Need Help! Breaking Cutters is breaking me

Page 1 of 2 12 LastLast
Results 1 to 20 of 27

Thread: Breaking Cutters is breaking me

  1. #1
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Question Breaking Cutters is breaking me

    Hi Guys,
    New member here "literally" and i have a question that i can not seem to get an answer to. I am a Cue builder by trade and have recently started working with metal (Aluminum) to be presice. I am using the chinese 3040T with 4th / Mach3 / Vetric max spindle speed is roughly 12,800.
    With that being said and i hope it helps, I am struggling to cut .125" aluminum flat stock. I am machining (or trying to) rather small parts and need to use a .0315 endmill to cut the part. It is the largest i can use. I do not know much about feeds and speeds and this is a different world for as i normally maching exotic woods. I can not stop breakng the Cutter can anyone help?

    Similar Threads:


  2. #2
    Member
    Join Date
    Feb 2009
    Location
    usa
    Posts
    6028
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    What type of aluminum? And what are you using for coolant and feedrate?

    Sent from my SM-T813 using Tapatalk



  3. #3
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Thank you for responding...
    I am milling flat stock purchased at lowes so i am sure it is not 6061. as far as feed and speed i have tried many different combinations but the last was as follows:

    DOC Per Pass = .005"
    Feed Rate = 3 IPM
    Spindle Speed = 10,753
    Air blast only



  4. #4
    Member handlewanker's Avatar
    Join Date
    Sep 2006
    Location
    Australia
    Posts
    6463
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Yessssss.............a .0315" diam end mill....... (how the heck do they make them that small).......is by any stretch of the imagination a very tiny cutter and the lands that the chips end up in get clogged by the aluminium sticking in there and blocking the path of the cutter's ability to penetrate into the next bit of material after the tooth has shaved off a chip

    If you're cutting dry that will exacerbate the problem as ally will heat up, soften and stick to the relatively rough surface of the land behind the tooth instead of ejecting like a rocket.

    Most people try some form of coolant like Kerosene, WD40......Milk???....or just plain water based coolant......anything to keep the cutter end wet and/or oily and provide a non stick environment to the swarf.

    Another reason why the Tin coated cutters (gold coloured) are used for that purpose to provide a non stick finish.

    The problem is when the land is blocked with a chip the feed rate will immediately break the cutter due to forces acting against it.

    With high speed the chip is heated and softened making it stick to the cutter......feeding more material against the cutter .......breaks it........imagine the hard cold ally material becoming almost like putty when it gets hot.....it deforms and rolls around into the land and stays there.

    My opinion is to keep the ally as cold as possible and lubricated......mist coolant and air blast is one solution.

    Also, you're working with a moving gantry machine .....not the most rigid machining platform......and there is also the possibility that the speed and feed rate are causing the X axis framework to deflect and make the cutter dig in when the feed rate overcomes the deflection.

    This will happen when the cutter is loaded with swarf and cannot cut but pushes like a solid pin against a solid piece of material especially when to the left or right and far off centre where the gantry can deflect away from the Y axis screw which is central.

    If you have a significant amount of backlash that will cause a problem too.

    With a tiny cutter like that the Z axis is hanging right down on the table and so you get cantilevering forces from the cutter acting against the X axis cross beam and trying to twist it.
    Ian.



  5. #5
    Member
    Join Date
    Feb 2009
    Location
    usa
    Posts
    6028
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    And watch the Lowe's junk. Some of that stuff is 20 series gummy ****e.

    Sent from my SM-T813 using Tapatalk



  6. #6
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    I only have the means of air blasting at the moment and can not sit there for 3 hours with an air hose lol. any suggestions asf ar as my settings based on the cutter size? The machine is very rigid considering the machine.



  7. #7
    Member
    Join Date
    Feb 2009
    Location
    usa
    Posts
    6028
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Your not going to get anywhere with a small cutter in aluminum without lube. Just get a air tool oiler from harbor freight, plumb it in line and fill it with olive oil. Set to drip every 10 or so seconds. Works like a charm, and no smell.

    Sent from my SM-T813 using Tapatalk



  8. #8
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Not a bad idea and i will try this. but what about my feeds and speeds are they close? im guessing here lol



  9. #9
    Member
    Join Date
    Feb 2009
    Location
    usa
    Posts
    6028
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Might be a bit slow on the feedrate at 10k. Carbide or hss?

