Results 1 to 15 of 15

Thread: Milling aluminium with Chinese 6040 - need tips for improving first attempt

  1. #1
    Join Date
    Nov 2011
    Location
    UK
    Posts
    412

    Milling aluminium with Chinese 6040 - need tips for improving first attempt

    We received a Chinese 6040 with three individual 24V microstepping driver boxes inside and 1.5kW spindle, so not the best in the world but a bit better than the cheaper blue box stuff from Ebay.

    I have set it up with LinuxCNC and Ebay parallel port PCI card and have tried CamBam with success - great success on soft materials and even slate, rapids at 3600mm/min don't seem bad to me for this sort of machine. I tried Pycam with some success but it seems limited in features, there are dependencies I can't sort out and it does tend to give errors whereas CamBam "just works" so far (once I ran as admin in Windows 8 to get it to not think the trial had expired before I'd ever opened the software). I them attempted to mill through a 2.2mm thick aluminium sheet (a 2d design) and organised my profile with 0.2mm deep steps with a twin fluted 3mm endmill that came with the machine. Initially I tried 250Hz spindle speed and 400mm/min but slowed it to 180mm/min during the job and also added some drops of oil into the path both of which helped.

    The steppers didn't skip, the bit didn't break, the spindle didn't overheat and the electronics all did what they should.

    Problems:

    The piece moved a bit so I will work on clamping
    The surface finish improved by slowing and oiling but is still rough

    Realism:

    I know it isn't a milling machine for metal really, but think I can do better
    I hear that some with this machine and a carbide bit are going through aluminium at 4 times the speed and depth with great results compared to my initial attempt.

    Solutions/questions:

    Should I use an end mill narrower than 3mm which is all I have with the machine so far? For this purpose I only need to cut through, not pocket, so presumably the narrower the better?
    Should I get a carbide bit?
    What should I spray on it?
    Any other tips?

    Many thanks!
    Last edited by john banks; 06-20-2013 at 8:11 AM.
    Shenhui 1280 100W RECI

  2. #2
    Aluminum depends on a lot of things. The type of aluminum makes a huge difference. Some is very gummy and some is hard. Gummy wants to weld itself to the flutes really easily. Hard machines a lot cleaner. Just depends on what you have.

    Also, can you translate your 250Hz into RPM? We need to know the RPM before we can help with the speeds/feeds.
    Lasers : Trotec Speedy 300 75W, Trotec Speedy 300 80W, Galvo Fiber Laser 20W
    Printers : Mimaki UJF-6042 UV Flatbed Printer , HP Designjet L26500 61" Wide Format Latex Printer, Summa S140-T 48" Vinyl Plotter
    Router : ShopBot 48" x 96" CNC Router Rotary Engravers : (2) Xenetech XOT 16 x 25 Rotary Engravers

    Real name Steve but that name was taken on the forum. Used Middle name. Call me Steve or Scott, doesn't matter.

  3. #3
    Join Date
    Nov 2011
    Location
    UK
    Posts
    412
    Thanks Steve, I'm really glad to have your help and advice on this!

    15000 RPM. At least that is what the VFD is set to, on a similar machine someone put a tacho on it and it was about right. It will go up to 24000 RPM.
    Last edited by john banks; 06-20-2013 at 8:17 AM.
    Shenhui 1280 100W RECI

  4. #4
    First, let me say that milling aluminum on a CNC router is an odd marriage. I say that because I see people that say "I cut it all the time, it cuts like butter and I run it a zillion RPM and a bazillion IPM", then you'll see someone say exactly the opposite and swear by it.

    The alloy really makes a huge difference. I've had stuff I just really fought because it was so gummy. I ran it fast, slow, used spray mist coolant on it, took light cuts, heavy cuts, and tried 4 different types of cutters. Then I've had stuff I can cut in one pass with no issues.

