In this video, we are showing 2 examples of cutting aluminum. The first example will be dry cutting which is cutting in the absence of a coolant or cutting fluid.

Video: greenBull CNC machine cutting aluminum

The first process in this example is drilling straight holes also called plunging. Typically, end mills are not the best tools to use for plunging unless the geometry of the end mill provides for this machining operation. The method I elected to use is pecking since the aluminum chips can be ejected more easily. If pecking were not used, the end mill would produce too much heat and the chips would melt in the cavity of the hole, potentially causing the end mill to freeze in the hole and break.

The next machining operation is profile cutting, or cutting in a horizontal fashion along a path.

Cutting without a fluid requires a machining method that ensures the proper temperature of the cutting tool (an end mill) and the proper temperature of the material at the cutting position. Aspects of machining that must be considered for dry cutting is the feedrate, spindle RPM, and depth of each cutting pass. The feedrate and RPM are intrinsically related. Feedrate is the velocity at which the end mill moves across the material and the RPM is how fast the tool is spinning. If the RPM is high, the feedrate must also match so that the tool will not cause too much heat. The depth of cut per pass is determined by the load against the tool during the cutting process. The depth per pass is generally determined by the manufacturer’s suggestion and the ability of the machine’s motors to provide the torque to overcome the load against the tool.

If these considerations are not carefully determined, undesirable results may occur, such as: increased tool wear, aluminum melting causing the tool to become clogged with aluminum chips and the edges of the aluminum showing a melted, gumming appearance.

The specifications I used for this dry cutting process is: 100 IPM (inches per minute) for the feedrate, 18,000 RPM for the spindle and a depth per pass of .05 inches (just shy of a 16th of an inch) (about 1.27 mm).

The end mill in use is a 65-026 which is a ¼” cutting diameter with a single flute that is recommended for wood, plastics and aluminum.

The 100 IPM feedrate was derived from the chipload formula of feedrate in inches per minute equals the spindle RPM multiplied by the number of flutes and then multiplied by the chip load. The chip load for cutting aluminum with this tool is a range from .003 to .006. That range gives a result of 54 to 108 ipm.

The resulting chip from the cutting process should be scrutinized to determine If the feedrate and RPM were within an acceptable range. The chips should be the size of the depth per pass by the length of the cavity of the flute and by the chipload thickness that was shown in the formula. The thickness of these chips are .0135 which is a bit thick as per the chip size recommendation. Even though the edge finish is acceptable for my purposes, a slower feedrate may create a better edge finish.

The hold down for the aluminum extruded sheet is important. Chatter and vibration should be avoided as much as possible. In this example, we used screws to hold down the aluminum into our spoilboard. To keep the part being cut out stable, holding tabs were used. Holding tabs are a bridge between the part being cut out and the surrounding aluminum. After the machining is complete, the part is removed using a multitool to cut through the holding tab. A grinder or file is used to remove the remnants of the holding tab on the edge of the part.

The next example cutting aluminum introduces a wet technique which uses a cutting fluid. The cutting fluid will remove much of the heat to decrease the tool wear. Since heat is the major cause of tool wear and failure, the cutting fluid helps maintain a tolerable temperature.

In our experience, the cutting fluid does not show a difference in the resulting finish along the edge of the part. However, the cutting fluid may improve the edge finish at slower feedrates with the same RPM to achieve more cutting action along a shorter length where dry cutting would melt the aluminum with this slower feedrate.

As shown, the cutting fluid is sprayed onto the aluminum surface using a bottle with extreme care. The smoke seen during the cutting process is the burning of the cutting fluid which shows how hot the cutting process with aluminum can be.

For both the dry and wet example, we use the climb cutting direction which provides the best edge finish as opposed to conventional cutting direction. The climb cutting direction takes into consideration the spindle rotation direction or the direction the tool is spinning. Using this method, the finished edge of the actual part will exhibit the end mill essentially spinning along this edge like the tires of a car spinning out on pavement. Conversely, conventional cutting direction is like a car spinning out in reverse, but being pulled by another car in the opposite direction.

Both the wet and dry cutting examples exhibited the same chip size. This demonstrates that feeds and speeds coupled with the RPM determine the chip size and cutting wet is a method of cooling the end mill during the cutting process.

