584,865 active members*
5,013 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 24
  1. #1
    Join Date
    Mar 2016
    Posts
    9

    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

  2. #2
    Join Date
    Apr 2015
    Posts
    113

    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
    Join Date
    Apr 2009
    Posts
    5516

    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
    Join Date
    Jul 2016
    Posts
    660

    Re: Cutting 1" thick aluminum on CNC

    @ OP You mean like this?







    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.

  5. #5
    Join Date
    Dec 2013
    Posts
    5717

    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
    Join Date
    Mar 2008
    Posts
    683

    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
    Join Date
    Apr 2009
    Posts
    5516

    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
    Join Date
    Mar 2016
    Posts
    9

    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
    Join Date
    May 2011
    Posts
    790

    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
    Join Date
    May 2005
    Posts
    3920
    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
    Join Date
    Apr 2009
    Posts
    5516
    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
    Join Date
    Apr 2009
    Posts
    5516
    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.

  13. #13
    Join Date
    May 2011
    Posts
    790

    Re: Cutting 1" thick aluminum on CNC

    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.
    I countersink holes in aluminum all the time this way on my hand operated mill, never had a problem, always peck drill them. Usually I have the hole already drilled that I am doing the countersink for. I don't use a high RPM (mill can't even do high RPMs) and I go very slow, so you know what, this is probably easier to mess up on a CNC machine, because like I said, I do it all the time on my small mill, no problems.

    For countersinking on a CNC I'd use the 4 flute 1/4" bit I mentioned previously, and cut out the larger circle and I have done this before also many times with no problems.

  14. #14
    Join Date
    Apr 2009
    Posts
    5516
    Quote Originally Posted by NIC 77 View Post
    I countersink holes in aluminum all the time this way on my hand operated mill, never had a problem, always peck drill them. Usually I have the hole already drilled that I am doing the countersink for. I don't use a high RPM (mill can't even do high RPMs) and I go very slow, so you know what, this is probably easier to mess up on a CNC machine, because like I said, I do it all the time on my small mill, no problems.

    For countersinking on a CNC I'd use the 4 flute 1/4" bit I mentioned previously, and cut out the larger circle and I have done this before also many times with no problems.
    Technically it's counterboring... since a mill typically has a slower RPM, and slower (manual) operation, many flutes are used so that each cutting edge meets the specs for chipload and SFM. Typically on a router, higher speed spindles are used, so unless one sets the feedrate very high (which may violate the SFM rating of the tool), a single flute tool is used, thus allowing the correct chipload at the higher RPM.

  15. #15
    Join Date
    Apr 2015
    Posts
    113

    Re: Cutting 1" thick aluminum on CNC

    Louie, chip load and feed have no effect on the SFM. The only variables are bit diameter and the RPM. Aluminum is good for 50-1000+ sfm as long as chip evac is there. On my manual mill at 1400rpm I still use a single flute countersink.
    A counter bore is a cyclinder pocket, usually concentric with a drilled hole. A counter sink is a drafted or angled wall
    Luthier/Woodworker/Machinist in NS, Canada.

  16. #16
    Join Date
    May 2005
    Posts
    3920
    Countersinking is a bit different if you have a predrilled hole.

    As for using a two flute end mill in solid aluminum im still of the opinion that they really dont like to be plunged into the material. At least that is my experoence with a limited number of two flute end mills that ive used. In a nut shell you can't feed them like a drill bit.

    As for the original poster it would be great to have more info. Im wondering if the cutter is loading up or maybe he just got a bad batch. Also im left a bit confused because it sounds like what he is trying to do is to put round holes in the plate something better done with drill bits. Sometimes with these posts what i think is being done or happening is completely different than what is actually going on. This could be the case here because originally i thought the problem was with cutting out some sort if shape out of that Aluminum.

    Quote Originally Posted by NIC 77 View Post
    I countersink holes in aluminum all the time this way on my hand operated mill, never had a problem, always peck drill them. Usually I have the hole already drilled that I am doing the countersink for. I don't use a high RPM (mill can't even do high RPMs) and I go very slow, so you know what, this is probably easier to mess up on a CNC machine, because like I said, I do it all the time on my small mill, no problems.

    For countersinking on a CNC I'd use the 4 flute 1/4" bit I mentioned previously, and cut out the larger circle and I have done this before also many times with no problems.

