Hi, we have a CNC converted Proxxon Micromill and need to CNC machine some sterling silver and high carat gold prototype electronic parts using 2 flute and 3 flute ball and fish tail mills with a maximum diameter of 0.5mm. The cut depths are less than 0.75mm and speed is not a requirement.
Before we press ahead and work our way through umpteen carbide mills in a feeble effort to determine the best feed rates etc. (yes we have vast experience of making unnecessary scrap!), I would be very grateful for any advice.
I'm on the same boat here and I've been breaking lots of tools.
Could you give some tips?
Who were you richard, what did you see, what did you see??
Gold and silver can be machined, but they tend to be "sticky", so some lubrication helps. If you don't have flood or mist coolant on your machine, then squirting it occasionally with WD-40 helps. It's a lot like machining copper, which is more commonly cut this way. The extra thing you need to think about is patrolling your chips, since each one is precious, especially lately.
When cutting with an endmill, the feedrate is determined by the chipload. That's the amount of metal removed by each flute as it revolves into the work. A larger tool can handle a bigger chipload than a smaller one, and with tiny tools like the one referred to above, you can't remove more than about .0001" at a time. On the Micro100 site, under Downlaods, there's a handy chart with lots of different materials including copper, which helps determine chiploads. But the smallest tool they talk about is 1/8" (with a chipload of .001" per tooth), so you have to extrapolate a bit.
So anyway, if you've got a 4-flute cutter that's .02" in diameter, that's .0008" you can remove per revolution (IPR). Using the formula IPR X RPM = IPM, if you're using the Proxxon above, which goes up to 20K RPM, that means at max speed you can remove 16 inches of material per minute. (IPM). If you had a spindle that went twice as fast, you could remove material at 32 IPM.
But there are some other considerations as well. These calculations are based on peripheral cutting, not cutting a slot, where both sides of the cutter are engaged at the same time. If you're doing that, you need to slow down about 50%. And the depth of cut matters too -you shouldn't count on cutting deeper than the diameter of the cutter at a time, and not exceeding half that is a good rule of thumb, at least until you've stopped breaking cutters and feel you could try going faster.
Of course, the rigidity and concentricity of your machine are important too. The charts always assume that your machine is big and perfectly true, so if yours isn't, then you need to slow down to compensate. A spindle with a little runout is not usually a problem if you're using big cutters, but if the runout or wobble is a significant proportion of the tool's total diameter, it becomes a big deal. It's also important to keep any chips out of the cut, since these tools really hate re-cutting their chips.
ComputerSculpture.com — Home Page for Discount Hardware & Software
sorry for my late reply. thank you mate! My machine is in repair, I'll use your info as soon as I get it back!