Cutting 1.6mm Aluminium sheet

New Home Forum Mostly Printed CNC – MPCNC Advice – MPCNC Cutting 1.6mm Aluminium sheet

This topic contains 48 replies, has 6 voices, and was last updated by  Manuel B. 2 years, 1 month ago.

Viewing 30 posts - 1 through 30 (of 49 total)
  • Author
    Posts
  • #42983

    Dennis Wright
    Participant

    I’m looking for guidance for a starting point to “cut out” a design from 1.6mm aluminium. I see reference to a Video with settings that Ryan posted about a year ago but I can’t find it and having read through some of the posts on the forum I can’t find any basic settings to start out: X and Y speeds, depth of cut, accelerations and router RPM etc. I plan to use a 3mm bit and accept that with a Makita router any suggestions would only be a starting point but any guidance would be appreciated. Using Estlcam 10 as the CAM generator and controlling from an SD card.

    Thanks

    Dennis

    #42984

    Barry
    Participant

    1mm depth of cut 15mm/s x/y 10% trochoidal length 50%width .05mm oscillation.  That’s my starting point, then I adjust from there.  You might be able to do full depth of cut.  Also, you have to have some way to get the chips out of the cut, vacuum, or air blast.

    2 users thanked author for this post.
    #43153

    Kevin Lopez
    Participant

    Since the plate is so thin, I would actually advise not to use trochoidal. Trochoidal only makes sense when you want to cut out a block of material, or at least thicker than the diameter of the tool. It helps with chip evacuation in deep slots and wears your tool more evenly. With something so thin though the advantages of that strategy become more of a setback. (longer time, bigger file, more conduit wear) If you have all the patience in the world ignore what I just said.

    I cut out like 70 individual small 1.5mm thick plates, and the way to go here is to just slot normally. I used .5mm DOC, 10mm/s, single flute at 30krpm. Those are kind of aggressive since remember, it is a full width cut. I would start off with a really shallow doc. Either way, try both and see what works for you.

    Most important, don’t go too slow at first! You need to keep the cutter engaged in material fast enough or it will just rub and it will get ugly quick.

    1 user thanked author for this post.
    #43441

    Manuel B.
    Participant

    HI all,

    I have just started some cutting/milling of aluminum.

    1.) I tried single flute, 3mm diameter with 2mm/s XY feedrate and 0,1 mm/s for Z, 1mm doc . Broke after 2 seconds, unbeliavable, lost 30USD. Cutting in depth was ok but as soon as the spindle started moving it broke in 2 pieces and one remained in the material.

    2.) Tried double flute 3mm dia, same settings and luckily used emergency stop after 10 seconds and saved the bit.

    3.) Used trochoidal milling with double flute 3mm with settings : 10mm FR, 4mm Plunge, 1,5 mm doc , 90% stepover, 2,5% Troc.step length , 50% and 0.05 oscillation. It went ok, nice and good only setback is the time. Small heart 30mm took 30 minutes.

     

    Are the settings in ESTL for feed rate anyhow connected with stepper rates? If stepper rates are 6400 is it affecting the feerate compared to stepper rates of 3200?

    I ask this becouse I see a lot of different settings for aluminum cutting over internet and in forum.

    I lost already 2 bits each 30USD. They stop cutting, spindle continues and bits get dragged, bend and break. Any advise would be appreciated.

     

     

    #43442

    Ryan
    Keymaster

    A video might help a lot here. If you aren’t sure if your machine is moving at the right speed you should probably switch back to marlin so we know it is right and/or put up a video so we can;t tell you if it looks like the speed you set.

    Have you done any wood or plastic milling yet?

     

     

    #43443

    Kevin Lopez
    Participant

    Are u sure ur feed is correct? It is hard to break a bit in 2 seconds when you’re running that slow. Too slow is more of a cutter overall life reduction, not instant failure. A video would be awesome

    2 users thanked author for this post.
    #43444

    Manuel B.
    Participant

    Few more questions:

    1.) Is it better to use 4mm  bit or 3mm ?

