Some of the alloys of aluminum have been machined successfully without any lubricant or cutting compound, but in order
to obtain the best results, some form of lubricant is desirable. For many purposes, 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
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 degree: 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 in order 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; however, it should not be allowed to progress too far before the tool is changed
A sulphurized mineral oil or 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 will generally produce a better finish on the machined surface than conventional 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. In some cases the use of
split-point drills is preferred. Carbide tipped twist drills can be used for drilling aluminum and its alloys which may
afford advantages in some production applications.
Ordinary hand and machine taps can be used to tap aluminum and its alloys although spiral-fluted thread taps give superior results.
Magnesium alloys are readily machined and with relatively low power consumption per cubic inch of metal removed.
The usual practice is to employ high cutting speeds with relatively coarse feeds and deep cuts. Exceptionally fine finishes
can be obtained so that grinding to improve the finish usually is unnecessary.
The horsepower normally required in machining magnesium varies from 0.15 to 0.30 per cubic inch per minute. While this value is low,
especially in comparison with power required for cast iron and steel, the total amount of power for machining magnesium usually
is high because of the exceptionally rapid rate at which metal is removed.
Carbide tools are recommended for maximum efficiency, although high-speed steel frequently is employed. Tools should be designed
so as to dispose of chips readily or without excessive friction, by employing polished chip-bearing surfaces, ample chip spaces,
large clearances, and small contact areas.
Feeds and Speeds for Magnesium: Speeds ordinarily range up to 5000 feet per minute for rough- and finish-turning, up to
3000 feet per minute for rough-milling, and up to 9000 feet per minute for finish-milling.
Lathe Tool Angles for Magnesium: The true or actual rake angle resulting from back and side rakes usually varies from
10 to 15 degrees. Back rake varies from 10 to 20, and side rake from 0 to 10 degrees. Reduced back rake may be employed to
obtain better chip breakage. The back rake may also be reduced to from 2 to 8 degrees on form tools or other broad tools to
Parting Tools: For parting tools, the back rake varies from 15 to 20 degrees, the front end relief 8 to 10 degrees,
the side relief measured perpendicular to the top face 8 degrees, and the side relief measured in the plane of the top face
from 3 to 5 degrees.
Milling Magnesium. In general, the coarse-tooth type of cutter is recommended. The number of teeth or cutting blades
may be one-third to one-half the number normally used; however, the two-blade fly-cutter has proved to be very satisfactory.
As a rule, the land relief or primary peripheral clearance is 10 degrees followed by secondary clearance of 20 degrees.
Drilling Magnesium. If the depth of a hole is less than five times the drill diameter, an ordinary twist drill with
highly polished flutes may be used. The drill should be kept sharp and the outer corners rounded to produce a smooth finish
and prevent burr formation. For deep hole drilling, use a drill having a helix angle of 40 to 45 degrees with large polished
flutes of uniform cross-section throughout the drill length to facilitate the flow of chips. Drilling speeds vary from 300
to 2000 feet per minute with feeds per revolution ranging from 0.015 to 0.050 inch.
Tapping Magnesium. Standard taps may be used unless Class 3B tolerances are required, in which case the tap should
be designed for use in magnesium. A high-speed steel concentric type with a ground thread is recommended. The concentric form,
which eliminates the radial thread relief, prevents jamming of chips while the tap is being backed out of the hole.
The positive rake angle at the front may vary from 10 to 25 degrees and the "heel rake angle" at the back of the tooth
from 3 to 5 degrees. The chamfer extends over two to three threads. For holes up to 1/4 inch in diameter, two-fluted
taps are recommended; for sizes from 1/2 to 3/4 inch, three flutes; and for larger holes, four flutes. Tapping speeds
ordinarily range from 75 to 200 feet per minute, and mineral oil cutting fluid should be used.
Threading Dies for Magnesium. Threading dies for use on magnesium should have about the same cutting angles as taps.
Narrow lands should be used to provide ample chip space. Either solid or self-opening dies may be used. The latter type is
recommended when maximum smoothness is required. Threads may be cut at speeds up to 1000 feet per minute.
Grinding Magnesium. As a general rule, magnesium is ground dry. The highly inflammable dust should be formed into
sludge by means of a spray of water or low viscosity mineral oil. Accumulations of dust or sludge should be avoided.
For surface grinding, when a fine finish is desirable, a low-viscosity mineral oil may be used.
Machining Zinc Alloy Die-Castings
Machining of zinc alloy die-castings is mostly done without a lubricant. For particular work, especially deep drilling and tapping,
a lubricant such as lard oil and kerosene or a 50-50 mixture of kerosene and machine oil may be used to advantage.
A mixture of turpentine and kerosene has been found effective on certain difficult jobs.
Reaming: In reaming, tools with six straight flutes are commonly used, although tools with eight flutes irregularly
spaced have been found to yield better results by one manufacturer. Many standard reamers have a land that is too wide for
best results. A land about 0.015 inch wide is recommended but this may often be ground down to around 0.007 or even 0.005
inch to obtain freer cutting, less tendency to loading, and reduced heating.
Turning: Tools of high-speed steel are commonly employed although the application of Stellite and carbide tools,
even on short runs, is feasible. For steel or Stellite, a positive top rake of from 0 to 20 degrees and an end clearance
of about 15 degrees is commonly recommended. For boring, facing, and other lathe operations, rake and clearance angles are
about the same as for tools used in turning.
Machining Monel and Nickel Alloys
These alloys are machined with high-speed steel and with cemented carbide cutting tools. High-speed steel lathe tools usually
have a back rake of 6 to 8 degrees, a side rake of 10 to 15 degrees, and relief angles of 8 to 12 degrees. Broad-nose finishing
tools have a back rake of 20 to 25 degrees and an end relief angle of 12 to 15 degrees. In most instances, standard commercial
cemented-carbide tool holders and tool shanks can be used which provide acceptable tool geometry. Honing the cutting edge
lightly will help if chipping is encountered.
The most satisfactory tool materials for machining Monel and the softer nickel alloys, such as Nickel 200 and Nickel 230,
are M2 and T5 for high-speed steel and crater resistant grades of cemented carbides. For the harder nickel alloys such as K Monel,
Permanickel, Duranickel, and Nitinol alloys, the recommended tool materials are T15, M41, M42,
M43, and for high-speed steel, M42. For carbides, a grade of crater resistant carbide is recommended
when the hardness is less than 300 Bhn, and when the hardness is more than 300 Bhn, a grade of straight tungsten carbide will
often work best, although some crater resistant grades will also work well.
A sulfurized oil or a water-soluble oil is recommended for rough and finish turning. A sulfurized oil is also recommended
for milling, threading, tapping, reaming, and broaching.
Nickel alloys have a high tendency to work harden. To minimize work hardening caused by machining, the cutting tools
should be provided with adequate relief angles and positive rake angles. Furthermore, the cutting edges should be kept
sharp and replaced when dull to prevent burnishing of the work surface. The depth of cut and feed should be sufficiently
large to ensure that the tool penetrates the work without rubbing.