Frustrated: Breaking bits milling Aluminum

[fivefishcnc]

Newbie here... I have no problems milling MDF and wood. I use them to test simple projects and learn how to operate my CNC machine, Mach3 software and Sheetcam software.

My main intention is to mill 0.60" alumnum, and maybe even 0.125"

The problem is I keep on breaking bits. I bought special aluminum "O" flute bits from Amana which says they're specifically for milling aluminum.

First the shaft broke. Okay, the tip was still fine so I just re-used it with the shorter shaft. Seems better.

But once in a while the bit will break.

I'm probably doing something stupid, so can anyone be kind enough to tell me what it is I'm doing bonehead?

My speed is now down to 3 IPM. It seems to be doing fine at this speed. But it takes forever. I can mill at 5 IPM (I thought so, until I broke the bit after my 6th square hole on a 1/16" aluminum sheet.

I bought a speed controller hooked up to my Rotozip. I don't know if I should go for maximum RPM or somewhat in the middle range. (I know, not enough data. I don't know my RPM).

Can anyone point me in the right direction? This is getting to be expensive buying bits.

I just want to mill some rear panel holes as you can see here. (my product)
http://www.fivefish.net/diy/1UX4-SC1.../SC-1-rack.jpg

My CNC is just ebay bought. Once I get this working and save money milling these rear panels in-house, eventually I'd like to buy an $8K milling machine. (I wish.) But for now, this is what I have.

I appreciate any help/pointers/tips you can give this newbie.

[fivefishcnc]

More info:

I forgot to mention these:

I'm using 1/8" bits. Z movement per pass is 0.4", 50% overlap, 3 IPM.

Software is Mach3. Gcode created by Sheetcam. Both registered and full version.

[Geof]

With a 1/8" diameter cutter your rpm should be as fast as possible even with HSS cutters; to get 500 surface feet per minute you need over 20,000 rpm.

With aluminum 2 flute cutters are better as they have more chip clearance.

Your depth of cut should be about 50% of the cutter diameter. The feed depends on the rpm and could be about 0.0005" per tooth, 0.001" per rev for 2 flutes so at 20,000 rpm you may be able to go at 20 ipm.

You definitely need cutting fluid/coolant.

But if you are cutting one of the softer alloys, which may be the case if it is a formable alloy with a low temper, then you have to back off on both the depth and feed by half or less.

[fivefishcnc]

Thanks Geof,

I had a typo... my Z movement was (.04") ... NOT 0.4" per pass.

I increased the RPM to max, kept it at 3" IPM, and so far it's holding up.

With aluminum 2 flute cutters are better as they have more chip clearance.

Thanks. I will try that next.

[altered]

If you don't know were your aluminum came from, it's probably utility grade wich is very sticky and more difficult to machine than 6061-t6.

[fivefishcnc]

Okay some update:

The eventual goal is milling Aluminum 5052, .06" thick. Ocassionally, may do .125" thick.

At the moment, I'm using scrap Aluminum I bought on eBay, trying out various thickness so I can play with it and not mess up my good aluminum panels which is meant for the final product.

I made some changes to my Sheetcam programming, now I'm doing ramping down instead of straight plunge. Set my router to spin at it's max RPM (still don't know what that nunber is, it's a Rotozip Z25) and doing passes at 0.03" Z depth per pass on a 1/8" end mill. So far so good. (maybe a little too much conservatively???)

I'm doing it at 3 IPM, and tried it at 4IPM which so far after running for (1) hour, still no bit breakage. (so that's good)

Of course, now... the goal is shorten that milling time. (1) Hour per panel is just too much. If I can reduce that to between 30 - 45 minutes, I'd be happy. But since this is just low volume production of my cases, I can live with 1 hour per job if I have to.

I still would like to try that 2 flute bit to see how it performs. Any brand recommendations? Anyone?

[Pres]

What are you using for coolant?

What are you using to remove the chips from the cutter flutes?

2 flute offers the most chip clearance but rattles the most.

3 flute can be a pretty good compromise.

Whatever you use, make sure it is solid carbide so as to last awhile.
(however, tool vibration is a death sentence to carbide)

hth,
Pres

[panaceabea]

sounds like a rigidity problem to me, either your spindle is allowing the tool to deflect and break or more than likely since you cutting thin sheet metal the work piece is riding up the tool and breaking it . I would avoid carbide unless you have a very rigid spindle and setup and your not cuttig sheet metal over 2" or so from a clamp

[LeeWay]

Another thing is mills do not like to cut sheet stuff. I have done it on my router for .063 5052 aluminum sheet using a PC 690 at full speed in one pass @ about 30 IPM.
I was using a 3/16" straight 2 flute and lots of WD40. The problem with sheet stuff is your hold downs have to be close to where you are cutting in order to hold rigidly enough not to lift material or break bits. The straight flute carbide cutters do stop the lifting part, but unless you have a rigid setup, you can still snap bits.
On the router, I had maybe 8 screws holding the sheet down. I was getting 25 parts in a 16" by 19" blank. I used the skeleton from the first blank to determine where the screws should go. I used toggle clamps on the edges.
I have been milling lots of sheet steel on my mill. 11, 12 and 13 gage. Would be easier with plasma, but it ain't done yet.
I use a magnetic chuck to hold the blanks and so far, so good. I haven't had any of the larger blanks slip yet. I did try to mill a part out of a 2 square inch part and there was not enough surface area to mill such a small part.

I am using a piece of 1/4" steel now to make a jig or fixture that mount on the mag chuck that will hold my aluminum sheet blanks now. I will probably only get 5 parts at a whack instead of 25 like on the router, but it is a better tool for the job. I didn't like seeing the aluminum chips flying into the router. Heat was also an issue for me, but my mill has coolant.

[fivefishcnc]

Thanks guys for the response. The last few posts got me thinking.

It may have to do with how stable the part is clamped to my table. I do remember the first 2 bits I broke it's because the sheet moved underneath. The sheet moved along with the bit during a change of direction. And snap... the bit broke... this was at the 2nd pass.

So I *thought*, maybe I should try milling a thinner sheet of aluminum first, then move up to the thicker material as I feel more confident. and this frustrated me even more... Im thinking this is a very thin piece of material and my bits are still breaking? But I do remember seeing deflection in the middle of the sheet (bowing up). It's clamped on 4 corners.

The last successful test I did was on a thicker aluminum with little deflection and was able to mill for more than an hour with no bit breakage, and actually got pretty good results.

I'll keep on debugging this. I know I'm close to workable solution, given the limited capabilities of my machine. Once this starts saving me money, I'd like to get a real machine. But it will be easier to convince the wife to buy a real machine if I can produce something with this setup.

[LeeWay]

If you have a lot of this to do, you could build a U or J shaped hold down that mounts to the mill head. Adjust is so that it will put tension on the sheet when the mill spindle engages. Kinda like a manual torch height control system. They sometimes use roller balls, but just aluminum arms waxed up should do the trick.

[PinMan]

Dont know if this will be beneficial, but here is an idea.

If you are having rigidity issues and your drill is breaking, and your part is only .060 thick, you can use a #4 centerdrill for a .125 hole. The drill diameter on that is .125 and the length of the drill nose is .125.

They are super rigid and you can run them slower (~950rpm @ 2ipm works great for aluminum)

Center Drill Chart