  17. #17
    Join Date
    Apr 2009
    Posts
    5516
    Quote Originally Posted by jahnj0584 View Post
    Louie, chip load and feed have no effect on the SFM. The only variables are bit diameter and the RPM. Aluminum is good for 50-1000+ sfm as long as chip evac is there. On my manual mill at 1400rpm I still use a single flute countersink.
    A counter bore is a cyclinder pocket, usually concentric with a drilled hole. A counter sink is a drafted or angled wall
    Yes, I know that. My point was that while a theoretical feedrate xan be calculated, it isn't necessarily acievable due to the manufacturer SFM rating. Just can't type as fast as my mind thinks with 2 thumbs and a 5" screen.....

  18. #18
    Join Date
    Dec 2014
    Posts
    640

    Re: Cutting 1" thick aluminum on CNC

    Knowing that my CNC machine was designed to cut wood, I'd probably just peck a hole deep enough in the aluminum to be able to take the piece to my drill press...counter sink it and drill it out there. The thickest aluminum I've cut is 1/8" and I had no issues with a single flute bit. My feeds and speeds were very, very conservative.

  19. #19
    Join Date
    Mar 2016
    Posts
    9

    Re: Cutting 1" thick aluminum on CNC

    Quote Originally Posted by wizard View Post
    Countersinking is a bit different if you have a predrilled hole.

    As for using a two flute end mill in solid aluminum im still of the opinion that they really dont like to be plunged into the material. At least that is my experoence with a limited number of two flute end mills that ive used. In a nut shell you can't feed them like a drill bit.

    As for the original poster it would be great to have more info. Im wondering if the cutter is loading up or maybe he just got a bad batch. Also im left a bit confused because it sounds like what he is trying to do is to put round holes in the plate something better done with drill bits. Sometimes with these posts what i think is being done or happening is completely different than what is actually going on. This could be the case here because originally i thought the problem was with cutting out some sort if shape out of that Aluminum.
    The bits had zero wear on them before using. They were brand new. The first bit broke very quickly while machining the profile, and not the plunge. The first bit made it through the plunge fine and broke after a minute of profiling while still in the profile. The second bit snapped same spot but on the instant it touched the material on the plunge. It wasn't even like the bit stalled for a second, not being able to plunge, it was like an instant snap the instant it made contact. I think this is due to it's long flute length, and not being designed for plunging. The fact I was able to finish the job with a much shorter bit without issue, and many of the same short single flute bits in the past, tells me that bit wasn't suited for my needs. It's probably intended to be used with very shallow cuts.

    I have decided to buy a 3/8" 2 flute HSS Onsrud bit since I can get them from a shop near home. I will use this for all the profiling. I have a 1/4" carbide spot drill I can use to mark out the through holes in the parts, and buy the required bits for drilling on the drill press. This was my method for all the steel in my machine, and works beautifully. I can use a 1/4" or 3/16" 2 flute short length bit for all the counterboring for screw heads. I may buy a 4 flute 1/4" for finishing passes, but I'll have to test the finish I get with the 3/8" cuter first.

    The thickest aluminum plate I've cut before this was 3/8" on a router, so I went into it thinking about machining everything in one go on the router, but the suggestions here point to spot drilling and finishing on a drill press or mill.

  20. #20
    Join Date
    Feb 2007
    Posts
    711

    Re: Cutting 1" thick aluminum on CNC

    I have cut 30mm aluminum plate on my cnc wood router, using both a cheap chinese 6mm x 30mm long single flute solid carbide, and a home depot freud 2 flute spiral solid carbide bit with only a 1" cut depth.

    If this is a one off job and you don't need to maximize effeciency, just use a very small step down, like 0.050" and take like 0.001" per tooth, while babysitting to clear the chips.

Page 1 of 2 12

Similar Threads

  1. Replies: 21
    Last Post: 01-13-2014, 04:10 AM
  2. My 1/2" Thick Aluminum Build
    By kolias in forum Open Source CNC Machine Designs
    Replies: 36
    Last Post: 12-10-2012, 06:58 AM
  3. aluminum shape cut 0.05" thick
    By threeninethree in forum North America RFQ's
    Replies: 5
    Last Post: 10-06-2012, 07:13 PM
  4. Replies: 5
    Last Post: 09-12-2012, 03:09 PM
  5. Rockwell blade runner good for cutting 2-3" thick aluminum?
    By autobot in forum Uncategorised MetalWorking Machines
    Replies: 3
    Last Post: 02-03-2012, 02:50 PM

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
  •