Aluminum tips?

This topic contains 31 replies, has 8 voices, and was last updated by Profile photo of Christian Knuell Christian Knuell 2 months, 2 weeks ago.

Viewing 30 posts - 1 through 30 (of 32 total)
  • Author
    Posts
  • #31460
    Profile photo of Mark
    Mark
    Participant

    Hi guys,
    Is it better to use a 1/8 or 1/16 endmill when milling aluminum? Both bits are double flute? I have an image of what I’m trying to do below. The shape is going to be milled of 1/4″ 6061 aluminum. The yellow areas will be pocket holes 1mm deep, the larger yellow area at bottom will be 4.7mm deep. The blue holes will be tapped with a thread mill and 5.35 deep. All other holes will be all the way thru.

    My thoughts, use 1/8 endmill to cut main shape and pocket holes, and use 1/16 endmill for the drill holes. Or should I just use the 1/16 endmill to cut everything?

    Am I better off going with trochoidal milling for this? And would anyone have any recommendations for settings? What would be a good setting for the holding tabs?

    Going from mdf to aluminum, should I not use the same endmill bit? A old time woodworker told me with router bits that mdf dulls them out well, not sure if it’s true or applies to endmills.

    Thanks,
    Mark

    Attachments:
    #31466
    Profile photo of Ryan
    Ryan
    Keymaster

    Pump the brakes!

    Do some test cuts first, looks like you will have a giant open area in the middle. Do a small test with all of the same features, a hole, pocket and a cut out.

    Test cuts will save you a ton of time and money.

    My biggest suggestion would be to get it as physically close as possible to your gantry, to increase rigidity. Start with the 1/8″ and see how it goes. The 1/16″ will need less force but will be much easier to break with bad CAM.

    #31478
    Profile photo of Christian Knuell
    Christian Knuell
    Participant

    Hi,

    Is it better to use a 1/8 or 1/16 endmill when milling aluminum? Both bits are double flute?

    1/8 will perform better because of larger flute spaces -> less risk of clogging.
    But for aluminum single flute is generally better.

    The shape is going to be milled of 1/4″ 6061 aluminum

    Let’s hope it is 6061 T6 instead of T4 – because the soft version of this alloy is hard to machine and has a strong tendency to clog and break tools. The hard version is OK.

    My thoughts, use 1/8 endmill to cut main shape and pocket holes, and use 1/16 endmill for the drill holes. Or should I just use the 1/16 endmill to cut everything?

    It is very likely the tool will break during drilling deep holes-> just drill 1mm and do the rest with a manual drill press.

    Am I better off going with trochoidal milling for this? And would anyone have any recommendations for settings?

    Much better. You’ll have to try settings on a scrap piece first – in Estlcam I’d suggest 1 – 2% trochoidal step length and 3mm depth per pass. Medium to high spindle RPM – feedrate so it does not shake up the machine too much.

    Going from mdf to aluminum, should I not use the same endmill bit? A old time woodworker told me with router bits that mdf dulls them out well, not sure if it’s true or applies to endmills.

    He is right – and a sharp bit is especially important for aluminum.

    #31485
    Profile photo of Mark
    Mark
    Participant

    Thanks for the replies guys!
    I’ll get the aluminum as close to the gantry as possible.

    Yup it’s 6061 T6. It’s a 2′ x 4′ x 1/4 plate, I was going to cut it down to 2’x2′, but I’m thinking now that I’ll just mill a straight line to cut it for practice. And I’ll do some practice cuts as well.

    Do you have any suggestions for feedrate?

    Thanks for your time!

    #31814
    Profile photo of Mark
    Mark
    Participant

    My first aluminum test..

    .1doc
    4mm/s feedrate
    2mm/s plunge
    12000rpm
    1/8″ upcut double flute carbide endmill
    40″x40″x3.5″ build, stainless steel tubing.

    I didn’t try trochoidal milling yet, will try it soon. With z axis raised to top, I built up and have about a 1/4″ clearance from tip of bit to material. I thinking about moving my spindle up so that the tip of my bit is just a little lower the the z rails.

    I needed to cut my plate in half so I figured would be a great test and no worries of any major screw ups. Took about 9hrs between two evenings after work. Two main factors for taking so long.. I engraved a line(not sure if it was the right option). With that is would cut left to right, raise and travel all the way back to starting point then start cutting again. The other factor, I wasn’t getting a consistent depth of cut, and started getting chatter, so I would stop, raise z axis a little and re zero and start again. Not sure if my spindle is enough power for cutting aluminum. I’m using the one in the parts links, 500w 12000rpm max.

    Things i need to do now..
    Raise spindle higher?
    Switch out spindle to my 1hp Bosch colt router?
    Face my work area so it’s level with my spindle/router
    Thinking about adding mid supports
    Connect vac or air to move the clips away
    Wire management

    #31839
    Profile photo of Ryan
    Ryan
    Keymaster

    Looked a lot faster than 4mm/s

    How did it turn out?

