Lettering in gummy aluminum (6063?)

I'm lettering some aluminum rack panels. Single line letters, 0.15 to 0.5 high, 0.032 line width, essentially just cutting a square groove which will be filled with enamel for contrast. Cutter is 0.032 carbide, 2F, uncoated, running at 27000 rpm at 10 ipm with 0.005 DOC, 0.0002 per tooth, air blast droplet cooling. Cutter is running in my 15-27K rpm aux spindle on an 1100, and has <0.0002 runout. Stock is mounted with tape/glue, flycut flat prior to lettering.

This works, but I'm essentially melting and plowing the groove in the panel- very obvious bead. Same happens at slower ipm, less depth. Cut depth is consistent, and a post lettering flycut gives a decent result. Not breaking cutters. I can live with it. But it's meatball machining. Embarrassing.

None of the rack panel manufacturers (Bud, Hammond) list an alloy type, but this is soft, gummy, sticky aluminum. Miserable to machine. I've heard that it's some variety of 6063, which seems possible.

Cutting parameters in this ballpark work fine on other alloys (7075, half-hard 6061). Crisp edges, no melting. The usual things I vary to tune the process -lower ipm, DOC- haven't helped here. Haven't tried an engraving cutter yet.

Does anyone have a proven, working cutting recipe/cutter in rack panel aluminum? Anyone know for sure what this alloy is?

(NB- I've read Ray L's thread from 2013; everybody agrees it's miserable stuff. But that said, what actually works for milling this goo?)

Later: carbide engraving cutter- effectively a sorta pointy D bit- is no better. Just shoves the stuff aside. No surprise.

1/8 shank HSS 0.032 cutters are not common. For some reason, they're all 3/16 shanks. Precision low-runout collet ordered.

I have found that sometimes carbide cutters that size aren’t sharp enough to cut really gummy aluminum and instead of cutting it they just push it out of the way.

You might consider trying high speed steel cutters.

Thanks, Steve. I'll try that.

I'm for sure getting push-it-out-of-the-way. It's ugly.

Try keeping it as cold as possible, as aluminum generates heat when cutting it gets gummy, I have seen it in various grades.
maybe some cutting oil or tapping fluid.

maybe engrave some 6061 tags and affix with glue or screws?

Hi,
I sometimes get into trouble machining heatsinks. No real telling what grade material it is but it is pretty soft and is suitable for a high extruded
products like heatsinks. Can be a sod to mill though.

The single biggest improvement is flood cooling, I suspect it is less about cooling but more about chip evacuation from the cutzone. Recutting soft
aluminum chips is a sure fire way to get Built-Up-Edge (BuE).

I personally prefer uncoated carbide. Most coatings are various nitirdes, (Aluminum nitride, Titanium nitride etc) and nitrides are tri-valent. Very slippery
in steels but show an affininty for aluminum which is also tri-valent.

I tried a four flute endmill but that was a mistake.....the flutes are very small and inclined to block up leading to BuE. Two flute endmills have larger flutes
and block less readily. I have not tried single flute tools but may extend the advantage of reduced blocking of the flute due to its greater size.

I bought (Harvey Tools) and used (and wore out) a 1/8 two flute endmill coated with Titanium DiBoride which is especially good and recommended for aluminum. It worked a treat
in some of the sticky stuff.

Craig