    #43445

    Manuel B.
    Participant

    Hi Ryan and Kevin,

    Unfortunatelly I dont have a video when the bit broke. I am using Marlin, didnt yet switched to ESTL controller albeith it is in my plans.

    Yes, I worked on HD foam, some plastics and wood but mostly engraving and using laser.

    I made a video of trochoidal milling  if it helps. The settings were 10mm/s FR, 1.5mm doc, 4mm/s Z Plunge , 2.5%Tr.step , 50% and 0.05osc. However the step over was set to 90% as I don`t know yet how last parameter affects cutting.

    I need to learn how to post the video though as it has 70Mb.

    Could I measure if set feed rate is correct by raising the bit above material and measure the length of movement against time?

    I was also surprised, like the bit stoppped cutting or the spindle was to fast. On one previous attempts I noticed aluminum got stuck to the bit, melted and reduced cutting force. I cleaned the bit afterwards and was better.

    So, I need first to determine if the feed rate is correct and mean time will try to see how to post video…

    Thanks for prompt answers btw.

    #43446

    Ryan
    Keymaster

    Barry has some good settings above in this thread.

    I think you should try them, in wood or plastic. Test cuts are a way of life. Make sure your file works in something softer first and then move up to metal. Save a ton of bits that way, might also be best to start with some cheaper ones. The expensive ones usually have very specific purposes and at $30 you might have the wrong ones. Some require coolant some will not work with coolant, etc.

    You are talking about speed settings in estlcam control, are you positive you didn’t upload them the the board? How do you actually run your files?

    You can watch some videos from the video page and do some visual comparisons to see if your speed is at least close.

    1 user thanked author for this post.
    #43449

    Manuel B.
    Participant

    Here the video of trochoidal milling aluminum settings 10mm/s XY, 4mm/s Z , 2.5%TS, 50%, 0.05osc 1.5mm doc

    http://www.youtube.com/embed/lNMcTmHBR7M

    #43450

    Manuel B.
    Participant

    Hi Ryan,

    I use ESTL CAM and generate gcode, after I upload it with Repetier. I ment the settings for feed rates in ESTLCAM when generating gcode. Currently with 3mm and 4mm double flute bits and using trochoidal is going ok. Since I want to cut a frame of aluminum 6mm thich, frame dimension is 450mm x 450 mm with trochoidal it could take 8 hours….

    Yes, I watched many videos and thought I am ready 🙂

    #43452

    Manuel B.
    Participant

    I just calculated the table speed (feed rate) from maker. For aluminum and 24K RPM is 24 mm/s till 72 mm/s .

    I guess I was milling just tooo slow , perhaps the material fused to bit.

    #43460

    Kevin Lopez
    Participant

    So you broke a bit while slotting at 1mm doc, 2mm/s, after 2 seconds? Something doesn’t add up. If a tool breaks within a few seconds chances are your feed and depth were way too high to the point where it bites off more than it can chew. Start with something softer like wood or plastic, and Ryan is right. Those expensive end mills are no place for our machines. The are tailored  torwards specific needs and because of it, have a high price tag and are not as forgiving. Using a cheaper and more general use end mill will save you the headache of watching 20 dollars break in half.

     

    As a general rule when slotting, do a shallow DOC with a fast feedrate. This way your chips will be the right width and you will have minimum cutting force due to such a low depth.

    1 user thanked author for this post.
    #43475

    Manuel B.
    Participant

    Thanks Kevin,

    sadly I can find locally only bits around 25€ which is roughly 30USD. Will try to find cheaper bits for sure. This bits are for  steels, hardened and alloyed steels, titan, brass, bonze and aluminum.

    You are write, also above you mentioned shallow cut – doc. I was actually slotting with 3mm dia single flute  1.5 mm(actually 2mm) deep with 2mm/s feed rate. Anyway the bit broke a bit too fast and I will revert back to maker.

    Performed again test with double flute with above settings and it flexed but didn`t break and still ok.

    As per maker the doc must be within 0.3 and 0.75mm with feed rate higher than 24 mm/s and RPM higher than 22K rpm. I only found the settings from the maker few hours ago.

