Cutting 1" thick aluminum on CNC


Page 1 of 2 12 LastLast
Results 1 to 12 of 24

Thread: Cutting 1" thick aluminum on CNC

  1. #1
    Registered
    Join Date
    Mar 2016
    Location
    Canada
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Cutting 1" thick aluminum on CNC

    Hi,

    I need to cut quite a few 1" thick aluminum parts for my DIY CNC router. I tested a 1/4" diameter 1-1/4" flute length single flute carbine end mill from tools today. I used G-Wizard to calculate all parameters of the cut making sure to be as conservative as possible the first time. My work was clamped directly to the surface of the machine which is an industrial 5' x 10' router made by AXYZ. There was minimal vibration in the cut as this is such a large machine and the work was clamped well.

    I broke two cutters at the top of the flute where the shank meets the flutes. Both times happened within a minute of cutting. The second one broke just touching the material with a very slow plunge rate. I should note it was a straight plunge and not a sprial or other type. Blew around $100 in a half hour. Before I cut again I need to figure out a new plan.

    I'm wondering why this happened. After I moved to a much shorter bit with a flute length of 3/8" made by onsrud, I cut 20 1/4" thick parts quite aggressively with no issues. The tool looks like it has much life left in it. I was cutting at 1/8" DOC and a 40 in/min feedrate and 18000 RPM. I was cutting with constant compressed air and a generous amount of WD-40 in this cut and my failed attempts.

    So either the vibrations induced in the machine were too high for that cutter length, and caused it to break pre-maturely. Or onsrud makes better bits than tools today. All aluminum cutting bits I used in high school were onsrud and I never experienced breaks like this. The bits just seemed to keep on going without fault.

    If the 1-1/4" cutter doesn't work for me, would it be possible for me to use a cutter with say a 1/2" flute length to cut 1" deep? As long as the shank matches the flute diameter to allow it to enter the cut the flutes have made, and I can successfully clear all chips using compressed air, I should be good right?

    Perhaps a 2 flute carbide is preferable?

    All input appreciated.

    Thanks,

    Matthew

    Similar Threads:


  2. #2
    Registered
    Join Date
    Apr 2015
    Location
    Canada
    Posts
    107
    Downloads
    0
    Uploads
    0

    Default Re: Cutting 1" thick aluminum on CNC

    single flute bits are very weak. Try a 3 flute with a higher feed or lower RP/m

    Luthier/Woodworker/Machinist in NS, Canada.


  3. #3
    Gold Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5312
    Downloads
    0
    Uploads
    0

    Default Re: Cutting 1" thick aluminum on CNC

    The Amana bits are not as polished as the Onsrud. But I've used them no problem. I think you're actually too slow...



  4. #4
    Registered KH0UJ's Avatar
    Join Date
    Jul 2016
    Location
    Philippines
    Posts
    563
    Downloads
    0
    Uploads
    0

    Default Re: Cutting 1" thick aluminum on CNC

    @ OP You mean like this?

    Cutting 1" thick aluminum on CNC-20171031_091835-jpg

    Cutting 1" thick aluminum on CNC-20171031_163821-jpg

    Cutting 1" thick aluminum on CNC-20171102_142033-jpg

    it`s a 40mm thick aluminum being cut by an ordinary 2 flute 1/4 carbide bit for wood worth $1.25 on a 24K spindle, on my opinion, if you cut more than 10 pieces the 1/4 (2 flute) carbide bit lets you cut two weeks of cutting work (8 hours/day) without worrying of getting dull, but if you cut less than 10 pieces the most efficient way to do it is to use a 1/8 carbide bit, very efficient in terms of material being used, the route path is only 1/8 compared to a 1/4 thick wasted aluminum material.

    Attached Thumbnails Attached Thumbnails Cutting 1" thick aluminum on CNC-20171102_142033-jpg   Cutting 1" thick aluminum on CNC-20171031_163821-jpg   Cutting 1" thick aluminum on CNC-20171031_091835-jpg  


  5. #5
    Gold Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    1870
    Downloads
    0
    Uploads
    0

    Default Re: Cutting 1" thick aluminum on CNC

    If you are going to do a straight plunge, make sure your bits are center cutting. It's best to ramp or spiral in, end mills don't like to plunge in the best of conditions. Many times I drill a pilot hole where the bit will plunge. As said above, a 2 or 3 flute bit would be my choice.

