours of milling-cut-clean-jpg   Need advice milling aluminum, broke endmill after 2 hours of milling-patt1-jpg   Need advice milling aluminum, broke endmill after 2 hours of milling-patt2-jpg  

    Need advice milling aluminum, broke endmill after 2 hours of milling-patt3-jpg   Need advice milling aluminum, broke endmill after 2 hours of milling-patt4-jpg  
    Last edited by zeox; 06-17-2017 at 10:00 PM.


  14. #14
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Just little update.
    Need advice milling aluminum, broke endmill after 2 hours of milling-12-jpgNeed advice milling aluminum, broke endmill after 2 hours of milling-13-jpg

    After a few more tool breakages, I not only altered the tool path, but lowered the rpm/feed and depth/stepover. You can see that the cut looks much better on those newly cut "triangles".

    I am now working at 1mm increments (both depth and stepover) 375mm/min feedrate and 8540rpm. So far I've been cutting for 6 hours without a breakage.
    It is taking forever, but I have no other option.

    I am also now using an emulsion for cooling, works great. After 4 hours of non-stop cutting and the workpiece is still cold.

    I am seriously considering an upgrade now. Been looking at some chinese routers.

    This one
    Mini woodworking cnc router 1212 for advertise sign making,DSP controller - Woodworking cnc router_wood cnc _Acctek Machinery - CNC MACHINES MANUFACTURER FROM CHINA-AccTek Machinery-

    Looks nice, I can order it with an upgraded 3kW spindle. And I can also add a second low rpm spindle (1200-9000rpm) so I can work with larger diameter tools at low rpm.
    All in all with all the extras it will cost about 5500$. Has a built in cooling system, stainless steel tray for coolant collection. It will be a significant upgrade from my current rig.



  15. #15
    Member dharmic's Avatar
    Join Date
    May 2015
    Location
    Australia
    Posts
    1422
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Don't forget that, when comparing one side with the other, on one the torque on the tool will be pushing it into the corner and the other will be trying to spit it out.

    Glad you got it sorted though.



  16. #16
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    As I need to repeat almost the same cut on the other side, I'll try to speed things up by using an 8mm endmill for the triangle shapes.
    Also The crabide 6mm mills that I have ordered should arrive soon, which should allow me to further speed things up.

    I have a lot of cutting to do with a 3mm endmill, but after I'm finished with those prototypes I'm thinking about simplifying the shape, so they can be cut mostly with a 6mm end mill.
    I'll get one of those 14 prototype pieces and use a dremel to cut the fins, and see if it affects its cooling capabilities. If all goes ok, I'll scrap the fins, and it will be much easier to cut those shapes.



  17. #17
    Registered
    Join Date
    Jan 2017
    Location
    Bulgaria
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    I was probably a bit too quick to celebrate
    Today after 3 more hours of cutting, the endmill broke again. This time however there was a visible wear on the tool. I guess that is the most that these mills can do. About 9 hours of cutting.
    This was the last of my batch of chinese 6mm HSS endmills.

    I obtained locally two more 6mm 2 flute HSS endmills, made in Russia. They have shorter flute length, but also a lower helix angle.
    Here is a picture of the broken chinese end mill next to the new russian one:


    Since these russian mills have shorter flutes, I was able to reduce the stickout. It was 33mm on the chinese mills (that was their flute length), with the russian mills the stickout is 26mm (I can make it even less, but I don't want to block the coolant mist, the deepest cut is 20.2 mm).
    With the lower helix angle and the reduced stickout, everything sounded much better. Especially when doing a helix ramp. I figured those end mills could take some more abuse.

    So I overided the feed rate to 450 mm/min (+20%) and increased the rpm just a bit to 8700 rpm, and so far everything looks and sounds better.
    If this endmill takes more than 9 hours of milling, it will be my new favourite, as they are really cheap (about 3.5$ a piece)

    Attached Thumbnails Attached Thumbnails Need advice milling aluminum, broke endmill after 2 hours of milling-wp_20170627_22_15_51_pro-jpg  


  18. #18
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    The Russian cutting tools I have purchased have been pretty good quality.



  19. #19
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Need advice milling aluminum, broke endmill after 2 hours of milling

    Like Jim, I use kero for misting, but I mix (cheap) olive oil in at 3 parts kero to 1 part olive oil. I use pulsed misting, down to 1/2 sec pulse every 20 seconds. The oil seems to 'wet' the cutter much better imho and prevents the dreaded Built Up Edge which snaps cutters. And olive oil is skin-compatible!

    Cheers
    Roger



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

Need advice milling aluminum, broke endmill after 2 hours of milling

Need advice milling aluminum, broke endmill after 2 hours of milling