    With trochoidal step of 0.3mm I could go 3 mm doc.

    Monday will measure if feed rate corresponds to the set up and test again with higher feed rate and shallow doc 0.3mm and hope for good results.

    I am not sure if I can use same bits on wood or plastics? Do you use same bits or specific for wood?

     

    #43476

    Ryan
    Keymaster

    You can use them on wood.

    #43477

    Ryan
    Keymaster

    I’m not sure what you are looking for the video was fine. You can probably mill all the way through and save some time.

    You keep switching your bit size in the posts, are you also switching them in your CAM, you have to update it to your exact bit each time or you will break things.

    #43512

    Manuel B.
    Participant

    HI Ryan,

    Thanks. Trochoidal milling was ok, only concern was it takes a lot of time and thus I wanted to mill straight trough to buy time.

    For 2 frames using troch mill and same settings I had would take more than 18 hours and this is long.  I will try settings as you suggested and test again on wood first.

    #43513

    Kevin Lopez
    Participant

    I’m just imaging what it would be like tunning a dw660 for 18 hours. Aaaah I would go nuts.

     

    With trochoidal, go heavy on the depth. You would be surprised how much depth it can handle. If you’re cutting 1.3mm sheet then I would say no to trochoidal, it makes no sense here. You should be able to do a shallow slot like that no problem. Thinner material is way more forgiving in my experience. Something tells me your CAM settings are really whacko. Maybe you’re moving way faster than the software value

     

     

    #43514

    Manuel B.
    Participant

    Thanks Kevin,

    Yes, will have to measure if speed – feed rates correspond to actuall settings.  And 18 hours is really long to stand, vacuum and watch :).

    I have 6400 steps on ramps with drv8825 for all axis.

    I thought would be as with 3d printing, let it do its job and come back when finished 🙂 .

    How do you adjust the z hight prior starting the job? I manually move the spindle until it touches the material, disconnect and connect back repetier host to zero the position and than start. In some occasions the bit first lowers down 0.5 mm, raise and moves to position.

    I am travelling now and eager to test new settings on monday. Will revert back.  After when all set , need to remove the dispaly from ramps and set up estl controller with probe and xbox controller to make it easier.

    #43518

    Jeffeb3
    Participant

    I have 6400 steps on ramps with drv8825 for all axis.

    What?!

    #43519

    Manuel B.
    Participant

    Hi Jeffeb,

    Isn’t 1/32 settings on ramps for steppers resulting in 6400 steps for revolution? All 3 jumpers in on drv8825.

    #43527

    Kevin Lopez
    Participant

    Going in I thought it would be like 3d printing too where you hit the green button and walk away. I was wrong…a lot of people on here look down in shame on that. Unless your machine is fully enclosed in like bulletproof chamber or it is rolled outside I wouldn’t trust mine for too long.

    Once, I did leave the machine running alone. Everything went fine but the router had to be left on not cutting about 2 hours. For some reason there was some sort of ash as if the wood underneath burned a little. Made no sense to me at all. I wasn’t cutting wood and the bit was retracted above my aluminum by 2mm. Nothing broke but I was confused.

    #43534

    Jeffeb3
    Participant

    Hi Jeffeb,

    Isn’t 1/32 settings on ramps for steppers resulting in 6400 steps for revolution? All 3 jumpers in on drv8825.

    Ah, I see what you’re saying. Yeah, that’s a mistake. It’s set to 200 steps/mm, but without the jumpers they are basically set to 6400 1/32 steps/mm… Yeah, that would break some stuff. Also, you’d end up with gigantic parts…

    #43662

    Manuel B.
    Participant

    Thank you all for support!

    I am learning and adjusting the settings. Cutting through wood and aluminum like trough butter now :).

    I found good settings for aluminum using trochoidal milling, it is excellent and the cuts looks fantastic.  Done quite some letters, squares and models without any problem. Started milling a small frame, all perfect at beggining and somewhere in the middle the bit started losing revs. I paused, raised the Z and cleaned the bit as small aluminum parts were fused to the bit. At that point continued the job but material fused again, I couldn`t “rewind” back the gcode for few seconds in repetier as it always returns when pause was activated.

