Machining aluminum 1

[lugnuts67]

Please advise any information on milling T6061 aluminum. I have tried O-flute, 2-flute, 3-flute and 4-flute (in high speed steel and carbide) at speeds from 2500rpm to 17Krpm and feed rates from 20 inches/min to 75 inches/min without coolant, with compressed air, with a mister and flooding it with 3 different types of coolant and have yet to produce a good part. I have however successfully welded end mills to the workpiece, broken a dozen mills of various sorts and stalled the 2.5hp router. Machine is a Technova CNC router with 2.5hp spindle. Cuts great for about 1 to 2 min with an O-flute @ 17Krpm, throws good size chip (suposedly what I am looking for to help remove heat)and then suddenly welds to the part. Part is 6" x 24" and 3/4"thick T6061 aluminum plate. Get halfway through and stops.
Any ideas? I can monitor the spindle speed on the display and it keeps speed up very well until the welding point.
I have heard that I am using the wrong coolant, too much coolant, too little coolant, too high /too low spindle speed, wrong cutter/cutter material, etc.
I am using a T-slot table and 6 T-lugs to hold the part in place so I do not think it is moving. The parts cut great out of wood and various plastics. The manufacturer has a video of this machine cutting aluminum on the web - asked them and they told me to go to brand X for mills and advise. Bought brand X mills for 27.95 ea and still have not cut first part correctly - brand X has done the best so far though at the recommended 17Krpm and 60in/min.

Any input?

 

[bklauba]

If you stop machining prior to breakage of the tool, and release the workpiece, does it distort/spring when released?

BK

 

[lugnuts67]

Will check and advise. Thanks for the new perspective.

 

[mrainey]

I would suggest a 3-flute end mill, but orient your thinking toward shallower depths of cut at high speeds and feeds. The shallower cuts allow the coolant to flush the chips out and reach the tool. No coolant at the cutting edges = dead tool.

Software For Metalworking

http://mrainey.freeservers.com

 

[btrueblood]

Are you using TiN or TiCN coated cutters?

 

[MechanicalChef]

What does your Machinery's Handbook tell you about cutting 6061?

 

[lugnuts67]

Unfortunately the machine's instructions are in Mandarin Chinese. I spoke with the rep and they said that rough translation was to follow the tooling manufacturers speed and feed rates - this has not been successful.

I have had a number of people suggest the 3 flute mills but the manufacturers of the mills say the o-flute or 1 flute are best for aluminum. They said that the key to cutting aluminum is to get the cutting surface into fresh material and generate a good chip to carry the heat away. If I use a 3 flute there are 3times as many cutting edges and the feed rate must go up (I would guess 3X for the same tool speed) to get enough material into the cutting edge. They explained the 3 and 4 flute failures as not getting enough material into the cutter and leaving heat for the next cutting surface and at 17,000rpm it starts melting its way through the material and eventually welds itself. Still does not explain why I have not been able to get the 0 and 1 flute cutters to work.

Frustrating

 

[mrainey]

By a wide margin, machining center pros in industry favor the combination of two-flute or three-flute end mills and heavy flood coolant for roughing aluminum.

There are several worthwhile discussions about end milling aluminum at:

http://www.practicalmachinist.com

examples:

http://www.practicalmachinist.com/ubb/ultimatebb.php/topic/13/5506.html#000006

http://www.practicalmachinist.com/cgi-bin/ubbcgi/ultimatebb.cgi/topic/13/5043.html?#000013

http://www.practicalmachinist.com/cgi-bin/ubbcgi/ultimatebb.cgi/topic/13/4752.html?#000000

http://www.practicalmachinist.com/cgi-bin/ubbcgi/ultimatebb.cgi/topic/13/4335.html?#000003

http://www.practicalmachinist.com/cgi-bin/ubbcgi/ultimatebb.cgi/topic/13/4254.html?#000000

http://www.practicalmachinist.com/cgi-bin/ubbcgi/ultimatebb.cgi/topic/13/4327.html?#000005

Software For Metalworking

http://mrainey.freeservers.com

 

[mullins]

In all of this, I never saw a step depth. You cannot just jump all the way down without expecting to break tools left and right.

I suggest googling ME Consultant. It is a free program where you can set your material and cutter and determine what your feeds and speeds should be. Thats what the problems sounds like to me.

 

[lugnuts67]

have the program set up to run 12passes to make it thorugh 3/4" plate. Thats 0.0625" bite each pass. Is that too much? I cannot get the ME Consultatnt to download - it keeps saying that the Bellsouth serever for that address is not avaliable.

 

[JDana]

I don't know about routers nor how their 2.5 hp spindles compare with our machines but...

We cut 6061 aluminum all day with 2 flute Ski-Carb end mills from Weldon running Trim E206 or Castrol Superedge 6754 for coolant. We have several machines, the smallest being a BT30 taper Sugino (not alot of HP nor spindle speed there)

I wouldn't hesitate to blow through properly heat treated 3/4" 6061-T6 with as small as a 5/8" end mill in only two passes. spindle speed 8000 to 10000 feedrate 20 to 30 IPM.

Softer metal seems to like high spindles with lower feeds as doo the smaller tools.

 

[JDana]

I should add that our Suginos have 6000 RPM spindles and we generally would run 4 or 5 passes and probably 10 IPM to get through the same plate. Actually we'd prefer to run it somewhere else.

 

[Ebug]

I am not sure if you solved your machining problem yet, but I have some input just the same.

6061 is a very gummy aluminum in comparison to 2024, 7050, or 7075, the three of which machine very nice.

In 6061 you should limit it to about 2000sfm, 1/2D DOC for slotting, and chip load is based on tool diamter. For a 1/4" dia tool stick to about .001" chip load, up to about .003" chip load for a 3/4" dia tool.

These are just starting points, but will get you running. With such little horsepower, you might have to reduce the DOC to get the machine to cut the way you want to.

If the tool is screaming with chatter, decrease rpm or increase feed rate.

Just for some comparison numbers, if you were using 7050AL on a machine with 20 hp you can run a 3/4" dia 3 flute 2.25"loc endmill at .250"doc, full width, 8000rpm and 400 plus IPM.

Good luck on your project.

Rob