Question
Does anyone here have experience routing aluminum? I have a job coming up that involves engraving, dados, bolt holes and cutting of 6061-T651 aluminum. Any information regarding feeds/speeds, bits, misting, or pitfalls to look out for would be greatly appreciated.
Forum Responses
(CNC Forum)
From contributor A:
Aluminum is a funny thing. I have had excellent results using the following tool sizes @ ipm @ rpm @ depth of cut/pass
.125 @ 12 to 16 @ 22750 @ .07 .1875 @ 28 to 37 @ 23900 @ .135 .25 @ 38 to 55 @ 23500 @ .1875 all were using a climb cut. These are only what have worked for me. You will need to make your tests and record each set of parameters in a notebook to fine tune yours. Pocket out smaller shapes to remove them. Tab shapes you think may leave the table abruptly, and use a multi pass so you can avoid having to hand shape the area where the tab was. As far as misting, it is a must from my experiences. What I would do is adjust my mist during the cut in accordance to the feed speed so I would attain a decent mist of lube directed at the cutter and material contact point, aimed to the right and left the general linear motion. Use one tip to shoot from the back of the tool so the cutter carries the lube with it thru the cut, and use the other if you have a multi jet mister to cool the chips upon extraction. Depth of cut is also an extremely relevant item to your feed and speed. You may break a few tools in the learning process. There are calculations to help you vector in on a starting point for feed and speed. You may want to research how to calculate chip load.
One last thing - do not forget to hold down your parts. I recommend double sided tape. If it is possible, select your cutting order to begin at the furthest point from your vacuum pump and work your way back towards it, selecting the inside shapes, then the outside shapes (i.e. inside of a diamond shaped frame then the outer cut). This will allow you to use the rigidity of the rest of your sheet to aid in stability and minimize the possibility of parts loss. I have seen a 3 x 5 x.125 aluminum part leave the table powered by 24k spindle speed - not a recommended experience.
Machining Aluminum - Some of the alloys of aluminum have been machined successfully without any lubricant or cutting compound, but some form of lubricant is desirable to obtain the best results. For many purposes, a soluble cutting oil is good.
Tools for aluminum and aluminum alloys should have larger relief and rake angles than tools for cutting steel. For high-speed steel turning tools the following angles are recommended: relief angles, 14 to 16 degrees; back rake angle, 5 to 20 degrees; side rake angle, 15 to 35 degrees. For very soft alloys even larger side rake angles are sometimes used. High silicon aluminum alloys and some others have a very abrasive effect on the cutting tool. While these alloys can be cut successfully with high-speed-steel tools, cemented carbides are recommended because of their superior abrasion resistance. The tool angles recommended for cemented carbide turning tools are: relief angles, 12 to 14 degrees; back rake angle, 0 to 15 degrees; side rake angle, 8 to 30 degrees.
Cut-off tools and necking tools for machining aluminum and its alloys should have from 12 to 20 degrees back rake angle and the end relief angle should be from 8 to 12 degrees. Excellent threads can be cut with single-point tools in even the softest aluminum. Experience seems to vary somewhat regarding the rake angle for single-point thread cutting tools. Some prefer to use a rather large back and side rake angle although this requires a modification in the included angle of the tool to produce the correct thread contour. When both rake angles are zero, the included angle of the tool is ground equal to the included angle of the thread. Excellent threads have been cut in aluminum with zero rake angle thread-cutting tools using large relief angles, which are 16 to 18 degrees opposite the front side of the thread and 12 to 14 degrees opposite the back side of the thread. In either case, the cutting edges should be ground and honed to a keen edge. It is sometimes advisable to give the face of the tool a few strokes with a hone between cuts when chasing the thread to remove any built-up edge on the cutting edge.
Fine surface finishes are often difficult to obtain on aluminum and aluminum alloys, particularly the softer metals. When a fine finish is required, the cutting tool should be honed to a keen edge and the surfaces of the face and the flank will also benefit by being honed smooth. Tool wear is inevitable, but it should not be allowed to progress too far before the tool is changed or sharpened. A sulphurized mineral oil or a heavy-duty soluble oil will sometimes be helpful in obtaining a satisfactory surface finish. For best results, however, a diamond cutting tool is recommended. Excellent surface finishes can be obtained on even the softest aluminum and aluminum alloys with these tools.
Although ordinary milling cutters can be used successfully in shops where aluminum parts are only machined occasionally, the best results are obtained with coarse-tooth, large helix-angle cutters having large rake and clearance angles. Clearance angles up to 10 to 12 degrees are recommended. When slab milling and end milling a profile, using the peripheral teeth on the end mill, climb milling (also called down milling) will generally produce a better finish on the machined surface than conventional (or up) milling. Face milling cutters should have a large axial rake angle. Standard twist drills can be used without difficulty in drilling aluminum and aluminum alloys although high helix-angle drills are preferred. The wide flutes and high helix-angle in these drills helps to clear the chips. Sometimes split-point drills are preferred. Carbide tipped twist drills can be used for drilling aluminum and its alloys and may afford advantages in some production applications. Ordinary hand and machine taps can be used to tap aluminum and its alloys although spiral-fluted ground thread taps give superior results. Experience has shown that such taps should have a right-hand ground flute when intended to cut right-hand threads and the helix angle should be similar to that used in an ordinary twist drill.
Sorry for the length of the post but sometimes it is worth it to revisit the basics. It has been my experience that 6061 is considerably more machinable than the 2000 series. Brand of cutter is not as important as support from the tooling manufacturer. The guidelines used from the Machinists Handbook provide a good description of how the tool should differ from other tools. I hope this helps!
