Milling Brass

Hi All,

First post here, although been lurking for a while. I need to mill some shapes from 2mm brass to make keys for early woodwind instruments. I will be using a Triac mill with a 2mm cutter. I have drawn the items in Draftsight and will use sheetcam to generate the Gcode. The keys are mostly about 50mm long, about 15mm wide. I have used the Triac for years but mostly for wood, so my question is, what would be a reasonable feed and cutter rpm for the job. Top speed available is 3000rpm. I have looked a various feed/speed calculators but they all seem very complex.

Slow and steady would be fine, if anyone can suggest an approximate figure as a starting point I'd be happy to experiment.

Sorry- another question- should I expect to do this in one pass?

Thanks for any advice, Richard E.

Use your max spindle speed with that size cutter, as for feeds is the cutter HSS or Carbide and how many flutes?

Full cutter width profiling cut and finish pass or adaptive clearing and a finish pass?

It's a 2 flute HSS cutter. Sorry, I don't really understand your second question, except that there will be no finish pass because I'll be filing a curved edge on the keys.

Thanks

Richard

Just had a quick look at Sheetcam and it looks like your tool will just be following around the outside of the shape to produce the profile so you will be cutting at the full 2mm width.

I would say to be safe go 0.5mm deep per pass, 3000rpm with a chip load of 0.005mm so that gives a speed of

3000 x 0.005 x 2flutes = 30mm per minute

Thank you Jason, very useful advice!

Richard

Quick look at LG-1's cutting data for a 2-flute uncoated HSS bit gives 0.007mm and as I said play on the safe side so 0.005mm as we don't know the parentage of the cutter.

Chip load goes down on small cutters, you could take 10 times that with an 10mm cutter for example

That’s interesting. The reason I asked was that a rule of thumb I was given some time ago was a chip load 1% of cutter diameter. This this has worked out ok for me in the past. For a 2 mm cutter that suggests .02 mm, just under a thou.

I looked up some CAM I wrote a few years back using a 2mm cutter in aluminium to form heatsink fins. I was running at 4000rpm, 0.02mm chip load, full width and a step down of 1mm. With more experience I'd keep to the same chip load and DOC but I'd be running at a much higher spindle speed.

Translating to a 3000rpm spindle the chip load equates to a feed rate of 120mm/min. Is the finished part clamped down? If not then you may need to restrict the total depth of cut to say, 1.9mm, or program some bridges to stop the part breaking away from the waste material.

Andrew

Thanks for the comments folks.

Andrew, the finished parts will not be clamped down so thanks for the suggestions. I was thinking of using double sided tape under the brass sheet.

Got a chance to cut some metal today. Excellent results using 50mm/min, 3000rpm, 0.7mm depth of cut.