[acannell]

since its so hard to find actual examples of feeds and speeds that work for micro mills, im posting this to help other beginners with some kind of data point.

material: 6061-T6
diameter: 0.015"
flute length: about 0.030"
shank dia: 1/8"
tool material: carbide
flutes: 2
feed: 1ipm full slot, 0.5ipm plunge
axial depth of cut: 0.010"
speed: 7000 rpm
holder: new chinese ebay ER32 (BT30)
mill: 15 year old dyna DM2900, not sure how much runout it has, because im not sure ive measured it correctly
coolant: rustlick WS 5050 30:1 at medium flow rate

the tool path was about 51 inches long. it took about an hour of continuous milling. several plunges were made. i suppose that since the end mill survived i can call this a success. im not sure how much faster i could run it, but it would be really nice if i could run it at say 0.020" doc and 1.5 ipm..to bring 51 minutes down to 17 minutes

the finish seems to be very nice, although i havent looked at it under a microscope yet.

just to be clear, i didnt do the entire cavity with the 15 thou, it was roughed out to the point where the letters had been surfaced and they just needed to be cut out of a 20 thou tall block

[awerby]

If you want to feed faster, you'll need a spindle that spins faster. 7000 RPM is very slow for such a small tool. If you used a spindle that could spin at 21k rpm, then you'd be able to do this toolpath in 17 minutes instead of 51. Go to 40k rpm, and you'd do it in under ten minutes.

Andrew Werby
www.computersculpture.com

[acannell]

If you want to feed faster, you'll need a spindle that spins faster. 7000 RPM is very slow for such a small tool. If you used a spindle that could spin at 21k rpm, then you'd be able to do this toolpath in 17 minutes instead of 51. Go to 40k rpm, and you'd do it in under ten minutes.

Andrew Werby
ComputerSculpture.com ? Home Page for Discount Hardware & Software

yes im aware of that..i think i can only get it up to 10k using a different pulley set available for this mill. other than that i think the only option would be some sort of speed multiplier or some kind of spindle tool thing

on the other hand, i havent pushed the feed yet..i dont have any idea where it stands as it is, i.e. if its right at the limit or far enough away to where i could significantly increase the doc or feedrate

[extanker59]

I think the DOC is too large and the feed too small. Haven't gone as small as you however so I'm not sure. I had a similar question a couple years back. It involved a 1/32" endmill in 17-4 SS. Making slots. Tools were not lasting when going .015 DOC and 1 IPM. Based on recommendations from the kind people here, I cut my DOC on my carbide .031 diameter 4 flute end mill to only .003 and increased feed to 5 IPM with 11000 RPM. Cut my cycle time down and the tools lasted the whole run (rough end mill and a finish end mill). I tried .005 DOC but that didn't work. I suspect I could have fed faster but just had under 50 parts and needed the job done so I didn't experiment further.

[acannell]

I think the DOC is too large and the feed too small. Haven't gone as small as you however so I'm not sure. I had a similar question a couple years back. It involved a 1/32" endmill in 17-4 SS. Making slots. Tools were not lasting when going .015 DOC and 1 IPM. Based on recommendations from the kind people here, I cut my DOC on my .031 diameter 4 flute end mill to only .003 and increased feed to 5 IPM. Cut my cycle time down and the tools lasted the whole run (rough end mill and a finish end mill). I tried .005 DOC but that didn't work. I suspect I could have fed faster but just had under 50 parts and needed the job done so I didn't experiment further.

i would think that pretty much all the parameters on the cut i described are way off given the 7k rpm..but what you are describing is an interesting idea, i think ill try it and see if i can decrease the overall machining time on that toolpath..i shall report back!

[Dylwad]

I think the DOC is too large and the feed too small. Haven't gone as small as you however so I'm not sure. I had a similar question a couple years back. It involved a 1/32" endmill in 17-4 SS. Making slots. Tools were not lasting when going .015 DOC and 1 IPM. Based on recommendations from the kind people here, I cut my DOC on my .031 diameter 4 flute end mill to only .003 and increased feed to 5 IPM. Cut my cycle time down and the tools lasted the whole run (rough end mill and a finish end mill). I tried .005 DOC but that didn't work. I suspect I could have fed faster but just had under 50 parts and needed the job done so I didn't experiment further.

I have been doing something similar on my router, cast stainless, not sure of the grade, .0469" 4 flute coated, 10k rpm, .0034 DOC .032 deep slots (engraving) 20ipm feed, 4 ipm straight plunge. Bits last a whole lot longer than I thought they would. .0055" DOC cuts the tool life in half or more. Parts are hard to rigidly fixture too.

[extanker59]

Hope it works out for you. Looking forward to your results.

[extanker59]

Nice. Yeah I thought I could go faster but never had the courage to try. Very cool.

[Dylwad]

Thanks, I am up to around 16 sets engraved now on the same $9 bit. Doesn't sound as nice as when it was new but still gets it done. I don't have flood or mist coolant either, just keep the area wet with 3 and 1 oil. Fixture is made from 3/4" birch ply.