PDA

View Full Version : Milling Aluminum



InventIt
02-19-2004, 08:28 PM
I am curious about milling alum. with my cnc router. I am still in the build process and I would like to incorporate the needed requirements into the design so the machine will perform as expected on harder materials like alum.

Can you guys who have experience will this give me some help.

What problems did you have when you milled alum in your router?

Thank You
Rob

balsaman
02-19-2004, 09:02 PM
I have had the endmills plug up and break. This is because of no coolant mostly. I also had trouble because my spindle was underpowered at 7 amps.

If you want to do it the machine needs to be stiff, and you need to take it easy. I had the most luck with a 1/4" endmill.

E

Hobbiest
02-19-2004, 09:11 PM
End mill may have also been plugging up from too high a spindle speed. It ends up almost melting it instead of cutting off chips. Don't know what proper speed is, Hu and Ballendo say that it depends upon the situation.

balsaman
02-19-2004, 09:55 PM
That's where the coolant comes in. Keeps things cool and provides a lubricant too. All I know is my router had to be on max to get enough power to keep it from stalling.

The 1/4" bit has bigger flutes so the material could get out of the way better. In hind sight I was probably cutting too deep in one pass too. .200"

E

strat
02-19-2004, 10:16 PM
All wrought aluminum alloys, 6061-T651, 5000, 6000, 7000 series
carbide .....opt f 15 s 620 avg f 8 s 2020
hss............ opt f15 s165 avg f 8 s 850
f= feed .001/tooth s=speed ft/min
this is from machinist handbook

ger21
02-20-2004, 06:24 AM
To mill aluminum with a ROUTER, you need tooling designed to be used with a ROUTER. The feeds and spindle speeds you listed are useless to someone using a router with 10x the spindle speed. (unless they can cut at 150+ ipm). Spend the money and get router bits designed to cut aluminum. As I mentioned in another thread, check out http://www.onsrud.com .they have a huge assortment of aluminum cutting bits designed to work at router rpms. One other thing to consider, as was mentioned, is coolant. If you dont want or can't use a liquid coolant, try setting up an air line to blow into the cut. This will help keep the chips clear and keep the cut a little cooler.

Gerry

steveald
02-20-2004, 08:19 AM
Hi,

I cut aluminum with a 3.25 hp router at work and with a 2.25 hp router at home. I use a water and oil mist coolant at work, but it's messy so I went with a Lenox Micronizer Jr. oil mist coolant system for home that works just as well. It blows compressed air at the bit, and adds 3 to 6 drops of cutting oil per minute to the air.
I use a 1/4" 2 flute up-spiral endmill TiN coated carbide router bit whenever possible, and 1/8" when I need sharper corners. I have heard of people using a 1/16" or smaller bit with aluminum, but I haven't had any luck with those bits.
The speeds and feeds I use are 10-15 ipm depending on the edge finish I need, 16,000 rpm for 1/4" bit and 19,000 rpm for 1/8" bit.
I cut up to the diameter of the bit per pass, and between 50 and 75% step-over for surfacing, again depending on the finish I need.
I use 6061-T6 whenever possible, increase the feedrate for utility grade to avoid melting and plugging up the bit.

Steve

peter
02-20-2004, 09:11 AM
hi guy's
don't be using endmills to many flute's
will cause it to clog up
use slotdrill's 2 flute 3 flute max
this will allow it to clear swarf in between cut's
just input
best regard's
peter

InventIt
02-20-2004, 09:11 AM
So it sounds like coolant is the biggie.
Do you guys have problems with the bit grabbing the work piece or a lot of chatter?

steveald
Are those the "alum cutting" end mills. the ones that have a different helix designed for soft metals? If not have you tried them?

steveald
02-20-2004, 11:39 AM
Hi,

The bits I use are general purpose router bits. Everyone I have dealt with in the sign industry refers to them as endmills, but they aren't like milling machine endmills, so they probably should be called a slotdrill.
I haven't tried any bits that were specifically for aluminum.

Steve

azsigns
02-23-2004, 10:05 PM
I cut out aluminum lettering all day long.
Here's what I do using a 3.25hp router on a medium built machine.