    Why would aluminum stick to the bit? Feed rate to high/low or bit is already damaged? How long your bits last usually?

    #43669

    Kevin Lopez
    Participant

    Aluminum is a soft material in respect to other metals. It also has a gumminess property. It isn’t just shown when milling either. Try cutting or filing it. It just likes to stick. Not to mention it makes big chips naturally.

     

    Either you’re feed is slow, your chip evacuation is not nearly good enough, or you’re cutting the wrong alloy. Go for 6061 t6. Or t6511 for flatbar is what I order.

    1 user thanked author for this post.
    #43681

    Barry
    Participant

    I’m just imaging what it would be like running a dw660 for 18 hours. Aaaah I would go nuts.  

    20 some odd hours!  I did leave a couple gallon ziplock bags full of water sitting outside the cutting area.  It’s also mdf.  I have a hard enough time catching the stuff on fire on purpose!  I think that was also one of the times I collapsed a 5 gallon bucket that sits under my dust deputy.

    https://goo.gl/photos/sLooSqcD1Rxz2NgQ7

    #43689

    Manuel B.
    Participant

    Thanks Kevin,

    Seems like the alloy is not homogenous and on some areas the material has different properties (probably not). I don`t know exactly which alloy are the plates I got but I will ask in future for specific alloy and the one you mentioned.  Will also play again with settings, decrease the step and increase the feed. Yesterday at one point was excellent and  I thought nothing can stop me anymore 🙂 .

     

    Attached video of trochoidal milling letter “B” , 27 mm/s feed rate , 3mm Z step , 3mm/s plunge , trochoidal width 50%. I started with trochoidal step 4% and each next “B” had 1% troch step more. At 9% (not on video) the aluminum start sticking to the bit and I stopped.

    I chose 8% trochoidal step as last best and started milling large piece when the alu sticked again on the bit somwhere at the middle. I saw on Kristian video, he had settings of 5% troch step and much higher feedrate(35 mm/s) and I will test those settings today.

    Barry mentioned above lower feed rate but higher troch step (10%) with less doc. I guess will have to cut more and test what works for me.

    http://www.youtube.com/embed/AXanbFgCHUk

    #43690

    Manuel B.
    Participant

    Barry,

    Nice picture. If you have time let me know how you made it?

    #43695

    Kevin Lopez
    Participant

    Oh no, if your aluminum plate has different material properties in different patches I would be really nervous lol. It would have to have been fabricated by wild rednecks!

    Wait so what end mill is that exactly? It better be a single flute!! Don’t even try double it doesn’t really make any sense. With how fast we are spinning those sharp edges around there is only a need for 1, any more is just asking for a clog barely, if any of us, have a proper mist lubricant system.

    Your chip evacuation looks pretty good but not great. If you plan on doing a lot of aluminum get some loc line and a source of air. Way better than policing the machine with your vacuum.

    If you’re running the ramps 1.4/arduino mega, you will find there is a speed limit. It could just be be especially since I have oscillation on estlcam on, but I max out at a certain speed. Probably my accel limit. After like 800mm/m for me I cant tell it circles any faster

    #43696

    Manuel B.
    Participant

    Hi Kevin,

    I am sure the problem is in the plate 🙂 , hehe.   Yes, I am using double flute 🙁 as my single flute broke and saw few videos where guys succeded and cutting nicely on MPCNC. I do understand the single flute is way better for aluminum and chips evacuation thus I am already on the way buying them.

    Noted related the evacuation system. Will get or print some loc line and have to find better air compressor as mine is quite loud.

    Currently I am trying to make a 3D printer frame – mk2.In case I start building 3D printers than I guess cutting them with laser or other ways will be much cheaper and easier.

    Wil have alook at the limits and accelerations. I could only measure if estimated job time corresponds to actual one.

     

Viewing 30 posts - 1 through 30 (of 49 total)

You must be logged in to reply to this topic.