    If you are trying to decrease job length you could start going a little deeper (deeper is my vote) or a little faster but not both at the same time.

    #31845
    Profile photo of Mark
    Mark
    Participant

    It turned out ok, could have been way better. Main issue was that I was getting chattering at certain times, so I would have to stop the machine. Not sure what was causing it. Few thoughts that may be causing the issue.. aluminum not secure enough to spoil board and with upcut bit it was lifghting little? I did have it screwed down though. Spindle is not strong enough? Slight flexing in tubing? I figure I’ll add mid supports just to rule that out.

    When I tried .2 and .3 depth of cut it chattered big time where I had to stop it immediately.

    Your right about feedrate, it took 2 minutes to cut 24″ (609.6mm) so if I’m doing the math right.. 609.6mm / 120sec (2minute cut time) would be 5.075mm/s. just looked at the gcode and F300 so was 5 mm/s, could have sworn I set it to 4mm/s.

    Do you think 12,000rpm is plenty for milling aluminum, not sure if spindle is 12,000rpm under load.

    #31851
    Profile photo of Ryan
    Ryan
    Keymaster

    Well you have an extremely large machine, that might be your top speed for aluminum. Very hard to say.

    Move your material up as high as you can to minimize gantry flexy. That spindle you bought has a very long shaft, extension, and collet. You might want to move it up a notch on the tool holder so the collet is just below the bottom.

    If you goal is to cut aluminum a lot more often you should make the machine smaller.

    #31895
    Profile photo of Mark
    Mark
    Participant

    I know the machine is on the larger side. I have a project that calls for a 20″x20″ 1/4″ aluminum part. Would love to scale it down.

    As of right now I blame the reason why the cut didn’t come out as well as I would have liked do to my own user error. With that said it did come out pretty clean considering I jogged the mill over a few .01 in the y direction between cuts, trying to realign after some movement issues when I had bad chatter.

    I won’t mind being stuck at 4/5mms cutting aluminum, just hopping to get a better doc from .1mm right now. I think it’s just comes down to learning, trial and error. I have smaller parts I want to cut out in aluminum so I’m going to test on those first before I go for cutting the big boy.. I figure when I’m ready to cut the large part I can’t break it up over a few evenings/weekends.

    I’m printing out the mid supports as of right now and already moved the spindle up. Think I need to rule out if my spindle can handle aluminum, if not I’ll try out my 1hp colt router. Hoping to have some free time this weekend to try cutting more aluminum.

    I gotta say, when I was building the mpcnc I kept saying man I can’t believe how ridgid this machine is designed.

    #31897
    Profile photo of Ryan
    Ryan
    Keymaster

    Raise the material up.

    The closer it is to the gantry the stiffer the machine. Im one of my videos you can see I have it on 3 pieces of wood. It makes a huge difference.

    #32033
    Profile photo of Mark
    Mark
    Participant

    I was able to get around to raising the spindle and raising the spoil board to the bed. I have a little bit more room then a 1/4″ to slide my material under. Also added mid supports on the x axis. Need to modify the parts to fit on the y axis. Currently facing my spoil board, then I’ll be able to get back on practicing aluminum milling.

    #32223
    Profile photo of Mark
    Mark
    Participant

    Gave it another go..

    3 mm/s feed rate
    2 mm/s plunge
    .2 doc
    1/8″ double flute endmill

    It was going great then it jumped over, belts are tight. I’m wondering if my spindle can’t give enough rpm for aluminum (it’s max is 12,000rpm).hin,king it hung up and caused it to jump over.Im using manual stops and got about 2.5mm through, so im going to try finishing this cut tomorrow. Also smaller holes aren’t coming out circular but the larger holes came out great, not sure if it’s gcode related.

    Still more learning to do lol.

    #32228
    Profile photo of Martin DB
    Martin DB
    Participant

    Keep an eye in tip clogging. Try with one flute end mill.
    Btw looks pretty good!

    #32230
    Profile photo of Barry
    Barry
    Participant

    I’m starting to sound like a parrot, but for your long cuts use a trochoidal path. It will really help. I’ve seen a few videos on youtube from a larger home built cnc router and he used them for everything, seems to work much better. The bit should stay cooler so it will cut better.

    #32247
    Profile photo of Ryan
    Ryan
    Keymaster

    Trochoidal, and maybe a bit more load, either a little faster or a little deeper.

    Your cuts are good you just need to run some test cuts. See how far you can push it, sometimes slower and shallower is not the answer, or maybe slower and deeper I feel you are leaving a lot of time on the table here.

    #32264
    Profile photo of Mark
    Mark
    Participant

    Thanks guys for the replies!