5052 Aluminum
1/4" Single Flute Carbide (Belin Yvon 33635)
Depth/pass 0.080" to 0.090"
Feed Rate 35 - 38 ipm
Spindle 13000 rmp
Mist Coolant (Oil Based)

This gives me a mirror finish on the edges and good tool life.
The Belin Yvon cutter is by far the best I've ever used.
Nice clean cool little aluminum curls for chips. Not those short sharp slivers you pick from your fingers for days.

The cutter being single flute has an extra large clearance for the chips so it never welds up. Expensive bits but worth every penny.

Just feed the Z axis slow around 10 ipm. They don't like to plunge.

Chris

ballendo
02-24-2004, 09:30 AM
Thank you for this info!

What is the typical total thickness of your part and/or cut depth?

Ballendo



Originally posted by azsigns
I cut out aluminum lettering all day long.
Here's what I do using a 3.25hp router on a medium built machine.

5052 Aluminum
1/4" Single Flute Carbide (Belin Yvon 33635)
Depth/pass 0.080" to 0.090"
Feed Rate 35 - 38 ipm
Spindle 13000 rmp
Mist Coolant (Oil Based)

This gives me a mirror finish on the edges and good tool life.
The Belin Yvon cutter is by far the best I've ever used.
Nice clean cool little aluminum curls for chips. Not those short sharp slivers you pick from your fingers for days.

The cutter being single flute has an extra large clearance for the chips so it never welds up. Expensive bits but worth every penny.

Just feed the Z axis slow around 10 ipm. They don't like to plunge.

Chris

azsigns
02-24-2004, 03:43 PM
Part thickness is usually 1/4" plate, sometimes 1/2".

On a 1/4" plate I take 3 passes @ 0.090" each.

The first 2 passes I set my tool offsets for a .27" dia cutter and on the final back to .25", just to shave off an extra .010" for safe measure incase of a slip.

Can't say enough about the Belin cutters. They are a work of art!
Never found a better made cutter for this type of work. I only wish I had found them years earlier.

BTW, I'm running a stepper machine made up from Techno slides & extrusions (not very heavy), using Ability Systems Indexer, & my own electronics. Nothing very fancy or heavy.

Chris

BT1
04-01-2004, 03:02 AM
I like HSS slot drills, 2 flutes.

Also some WD40 works well on the finish cut.

ger21
04-17-2004, 11:40 AM
Anyone know where to purchase these Belin cutters in the US?

Cold Fusion
04-17-2004, 11:51 AM
I would also like to know where to buy these great cutters.

steveald
04-17-2004, 12:06 PM
Hi,

I'm not sure about the US, but they can be ordered through Acme Sign Supplies in Canada.

Steve

Ken_Shea
04-17-2004, 09:49 PM
Gerry,
If you cannot find the Belin cutters you are looking for, you should give these a try, 1/4" carbide, aluminum cutting end mills. I have dealt with this company and there tools and as is obvious, recommend them. These cutters are under $8

I have tried good quality made in the USA HSS cutters in aluminum and they don’t touch the performance these carbide do. I am not making a blanket statement only what I have experienced.


http://www.american-carbide.com/EndMills/ACEM.aspx?SubCategoryID=7&selection=6&Cat=1


Ken

ger21
04-17-2004, 11:36 PM
I just wanted to try the Belin cutters, haven't used them myself.

jstuedle
07-05-2004, 08:02 PM
The poor mans was to keep your cutting cool, lubed, and free of chips is to keep a small dia. nozzle of compressed air at the cutter, and swab the cutter with an acid brush dipped in # 2 fuel oil or kero. A drop or two every few seconds works magic and if you are stingy enough it keeps down the mess. The air volume should be moderate, not excesive, and close to the cut. Less than 1/2" works well. The trick is to only keep the cutter moist, not dripping and slinging excess oil. Let the air do the work of clearing chips and the oil barely lubricating the tool.

ezdonedeal
12-05-2011, 08:20 PM
Hi everyone,
can anyone help me choose the correct equipment and the best method to create an aluminum handle like in the picture below?

is this something i can make in house?
im a rookie when it comes to machining, I have just recently been researching about this topic. any tips?

http://djnir1.com/handle.jpg
http://djnir1.com/handle4.jpg
http://djnir1.com/handle2.jpg
http://djnir1.com/handle1.jpg
http://djnir1.com/handle3.jpg