Both wet and dry cutting examples also exhibited the same edge finish and appearance.

In this video we’re cutting an aluminum ring from a solid block of 6061 aluminum. The client gave us specifications that the ring needs to be 1 and a half inches in length, about 4 inches for the outside diameter, and about 1/4 inch for the wall thickness.

Video: Cutting Aluminum With a Cheap End Mill

This job could have easily been done using an aluminum extruded round tube stock by cutting the stock at a specified length then refining the stock in a lathe, but the customer was under a time crunch so we offered our services to make an attempt to mill a ring out of a solid block.

The CAMing of the part is pretty simple. We create the geometry to provide machining operations for the machine. The ring is composed of just two circles: one for the outside and inside diameter. I also wanted to create the geometry for the block so that we can find the correct origin on the aluminum block so the ring would be milled generally in the center of the block. The thickness of the ring is determined by the stock thickness, then a machining operation is applied to the circles, the outside is an outside profile so the end mill will mill along the outside of the line creating an outer wall. The inside will mill along the inside of the line creating an inner wall.

During the creation of the milling operations, I didn’t take care to adjust the depth per pass. I left the depth per pass at the default values that I use for plexiglass that is a bit deeper than a quarter inch. The value I should have started with is .1 inches, that is if I was using an Onsrud end mill, rather than a general purpose (cheap) end mill.

This is a general purpose end mill so I’m never quite sure what to expect. I always provide a roughing and finishing pass to correct any issues that may be caused by load on the bit while machining. Finally, I created the holding tabs so the ring would be in place during all of the machining operations.

We’ve cut aluminum before, but using a quarter inch end mill, cutting into a quarter inch aluminum stock, our quarter inch end mills have a 1 1/8” flute length, not quite enough to penetrate the entire stock. Quite a bit of shank from the end mill would have rubbed along the top of the aluminum causing a great amount of heat, so we couldn’t use it. We had to use the ½” end mill which has a 2 inch flute length.

Heat is the main attribute of machining that you want to eliminate, especially with aluminum since it has a low melting point. When you start machining aluminum, the bit can get too hot and start melting the chips. When the aluminum starts melting, the chips can get sticky and fuse into the flutes of the end mill, rendering it useless and it will eventually get stuck.

In this attempt I reduced the depth per pass to .1 inches instead of the default that I was using before. I’m using .1 inches because our quarter inch end mills can use this in .05 and now we’re using a half inch end mill so I’m doubling depth per pass. I should be able to go even deeper with a better end mill, but we’re using a cheap end mill.

I kept the feed rate as fast as possible. I want to maintain the feed rate because I want to make sure the end mill is always digging into cooler material, so the material always acts as sort of a coolant. The faster you go around the material, the cooler the material will be. This seems counterintuitive but this is actually the way dry cutting is done. You go through the material faster. You might do a shallower depth per pass. Even though we do maintain the speed, it seemed like the end mill was still getting very hot.

I really should have selected a higher quality end mill. One that exhibits the flute geometry specifically appropriate for cutting aluminum. In this third attempt, the end mill was still having a hard time during some deep passes and I believe this is attributed to the heat build-up. The chips were fusing into the flutes of the end mill.

Another condition that we saw that could be building up heat is that the end mill was actually stopping at another portion of the circle, and it was stopping at multiple points. This is a condition called a lead-in. The lead-in was at a 10 degree angle, so when you reduce the depth per pass, the lead angle is shorted. So we reduced the angle to about 1 degree so it will have a longer lead in so when it comes around it will start to lead in and then continue on to reduce some heat as well.

In our last attempt, which wasn’t entirely successful, we were able to cut out the entire ring, but we had to go to a .025 which is an incredibly small depth per pass. Our quarter inch end mill can surpass this, but again this was because we weren’t using a higher quality end mill. We added cutting fluid so we could get less heat. One of the problems was the machine was starting to vibrate, so we ended that process without doing the finishing passes, so our wall thickness was not consistent with what the customer needed.

I would like to attempt cutting aluminum again with a better end mill. We’re going to get a single flute, half inch Onsrud bit and we will demonstrate cutting an aluminum block with the same dimensions.