Looking for advice to cut aluminum plate

How To Machining
1

hey y’all,

i’m looking at cutting .1" aluminum plate. i have stock xxl, mikita router, carbide end mills, no mist system.

i understand there’s a fine line between melting the aluminum and actually cutting it. i’m wondering, based on everyone’s experiences, if the suggested feeds and speeds in carbide create are a good starting point and if i should use a flat end mill or a ball mill? 1/4"? 1/8"? should i use cutting fluid and water in a spray bottle? or just one or the other, or anything at all?

suggested: depth per pass .05", plunge rate 10, feed 24, speed 16000.

would appreciate any info y’all have or if you need more info from me. i don’t really have extra stock, so i’m hoping to get this right on the first go around, even if it means taking more shallow passes.

thanks in advance

2

First, a question, “What alloy is the plate?”

Second, another question, “What sort of cuts do you wish to make?”

Third, “How will you be securing the stock?”

1 Like
3

I would start with the default values in the CC library and work from there.
I think the DOC is 0.015, stepover 10%, RPM 18000

Feed rate seems to be bit specific. 1/4 end mill (201) is 48 ipm. 1/8 end mill (101) is 24 ipm.

I have used these numbers without any lubricant successfully. As noted by @wmoy these number work for slotting ( the worst condition ).

2 Likes
4

alloy is 3003 temper h14

i’m cutting down a 12x24 piece into 3x4 tags, was just going to do square cuts, but if this proves to be fairly simple i’d like to scallop or chamfer the corners.

was planning on painters tape on the waste board and the aluminum, then two sided tape or glue. trying to avoid having to clean a bunch of sticky residue off the piece.

5

Keep in mind that you need to keep heat build up down in the aluminum. It doesn’t take much to make the tape fail due to heat.

I’d also suggest buying a couple of 1/4” o flute bits, I’ve used some cheap spetool ones off Amazon with luck.

6

i’ll see if i can approval to buy new bits- the single flute really makes that much of a difference in keeping the heat down? i haven’t used one before.

7

Not familiar w/ this alloy — will the tags have holes which can be used for workholding?

See the videos at:

and definitely get a suitable single flute tool w/ a compatible coating such as ZRN.

8

3000 and 5000 series aluminum are pretty gummy and the sweet spot between gumming up and cutting good is really narrow. I’ve cut 5000 series, but not 3000 series

1 - I would use a flat 1/8" single flute upcut. The 1/4" is more rigid, but for a given RPM, it is traveling way faster, so you would have to kick up your feed rate a lot to get the proper chip load. The single flute helps chips clear out and reduces the chip load.

2 - I would reduce the depth of pass to more like 0.020". There is less material to clog the flutes of the endmill and less friction on the sides imparting heat. This also allows you to increase the chipload by increasing feedrate. If I have a choice in aluminum I increase the feedrate and reduce the depth of cut and/or stepover.

3 - I would use a ramping entry rather than a plunge.

4 - I would double that plunge rate to 20, and the feed to more like 50 or 75. The RPM should be good.

5 - I like to do a roughing then a finishing pass. That gets the wall finish better and for the finishing pass, gives the chips a place to help them eject.

6 - I would get some air blast on the cut as well. Help it all cool off a little as well as get the chip away.

3 Likes
9

It’s more about chip extraction. With Single flute.

Aluminum is not forgiving like wood. If you can’t extract the chips and get a chip between the material and the bit you break the bit.

An Air blast does a lot to help with this too.

Heat build up is more about feeds and speeds. But the oflute will help with larger chips.

10

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.