Aluminum milling "yes again"

[Woodenspoke]

My first foray into milling aluminum was less than spectacular on a CNC'd mini mill. The bits quickly became caked with aluminum and things went down hill. I have since read numerious posts on this forum, and there are many on this subject, so I have begun to start again first by:

1. ordering a simple misting unit for lubrication.
2. carbide cutters made specifically for aluminum (the carbide was on sale).
3. stop using climb milling on such a small mill in aluminum.
4. prayers to the machining gods.

So far I have wasted several cheap HSS cutters 2 flute and 4 flute, not a big loss but annoying. I read somewhere that you could use muriatic acid to remove some of the hard to get at aluminum, only they were mentioning carbide cutters and these bits are HSS; will it work?

Questions to the group about the job I need to do. Its milling a slot and two holes through a 1/4" 6061 aluminum plate, for 100 pieces. The holes are small 1/2" and 5/16 "and the slot 5/16" x 3/4". Not a big job. I want to do this in one pass using a 1/4" cutter. I was using a 3000 rpm spindle speed and slow feeds 6 ips with light cuts at a .02" depth and a very slow plunge rate. I would love to speed up the process. I am trying to stay away from the math since the mill has limited capability to preform. The max spindle speed on the mill is 4300 rpm if that is any help and ips is what i set it at. Its a mini mill so be realistic.

My assumption right now is the feeds are to low for such a high spindle speed added to no lubrication.

Thanks for any help or direction you can provide

woodenspoke.

[cdlenterprises]

Never cut aluminum dry. It doesn't matter what type of tool material you are using, coatings, geometry, etc. aluminum will bake load up the tool. Whether you use a Spray-Mist or get some cutting fluid in a can you need to have some type of lubrication. Once you get some lube, for slotting use a 2 flute endmill. Considering it is such a small diameter cutter I would run the spindle as high as you can but stay a little below max.

[Verfur]

woodenspoke,

Does this machine have ball screws, tight lead screw or acme screw with half a turn clearance in it (back lash)? This does make a diferance. also the rule of thumb for sloting is 1 diam max for the depth of cutt and your horse power also has to be high enough.

I think I would start out at 1/4 Diam and work my way up/down to 1 Diam. if the spindle has enough power and the machine has the rigidity.

chip packing is a big issue with alum. so coolant (flood) or mist (nasty) to lube the cutter and blow the chips out.

Use a 2 flute stub mill with a high helix and sharp (newish) start at 4000 rpm and a chip load at .001 a tooth aprox 8 ipm this is for climb cutting a less depth cut could run a slightly higher feed per tooth. If you have a lot of slack in the drive system then you will have give up the climb cutting as it will self propell and do nasty things to the chip load.

please note all machines are diffrent and material is diffrent slightly.

So you will Have to Salt to taste as these numbers are from the top of my head

[NC Cams]

Give the cutter a shot of WD-40 or dip the cutter in Dexron ATF before you start cutting. EIther will do a nice job of preventing the metal from adhering to the cutter like peanut butter does to the roof of your mouth. HSS should work fine with either of the above lubes based on our experience with cutting aluminum.

A light misting of WD-40 applied to the alumium will also enhance the finish and prevent the material from balling up while cutting/milling/facing.

For those who contend that WD-40 is not a cutting lubricant, I picked up the trick from a machine shop foremnan. He learned the trick when they got into a bind machining billet heads and WD-40 was all they had. Worked REAL good - so good that it became the shop lube for milling aluminum.

Necessity is truly the mother of invention.

[Woodenspoke]

I ordered the high helix, 2 flute, stub aluminum (name brand) end mills in carbide and only because the carbide end mills were on sale.

The machine is all ball screws and tight with 276 in steppers. I was under the impression that too shallow a cut and high spindle speeds was bad in aluminum and will take a toll on your end mill, maybe I read this wrong?

The machine had no problem cutting at a .02 chip load until the end mill was loaded. Then I noticed heavy vibration. I only tried the 4 flute because thats all I had left in a 1/4" size from a cheapo 20 bit 2 & 4 flute set.

Is there any reason I should stick with climb milling if these holes are not for show?

