Results 1 to 12 of 12

Thread: Milling brass

  1. #1
    Registered
    Join Date
    Jan 2010
    Location
    England
    Posts
    6
    Downloads
    0
    Uploads
    0

    Default Milling brass

    Hi, sorry if this has been covered before, but Iíve used the search and couldnít find anything to solve my problem.

    Basically, Iím a complete novice at machining, and having made the classic mistake (I now realise) of thinking if I bought a CNC machine I could quickly and effortlessly make anything my naive heart desired, I bought a Heiz S400 and started making steady, but slow, progress, using MDF as my main material, mainly to save cost. I recently bought some brass (CZ121), which Iím lead to believe has great machining properties. It seems to cut brilliantly, but Iím having no end of trouble with snapping end mills part way through the work, ruining the piece in the process, and costing me, as a hobbyist, an unaffordable small fortune!

    Iím trying to cut small gears (around 12mm diameter) so in order to get the detail, Iím using 1mm carbide end mills, which I assume are adequate for the purpose. Iíve gone down to taking 0.2mm cuts at a slow feed, and around 8,000rpm on my spindle (a Kress 1050), and although the end mills last a while longer, theyíre still breaking with alarming regularity. Does anyone have any advice, as although Iíve seen plenty of feed and speed calculators, Iíve either missed the point, or canít seem to apply them to my situation. I appreciate that I could continue reducing speeds etc, but canít really afford to keep breaking end mills until I find the idea settings.

    Sorry for rambling, but my brain and wallet are now hurting and Iím desperate to get this sorted. Thanks!

    Similar Threads:


  2. #2
    Gold Member
    Join Date
    Apr 2004
    Location
    Oakland CA USA
    Posts
    2309
    Downloads
    0
    Uploads
    0

    Default There are lots of variables

    in any CNC cutting operation, most of which you haven't told us about yet. There's the tool, for instance. You mention a 1mm carbide tool, but not how many flutes it has, the length, the helix slope, or the cutting angle. More flutes make a tool stronger, but the shallower flutes of a 4-flute cutter will clog easier, and clogged tools tend to break. A longer tool, obviously, is also more prone to breakage than a shorter one of the same diameter. A higher helix will eject chips faster, but also can tend to grab the material more. Brass wants a fairly flat cutting angle, but most endmills are designed for aluminum, which wants a more acute one. See if you can find some recommended specifically for brass. Carbide is a very hard material, and it wears out slowly, but that doesn't seem to be your immediate issue. Carbide doesn't hold as sharp an edge as High Speed Steel, and it's a lot more brittle. It might be that using HSS tooling instead of carbide will solve your problem.

    Then there's the speeds and feeds. You say you're going "slow", but not what you mean by that. Metals are cut much more slowly than wood. If you're breaking bits, try .5ipm and work your way up from there. Your 8k rpm spindle might be fine for wood, but it's quite fast for brass. If you can slow it down further without losing torque, that might help. And while .2mm (is that depth or width of cut?) doesn't sound like much, you could reduce it by half - remember, this is CNC; you don't have to crank the mill, just let it run; it'll finish in its own good time if nothing breaks.

    Another thing to consider is the cutting strategy. Are you engaging the tool on both sides, or just cutting one side away? It's much more stressful to do the former than the latter, so if you must do that, reduce feedrates accordingly. And if you're plunging straight into the material, that can break tools as well; endmills don't drill particularly well. Make sure you've got center-cutting endmills (some aren't capable of plunge-cutting at all) and try to design your toolpaths with ramping entries rather than plunges.

    Metal-cutting operations are dependant on rigidity above all. If the spindle runs out a little, big wood-cutting tools won't be affected much, but small metal-cutting ones will break. Likewise any untoward movement in the stock, or in the machine itself, will break tools. There may be a better way of holding onto your brass stock that will keep it from flexing at a certain point, and messing up the machining operation. It may be that your router just isn't rigid enough to deal with machining metal; that type of machine was primarily designed to cut wood, after all. While some metal-cutting operations might be possible for it, others may not. But try some of the suggestions above before you give up...

    Andrew Werby
    www.computersculpture.com







    Quote Originally Posted by dextavier99 View Post
    Hi, sorry if this has been covered before, but Iíve used the search and couldnít find anything to solve my problem.

    Basically, Iím a complete novice at machining, and having made the classic mistake (I now realise) of thinking if I bought a CNC machine I could quickly and effortlessly make anything my naive heart desired, I bought a Heiz S400 and started making steady, but slow, progress, using MDF as my main material, mainly to save cost. I recently bought some brass (CZ121), which Iím lead to believe has great machining properties. It seems to cut brilliantly, but Iím having no end of trouble with snapping end mills part way through the work, ruining the piece in the process, and costing me, as a hobbyist, an unaffordable small fortune!

    Iím trying to cut small gears (around 12mm diameter) so in order to get the detail, Iím using 1mm carbide end mills, which I assume are adequate for the purpose. Iíve gone down to taking 0.2mm cuts at a slow feed, and around 8,000rpm on my spindle (a Kress 1050), and although the end mills last a while longer, theyíre still breaking with alarming regularity. Does anyone have any advice, as although Iíve seen plenty of feed and speed calculators, Iíve either missed the point, or canít seem to apply them to my situation. I appreciate that I could continue reducing speeds etc, but canít really afford to keep breaking end mills until I find the idea settings.

    Sorry for rambling, but my brain and wallet are now hurting and Iím desperate to get this sorted. Thanks!




