There are many types of aluminum in two basic conditions. The conditions have more effect on the routing cuts than the types. The conditions are treated, which is hard, and untreated/annealed, which is soft. The hard material forms chips which can be routed much easier than the soft material. The condition is noted on all materials from the manufacturer i.e. 6061 T-6 or 2024 O. If this is missing from the raw material, a simple bend test will indicate the type. If the material bends like solder, it is probably soft. If the material is difficult to form a bend and tends to spring back, it is likely hard. The common types and the difference in hardness are noted in the chart. Note the hardness can be two to three times the soft condition as compared to the hard in most of the types shown. A good comparison of the two conditions is that they are similar to wood and plastics. Wood has the soft pliable – popular, cedar, pine, cottonwoods, versus the much harder rigid – oak, maple, hickory, teaks. Plastics are split into the soft flexible – ABS, PVC, polyethene, polypropylene, UMHW, versus the harder rigid – acrylic, nylon, Delrin. Traditionally, high-speed steel (HSS)tools in spiral flutes have been used in routing aluminum for over 60 years. This tool material was used because it can carry a very sharp edge and is very tough. Most applications were hand-fed or hand-controlled and the other materials such as solid carbide (SC) were too brittle to be used in these operations. The advent of more advanced CNC routers, which have very good control of the feed has created more uses for the more refined SC tools. The newer SC tools have sharper stronger edges and are more shock resistant than earlier SC types.
As a general rule of thumb, most aluminum applications are covered by the use of HSS spirals in hand and older CNC applications, SC spirals in more advanced CNC applications, single edge tools for “O” condition aluminum and double edge tools for “T” condition aluminum.
CNC routers are used for aluminum routing in four modes: single sheet, vacuum held, stack sheet-screw held, stack sheet-rivet held and stack sheet-pressure foot. In all operations, the conventional cut path is recommended. However, it is suggested that the scrap be examined. If it is cleaner than the part, then use climb cutting. If two passes are needed because of tool deflection, the higher requirement for the part finish, or it is faster, then leave at least .030” (1/32”) of material on the part for the finish cut. Use climb cut direction. Both of these items will stabilize the tool and should yield a better part finish. The single sheet applications run 14,000 to 24,000 RPM and up to 300 IPM feed. Stack sheets run 14,000 to 20,000 RPM and up to 160 IPM feed.
This operation has a composite wood table. The vacuum draws the part to the table and eliminates the use of fasteners to hold down the parts. Solid carbide tools are required due to the abrasiveness of the table. Skip tabs are
recommended for smaller parts because they tend to move after several parts are cut which opens up more area for vacuum loss. Since most parts are less than .125” thickness, 1/8” and 3/16” tools can be used to help minimize vacuum loss by cutting a smaller path. Use the shortest CEL
Stacked sheet screwed down
In order to make a solid mounting for the screws, most tables are plywood. This allows the use of HSS spiral up-cuts. Because the plies in the plywood are solid wood and not abrasive like the MDF or PB, the stack height should not exceed 1/2”. An up-cut it required because there is no exit path for the chips. Single edge tools mostly 1/4” to 5/16” on 1/2” shanks provide the most stable cuts and allow chips to be cut and cleared from the path. There will
be some tool deflection. A secondary pass can be used to eliminate the variance. If a second pass is used, it should be in a climb cut direction and a minimum of .030” left on the part for the final cut.
Coolants should be used on all CNC applications. The synthetic or soluble oil mists should be mixed at highwater/coolant ratios to provide a greater measure of cooling effect. Flood coolants run best in applications for stack routing where the cut paths are deep. In hand router applications, a brushed on oil or dipping the tool in bee’s wax or bar soap will add lubricity to the cutting action and extend tool life.
This can be caused by many different factors or a combination of them. Spindle run-out and the wrong tool type are the most common errors. Dull tools, poor chip loads, wrong feed direction, loss of coolant during the cut are other factors that contribute to chip welding on the cutting edge. Chips welding back into the cut path occurs when the chip load is too light or the flute of the tool cannot eject it. This can happen when the CEL is not long enough to clear the top of the deep cuts.
This is a common occurrence when there is excessive spindle run-out. It also happens when the feed rates are too slow on a CNC router and the chips are forced into the back of the tool because they cannot be ejected from the cut path.