I have heard of using WD40 but I wanted to have the operation less of user interactive experience. With 100 pieces to do I just want to set it up for each run and come back to it in 10 minutes to change pieces. I really don't like the idea of misting but thats my only logical choice because I am not set up too flood cool.

Woodenspoke

[mrk]

Originally Posted by Woodenspoke My first foray into milling aluminum was less than spectacular on a CNC'd mini mill. The bits quickly became caked with aluminum and things went down hill.

This is a recycled tip from something I saw in another thread. If you have bits that are caked with aluminum you can clean the aluminum off by soaking in Drano. Just be very careful since Drano is dangerous stuff but if you take care and soak the bits the aluminum will melt away and the HSS bits will be clean and ready for more abuse.

-Mark

[Verfur]

.02 chip load or .02 depth???

chip load should be more like .001

the depth will pend on the tool strength and machine horse power and rigidity.

generaly speaking carbide would be for high prodution and higher feed because of tool rigidity. Carbide is less forgiving on chip re-cuting during sloting.

flood coolant = little giant water pump, a wash and five gallon bucket add a few feet of vinyl tubing. Real simple and worth every $$

not as nasty as mist by far

[wildcat]

Based on my limited experience I would not try to do what you need in a single pass at full depth. I would ramp down while climb milling at the proper feed rate down and around the slot with a good 2 flute endmill. If you don't want to ramp then I would not go deeper than 1/8" (1/2 diameter) at a time. The mister will be really helpful as well. Using a mister and climb milling at proper speeds my chips come off so hot they burn on contact though the part is only slightly warm and the endmill, when retracted, is cold. FWIW: I mainly only use HSS for > 1/8" diameter endmills and cobalt for smaller diameter or extra long ones.

[holbieone]

use one of those cobalt corncob cutters and some wd-40 in that mister (just a very lite mist)

the cutter will do it in one pass but will leave a serrated edge
you would need to go back in with a regular mill to clean the walls

[Verfur]

even if you make it in one pass you will still need a spring pass (finish pass).
What you will generaly find is the full diam pass pulled to the inside of the slot slightly. This may only be relitive if the tollerance/finish needs require it else zip burr it and awayit goes.

Holbione
Roughing endmills are a wondefull thing for removing mass amounts of meteal with limited hourse power and rigidity but generaly require flood coolant and I have never seen any 2 flute corn cobb roughers myself. So that leaves you with a min of 3 flutes and most likely 4 flutes for the common. At the 4 flute level, depth of cutt in a slot I would be very wary of chip packing.

I defently use the heck out of roughers when I can as they greatly decrese the time needed to do the job.

I hope this helps out as it comes from many years of getting dirty for a money.

[Verfur]

realy flood coolant is not as hard to do as one would think.

The wash tub (rubbermaid tub) and a little giant water pump and a seperate 3-5 gallon bucket to put the coolant mix with little giant pump in som hose (vinyle from home depot or Lowes) and a few plastic fittings.

The most exspensive thing would be a one gallon container of coolant mix and it only needs to be about 10% ratio with clean water.

Just a note: Somtimes the coolant guys will even give/sample you a gallon for free. You know the story there the first one is free than the rest will cost you after you are hooked on it. LOL

Just use a nice coolant mix that is good for alum and has a anti-rust in it.

the coolant has a mutifunction, as it is to keep the tool, part cool, provide lube for less friction and flush chips away from the tool.

surly there has to be a post on here (CNCZONE) where some one has done this on a small mill.

[Woodenspoke]

I finally went and checked out some sites talking about chip load and figured out that .005 -.002 is the proper range. thanks Verfur who suggested .001 chip load, 4000 rpm at 8 ipm. That seems about right for this mill.

I also read that you should try for 1/2 the diameter as a depth for any bit. Of course they are not talking about a mini mill with limited power and the unfortunate habit of cutting drive power if the bit bogs down (fine for manual cut a disaster when you start loosing motor steps before you can hit the estop).

I have been using a depth of cut of .02" what should I be striving for. Certainly not .125" as recommended. Should I go deeper of stay shallow?

For all those WD40 freaks out there I will spray the bit first with WD40 then use my mist coolant system which is now set up. By the way WD40 also removes contact glue (like labels) if you want to remove the glue without using harsher chemicals especially on a nice surface finish.

Woodenspoke