  3. #3
    Registered
    Join Date
    Jan 2010
    Location
    England
    Posts
    6
    Downloads
    0
    Uploads
    0

    Default

    Thanks for your informative reply, youíve given me plenty to work from. Hopefully Iíll get there sooner rather than later



  4. #4
    Registered RotarySMP's Avatar
    Join Date
    Mar 2004
    Location
    Vienna, Austria
    Posts
    1097
    Downloads
    0
    Uploads
    0

    Default

    What is the run-out of that Kress spindle? You are cutting slowly with a 1mm cutter, so any runout on the spindle is going to turn your tiny cutter into a 1 flute.

    Regards,
    Mark
    www.wrathall.com


  5. #5
    Registered
    Join Date
    Jan 2010
    Location
    England
    Posts
    6
    Downloads
    0
    Uploads
    0

    Default

    Iíve just had a quick search on this forum, and the run out on the Kress is less than 1/1000th, which having only just looked up what run out is, seems to be ok. Is that right, or with such small end mills, would this be too much? If this measurement is critical, I could try to measure my own rather than rely on someone elseís data.



  6. #6
    Registered RotarySMP's Avatar
    Join Date
    Mar 2004
    Location
    Vienna, Austria
    Posts
    1097
    Downloads
    0
    Uploads
    0

    Default

    Put a DTI on a peice of drill rod in your spindle.

    I looked up that Heiz S400 and it is not exactly a rigid machine.

    Regards,
    Mark
    www.wrathall.com


  7. #7
    Registered
    Join Date
    Jan 2010
    Location
    England
    Posts
    6
    Downloads
    0
    Uploads
    0

    Default

    Right, Iíve just done an admittedly fairly unscientific test using a DTI and one of the snapped end mills turned upside down in the spindle, and Iím quite surprised to say the least! At the lowest speed (~5000rpm) the run out is around 0.060-0.080mm. Moving up to around 8000rpm, which is what Iíve been running it at, the run out is 0.2-0.3mm! Like I say, it wasnít done with great care, but itís a ball park figure, and goes some way to explaining why they keep snapping. Just out of interest, I ran the spindle at 21,000rpm and got a run out of 1mm!! I knew the Heiz was no world-beater when I bought it, but it was all I could afford - Iím starting to see why people spend magnitudes more on these machines



  8. #8
    Registered RotarySMP's Avatar
    Join Date
    Mar 2004
    Location
    Vienna, Austria
    Posts
    1097
    Downloads
    0
    Uploads
    0

    Default

    How on earth can you measure run out on a running spindle at 21Krpm? That will kill you DTI really fast.

    Regards,
    Mark
    www.wrathall.com


  9. #9
    Registered
    Join Date
    Jan 2010
    Location
    England
    Posts
    6
    Downloads
    0
    Uploads
    0

    Default

    It's easy when you don't really know what you're doing and have no idea that doing that sort of thing will kill a DTI...Guess I won't be doing it again though!

    Still, thanks for the help - I'd no idea that the speed would have that much of an effect, so I'll try running it as slow as possible in future



  10. #10
    Registered
    Join Date
    Jan 2006
    Location
    USA
    Posts
    615
    Downloads
    0
    Uploads
    0

    Default

    Keep working on the advice that Andrew and Mark gave you above. Runout on the Kress could definitely be an issue, but they're generally high quality tools with good accuracy. I also think you're pushing your machine too hard. The S-400 is a light weight machine with unsupported linear rails. Vibration and deflection could also be issues.

    On my own machine, which is larger and more robust/powerful than the Heiz, I take light cuts (.005-.010"/.2mm) with much larger (.125/.25") 2 flute carbide endmills. I'm also using 120 IPM and 12K RPM for a .005" chipload on the larger endmills. With your small 1mm endmills, I would definitely start with much lighter cuts (.002"/.05mm) and work my way from there.

    Also, you should be able to calculate a reasonable feedrate/RPM based on chipload. Assume a 2% load on a 2 flute 1mm cutter and that works out to .0008" chipload, and 12 IPM at 8K RPM. You might actually be running that tool too slowly for the RPMs that your spindle is capable of. You're also losing torque running at slower RPM and may have better luck at 19 IPM and 12K RPM. It will take a fair amount of experimenting to find what works for the tool you own and the specific characteristics that is has.

    It may also help to make sure you're clearing the swarf out of the cut and maintain a good chipload.

    http://www.custompartnet.com/calcula...speed-and-feed

    Steve



  11. #11
    Registered
    Join Date
    Oct 2005
    Location
    Australia
    Posts
    2392
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by RotarySMP View Post
    How on earth can you measure run out on a running spindle at 21Krpm? That will kill you DTI really fast.
    It was probably bouncing off the tool, which might explain the figures...



  12. #12
    Registered
    Join Date
    Aug 2010
    Location
    uk
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default

    Hiya

    Dont want to hijack your thread (I sent you a PM but not sure it went, not showing in my out box... )

    I'm a TOTAL machining newb but I want to rout/mill some pretty straight forward aluminium parts and was thinking of buying a Heiz 400 (or Marchant & Dice, or RoutoutCNC??!!) but like you I WAS really hoping for easy plug and play!

    Could you offer advice? My parts are pretty simple with only quite loose tolerances required +/- .1mm or so (link to drawings below) but perhaps true 'plug and play' cutting for a real novice is impossible?

    Maybe you'd be interested in cutting some parts for me for a fee which might help us both learn? I could supply material and even cutting tool if required!? I'm in Northampton area.

    Any feedback really really appreciated.

    http://tinyurl.com/333qub7
    (Above link goes to google docs page with 4 jpegs of drawings made with Sketchup)

    Many Thanks



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 from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed