Aluminum

Talk about all things CNC
danimal
Posts: 332
Joined: Wed Mar 13, 2013 5:53 pm
Location: Colorado

Aluminum

Post by danimal » Fri May 03, 2013 3:36 pm

So I finally took the plunge and started milling aluminum. I broke my Onsrud 63-602 end mill in about the first 5 seconds, :cry: but after that I just grabbed the one that came with the shapeoko and went to town. I wanted to see if we could get a solid list of mills that work well with aluminum for various purposes as well as a list of feed speeds, plunge depth etc. I downloaded just about every calculator that I could find, and they are all geared toward more production level machines and have variables that I do not know or understand as of yet. I know that there are little bits of information here and there around the forum, but it is spread out. Also there is more than one way to skin a cat, so I was hoping to get contributions from several people on here about their methods and chosen tools.

Somehow I managed to miss my target depth by a full 2.8mm. Not sure how that happened, but I know that I need to find a more accurate solution for leveling my work table to the plane of the machine. Now that I am finally making it rigid enough to do the work I want to do, I need to square everything up and get the accuracy where I want it. I will probably build an adjustable table and weld up a steel structure that holds everything a hell of a lot tighter. This is going to be a stronger mount for my 660.

Here is what I have so far, and I know that it is slow, probably rubbing like crazy, but the load on the mill was too much when I tried to use calculated speeds and it just snapped. I walked up to this using a couple test passes and depth range tests to see if I could see where deflection of the bit became a problem. This is just at the point where I gritted my teeth expecting it to snap at any time. I am going to get an Onsrud 63-604 and give that a go, but for the little two flute mill that I had this was givin her all she's got.

Feed = 160 mm/min
plunge = .2 mm
DW 660 RPM = 20000

Image

Image
Shapeoko # 1458

RT0701C Spindle || dual y motor || x axis nema23 with custom carriage 1000mm length || z axis nema23 linear rail upgrade with 1/2-10 ACME

WillAdams
Posts: 8488
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Aluminum

Post by WillAdams » Fri May 03, 2013 3:47 pm

_That_ is great!

Makes me anxious to get my machine up-and-running again (and I could use it too, looks like I may need to cut a motor mount plate to accommodate the coupler and pulley for my drive shaft).

Wikified!
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

Improbable Construct
Posts: 997
Joined: Tue Apr 10, 2012 3:21 am
Location: Fairhope, AL
Contact:

Re: Aluminum

Post by Improbable Construct » Fri May 03, 2013 4:11 pm

Using a DWP611 I have been cutting 3/8" 6061 aluminum with a Destiny Tool "Viper" 3 flute 1/8" end mill.
400 mm/min feed.
20,000 RPM.
0.1 mm depth per pass.

I broke one bit using a spiral down cutting path.
It worked until I got to the tabs.
Then the end of the bit clogged and it all went very bad.
Shapeoko #Classified some of the bolts may be original parts.
Shapeoko 1 # ???? Stainless plates, still in the box.
Shapeoko 2 # 3926 not stock
Shapeoko 3 # 0003
Store:
http://ImprobableConstruct.com
Twitter:
https://twitter.com/ImprblConstruct

twforeman
Posts: 1347
Joined: Tue Jan 29, 2013 4:51 pm
Location: Minneapolis, MN
Contact:

Re: Aluminum

Post by twforeman » Fri May 03, 2013 5:43 pm

The main issues are cooling and chip removal.

When I worked in a machine shop (many years ago) there were two main methods they used for milling aluminum.

1. Flood it with liquid coolant. This is very messy and probably not very usable with the ShapeOko.
2. Constant air blow - there are some flexible hoses you can use to direct the air flow. Like this http://www.mscdirect.com/product/09777012 The problem with this is then the chips go all over the place.

There are also specific end mill geometries designed for milling aluminum to prevent clogging.
Ender 3 3D Printer
ShapeOko v3 serial #0004 - upgrade thread
All of my ShapeOko related blog posts

danimal
Posts: 332
Joined: Wed Mar 13, 2013 5:53 pm
Location: Colorado

Re: Aluminum

Post by danimal » Fri May 03, 2013 8:13 pm

Here is the finished product:

Image

I bet that I could run about 400 mm/min with .1 mm passes. I will have to give that a shot.

As far as cooling goes, I did not seem to need any, though my vacuuming system did nothing for removing the chips from the cut as it got deeper. I might have to build a puffer system to lift the chips out so that the vacuum can do its job. I think that as long as you are achieving a reasonable chip size the aluminum acts like a giant heat sink and will keep the tool cool. This is only a function of the mill size though, so I assume as your spindle power and bit diameter increase so too will your need for cooling. Chip removal does need some attention though, and I am just trying to engineer a cyclone style system that utilize the same vacuum unit so to minimize energy consumption. It took about 5 hours to mill these parts out, so there is a real need to optimize the cutting and secondary systems.
Shapeoko # 1458

RT0701C Spindle || dual y motor || x axis nema23 with custom carriage 1000mm length || z axis nema23 linear rail upgrade with 1/2-10 ACME

danimal
Posts: 332
Joined: Wed Mar 13, 2013 5:53 pm
Location: Colorado

Re: Aluminum

Post by danimal » Fri May 03, 2013 8:33 pm

Improbable Construct wrote:Using a DWP611 I have been cutting 3/8" 6061 aluminum with a Destiny Tool "Viper" 3 flute 1/8" end mill.
400 mm/min feed.
20,000 RPM.
0.1 mm depth per pass.

I broke one bit using a spiral down cutting path.
It worked until I got to the tabs.
Then the end of the bit clogged and it all went very bad.
I noticed that tabs do not work at all. They stop the bit in place too long and seem to clog everything up. I just sat there on the stop button for the last few passes so that I could stop it if anything shifted, but after my secondary measurements the last pass left a sheet of aluminum foil connected to the parts that was easy to tear off and luckily nothing moved. I had to measure everything perfectly though, so I am not sure what the long term solution would be for parts like this that have no pre located screw holes to mount the parts down.
Shapeoko # 1458

RT0701C Spindle || dual y motor || x axis nema23 with custom carriage 1000mm length || z axis nema23 linear rail upgrade with 1/2-10 ACME

LTMNO
Posts: 172
Joined: Sat Mar 09, 2013 2:56 am

Re: Aluminum

Post by LTMNO » Sat May 04, 2013 12:55 am

nice, very promising.. great write up... I have been wondering which bits to buy....

Thanks for the post.
ShapeOko #1508, TinyG Controller, Dual Y, ACME Z-Axis, MeanWell(S-350-24v), NEMA 23's, 1m Squared t-slot table, OpenRail and the Original Z Makerslide and all Motor Plates...

jhllt67
Posts: 47
Joined: Fri May 04, 2012 1:57 am

Re: Aluminum

Post by jhllt67 » Mon May 06, 2013 2:33 am

I have been cutting a lot of 1/4" 6061 lately and have had good results with the standard 1/8" 2 flute carbide end mills that I use for everything else (the ones from eBay seller drillman1). I did buy one of the Destiny Viper end mills that I.C. mentioned but it didn't really seem to be any better than the two flute, not worth the premium price in my opinion. I have been running pretty fast at 30 IPM, .005" depth of cut (DW660 spindle).

I do have some lock-line connected to compressed air for a puffer because clearing chips in a deeper cut can be a problem as was mentioned.

As for work holding I have found it easiest to run the drills and interior holes first and then screw the part to the spoil board, followed by the outside profile. It seems to be really important to have it solid as aluminum is much less forgiving wood, very easy to pinch the cutter and break it.

The only thing I have had problems with is when the end mill is just about to cut through the bottom, sometimes it can pull the thin layer that is left up into the cutter. This makes the already heavy cut to much and causes some pretty nasty vibrations, occasionally breaking an end mill or gouging up a part. I sometimes slow a long profile cut down to 20 IMP for this reason. It is pretty rare though, I think I have broken 3 end mills in well over 100 hours of aluminum cutting.

danimal
Posts: 332
Joined: Wed Mar 13, 2013 5:53 pm
Location: Colorado

Re: Aluminum

Post by danimal » Mon May 06, 2013 4:58 am

jhllt67 wrote:I have been cutting a lot of 1/4" 6061 lately and have had good results with the standard 1/8" 2 flute carbide end mills that I use for everything else (the ones from eBay seller drillman1). I did buy one of the Destiny Viper end mills that I.C. mentioned but it didn't really seem to be any better than the two flute, not worth the premium price in my opinion. I have been running pretty fast at 30 IPM, .005" depth of cut (DW660 spindle).

I do have some lock-line connected to compressed air for a puffer because clearing chips in a deeper cut can be a problem as was mentioned.

As for work holding I have found it easiest to run the drills and interior holes first and then screw the part to the spoil board, followed by the outside profile. It seems to be really important to have it solid as aluminum is much less forgiving wood, very easy to pinch the cutter and break it.

The only thing I have had problems with is when the end mill is just about to cut through the bottom, sometimes it can pull the thin layer that is left up into the cutter. This makes the already heavy cut to much and causes some pretty nasty vibrations, occasionally breaking an end mill or gouging up a part. I sometimes slow a long profile cut down to 20 IMP for this reason. It is pretty rare though, I think I have broken 3 end mills in well over 100 hours of aluminum cutting.

It did the exact same thing to me regarding the last two passes. There is a slight tilt to my workstation in relation to the gantry that I am trying to work out. On half of my last cut it pulled all the way through cutting roughly twice the desired plunge depth and it made a bunch of large chips that would cause it to rattle a little. The 660 sounds like a jet taking off in my office, but I could still hear the grinding over that so I know that it was not good. I cant really think of a solution to that problem other than maybe using a down cut mill? I'm not sure how that would work out with aluminum, and I could only assume that it would cause all kinds of rubbing issues with a machine running 30000 rpm.

I agree, the 2 flute seemed to do a nice job. I just want to find a nice single flute and give that a shot because I think that the 660 has the torque to run a little faster through the aluminum and if you could up the chip size I bet that you could run through aluminum quite a bit easier and faster than the two flute. I don't know about you, but .15 mm passes take forever to finish a job. This one took me just over 5 hours of continuous run time. The plate was 1/2" so it had to make about 100 passes. Thanks for the info.
Shapeoko # 1458

RT0701C Spindle || dual y motor || x axis nema23 with custom carriage 1000mm length || z axis nema23 linear rail upgrade with 1/2-10 ACME

iowajames
Posts: 1
Joined: Mon May 06, 2013 1:53 pm

Re: Aluminum

Post by iowajames » Mon May 06, 2013 1:54 pm

Maybe try one of these?

http://www.toolstoday.com/p-5801-solid- ... -bits.aspx

Never used one myself, but it would probably work nicely for aluminum as it makes large chips.

Post Reply