    I found High Speed Tooling to work the best. I use 2 flute, high helix end mills. I cut at 6500 RPM and run about 42 IPM for a cutter that small. I'd probably also take a number of light cuts with a small cutter like that, versus deeper cuts for a larger diameter cutter.

    I've cut a lot of it over the years and that's where I've ended up. I also use a spray mist coolant system with a synthetic coolant (water based will ruin your spoil board).
    Lasers : Trotec Speedy 300 75W, Trotec Speedy 300 80W, Galvo Fiber Laser 20W
    Printers : Mimaki UJF-6042 UV Flatbed Printer , HP Designjet L26500 61" Wide Format Latex Printer, Summa S140-T 48" Vinyl Plotter
    Router : ShopBot 48" x 96" CNC Router Rotary Engravers : (2) Xenetech XOT 16 x 25 Rotary Engravers

    Real name Steve but that name was taken on the forum. Used Middle name. Call me Steve or Scott, doesn't matter.

  5. #5
    Join Date
    Nov 2011
    Location
    UK
    Posts
    412
    http://www.aalco.co.uk/datasheets/Al...50-H14_57.ashx

    This is what I got which says machinability "poor".

    I clearly have a steep learning curve for understanding the material properties. Any tips of what sort of alloy is best for milling?
    Shenhui 1280 100W RECI

  6. #6
    I can't help too much with the sheet metal grade side of it. I cut what customers bring me and more often than not, I don't know what it is, nor do they. On the few times I've had to supply the material, on 1/4", I've always tried to get 6061. It's hard and cuts clean, and it's not gummy. I think the 5000 and 6000 series materials would machine the best. That might not work for the application, since it might be something getting cut and bend, which 6061 doesn't do well with. It's also more expensive.

    Most people buying aluminum sheet buy the cheapest stuff they can buy, which is most always the least machinable, in my opinion.

    I've read many posts saying carbide o-flutes are the ticket, but I've had a lot of problems with carbide on aluminum. High Speed Steel has served me very well and I don't think I'd ever go back.

    There are some significant differences in machine aluminum on a milling machine and a router. I think the lack of rigidity in cnc routers compared to cnc mills introduces a whole host of method modifications needed for machining it. On a stout cnc mill, you can machine aluminum with carbide and insane speeds and feeds. You can machine at 100's of inches per minute. Watching high speed machining on a milling machine is like watching a magic trick right in front of your eyes it's so fast. Holding something with vacuum tables and not having flood coolant causes many issues. Carbide hates shock and hates vibration. Vacuum tables and gantry type tables assure vibration.
    Lasers : Trotec Speedy 300 75W, Trotec Speedy 300 80W, Galvo Fiber Laser 20W
    Printers : Mimaki UJF-6042 UV Flatbed Printer , HP Designjet L26500 61" Wide Format Latex Printer, Summa S140-T 48" Vinyl Plotter
    Router : ShopBot 48" x 96" CNC Router Rotary Engravers : (2) Xenetech XOT 16 x 25 Rotary Engravers

    Real name Steve but that name was taken on the forum. Used Middle name. Call me Steve or Scott, doesn't matter.

  7. #7
    Hi John,

    I see you bought a CNC machine (router). As you already find out it is more complex to have a nice cut than a laser. Back to your questions:
    - machine must be very stiff (small amchine arent) - solution on this is relative high speed (on spindle) and light passes (Z level);
    - mist WD 40 or something else - you will see that will help dosent matter what kind of material you use;
    - material is very important T6062 is cutting and engraving very well (it must be T6062 not something else);
    - tooling must be very specialisezd (from material point of view) to have same results all time;
    - Z depth as rule of thumb can be half of the tool diameter - in time and depend on milling strategy you will modifiy that;
    - carbide bits are good for some materials but not so good for others;
    - depending of your knowledge level - visit cnczone, bit manufacturer site and pick up settings for milling depth, speed (for spindle RPM and milling IPM and so on);
    - software is also important -CamBam is good - have a look at SheetCam (also written by an English guy) - much better in my opinion Les the programmer is very very good in terms of bugs and also helping users (dosent matter if you are a machinist with 30 years experience or a newbie) - both are good 2D milling - not 2,5D or 3D if your machine can do that (4th, or more axes);