    I’m going to give it another go this evening.

    Would anyone have any suggestions on settings to try out for trochoidal milling? Seems like I get crazy long mill times when setting it.

    #32271
    Profile photo of Ryan
    Ryan
    Keymaster

    Christian gave you some suggestions above.

    #32278
    Profile photo of Mark
    Mark
    Participant

    Think I jumped the gun before posting. I didn’t see anything about a good feed rate. Just watched the video Christian made on trochoidal milling. Tested a 45mm line at 20mm/s and worked nicely. Think I can bump up my feed rate more as well.

    #32358
    Profile photo of Mark
    Mark
    Participant

    First successful aluminum part milled out of 1/4″ with trochoidal milling. Very very happy with the result and how well it milled overall. Still have some tweaking to figure out. Not sure why the line about 1mm from bottom. Now I need to figure out a good size for holding tabs and then work on figuring out a finish pass.

    #32363
    Profile photo of Ryan
    Ryan
    Keymaster

    Looks pretty good. What settings did you end up with?

    #32366
    Profile photo of Mark
    Mark
    Participant

    Thanks Ryan,
    20 mm/s feed rate
    .2mm/s plunge
    3 mm doc
    12,000rpm
    1/8 double flute endmill

    Trochoidal
    2% step length
    50% width
    .05mm oscillation

    I feel I can easily up the feed rate without issues, I may try 30 mm/s. but I’m happy with 20 mm/s, giving the size of my machine.

    #32368
    Profile photo of Ryan
    Ryan
    Keymaster

    I think 20 is pretty fast I would stick with that and increase your depth or step length instead. If you feel the need to push it harder.

    The part looks great. I’d be happy if I cut that!

    1 user thanked author for this post.
    #32405
    Profile photo of Johnny
    Johnny
    Participant

    Looking great Mark. Those are some nice cuts. The guys are giving you some great advice. Remember when cutting metal its not always about the speed of the bit, its about torque and the amount of metal your bit can effectively clean away with each pass. The chatter you were getting earlier can result from a few things. The main factors in my mind are load on the bit, horizontal in this case, and the speed or effective cut of the bit. And in some cases harmonics depending on how well the material is fastened to the table and if it is reverberating or not. Looked like it was held down pretty well so harmonics is the least likely. The Trochoidal seems to be the way to go with these machines as the guys suggested above. Keep playing with the settings and let us know what works. You also might try a single flute bit as Christian suggested above. It’s a juggling act between speed and torque of the spindle and the effective material removal of the bit at those given rates. I plan to have my MPCNC built in the next few months and will be trying some aluminum as well even though the primary use for the machine will be wood.

    1 user thanked author for this post.
    #32518
    Profile photo of Mark
    Mark
    Participant

    Thanks for the reply Johnny.
    Thanks for the advice, the guys here have been a big help as well.

    Each time I turn my machine on and cut aluminum it’s getting better, tweaking and adjusting as I learn. Just did two more parts. Trochoidal is working very well for me. I’m going to order some single flute bits to try out.

    #32524
    Profile photo of Johnny
    Johnny
    Participant

    Very nice! Cuts are looking really good. Im excited to see how you progress. Once the 3d printer gets here I be getting started on my mpcnc as well. Most of my cnc background comes from running lathes instead of mills, but cutting chips translates some from method to method. Let us know how that single flute works. Speaking of I saw a video from a tool company on YouTube specifically about Trochoidal. The make bits specifically for that style of cutting and use what looked like a 5 tooth or flute bit. But its for larger machines mostly. Very interesting cutting method that I am interested to explore myself.

    1 user thanked author for this post.
    #32782

    Very interesting topic, congratulations on your results!
    I really want to try that soon!

    1 user thanked author for this post.
    #33136
    Profile photo of Mark
    Mark
    Participant

    Jonny I seen a video too on the trochoidal bits but didn’t see on their website where to order them, would be interesting to try out.

    Thanks Dui, I really like your build!

    #33201
    Profile photo of Ryan
    Ryan
    Keymaster

    Trochoidal is a milling strategy that works with any bit but generally is used with a square endmill.

    #33204
    Profile photo of David Walling
    David Walling
    Participant

    For those using Fusion 360, I believe they call this ‘adaptive’ milling

    #33205
    Profile photo of Ryan
    Ryan
    Keymaster

    A little different but the milling strategy I think most beginners should start with, and this video has a really clear explanation of it. https://youtu.be/_N5VaTchhys

    I think this is a little closer to the “peel” in estlcam. I am not positive but I think the strength of Tricoidal is in using it on a single cutout type path So you get a constant load of half the bit instead of climb and conventional milling at the same time, where peel and adaptive are clearing strategies. Again I am not 100% on this.

Viewing 30 posts - 1 through 30 (of 32 total)

You must be logged in to reply to this topic.