Aluminium Grades - cutting

[Simops]

I had a search on the forum but scant info found.....its abot the grade of Aluminium.

I cut a bit of 2mm (5/64") and 3mm (1/8") aluminum sheeting.....just simple 2D through cuts. I was recently told to use 8035 aluminium as was best grade for cutting on a CNC. OK...so went to my supplier and asked him if the stuff I bought was 8035.....nah he said, its 5005. He said its the only grade they have and was an all round frabication grade. Didn't know anything about CNC.

So question is do the guys here that cut aluminium have any preference for Grade? Is 5005 OK to use? Is Grade really that important....it seems to cut OK for me but not sure yet if it will have deterimental impact on cutter life or cut quality?

Cheers

[Brady Watson]

It doesn't matter a whole lot when it comes to sheets, because the majority of the sheets they make are only a few different alloys. Single flute spiral-O upcut...1.2,0.7 IPS @ 13-15k RPM. Start there. Slow MS down if using dia under 1/8" or 3mm. Gotta try to keep them expensive cat whiskas intact ;)

When you start to get into AL bar, tube and rounds, the alloys start to matter because you are typically machining thicker sections than sheets, and some get heat soaked more than others & tend to gum up. This is where knowing about the attributes of the specific allow comes in handy. For sheet goods however, you aren't going to be in them long enough to cause any problems, so it isn't much of a concern. Same goes for most non-ferrous until they get over .25" thick or so.

You should not have to worry about coolant, although I would use dust collection. Also, word to the wise...watch polarity shifts when using vacuum hold down...keep your safety glasses ON until all material is off of the machine bed!

-B

[Simops]

Copy Brady....at 1.2ips....how many passes would you use for 5/64 and 1/8" thick sheet? I tend to be conservative and use 0.5ips with two passes with 1/8" cutter. Am I being too cautious?

Cheers

[Brady Watson]

I would speed it up a bit...it really boils down to how delicate and small the parts are. You DON'T want to overheat the bit, so a little more chipload will help pull some of that heat out.

-B

[Ajcoholic]

2011-T3 is a very, very good, free machining Al alloy. It is to aluminum what free machining leaded steel is in the world of steels. Here in Canada, 2011-T3 is about 3X the cost of 6061-T6 (the most common "aircraft grade" aluminum alloy - about the middle of the road in terms of strength, machine-ability and still has good anti corrosion properties)

The 7XXX grades of aluminum are the strong ones, and trickier to machine.

I used to make a lot of model engine parts, mainly lathe turned but some milling operations as well. If you can get 2011, it cuts like a hot knife through butter, and doesnt gum up.

AJC

[Simops]

Been asking my trade supplier and couple others (not many suppliers around that supply small quantities) and none of them new about what grade to use with CNC, in fact the ignorance shown about types of grades was outstounding!

One thing I have learnt since starting this game is the incredible lack of choice available and how high prices are for materials here compared to Canada and the US. Guys you can out yourself lucky in the States with the price of things and the choice you have!!!

Enough ranting.....I will stick with 5005 as that is whati can get easily......now two questions remain:
1. Pass depth....with 2mm aluminium say....what do you use?
2. Down cut or upcut bit.....preference? Requirement?

Cheers

[Brady Watson]

Material isn't that cheap here in the States anymore...3/4"/18mm MDF used to be a solid $16 all day long. Now that junk is $30 a sheet. Go figure.

Most suppliers have no idea what they stock, and unless you need to select specific attributes of the material for post processes, like the ability to weld it etc, then it doesn't matter too much. 'Round these parts' my supplier stocks 2000 and 5000 series in lighter gauge sheets. You can get 6063 and 6061 as well, but you have to shop around for it.

In terms of cutting, nearly all non-ferrous metal will cut well using a single flute spiral-o upcut or 2 or 3 flute straight designed for cutting metal. Start with the settings I gave you as a baseline. Looks, listen, learn and adjust accordingly. Cutting AL is unnerving the 1st time. It sounds 'all wrong' and the harmonics are different than anything else you've cut.

Good hold down is really important. Screws and clamps are tricky because they can tork the sheet where it won't lay flat. Vacuum is best. Adhesive is hard to use, unless you use my Vacuum Film Technique.

-B

[Simops]

Material isn't that cheap here in the States anymore...3/4"/18mm MDF used to be a solid $16 all day long. Now that junk is $30 a sheet. Go figure.
-B

Hey Brady......try 8 x 4 x 3/4 MDF sheet 5th grade from China $40 less if you want to buy 100 sheets. Birch Ply 8 x 4 x 3/4 sheet at $140

Anyhow roger wilco on the upcut.....what about passes....would you suggest max 1 mm (0.04") per pass depth?

Cheers

[Brady Watson]

I would shoot for .04" max per pass until you get a feel for how the material is cutting. This would be with a 3/16 to 3/8" dia cutter. Smaller, go less. As a general rule, I tend to be very conservative with speeds when cutting AL. My machine isn't anywhere near as rigid as my Bridgeport CNC mill...so I treat it accordingly. Even when cutting thick AL, I tend to limit cut depths to no more than .06" per pass, and lighten up the stepover for pocketing to 20% or less. Things like brass and bronze need to be lightened up to minimize shock loads when stepping over on pockets etc. Make sure you ALWAYS XZ/YZ ramp into the cut using the profile toolpath options in PWorks/Aspire & never EVER drill AL. Always an inside profile cut using spiral ramp and a smaller bit than the hole you need to 'drill'.

When you get into smaller dia bits like single flute spiral-O @ 1/16" dia, you want to pull back stepdowns to .015-.02" per pass to keep that cat whisker of a bit intact :) Don your safety glasses and pull that dust foot off for one or two parts. Get in there & SEE what is going on...grab some of those chips rooster tailing off of the router and mic them out. That's your chipload, BTW...and it doesn't hurt just to see where you are. Don't get hung up on chipload...as a general rule, these light machines take a much lighter cut than the manufacturer says the tool can be run, and chiploads are just 'ballpark' estimations. No where does it factor in your hold down solution & what it can take before it fails...and other factors. If you run too light a chipload, you will break the bit because it couldn't get the heat away by forming a large enough chip. If you run too high a chipload, the sheer force of pushing the tool faster than it can cut through the material will cause it to break. AL is no different.

Don't be skeered...If I can do it, you can do it. Here's an analogy for you:

Eggs:Omelettes :: Tools:Parts

Ya gotta break a few :D

Also - don't underestimate the importance of a nice flat spoilboard AND keeping your material held down flat. I've seen it where the spoilboard wasn't flat and the material was also tweaked, causing a condition where a 1/16" cutter would have to cut nearly 0.125" deep because of variations in the table and the material not being held flat.

-B

[Simops]

Thanks Brady for the detail given.....

Cheers