    Sent from my SM-T813 using Tapatalk



  10. #10
    Member
    Join Date
    Feb 2009
    Location
    usa
    Posts
    6028
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Here is a quick calculator. It shows your 10x too slow.
    Feed Rate Calculator

    Sent from my SM-T813 using Tapatalk



  11. #11
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    I am not sure what that aluminum is that comes from the big box stores, but I think it's part butter. Nasty gooey stuff to machine, and normally has a hard anodized surface which makes even harder to machine and hard on end mills.

    I agree with Ian above. Coolant/lubricant is required, kerosene or WD-40 is your best bet. To run an endmill that small really requires a rigid machine, but I think your problem is aluminum welding to the tool bit. You might bump your feed up to 5 or 6 IPM and see if that is any better, that way the endmill might be cutting rather than rubbing which will dull the tool bit quickly and also cause breakage. If possible, make a roughing pass(s) with a 1/8 carbide tipped router bit and leave 0.005 for finish, then finish with the 0.031 endmill, that way you just have to trim out the corner radii with the 0.031 endmill. I would suggest a solid carbide endmill, but I think that your machine is not rigid enough to have good results.



  12. #12
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Using carbide and as a foot note i can mill with perfection using a 1/8" if this helps



  13. #13
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Quote Originally Posted by ChrisWalker View Post
    Using carbide and as a foot note i can mill with perfection using a 1/8" if this helps
    That is what I was getting at above, I'm sure it runs just fine with a 1/8''. A carbide endmill is much less forgiving to vibration and minor deviations than HSS. The smaller the endmill the more rigid the machine needs to be.



  14. #14
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    And as was mentioned, the aluminum at Lowes is the gummy type.
    Get some 6061 and it should be better, but you're going to have an uphill battle.

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  15. #15
    Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5516
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Hardware store aluminum is gummy 6063, or worse 3003. You can mill them effectively, BUT I'd recommend a low helix end mill. This would help break up the "stringiness" in the chips, which should help prevent build up on the tool. I would also use a coated tool such as ZrN, TiN, TiCN, CVD, and recommend a lubricant such as WD-40 at the least. Also if you're using a high speed spindle, use a si gle flute tool. LMT/Onsrud sells a tool specifically for this, though they only currently have 3/16" and 1/4".



  16. #16
    Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5516
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Also rough with a 1/4" endmill, then re-rough with progressively smaller endmills till you get to your smallest for the finish pass. This will give clearance for the chips that are invariably jamming up the small slots and pockets. Air gun and/or brush to help out. Also get the shank of the tool in that collet. Very little of the shank should show, which should ensure the least run out possible.



  17. #17
    Member
    Join Date
    Jul 2014
    Posts
    215
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Quote Originally Posted by ChrisWalker View Post
    Thank you for responding...
    I am milling flat stock purchased at lowes so i am sure it is not 6061. as far as feed and speed i have tried many different combinations but the last was as follows:

    DOC Per Pass = .005"
    Feed Rate = 3 IPM
    Spindle Speed = 10,753
    Air blast only
    The small stock they sell at Lowes is not likely 6061. It is probably a softer aluminum alloy which will be more gummy and harder to mill. Check to see if the aluminum stock says 6061.
    The softer alloys are often used for building trim and for general fabrication. They are not suitable for some kinds of parts.

    When using small cutting tools you need a high degree of rigidity in the machine tool. Small errors can break the cutting tool. By rigidity standards for mills the 3040T is a wet noodle. But you still may be able to succeed to some degree.
    One of the big problems when milling small parts is holding them down so they don't move or vibrate. You may need to create a special soft jaw vice in the shape of the part to hold it properly.

    Also, are you face milling or side milling. You may need adjust your strategy or fixturing method to reduce the cutting forces. Or change your method so you can use a larger cutting tool. With cutting tools that small you will have to get the feeds and speeds just right. You will need to
    get a machinist textbook or handbook and start with a simple calculation to make sure you are close to the ballpark. You really should be using flood coolant for that just to keep all of the chips clear
    and the tool cool. The kind of machine you have is not really designed to do that. The problem with milling soft metals is that they gum up the cutting blades and mist coolants and small hand shots just help the small chips to gum up more. That's why you needs lots of flood coolant to keep the
    chips away from the cutter.