    Jim Dawson
    Sandy, Oregon, USA


  6. #6
    Registered
    Join Date
    Mar 2008
    Location
    USA
    Posts
    448
    Downloads
    0
    Uploads
    0

    Default Re: Cutting 1" thick aluminum on CNC

    Why 18k RPM? Sounds too high. And I don't like using WD40 for cutting fluid. It is a lubricant / water repellent. Not a cutting fluid. Get yourself some A9 or other. I too have Gwizard. but I don't use it. It can sometimes be useful for a starting point but some of the calculations in real world applications are way out of what actually works. Just see what happy compromise you can find that works for your particular machine, cutter, and the AL.

    The problem is here "1/4" diameter 1-1/4" flute length single flute carbine". That cutter is so weak and flimsy even the centrifugal force at 18k will snap it without a super rigid machine. A bit like that shouldn't be used for roughing 1" thick aluminum. Use a larger bit for roughing, and if needed use the 1/4 for finishing. Personally. I would never use a 1/4 single flute bit with a 1 1/4 DOC for anything other than extremely small steps, DOC,on a finishing operation. If you are stuck using a 1/4 collet then find yourself a 2 or 3 flute bit made for cutting aluminum. Another option is what kind of toolpath operation you are using. If you have a HSM option use that for your slotting then finish the walls with a light pass or 2 for clean up.

    Onsrud makes fantastic bits for routers that cut wood, composites, and exotics. But I've never used them for aluminum or steel.



  7. #7
    Gold Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5312
    Downloads
    0
    Uploads
    0

    Default Re: Cutting 1" thick aluminum on CNC

    Onsrud makes tools for rhe aerospace induatry with up to 12 flute tools for the hardest materials... including MCD and PCD tooling.

    Also, regardless of what people think, WD-40 corporation themselves list their product as a lubricant. Which is basically solvent (similar to lighter fluid), oil, and a propellant if using the aerosol.

    I'd agree that .25" diameter is probably too small for this work and think 3/8" would be better. The Amana O flutes are center cutting if I remember correctly, but j feel ramping in reduces the pressure on the bit. Clearance helps; what I do is start about .020 away from the finished part, and step in about .004 with each depth pass. This way you end up with clearance on one side of the tool. If you just profile, you have zero clearance and 180° engagement, so if your slot is not clean and lubed, and your spindle not perfectly trammed, you'll run inyo issues like excessive tool load and recutting chips.



  8. #8
    Registered
    Join Date
    Mar 2016
    Location
    Canada
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: Cutting 1" thick aluminum on CNC

    Thanks for all your info guys. Definitely wont be using the cutter again for roughing passes. My problem is I'm limited to a 1/4 cutter for all inside holes and pockets since all my holes are 1/4" or a little over 1/4" but almost all are smaller than 3/8" so I can't move up a fraction size for all inside features. For profiling I will opt for the larger diameter 2 or 3 flute and for the smaller holes and pockets I will use a 1/4" 2 or 3 flute. I'll also be trying a ramp in on the profile and spiral for the holes.

    But what flute length should I use for the smaller inside holes? Is it safe to use a flute length lower than my total DOC? I feel most comfortable choosing the shortest bit possible to minimize deflection, but is there a rule of thumb for this sort of situation? I would think chip clearance is the only issues since the shank is the same size as the bit (or even slightly smaller - I measured an amana shank and it was a half thou undersized) so I think the shank should clear the walls that the cutter is creating as it plunges deeper. I'm thinking I can retract on every plunge and the compressed air should clear the chips for the next cut. otherwise I suspect that with a hole roughly the same diameter of the bit will get clogged with chips since they have no where to escape, especially with more flutes.

    I will look into if RhinoCAM is capable of doing step-over passes with each profile plunge. We have MasterCAM as well but I haven't been trained on it yet and my boss prefers we stick with RhinoCAM since all cutting outside mine is wood and plastics. This makes sense to me for chip evacuation and I can see why 180 degree engagement would be an issue. Thanks for the tip.



  9. #9
    Registered
    Join Date
    May 2011
    Location
    Canada
    Posts
    593
    Downloads
    0
    Uploads
    0

    Default Re: Cutting 1" thick aluminum on CNC

    OK, so you're not hogging it out, the 1" piece, you're making holes?

