[DeusExMachina]

Been trying to do a bit of engraving in 6061-T6... I have a 3 edged, 60 degree carbide 1/8" shank engraver with a 0.03" tip. I've got a taig cnc that I'm trying to do this on, but I can't seem to get a good engraving...

It looks like the material is getting pushed around, not actually cutting but almost like its melting and pushing the material around the engraving path. I've tried 10k rpm, at ~12ipm which wasn't too bad, and I've tried ~18ipm and just about everything in between. I can't seem to find an optimal feed rate to engrave at. Perhaps I'm taking too deep of a cut (0.01")?

Does anyone have some good tips engraving, or general rules of thumb?

[Jason3]

That's odd - your numbers look good to me. The cut is deeper than I'd usually go in one pass - I suggest about half that or less - I like the look of a single pass at 0.004" best, but you may need a deeper/wider line of course. I would expect it to get worse with the faster feed - was that the case? Is the tool coated (I've had trouble with TiN coated tools in 6061 Al.)? Are you using any cutting fluid?

I'm guessing more RPM isn't an option? I'd suggest trying a lighter cut, maybe squirt some kerosene or similar on it, even drop the feed a little more and see how you go. The tiny flutes on those little engravers don't give much room for the chips to clear, and without stratospheric RPM, the only way to get rid of them and not smear them about seems to be running a really minute chip load (like 0.0004" per flute). That seems to give me the best results. The deeper the cut, the more the chips seem to roll up and clog the tip. Three flutes instead of one or two won't be helping either, especially considering the limited RPM.

I've had good results using the 60° uncoated cutters from here (at 40K rpm, 32 ipm, no cutting fluid) : http://www.precisebits.com/products/...oreengrave.asp

Hope you can sort it out!

Best regards,

Jason

[mc-motorsports]

Use plain carbide, or even HSS, single edge is better. As much speed as you can and I run 2 passes of .004" for a total of .008" deep. Your biggest problem is more than likely the 3 edge cutter.

[dertsap]

i agree that the 3 flute is probably the issue , single flute is best for engraving , you'd get better results using a 1/32 ballnose

[mc-motorsports]

Spot drills is another thing some guys reccomend. Or center drills, not sure what size because I haven't tried them, but readily available, something to think about.