    You would most likely have the best success with air to blow away the chips with that mill. The high spindle speed on a small mill like that makes it more suitable for engraving than milling.

    You need to find out what the chip load is for that milling cutter from the manufacturer is. Then your rpm and feed needs to be in the range that the cutter can handle for it's chip load. You can't just use any values of speed or feed. If you go too slow in gummy material the metals will just build up
    on the tool edge and start creating high cutting forces and vibration. Then the tool will break. On the other hand, if you go to fast you will also create too high cutting forces and the tool will also break.

    Here is a link to website that can help you calculate the right speeds.

    Spindle RPM & Feed Rates | Calculate Chip Load per Tooth

    I'm estimating the chip load for a .0315 mill is about .001 and that may be generous. So by my calculations your feed rate is way off. It should be around 20-22 IPM. At 10750 RPM. That is for a two flute end mill.

    Here is a website that will give you more accurate results because they use cutting speed in SFM (surface feet per minute). That is how fast the tool tip is moving through the material. It is not the feed rate.

    Feed Rate Calculator

    My guess is that you are using some of the 2024 stuff form Lowes. I would find another source unless you need a soft alloy for your application.

    That website recommends a cutting speed of 200 SFM for 2024 aluminum with a HSS cutter. Doesn't list for carbide.

    Calculations give about 21.5 IPM for the feed rate at 10750 RPM and a .001 chip load.

    Bear in mind that these calculations assume a somewhat rigid commercial machine which is typical for a commercial CNC machine. Your little machine may not be rigid enough for these calculations and so both the RPM and the feed rate may need to be slowed down.

    For the 3 IPM feedrate that you mentioned you would need to slow down your RPM to 1500 rpm.

    Last edited by Hezz; 06-29-2017 at 02:42 PM.


  18. #18
    Member
    Join Date
    Mar 2012
    Location
    USA
    Posts
    378
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    As others have said, you are most likely using gummy 6063. I would buy 6061 from somewhere else. You are also likely using a machine that is not ridged enough for what you are trying to do. If that is the case you will need to do the cuts in more depth passes. You may also need to lower your RPM or use a bit with less flutes because you can't move your axes fast enough. See the link I have below.

    I recommend downloading the trial copy of the CNCcookbook feed rate calculator and reading some of the very good articles on their web site. That will help you a lot once you understand what is going on. I would start here: Complete Guide to CNC Mill Feeds and Speeds



  19. #19
    Member handlewanker's Avatar
    Join Date
    Sep 2006
    Location
    Australia
    Posts
    6463
    Downloads
    0
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Hi, one other thing that applies to all soft materials.......the cutter must be sharp, high top rake etc, not previously used on steel that takes the edge off,

    I think you could get good results with a single tooth flat bladed cutter in carbide........it has no gullet between the teeth, as in a multi tooth end mill cutter so cannot trap swarf, but swarf can stick to the cutting edge so coolant is a must.

    The big problem with that soft material is, if the cutter isn't sharp enough to cut it. the material is just being bulldozed and eventually makes a ball of swarf.

    I cut soft ductile aluminium with a fly cutter that has a single pointed very sharp hook..... or top rake.... and a fine honed edge......under a microscope the edge should not look like it has a saw tooth cutting edge profile.....otherwise it grabs the material and holds onto it instead of it sliding off the face.....coolant is a must.

    BTW.....the rule of 4D for deflection forces applies here........at .78mm diam (.031") the length of stick out from the collet face should not exceed 3mm.

    Going to a larger scale, imagine trying to mill a side face with a 25mm diam cutter that sticks out 200mm....that's 8D......for 4D to apply the stick out would be 100mm.
    Ian.



  20. #20
    Member
    Join Date
    Apr 2013
    Location
    Sweden
    Posts
    1899
    Downloads
    2
    Uploads
    0

    Default Re: Breaking Cutters is breaking me

    Quote Originally Posted by handlewanker View Post
    Yessssss.............a .0315" diam end mill....... (how the heck do they make them that small)......
    ...the smallest I am using is half that size... but VERY carefully and only in Delrin.

    https://www.youtube.com/c/AdaptingCamera/videos
    https://adapting-camera.blogspot.com


Page 1 of 2 12 LastLast

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

Breaking Cutters is breaking me

Breaking Cutters is breaking me