machining Aluminum for the first time.

[carguy327]

Hello everyone.

I have a customer that needs 16 brackets cut from a sheet of 0.19" aluminum.
He doesn't know what it is as far as grade, but it's pretty heavy for it's size
(32"X48").

I have an AXYZ 4X8 CNC router table with a Unist mister with aluminum cutting fluid within. I have my tooling depth set at 0.05" per pass, cutting with a 0.25" end mill.

How fast can I set my feed rate?

Thanks,

Gerald

[fpworks]

How fast can you turn your spindle?

Depending on how well your process evacuates chips, I would start at 0.002" or 0.003" per flute (with a 3 or 2 flute tool, respectively) and go from there.

...0.002"-0.003" per flute is a bit aggressive since it is a router. (didn't read)

[mxtras]

I am guessing you have Perske spindles on that machine? 20,000 RPM? Actually - I think the Perskes were 18K....??

I would guess max feed would be in the 12-15 IPM range. Use lots of air to keep the chips from clogging the flutes.

Scott

[Geof]

I think 12 - 15ipm is a bit conservative. If you have a 45 degree helix two flute cutter (GARR series 242M; part #GAR85200 from Thomas Skinner & Son Ltd), held as short as possible running at anything above 10,000 rpm you should be able to handle 40 ipm feed at 0.1" depth of cut. Make sure your mister is keeping a good cloud of coolant around the cutter.

[carguy327]

I have an Elte 10hp spindle capable of 24,000 rpm. I have a 2 flute endmill.

Thanks for the info so far

Gerald

[mxtras]

The limitation on that machine is not the spindle speed - it's the rigidity of the gantry. It will sing like Mariah Carey when you try to push it - or least that has been my experience with the AXYZ routers. They are good machines, but not meant for cutting much other than MDF, etc. I understand they use the machines at the factory to cut parts for their machines from 1/2" AL plate and when I talked to the guys that run those parts, I learned that they were not able to run any faster than I was running - see below.

I have made probably 500-750 parts from 6061 1/4" AL plate using an AXYZ router. I have found the best results using 24,000 RPM (Elte spindle) and I used a .25", 2 flute EM. The best balance I found was running a depth of cut = .0625" and a feed of 9-12 IPM. You can run faster with less depth but then it requires more passes. Chatter is an issue.

Let us know what you end up with! I am interested to know.

Scott

[lakeside]

most of the time when you hear a spindle with a high pitch singing it mean your rpm are to high if you can slow the rpms decrease cut depth and increase feed rate this will increase tool load and you will find that a better cut can be had but if you only have a set speed than keep the coolant on it and let it sing

[rmtucker]

I just finished cutting these on my home made router:-
www.weardalecnccarving.co.uk
goto vwtrike project and Press the March button (and scroll to bottom of page)

This was 1" thick aluminium using a 5mm cutter at 22,000 rpm and a feed of 700mm min and .025" depth of cut with no coolant just vac.

It will run at this all day,Hope this helps

Regards
Mark

[carguy327]

Well the job is done.

I first "drew" on the face of the bracket with a 0.25" v bit. It didn't cut very smoothly. Once on the cutting pass though, 40 ipm and 18000rpm went very smoothly. My depth of cut was pretty conservative at 0.045".

I took a couple camera pics.

Thanks for the help,

Gerald

Owner / Artist
www.imperium-design.com

[lakeside]

nice work

[Braltie]

I'm just learning the cnc router at work, cutting aluminum various guages, mostly using 3/16" single flute cutter, how many sheets can be stacked at a time? does it matter if you run multiple passes?