    Peck drill them. Using a drill bit. Then finish on a drill press with the exact bit size (assuming you don't have a collet for the exact bit size for the CNC). I'm saying to get a bit set with all the in between sizes, or at least the couple bits you need, you should find something that will work within the numbered / lettered odd size drill bits.

    For the countersink, you could CNC those with a 1/4" bit after you peck drill. I've never used any of the single flute bits, I have done CNC countersinks with a 1/4" 4 flute carbide bit, worked out nicely. Mostly when I countersink, I do it on my mini mill, 1/2" or 3/4" center cutting cheap end mill countersinks well in aluminum, just peck at it the same as you would do with a drill bit.

    As others have mentioned, the depth of cut was too much and the RPM was too high. For a long 1/4" bit I personally would use less than 1mm DOC, perhaps even half a mm.

    Quote Originally Posted by Matthew_ View Post

    If the 1-1/4" cutter doesn't work for me, would it be possible for me to use a cutter with say a 1/2" flute length to cut 1" deep? As long as the shank matches the flute diameter to allow it to enter the cut the flutes have made, and I can successfully clear all chips using compressed air, I should be good right?
    No, you never want to cut beyond the length of flute you are using if there is a possibility based on the geometry (ie square pocket) of the shank touching the sides. You could if you had a step down like a pyramid where the tool shank could never touch the side of the work piece.



  10. #10
    Gold Member
    Join Date
    May 2005
    Location
    USA
    Posts
    3344
    Downloads
    0
    Uploads
    0

    Default

    This fact from Jim is very important, rven two flute center cottong end mills dont like to be plunged directly into the work. Use some sort of interpolation.

    As for your carbide, quality could be an issue. I have to woder if there is an Aluminum specific coating on the end mills. Some coatings designed for other metals don't work well with aluminum. So this brings up a question is there signs of welding to the cutter?

    Quote Originally Posted by Jim Dawson View Post
    If you are going to do a straight plunge, make sure your bits are center cutting. It's best to ramp or spiral in, end mills don't like to plunge in the best of conditions. Many times I drill a pilot hole where the bit will plunge. As said above, a 2 or 3 flute bit would be my choice.




  11. #11
    Gold Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5312
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by NIC 77 View Post
    OK, so you're not hogging it out, the 1" piece, you're making holes?

    Peck drill them. Using a drill bit. Then finish on a drill press with the exact bit size (assuming you don't have a collet for the exact bit size for the CNC). I'm saying to get a bit set with all the in between sizes, or at least the couple bits you need, you should find something that will work within the numbered / lettered odd size drill bits.

    For the countersink, you could CNC those with a 1/4" bit after you peck drill. I've never used any of the single flute bits, I have done CNC countersinks with a 1/4" 4 flute carbide bit, worked out nicely. Mostly when I countersink, I do it on my mini mill, 1/2" or 3/4" center cutting cheap end mill countersinks well in aluminum, just peck at it the same as you would do with a drill bit.

    As others have mentioned, the depth of cut was too much and the RPM was too high. For a long 1/4" bit I personally would use less than 1mm DOC, perhaps even half a mm.



    No, you never want to cut beyond the length of flute you are using if there is a possibility based on the geometry (ie square pocket) of the shank touching the sides. You could if you had a step down like a pyramid where the tool shank could never touch the side of the work piece.
    A single edge spiral O flute IS DESIGNED for high spindle speed applications, for the exact same reason you'd use a 3 or 4 flute on a manual mill.

    You can get an endmill that's necked, meankng that the shaft is narrowed above the flutes to the shank.



  12. #12
    Gold Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5312
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by wizard View Post
    This fact from Jim is very important, rven two flute center cottong end mills dont like to be plunged directly into the work. Use some sort of interpolation.

    As for your carbide, quality could be an issue. I have to woder if there is an Aluminum specific coating on the end mills. Some coatings designed for other metals don't work well with aluminum. So this brings up a question is there signs of welding to the cutter?
    Coatings that have aluminum! Like TiAlN... designed for harder materials. The Amana O flute bits in question are uncoated. They are center cutting too, but best to ramp them.



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

Cutting 1" thick aluminum on CNC
Cutting 1" thick aluminum on CNC