    I belive that machine came with a DSP like lasers. I have one of that controllers and I didnt like it. I prefer the Fanuc style which give you more felxibility (in terms of settings).
    In short (which will be not very short) you need:
    - stiff machine:
    - very well clamp material:
    - good approach of material;
    - good tolling;
    - learn g-code commands (what every commnad does and how the machine is moving)
    - good milling strategy.
    In years when you read and remember this posts you will be smiling. but the truth is you need to learn alot and practice alot to have good results for your products and customers.

    HTH
    Gabi

    P.S.
    In the Engravers forum there is a guy John Stevenson which bought a laser and is a newbie in that area but is one of the most good machinist I ever meet. Sending a PM dosent hurt. It is possible not to respond quickly since it is very busy making commercial chips.
    SH-G570 80 W RECI
    Homemade CNC Router
    Emco CNC Lathe
    ArtCam 2009
    Rhinoceros V4.0
    All Vetric products
    SolidWorks 2012
    CorelDraw X5
    Many ideas and very limited time

  8. #8
    Join Date
    Nov 2011
    Location
    UK
    Posts
    412
    Thanks Steve and Gabi. I will hopefully report back with more success following your advice
    Shenhui 1280 100W RECI

  9. #9
    Join Date
    Feb 2010
    Location
    San Jose del Cabo, Mexico
    Posts
    329
    13mm t6061 3.125 endmill feeds 762mm/min xy 381mm/min z 15k spindle speed
    Attached Images Attached Images
    Creative Woodwork and Design
    Vector Studio 22

  10. #10
    Join Date
    Nov 2011
    Location
    UK
    Posts
    412
    Looks good, thanks.
    Shenhui 1280 100W RECI

  11. #11
    Hi John,

    if you have a smartphone (android) have a look on google play about feeds and speeds application. I dont use that (there are many other table), but for a quick ideea....

    HTH
    Gabi
    SH-G570 80 W RECI
    Homemade CNC Router
    Emco CNC Lathe
    ArtCam 2009
    Rhinoceros V4.0
    All Vetric products
    SolidWorks 2012
    CorelDraw X5
    Many ideas and very limited time

  12. #12
    Join Date
    Sep 2010
    Location
    Conroe, TX
    Posts
    179
    The harder aluminum like 6061 engraved well. The softer architectural aluminum like 6063 is too gummy. If you are doing extruded material like angles, look at the inside corners of the angle. If they are square, it will be 6063, if there is a radius, then you have structural material (6060-T6) and it will be much harder but engrave better. Another trick is to run the job twice. The first pass may raise burrs down in the engraving. The second pass will remove the burrs. For lubrication, use tapping fluid made for aluminum, like Tapmatic for Aluminum. It will make a big difference, especially with the softer alloys.
    The panel below was engraved on the same machine you have. I used a 60 degree carbide V bit with V-Carve generating the toolpath. This panel was for a new larger machine I built.

    control panel 2a.jpg

  13. #13
    Join Date
    Aug 2010
    Location
    Tonasket, Wa
    Posts
    46
    My thought was to keep the part to one side of the machine's bridge or the other.
    Fixture the part as high as possible to reduce as much cantilever as possible.
    Spin it up!

  14. #14
    Join Date
    Nov 2011
    Location
    UK
    Posts
    412
    Some 6082 has worked fantastic. Machine has two faulty stepper driver units though, they miss steps. Confirmed by switching everything around between axes. Will see how helpful the supplier is in replacing, on the Chinese laser that had an early stepper driver fault and they airmailed a replacement in a few days.
    Shenhui 1280 100W RECI

  15. #15
    Join Date
    Nov 2008
    Location
    Williamsburg, VA
    Posts
    62
    I had a remarkable improvement in cut when I switched to climb-cutting.

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •