MATERIAL REMOVAL PROCESSES AND MACHINE TOOLS
Material removal processes, which include machining, cutting, grinding,
and various nonmechanical chipless processes, are desirable or
even necessary for the following basic reasons: (1) Closer dimensional
tolerances, surface roughness, or surface-finish characteristics may be
required than are available by casting, forming, powder metallurgy, and
other shaping processes; and (2) part geometries may be too complex or
too expensive to be manufactured by other processes. However, material
removal processes inevitably waste material in the form of chips,
production rates may be low, and unless carried out properly, the processes
can have detrimental effects on the surface properties and performance
of parts.
Traditional material removal processes consist of turning, boring, drilling, reaming, threading, milling, shaping, planing, and broaching,
as well as abrasive processes such as grinding, ultrasonic machining,
lapping, and honing. Nontraditional processes include electrical and
chemical means of material removal, as well as the use of abrasive jets,
water jets, laser beams, and electron beams. This section describes the
principles of these operations, the processing parameters involved, and
the characteristics of the machine tools employed.
BASIC MECHANICS OF METAL CUTTING
The basic mechanics of chip-type machining processes (Fig. 13.4.1) are
shown, in simplest two-dimensional form, in Fig. 13.4.2. A tool with a
certain rake angle a (positive as shown) and relief angle moves along the
surface of the workpiece at a depth t1 . The material ahead of the tool is
sheared continuously along the shear plane, which makes an angle of f
Fig. 13.4.1 Examples of chip-type machining operations.
with the surface of the workpiece. This angle is called the shear angle
and, together with the rake angle, determines the chip thickness t2 . The
ratio of t1 to t2 is called the cutting ratio r. The relationship between the
shear angle, the rake angle, and the cutting ratio is given by the equation
tan f 5 r cos a/(1 2 r sin a). It can readily be seen that the shear angle
is important in that it controls the thickness of the chip. This, in turn, has
great influence on cutting performance. The shear strain that the material
undergoes is given by the equation g 5 cot f 1 tan (f 2a). Shear
strains in metal cutting are usually less than 5.
Fig. 13.4.2 Basic mechanics of metal cutting process.
Investigations have shown that the shear plane may be neither a plane
nor a narrow zone, as assumed in simple analysis. Various formulas
have been developed which define the shear angle in terms of such
factors as the rake angle and the friction angle b. (See Fig. 13.4.3.)
Because of the large shear strains that the chip undergoes, it becomes
hard and brittle. In most cases, the chip curls away from the tool.
Among possible factors contributing to chip curl are nonuniform normal
stress distribution on the shear plane, strain hardening, and thermal
effects.
Regardless of the type of machining operation, some basic types of
chips or combinations of these are found in practice (Fig. 13.4.4):
Continuous chips are formed by continuous deformation of the workpiece
material ahead of the tool, followed by smooth flow of the chip
along the tool face. These chips ordinarily are obtained in cutting ductile
materials at high speeds.
Discontinuous chips consist of segments which are produced by fracture
of the metal ahead of the tool. The segments may be either loosely
Fig. 13.4.3 Force system in metal cutting process.
connected to each other or unconnected. Such chips are most often
found in the machining of brittle materials or in cutting ductile materials
at very low speeds or low or negative rake angles.
Inhomogeneous (serrated) chips consist of regions of large and small
strain. Such chips are characteristic of metals with low thermal conductivity
or metals whose yield strength decreases sharply with temperature.
Chips from titanium alloys frequently are of this type.
Built-up edge chips consist of a mass of metal which adheres to the tool
face while the chip itself flows continuously along the face. This type of
chip is often encountered in machining operations at low speeds and is
associated with high adhesion between chip and tool and causes poor
surface finish.
The forces acting on the cutting tool are shown in Fig. 13.4.3. The
resultant force R has two components, Fc and Ft . The cutting force Fc in
the direction of tool travel determines the amount of work done in
cutting. The thrust force Ft does no work but, together with Fc , produces
deflections of the tool. The resultant force also has two components on
the shear plane: Fs is the force required to shear the metal along the
shear plane, and Fn is the normal force on this plane. Two other force
components also exist on the face of the tool: the friction force F and the
normal force N.
Whereas the cutting force Fc is always in the direction shown in Fig.
13.4.3, the thrust force Ft may be in the opposite direction to that shown
in the figure. This occurs when both the rake angle and the depth of cut
are large, and friction is low.
From the geometry of Fig. 13.4.3, the following relationships can be
derived: The coefficient of friction at the tool-chip interface is given by
m 5 (Ft 1 Fc tan a) / (Fc 2 Ft tan a). The friction force along the tool is
F 5 Ft cos a 1 Fc sin a. The shear stress in the shear plane is
t 5 (Fc sin f cos f 2 Ft sin2 f) / A0 , where A0 is the cross-sectional
area that is being cut from the workpiece.
The coefficient of friction on the tool face is a complex but important
factor in cutting performance; it can be reduced by such means as the
use of an effective cutting fluid, higher cutting speed, improved tool
material and condition, or chemical additives in the workpiece material The net power consumed at the tool is P 5 FcV. Since Fc is a function
of tool geometry, workpiece material, and process variables, it is difficult
reliably to calculate its value in a particular machining operation.
Depending on workpiece material and the condition of the tool, unit
power requirements in machining range between 0.2 hp? min/in3 (0.55
W?s/mm3) of metal removal for aluminum and magnesium alloys, to
3.5 for high-strength alloys. The power consumed is the product of unit
power and rate of metal removal: P 5 (unit power)(vol/min).
The power consumed in cutting is transformed mostly to heat. Most
of the heat is carried away by the chip, and the remainder is divided
between the tool and the workpiece. An increase in cutting speed or feed
will increase the proportion of the heat transferred to the chip. It has
been observed that, in turning, the average interface temperature between
the tool and the chip increases with cutting speed and feed, while
the influence of the depth of cut on temperature has been found to be
limited. Interface temperatures to the range of 1,500 to 2,000°F (800 to
1,100°C) have been measured in metal cutting. Generally the use of a
cutting fluid removes heat and thus avoids temperature buildup on the
cutting edge.
In cutting metal at high speeds, the chips may become very hot and
cause safety hazards because of long spirals which whirl around and
become entangled with the tooling. In such cases, chip breakers are
introduced on the tool geometry, which curl the chips and cause them to
break into short sections. Chip breakers can be produced on the face of
the cutting tool or insert, or are separate pieces clamped on top of the
tool or insert.
A factor of great significance in metal cutting is tool wear. Many
factors determine the type and rate at which wear occurs on the tool. The
major critical variables that affect wear are tool temperature, type and
hardness of tool material, grade and condition of workpiece, abrasiveness
of the microconstituents in the workpiece material, tool geometry,
feed speed, and cutting fluid. The type of wear pattern that develops
depends on the relative role of these variables.
Tool wear can be classified as (1) flank wear (Fig. 13.4.5); (2) crater
wear on the tool face; (3) localized wear, such as the rounding of the
cutting edge; (4) chipping or thermal softening and plastic flow of the
cutting edge; (5) concentrated wear resulting in a deep groove at
the edge of a turning tool, known as wear notch.
In general, the wear on the flank or relief side of the tool is the most
dependable guide for tool life. A wear land of 0.060 in (1.5 mm) on
high-speed steel tools and 0.015 or 0.030 in (0.4 or 0.8 mm) for carbide
tools is usually used as the endpoint. The cutting speed is the variable
which has the greatest influence on tool life. The relationship between
tool life and cutting speed is given by the Taylor equation VTn 5 C,
where V is the cutting speed; T is the actual
cutting time to develop a certain wear land,
min; C is a constant whose value depends on
workpiece material and process variables, numerically
equal to the cutting speed that gives
a tool life of 1 min; and n is the exponent
whose value depends on workpiece material
and other process variables. The recommended
cutting speed for a high-speed steel
tool is generally the one which produces a 60-
to 120-min tool life. With carbide tools, a 30-
to 60-min tool life may be satisfactory. Values
of n range from 0.08 to 0.2 for high-speed
steels, from 0.2 to 0.5 for carbides, and from
0.5 to 0.7 for ceramic tools.
Fig. 13.4.5 Types of
tool wear in cutting.
When one is using tool-life equations, caution should be exercised in
extrapolation of the curves beyond the operating region for which they
are derived. In a log-log plot, tool life curves may be linear over a short
cutting-speed range but are rarely linear over a wide range of cutting
speeds. In spite of the considerable data obtained to date, no simple
formulas can be given for quantitative relationships between tool life
and various process variables for a wide range of materials and conditions.
An important aspect of machining on computer-controlled equipment
is tool-condition monitoring while the machine is in operation with little
or no supervision by an operator. Most state-of-the-art machine controls
are now equipped with tool-condition monitoring systems. Two common
techniques involve the use of (1) transducers that are installed on
the tool holder and continually monitor torque and forces and (2) acoustic
emission through a piezoelectric transducer. In both methods the
signals are analyzed and interpreted automatically for tool wear or chipping,
and corrective actions are taken before any significant damage is
done to the workpiece.
A term commonly used in machining and comprising most of the
items discussed above is machinability. This is best defined in terms of
(1) tool life, (2) power requirement, and (3) surface integrity. Thus, a
good machinability rating would indicate a combination of long tool
life, low power requirement, and a good surface. However, it is difficult
to develop quantitative relationships between these variables. Tool life
is considered as the important factor and, in production, is usually ex- from 1.25 to 20 percent. Vanadium increases hot hardness and abrasion
resistance; in high-speed steels, it ranges from 1 to 5 percent.
High-speed steels are the most highly alloyed group among tool steels
and maintain their hardness, strength, and cutting edge. With suitable
procedures and equipment, they can be fully hardened with little danger
of distortion or cracking. High-speed steel tools are widely used in
operations using form tools, drilling, reaming, end-milling, broaching,
tapping, and tooling for screw machines.
Diamond, cubic boron nitride
Strength and toughness
Aluminum oxide (HIP)
Aluminum oxide 1 30%
titanium carbide
Silicon nitride
Cermets
Coated carbides
Carbides
HSS
Hot hardness and wear resistance
Fig. 13.4.7 Ranges of properties of various groups of tool materials.
Cast alloys maintain high hardness at high temperatures and have
good wear resistance. Cast-alloy tools, which are cast and ground into
any desired shape, are composed of cobalt (38 to 53 percent), chromium
(30 to 33 percent), and tungsten (10 to 20 percent). These alloys are
recommended for deep roughing operations at relatively high speeds
and feeds. Cutting fluids are not necessary and are usually used only to
obtain a special surface finish.
Carbides have metal carbides as key ingredients and are manufactured
by powder-metallurgy techniques. They have the following properties
which make them very effective cutting-tool materials: (1) high
hardness over a wide range of temperatures; (2) high elastic modulus, 2
to 3 times that of steel; (3) no plastic flow even at very high stresses; (4)
low thermal expansion; and (5) high thermal conductivity. Carbides are
used in the form of inserts or tips which are clamped or brazed to a steel
shank. Because of the difference in coefficients of expansion, brazing
should be done carefully. The mechanically fastened tool tips are called
inserts (Fig. 13.4.8); they are available in different shapes, such as
square, triangular, circular, and various special shapes.
There are three general groups of carbides in use: (1) tungsten carbide
with cobalt as a binder, used in machining cast irons and nonferrous
abrasive metals; (2) tungsten carbide with cobalt as a binder, plus a solid
solution of WC-TiC-TaC-NbC, for use in machining steels; and
Seat
Clamp Shank
screw
Clamp
Insert
Fig. 13.4.8 Insert clamped to shank of a toolholder.
(3) titanium carbide with nickel and molybdenum as a binder, for use
where cutting temperatures are high because of high cutting speeds or
the high strength of the workpiece material. Carbides are classified by
ISO and ANSI, as shown in Table 13.4.2 which includes recommendations
for a variety of workpiece materials and cutting conditions. (See
also Sec. 6.4.)
Coated carbides consist of conventional carbide inserts that are coated
with a thin layer of titanium nitride, titanium carbide, or aluminum
oxide. The coating provides additional wear resistance while maintaining
the strength and toughness of the carbide tool. Coatings are also
applied to high-speed steel tools, particularly drills and taps. The desirable
properties of individual coatings can be combined and optimized by using multiphase coatings. Carbide tools are now available with, e.g.,
a layer of titanium carbide over the carbide substrate, followed by aluminum
oxide and then titanium nitride. Various alternating layers of
coatings are also used, each layer being on the order of 80 to 400 min (2
to 10 mm) thick. New developments in coatings include diamond, titanium
carbonitride, chromium carbide, zirconium nitride, and hafnium
nitride.
Stiffness is of great importance when using carbide tools. Light feeds,
low speeds, and chatter are deleterious. No cutting fluid is needed, but if
one is used for cooling, it should be applied in large quantities and
continuously to prevent heating and quenching.
Ceramic, or oxide, inserts consist primarily of fine aluminum oxide
grains which have been bonded together. Minor additions of other elements
help to obtain optimum properties. Ceramic tools have very high
abrasion resistance, are harder than carbides, and have less tendency to
weld to metals during cutting. However, they lack impact toughness,
and premature tool failure can result by chipping or general breakage.
Ceramic tools have been found to be effective for high-speed, uninterrupted
turning operations. Tool and setup geometry is important.
Tool failures can be reduced by the use of rigid tool mountings and rigid
machine tools. Included in oxide, cutting-tool materials are cermets
(such as 70 percent aluminum oxide and 30 percent titanium carbide),
combining the advantages of ceramics and metals.
Polycrystalline diamond is used where good surface finish and dimensional
accuracy are desired, particularly on soft nonferrous materials
that are difficult to machine. The general properties of diamonds are
extreme hardness, low thermal expansion, high heat conductivity, and a
very low coefficient of friction. The polycrystalline diamond is bonded
to a carbide substrate. Single-crystal diamond is also used as a cutting
tool to produce extremely fine surface finish on nonferrous alloys, such
as copper-base mirrors.
Next to diamond, cubic boron nitride (CBN) is the hardest material
presently available. Polycrystalline CBN is bonded to a carbide substrate
and used as a cutting tool. The CBN layer provides very high wear
resistance and edge strength. It is chemically inert to iron and nickel at
elevated temperatures; thus it is particularly suitable for machining
high-temperature alloys and various ferrous alloys. Both diamond and
CBN are also used as abrasives in grinding operations.
CUTTING FLUIDS
Cutting fluids, frequently referred to as lubricants or coolants, comprise
those liquids and gases which are applied to the cutting zone in order to
facilitate the cutting operation. A cutting fluid is used (1) to keep the
tool cool and prevent it from being heated to a temperature at which the
hardness and resistance to abrasion are reduced; (2) to keep the workpiece
cool, thus preventing it from being machined in a warped shape to
inaccurate final dimensions; (3) through lubrication to reduce the power
consumption, wear on the tool, and generation of heat; (4) to provide a
good finish on the workpiece; (5) to aid in providing a satisfactory chip
formation; (6) to wash away the chips (this is particularly desirable in
deep-hole drilling, hacksawing, milling, and grinding); and (7) to prevent
corrosion of the workpiece and machine tool.
Classification Cutting fluids may be classified as follows: (1) air
blast, (2) emulsions, (3) oils, and (4) solutions. Cutting fluids are also
classified as light-, medium-, and heavy-duty; light-duty fluids are for
general-purpose machining.
Induced air blast may be used with internal and surface grinding and
polishing operations. Its main purpose is to remove the small chips or
dust, although some cooling is also obtained, especially in machining of
plastics.
Emulsions consist of a soluble oil emulsified with water in the ratio of
1 part oil to 10 to 100 parts water, depending upon the type of product
and the operation. Emulsions have surface-active or extreme-pressure
additives to reduce friction and provide an effective lubricant film under
high pressure at the tool-chip interface during machining. Emulsions are
low-cost cutting fluids and are used for practically all types of cutting
and grinding when machining all types of metals. The more concentrated
mixtures of oil and water, such as 1 : 10, are used for broaching,
threading, and gear cutting. For most operations, a solution of 1 part
soluble oil to 20 parts water is satisfactory.
A variety of oils are used for metal cutting. They are used where
lubrication rather than cooling is essential or on high-grade finishing
cuts, although sometimes superior finishes are obtained with emulsions.
Oils generally used in machining are mineral oils with the following
compositions: (1) straight mineral oil, (2) with fat, (3) with fat and
sulfur, (4) with fat and chlorine, and (5) with fat, sulfur, and chlorine.
The more severe the machining operation, the higher the composition of
the oil. Broaching and tapping of refractory alloys and high-temperature
alloys, for instance, require highly compounded oils. In order to avoid
staining of the metal, aluminum and copper, for example, inhibited
sulfur and chlorine are used.
Solutions are a family of cutting fluids that blend water and various
chemical agents such as amines, nitrites, nitrates, phosphates, chlorine,
and sulfur compounds. These agents are added for purposes of rust
prevention, water softening, lubrication, and reduction of surface tension.
Most of these chemical fluids are coolants but some are lubricants.
The selection of a cutting fluid for a particular operation requires
consideration of several factors: the workpiece material, the difficulty
of the machining operation, the compatibility of the fluid with the
workpiece material and the machine tool components, surface preparation,
method of application and removal of the fluid, contamination of
the cutting fluid with machine lubricants, and the treatment of the fluid
after use. Also important are the biological and ecological aspects of the
cutting fluid used. There may be potential health hazards to operating
personnel from contact with or inhalation of mist or fumes from some
fluids. Recycling and waste disposal are also important problems to be
considered.
Methods of Application The most common method is flood cooling
in quantities such as 3 to 5 gal/min (about 10 to 20 L/min) for singlepoint
tools and up to 60 gal/min (230 L/min) per cutter for multipletooth
cutters. Whenever possible, multiple nozzles should be used. In
mist cooling a small jet equipment is used to disperse water-base fluids as
very fine droplets in a carrier that is generally air at pressures 10 to 80
lb/in2 (70 to 550 kPa). Mist cooling has a number of advantages, such as
providing high-velocity fluids to the working areas, better visibility, and
improving tool life in certain instances. The disadvantages are that
venting is required and also the cooling capability is rather limited.
MACHINE TOOLS
The general types of machine tools are lathes; turret lathes; screw, boring,
drilling, reaming, threading, milling, and gear-cutting machines;
planers and shapers; broaching, cutting-off, grinding, and polishing machines.
Each of these is subdivided into many types and sizes. General
items common to all machine tools are discussed first, and individual
machining processes and equipment are treated later in this section.
Automation is the application of special equipment to control and
perform manufacturing processes with little or no manual effort. It is
applied to the manufacturing of all types of goods and processes, from
the raw material to the finished product. Automation involves many
activities, such as handling, processing, assembly, inspecting, and packaging.
Its primary objective is to lower manufacturing cost through
controlled production and quality, lower labor cost, reduced damage to
work by handling, higher degree of safety for personnel, and economy
of floor space. Automation may be partial, such as gaging in cylindrical
grinding, or it may be complete.
The conditions which play a role in decisions concerning automation
are rising production costs, high percentage of rejects, lagging output,
scarcity of skilled labor, hazardous working conditions, and work requiring
repetitive operation. Factors which must be carefully studied
before deciding on automation are high initial cost of equipment, maintenance
problems, and type of product (See also Sec. 16.)
Mass production with modern machine tools has been achieved
through the development of self-contained power-head production and the development of transfer mechanisms. Power-head units, consisting
of a frame, electric driving motor, gearbox, tool spindles, etc.,
are available for many types of machining operations. Transfer mechanisms
move the workpieces from station to station by various methods.
Transfer-type machines can be arranged in several configurations, such
as a straight line or a U pattern. Various types of machine tools for mass
production can be built from components; this is known as the buildingblock
principle. Such a system combines flexibility and adaptability
with high productivity. (See machining centers.)
Numerical control (NC), which is a method of controlling the motions
of machine components by numbers, was first applied to machine tools
in the 1950s. Numerically controlled machine tools are classified according
to the type of cutting operation. For instance, in drilling and
boring machines, the positioning and the cutting take place sequentially
(point to point), whereas in die-sinking machines, positioning and cutting
take place simultaneously. The latter are often described as continuous-
path machines, and since they require more exacting specifications,
they give rise to more complex problems. Machines now perform over a
very wide range of cutting conditions without requiring adjustment to
eliminate chatter, and to improve accuracy. Complex contours can be
machined which would be almost impossible by any other method. A
large variety of programming systems has been developed.
The control system in NC machines has been converted to computer
control with various software. In computer numerical control (CNC), a
microcomputer is a part of the control panel of the machine tool. The
advantages of computer numerical control are ease of operation, simpler
programming, greater accuracy, versatility, and lower maintenance
costs.
Although numerical control of machine tools has many advantages
such as high productivity and flexibility, it has certain limitations.
Among these are high initial cost of equipment and the need for trained
personnel and special maintenance.
Further developments in machine tools are machining centers. This is
a machine equipped with as many as 200 tools and with an automatic
tool changer (Fig. 13.4.9). It is designed to perform various operations
on different surfaces of the workpiece, which is placed on a pallet
capable of as much as five-axis movement (three linear and two rotational).
Machining centers, which may be vertical or horizontal spindle,
have flexibility and versatility that other machine tools do not have, and
thus they have become the first choice in machine selection in modern
manufacturing plants and shops. They have the capability of tool and
part checking, tool-condition monitoring, in-process and postprocess
gaging, and inspection of machined surfaces. Universal machining
centers are the latest development, and they have both vertical and hori-
Traveling column
Tool storage
Tools
(cutters)
Tool
interchange
arm
Bed
Saddle
Pallet or
module
Spindle
Spindle carrier
Fig. 13.4.9 Schematic of a horizontal spindle machining center, equipped with
an automatic tool changer. Tool magazines can store 200 different cutting tools.
(Source: Courtesy of Cincinnati Milacron, Inc.)
zontal spindles. Turning centers are a further development of computercontrolled
lathes and have great flexibility. Many centers are now constructed
on a modular basis, so that various accessories and peripheral
equipment can be installed and modified depending on the type of product
to be machined.
An approach to optimize machining operations is adaptive control.
While the material is being machined, the system senses operating conditions
such as forces, tool-tip temperature, rate of tool wear, and surface
finish, and converts these data into feed and speed control that
enables the machine to cut under optimum conditions for maximum
productivity. Combined with numerical controls and computers, adaptive
controls are expected to result in increased efficiency of metalworking
operations.
With the advent of sophisticated computers and various software,
modern manufacturing has evolved into computer-integrated manufacturing
(CIM). This system involves the coordinated participation of
computers in all phases of manufacturing. Computer-aided design combined
with computer-aided manufacturing (CAD/CAM), results in a much
higher productivity, better accuracy and efficiency, and reduction in
design effort and prototype development. CIM also involves the management
of the factory, inventory, and labor, and it integrates all these
activities, eventually leading to untended factories.
The highest level of sophistication is reached with a flexible manufacturing
system (FMS). Such a system is made of manufacturing cells and an
automatic materials-handling system interfaced with a central computer.
The manufacturing cell is a system in which CNC machines are
used to make a specific part or parts with similar shape. The workstations,
i.e., several machine tools, are placed around an industrial robot
which automatically loads, unloads, and transfers the parts. FMS has the
capability to optimize each step of the total manufacturing operation,
resulting in the highest possible level of efficiency and productivity.
The proper design of machine-tool structures requires analysis of such
factors as form and materials of structures, stresses, weight, and manufacturing
and performance considerations. The best approach to obtain
the ultimate in machine-tool accuracy is to employ both improvements
in structural stiffness and compensation of deflections by use of special
controls. The C-frame structure has been used extensively in the past
because it provides ready accessibility to the working area of the machine.
With the advent of computer control, the box-type frame with its
considerably improved static stiffness becomes practical since the need
for manual access to the working area is greatly reduced. The use of a
box-type structure with thin walls can provide low weight for a given
stiffness. The light-weight-design principle offers high dynamic stiffness
by providing a high natural frequency of the structure through
combining high static stiffness with low weight rather than through
the use of large mass. (Dynamic stiffness is the stiffness exhibited by
the system when subjected to dynamic excitation where the elastic, the
damping, and the inertia properties of the structure are involved; it is a
frequency-dependent quantity.)
TURNING
Turning is a machining operation for all types of metallic and nonmetallic
materials and is capable of producing circular parts with straight or
various profiles. The cutting tools may be single-point or form tools.
The most common machine tool used is a lathe; modern lathes are
computer-controlled and can achieve high production rates with little
labor. The basic operation is shown in Fig. 13.4.10, where the workpiece
is held in a chuck and rotates at N r/min; a cutting tool moves
along the length of the piece at a feed f (in/r or mm/r) and removes
material at a radial depth d, reducing the diameter from D0 to Df .
Lathes are generally considered to be the oldest member of machine
tools, having been first developed in the late eighteenth century.
The most common lathe is called an engine lathe because it was one of the
first machines driven by Watt’s steam engine. The basic lathe has the
following main parts: bed, headstock, tailstock, and carriage. The types of
lathes available for a variety of applications may be listed as follows:
engine lathes, bench lathes, horizontal turret lathes, vertical lathes, and automatics. A great variety of lathes and attachments are available
within each category, also depending on the production rate required.
It is common practice to specify the size of an engine lathe by giving
the swing (diameter) and the distance between centers when the tailstock
is flush with the end of the bed. The maximum swing over the ways is
usually greater than the nominal swing. The length of the bed is given
frequently to specify the overall length of the bed. A lathe size is indicated
thus: 14 in (356 mm) (swing) by 30 in (762 mm) (between
centers) by 6 ft (1,830 mm) (length of bed). Lathes are made for light-,
medium-, or heavy-duty work.
Geometric progression is used extensively in designing machine-tool
feeds and speeds. Feeds in geometric progression are used on cylindrical
grinders, boring mills, milling machines, drilling machines, etc.; but
for screw-cutting lathes, the power feeds for thread cutting and turning
must be in proportion to the pitch of threads to be cut.
All geared-head lathes, which are single-pulley (belt-driven or
arranged for direct-motor drive through short, flat, or V belts, gears, or
silent chain), increase the power of the drive and provide a means for
obtaining 8, 12, 16, or 24 spindle speeds. The teeth may be of the spur,
helical, or herringbone type and may be ground or lapped after hardening.
N
d
Workpiece
Tool
Chuck
Feed, f
Df Do
Fig. 13.4.10 A turning operation on a round workpiece held in a three-jaw
chuck.
Variable speeds are obtained by driving with adjustable-speed dc
shunt-wound motors with stepped field-resistance control or by electronics
or motor-generator system to give speed variation in infinite
steps. AC motors driving through infinitely variable speed transmissions
of the mechanical or hydraulic type are also in general use.
Modern lathes, many of which are now computer-controlled (turning
centers), are built with the speed capacity, stiffness, and strength capable
of taking full advantage of new and stronger tool materials. The main
drive-motor capacity of lathes ranges from fractional to more than
200 hp (150 kW). Speed preselectors, which give speed as a function of
work diameter, are introduced, and variable-speed drives using dc
motors with panel control are standard on many lathes. Lathes with
contour facing, turning, and boring attachments are also available.
Tool Shapes for Turning
The standard nomenclature for single-point tools, such as those used on
lathes, planers, and shapers, is shown in Fig. 13.4.11. Each tool consists
of a shank and point. The point of a single-point tool may be formed by
grinding on the end of the shank; it may be forged on the end of the
shank and subsequently ground; a tip or insert may be clamped or
brazed to the end of the shank (see Fig. 13.4.8). The best tool shape for
each material and each operation depends on many factors. For specific
information and recommendations, the various sources listed in the
References should be consulted. See also Table 13.4.3.
Positive rake angles improve the cutting operation with regard to
forces and deflection; however, a high positive rake angle may result in
early failure of the cutting edge. Positive rake angles are generally used
in lower-strength materials. For higher-strength materials, negative rake
angles may be used. Back rake usually controls the direction of chip
flow and is of less importance than the side rake. The purpose of relief
angles is to avoid interference and rubbing between the workpiece and
tool flank surfaces. In general, they should be small for high-strength
materials and larger for softer materials. Excessive relief angles may
weaken the tool. The side cutting-edge angle influences the length of chip
contact and the true feed. This angle is often limited by the workpiece
geometry, e.g., the shoulder contour. Large angles are apt to cause tool
chatter. Small end cutting-edge angles may create excessive force normal
to the workpiece, and large angles may weaken the tool point. The
purpose of the nose radius is to give a smooth surface finish and to obtain
longer tool life by increasing the strength of the cutting edge. The nose
radius should be tangent to the cutting-edge angles. A large nose radius
gives a stronger tool and may be used for roughing cuts; however, large
radii may lead to tool chatter. A small nose radius reduces forces and is
therefore preferred on thin or slender workpieces.
Fig. 13.4.11 Standard nomenclature for single-point cutting tools.
Turning Recommendations Recommendations for tool materials,
depth of cut, feed, and cutting speed for turning a variety of materials
are given in Table 13.4.4. The cutting speeds for high-speed steels for
turning, which are generally M2 and M3, are about one-half those for
uncoated carbides. A general troubleshooting guide for turning operations
is given in Table 13.4.5.
Turret Lathes
Turret lathes are used for the production of parts in moderate quantities
and produce interchangeable parts at low production cost. Turret lathes
may be chucking, screw machine, or universal. The universal machine
may be set up to machine bar stock as a screw machine or have the work
held in a chuck. These machines may be semiautomatic, i.e., so
arranged that after a piece is chucked and the machine started, it will
complete the machining cycle automatically and come to a stop. They
may be horizontal or vertical and single- or multiple-spindle; many of
these lathes are now computer-controlled and have a variety of featuresslides directly on the bed. Hence, the length of stroke is limited only by
the length of bed. A separate square-turret carriage with longitudinal
and transverse movement can be mounted between the head and the
hex-turret saddle so that combined cuts from both stations at one time
are possible. The saddle type of turret lathe generally has a large hollow
vertically faced turret for accurate alignment of the tools.
Screw Machines
When turret lathes are set up for bar stock, they are often called screw
machines. Turret lathes that are adaptable only to bar-stock work are
constructed for light work. As with turret lathes, they have spring collets
for holding the bars during machining and friction fingers or rolls to
feed the bar stock forward. Some bar-feeding devices are operated by
hand and others semiautomatically.
Automatic screw machines may be classified as single-spindle or multiple-
spindle. Single-spindle machines rotate the bar stock from which
the part is to be made. The tools are carried on a turret and on cross
slides or on a circular drum and on cross slides. Multiple-spindle machines
have four, five, six, or eight spindles, each carrying a bar of the
material from which the piece is to be made. Capacities range from 1⁄3 to
6 in (3 to 150 mm) diam of bar stock.
Feeds of forming tools vary with the width of the cut. The wider the
forming tool and the smaller the diameter of stock, the smaller the feed.
On multiple-spindle machines, where many tools are working simultaneously,
the feeds should be such as to reduce the actual cutting time to
a minimum. Often only one or two tools in a set are working up to
capacity, as far as actual speed and feed are concerned.
BORING
Boring is a machining process for producing internal straight cylindrical
surfaces or profiles, with process characteristics and tooling similar to
those for turning operations.
Boring machines are of two general types, horizontal and vertical, and
are frequently referred to as horizontal boring machines and vertical
boring and turning mills. A classification of boring machines comprises
horizontal boring, drilling, and milling machines; vertical boring and
turning mills; vertical multispindle cylinder boring mills; vertical cylinder
boring mills; vertical turret boring mills (vertical turret lathes); carwheel
boring mills; diamond or precision boring machines (vertical and
horizontal); and jig borers.
The horizontal type is made for both precision work and general manufacturing.
It is particularly adapted for work not conveniently revolved,
for milling, slotting, drilling, tapping, boring, and reaming long
holes, and for making interchangeable parts that must be produced
without jigs and fixtures. The machine is universal and has a wide range
of speeds and feeds, for a face-mill operation may be followed by one
with a small-diameter drill or end mill.
Vertical boring mills are adapted to a wide range of faceplate work that
can be revolved. The advantage lies in the ease of fastening a workpiece
to the horizontal table, which resembles a four-jaw independent chuck
with extra radial T slots, and in the lessened effect of centrifugal forces
arising from unsymmetrically balanced workpieces.
A jig-boring machine has a single-spindle sliding head mounted over a
table adjustable longitudinally and transversely by lead screws which
roughly locate the work under the spindle. Precision setting of the table
may be obtained with end measuring rods, or it may depend only on the
accuracy of the lead screw. These machines, made in various sizes, are
used for accurately finishing holes and surfaces in definite relation to
one another. They may use drills, rose or fluted reamers, or single-point
boring tools. The latter are held in an adjustable boring head by which
the tool can be moved eccentrically to change the diameter of the hole.
Precision-boring machines may have one or more spindles operating at
high speeds for the purpose of boring to accurate dimensions such surfaces
as wrist-pin holes in pistons and connecting-rod bushings.
Boring Recommendations Boring recommendations for tool materials,
depth of cut, feed, and cutting speed are generally the same as
those for turning operations (see Table 13.4.4). However, tool deflections,
chatter, and dimensional accuracy can be significant problems
because the boring bar has to reach the full length to be machined and
space within the workpiece may be limited. Boring bars have been
designed to dampen vibrations and reduce chatter during machining.
DRILLING
Drilling is a commonly employed hole-making process that uses a drill
as a cutting tool for producing round holes of various sizes and depths.
Drilled holes may be subjected to additional operations for better surface
finish and dimensional accuracy, such as reaming and honing,
described later in this section.
Drilling machines are intended for drilling holes, tapping, counterboring,
reaming, and general boring operations. They may be classified
into a large variety of types.
Sizes of Drilling Machines Vertical drilling machines are usually
designated by a dimension which roughly indicates the diameter of the
largest circle that can be drilled at its center under the machine. This
dimensioning, however, does not hold for all makes of machines. The
sizes begin with about 6 and continue to 50 in. Heavy-duty drill presses
of the vertical type, with all-geared speed and feed drive, are constructed
with a box-type column instead of the older cylindrical column.
The size of a radial drill is designated by the length of the arm. This
represents the radius of a piece which can be drilled in the center.
Twist drills (Fig. 13.4.12) are the most common tools used in drilling
and are made in many sizes and lengths. For years they have been
grouped according to numbered sizes, 1 to 80, inclusive, corresponding
approximately to Stub’s steel wire gage; some by lettered sizes A to Z,
inclusive; some by fractional inches from 1⁄64 up, and the group of
millimeter sizes.
Straight-shank twist drills of fractional size and various lengths range
from 1⁄64 in diam to 11⁄4 in by 1⁄64 in increments; to 11⁄2 in by 1⁄32 in; and
to 2 in by 1⁄16 in. Taper-shank drills range from 1⁄8 in diam to 13⁄4 in by 1⁄64
increments; to 21⁄4 in by 1⁄32 in; and to 31⁄2 in by 1⁄16 in. Larger drills are
made by various drill manufacturers. Drills are also available in metric
dimensions.
Tolerances have been set on the various features of all drills so that
the products of different manufacturers will be interchangeable in the
user’s plants.
Twist drills are decreased in diameter from point to shank (back
taper) to prevent binding. If the web is increased gradually in thickness
from point to shank to increase the strength, it is customary to reduce
the helix angle as it approaches the shank. The shape of the groove is
important, the one that gives a straight cutting edge and allows
Fig. 13.4.12 Straight shank twist drill.
a full curl to the chip being the best. The helix angles of the flutes vary
from 10 to 45°. The standard point angle is 118°. There are a number of
drill grinders on the market designed to give the proper angles. The point
may be ground either in the standard or the crankshaft geometry. The
drill geometry for high-speed steel twist drills for a variety of workpiece
materials is given in Table 13.4.6.
Among the common types of drills (Fig. 13.4.13) are the combined
drill and countersink or center drill, a short drill used to center shafts
before squaring and turning: the step drill, with two or more diameters;
the spade drill which has a removable tip or bit clamped in a holder on
the drill shank, used for large and deep holes; the trepanning tool used to 0.4 mm) wide for machine-finish reaming and 0.004 to 0.006 in (0.1
to 0.15 mm) for hand reaming, to provide free cutting of the edges due
to the slight body taper and also to pilot the reamer in the hole. The hole
to be flute- or finish-reamed should be true. A rake of 5° is recommended
for most reaming operations. A reamer may be straight or helically
fluted. The latter provides much smoother cutting and gives a
better finish.
Expansion reamers permit a slight expansion by a wedge so that the
reamer may be resharpened to its normal size or for job shop use; they
provide slight variations in size. Adjustable reamers have means of adjusting
inserted blades so that a definite size can be maintained through
numerous grindings and fully worn blades can be replaced with new
ones. Shell reamers constitute the cutting portion of the tool which fits
interchangeably on arbors to make many sizes available or to make
replacement of worn-out shells less costly. Reamers float in their holding
fixtures to ensure alignment, or they should be piloted in guide
bushings above and below the work. They may also be held rigidly,
such as in the tailstock of a lathe.
The speed of high-speed steel reamers should be two-thirds to threequarters
and feeds usually are two or three times that of the corresponding
drill size. The most common tool materials for reamers are M1, M2,
and M7 high-speed steels and C-2 carbide.
THREADING
Threads may be formed on the outside or inside of a cylinder or cone (1)
with single-point threading tools, (2) with threading chasers, (3) with
taps, (4) with dies, (5) by thread milling, (6) by thread rolling, and (7) by
grinding. There are numerous types of taps, such as hand, machine
screw, pipe, and combined pipe tap and drill. Small taps usually have no
radial relief. They may be made in two, three, or four flutes. Large taps
may have still more flutes.
The feed of a tap depends upon the lead of the screw thread. The
cutting speed depends upon numerous factors: Hard tough materials,
great length of hole, taper taps, and full-depth thread reduce the speed;
long chamfer, fine pitches, and a cutting fluid applied in quantity increase
the speed. Taps are cut or formed by grinding. The ground-thread
taps may operate at much higher speeds than the cut taps. Speeds may
range from 3 ft/min (1 m/min) for high-strength steels to 150 ft/min (45
m/min) for aluminum and magnesium alloys. Common high-speed steel
tool materials for taps are M1, M7, and M10.
Threading dies, used to produce external threads, may be solid, adjustable,
spring-adjustable, or self-opening die heads. Replacement chasers
are used in die heads and may be of the fixed or self-opening type.
These chasers may be of the radial type, hobbed or milled; of the tangenital
type; or of the circular type. Emulsions and oils are satisfactory
for most threading operations.
MILLING
Milling is one of the most versatile machining processes and is capable
of producing a variety of shapes involving flat surfaces, slots, and contours
(Fig. 13.4.14).
Milling machines use cutters with multiple teeth in contrast with the
single-point tools of the lathe and planer. The workpiece is generally fed
past the cutter perpendicular to the cutter axis. Milling usually is face or
peripheral cutting.
Standard spindle noses and arbors for milling machines provide interchangeability
of arbors and face-milling cutters, regardless of make or
size of machine. The taper of the spindle end and arbor is 31⁄2 in/ft, to
make them self-releasing. The retention of the shank is dependent upon a
positive locking device, such as screws or draw-in bolt. When unlocked,
these tapers release themselves.
Milling-machine classification is based on design, operation, or purpose.
Knee-and-column type milling machines have the table and saddle
supported on the vertically adjustable knee gibbed to the face of the
column. The table is fed longitudinally on the saddle, and the latter
transversely on the knee to give three feeding motions.
Knee-type machines are made with horizontal or vertical spindles.
The horizontal universal machines have a swiveling table for cutting
helices. The plain machines are used for jobbing or production work,
the universal for toolroom work. Vertical milling machines with fixed or
sliding heads are otherwise similar to the horizontal type. They are used
for face or end milling and are frequently provided with a rotary table
for making cylindrical surfaces.
The fixed-bed machines have a spindle mounted in a head dovetailed
to and sliding on the face of the column. The table rests directly on the
bed. They are simple and rigidly built and are used primarily for highproduction
work. These machines are usually provided with work-holding
fixtures and may be constructed as plain or multiple-spindle machines,
simple or duplex.
Rotary-type millers usually have a rotating table on which fixtures
carrying the workpiece are mounted. The cutter spindles are mounted
over the edge of the table past which the workpiece is fed.
Drum-type millers consist of a drum carrying the work and rotating on
a horizontal axis. Both rotary and drum types are mass-production machines,
there being no idle time, for the drums rotate continuously while
the parts, loaded on one side of the machine, pass first the roughing and
then the finishing cutters and are replaced when they return to the loading
position.
In planetary milling machines the workpiece is stationary on the bed
or clamped to the tailstock while the cutter rotates. Plain and formed
internal or external surfaces and threads are produced by inserting the
cutter into the bore to be milled, feeding it to depth radially, making a
sweeping cut about the bore, and withdrawing first radially and then
axially.
Planer-type millers are used only on the heaviest work. They are used
to machine a number of surfaces on a particular part or group of parts
arranged in series in fixtures on the table.
Thread millers are used to cut threads and worms. A single formed
cutter may be used or all the threads may be cut at one time by a
multiple-thread cutter.
Milling Cutters
Milling cutters are made in a wide variety of shapes and sizes.
The nomenclature of tooth parts and angles is standardized as in Fig. 13.4.15. Milling cutters may be classified in various ways, such as
purpose or use of the cutters (Woodruff keyseat cutters, T-slot cutters,
gear cutters, etc.); construction characteristics (solid cutters, carbidetipped
cutters, etc.); method of mounting (arbor type, shank type, etc.);
and relief of teeth. The latter has two categories: profile cutters which
produce flat, curved, or irregular surfaces, with the cutter teeth sharpened
on the land; and formed cutters which are sharpened on the face to
retain true cross-sectional form of the cutter.
Two kinds of milling are generally considered to represent all forms
of milling processes: peripheral (slab) and face milling. In the peripheralmilling
process the axis of the cutter is parallel to the surface milled,
whereas in face milling, the cutter axis is generally at a right angle to the
surface. The peripheral-milling process is also divided into two types:
conventional (up) milling and climb (down) milling. Each has its advantages,
and the choice depends on a number of factors such as the type
and condition of the equipment, tool life, surface finish, and machining
parameters.
Milling Recommendations Recommendations for tool materials,
feed per tooth, and cutting speed for milling a variety of materials are
given in Table 13.4.9. The cutting speeds for high-speed steels for turning,
which are generally M2 and M7, are about one-half those for uncoated
carbides. A general troubleshooting guide for milling operations is
given in Table 13.4.10.
GEAR MANUFACTURING
(See also Sec. 8)
Gear Cutting Most gear-cutting processes can be classified as either
forming or generating. In a forming process, the shape of the tool is
reproduced on the workpiece; in a generating process, the shape produced
on the workpiece depends on both the shape of the tool and the
relative motion between the tool and the workpiece during the cutting
operation. A soft live center on a lathe can be formed by means of a
broad, flat-form tool fed at right angles to the lathe spindle, or generated
by a single-point tool fed at the point angle in the compound rest. In
general, a generating process is more accurate than a forming process.
In the form cutting of gears, the tool has the shape of the space between
the teeth. For this reason, form cutting will produce precise tooth
profiles only when the cutter is accurately made and the tooth space is of
constant width, such as on spur and helical gears. A form cutter may cut
or finish one of or all the spaces in one pass. Single-space cutters may be
disk-type or end-mill-type milling cutters. In all single-space operations,
the gear blank must be retracted and indexed, i.e., rotated one
tooth space, between each pass.
Single-space form milling with disk-type cutters is particularly suitable
for gears with large teeth, because, as far as metal removal is
concerned, the cutting action of a milling cutter is more efficient than
that of the tools used for generating. Form milling of spur gears is done
on machines that retract and index the gear blank automatically.
For the same tooth size (pitch), the shape (profile) of the teeth on an
involute gear depends on the number of teeth on the gear. Most gears
have active profiles that are wholly, partially, or approximately involute,
and, consequently, accurate form cutting would require a different
cutter for each number of teeth. In most cases, satisfactory results can be
obtained by using the eight cutters for each pitch that are commercially
available. Each cutter is designed to cut a range of tooth numbers; the
no. 1 cutter, for example, cuts from 135 teeth to a rack, and the no. 8 cuts
12 and 13 teeth. (See Table 13.4.11.)
Multiple-space form cutting is done with a broach or with a patented
Shear Speed toolhead. The broach is pushed down into or over the gear
blank, usually on a hydraulic press, and all the spaces can be cut in one
pass.
The Shear-Speed toolhead contains three main parts: a housing, a
member with radial slots in which a tool for each of the tooth spaces on
the gear being cut can slide, and a movable, double cone-shaped guiding
unit that controls the radial movement (feed) of the tools. With the
toolhead stationary, the part is reciprocated past the cutting tools; each
tool is fed radially a predetermined amount each stroke until the full
tooth depth is cut. To avoid drag, the tools are retracted on each return
(noncutting) stroke of the gear.
Gears always operate in pairs and are usually required to have contacting
profiles of such a shape that the ratio of the speeds of the pair
remains constant at all times; such gears are said to be conjugate to one
another.
In a gear generating machine, the generating tool can be considered
as one of the gears in a conjugate pair and the gear blank as the other
gear. The correct relative motion between the tool arbor and the blank
arbor is obtained by means of a train of indexing gears within the
machine.
One of the most valuable properties of the involute as a gear-tooth
profile is that if a cutter is made in the form of an involute gear of a
given pitch and any number of teeth, it can generate all gears of all tooth
numbers of the same pitch and they will all be conjugate to one another.
The generating tool may be a pinion-shaped cutter, a rack-shaped
(straight) cutter, or a hob, which is essentially a series of racks wrapped
around a cylinder in a helical, screwlike form.
On a gear shaper, the generating tool is a pinion-shaped cutter that
rotates slowly at the proper speed as if in mesh with the blank; the
cutting action is produced by a reciprocation of the cutter parallel to the
work axis. These machines can cut spur and helical gears, both internal
and external; they can also cut continuous-tooth helical (herringbone)
gears and are particularly suitable for cluster gears, or gears that are
close to a shoulder.
On a rack shaper the generating tool is a segment of a rack that moves
perpendicular to the axis of the blank while the blank rotates about a
fixed axis at the speed corresponding to conjugate action between the
rack and the blank; the cutting action is produced by a reciprocation of
the cutter parallel to the axis of the blank. Since it is impracticable to
have more than 6 to 12 teeth on a rack cutter, the cutter must be disengaged
from the blank at suitable intervals and returned to the starting
point, the blank meanwhile remaining fixed. These machines can cut
both spur and helical external gears.
A gear-cutting hob is basically a worm, or screw, made into a generating
tool by cutting a series of longitudinal slots or ‘‘gashes’’ to form
teeth; to form cutting edges, the teeth are ‘‘backed off,’’ or relieved, in a
lathe equipped with a backing-off attachment. A hob may have one,
two, or three threads; on involute hobs with a single thread, the generating
portion of the hob-tooth profile usually has straight sides (like an
involute rack tooth) in a section taken at right angles to the thread.
In addition to the conjugate rotary motions of the hob and workpiece,
the hob must be fed parallel to the workpiece axis for a distance greater
than the face width of the gear. The feed, per revolution of the work- piece, is produced by the feed gears, and its magnitude depends on the
material, pitch, and finish desired; the feed gears are independent of the
indexing gears. The hobbing process is continuous until all the teeth are
cut.
The same machines and the same hobs that are used for cutting spur
gears can be used for helical gears; it is only necessary to tip the hob
axis so that the hob and gear pitch helices are tangent to one another and
to correlate the indexing and feed gears so that the blank and the hob are
advanced or retarded with respect to each other by the amount required
to produce the helical teeth. Some hobbing machines have a differential
gear mechanism that permits the indexing gears to be selected as for
spur gears and the feed gearing to be chosen independently.
The threads of worms are usually cut with a disk-type milling cutter
on a thread-milling machine and finished, after hardening, by grinding.
Worm gears are usually cut with a hob on the machines used for hobbing
spur and helical gears. Except for the gashes, the relief on the teeth,
and an allowance for grinding, the hob is a counterpart of the worm. The
hob and workpiece axes are inclined to one another at the shaft angle of
the worm and gear set, usually 90°. The hob may be fed in to full depth
in a radial (to the blank) direction or parallel to the hob axis.
Although it is possible to approximate the true shape of the teeth on a
straight bevel gear by taking two or three cuts with a form cutter on a
milling machine, this method, because of the taper of the teeth, is obviously
unsuited for the rapid production of accurate teeth. Most straight
bevel gears are roughed out in one cut with a form cutter on machines
that index automatically and then finished to the proper shape on a
generator.
The generating method used for straight bevel gears is analogous to
the rack-generating method used for spur gears. Instead of using a rack
with several complete teeth, however, the cutter has only one straight
cutting edge that moves, during generation, in the plane of the tooth of a
basic crown gear conjugate to the gear being generated. A crown gear is
the rack among bevel gears; its pitch surface is a plane, and its teeth
have straight sides.
The generating cutter moves back and forth across the face of the
bevel gear like the tool on a shaper; the ‘‘generating roll’’ is obtained by
rotating the gear slowly relative to the tool. In practice two tools are
used, one for each side of a tooth; after each tooth has been generated,
the gear must be retracted and indexed to the next tooth.
The machines used for cutting spiral bevel gears operate on essentially
the same principle as those used for straight bevel gears; only the
cutter is different. The spiral cutter is basically a disk that has a number
of straight-sided cutting blades protruding from its periphery on one
side to form the rim of a cup. The machines have means for indexing,
retracting, and producing a generating roll; by disconnecting the roll
gears, spiral bevel gears can be form cut.
Gear Shaving For improving the surface finish and profile accuracy
of cut spur and helical gears (internal and external), gear shaving, a
free-cutting gear finishing operation that removes small amounts of
metal from the working surfaces of the teeth, is employed. The teeth on
the shaving cutter, which may be in the form of a pinion (spur or helical)
or a rack, have a series of sharp-edged rectangular grooves running from
tip to root. The intersection of the grooves with the tooth profiles creates
cutting edges; when the cutter and the workpiece, in tight mesh, are
caused to move relative to one another along the teeth, the cutting edges
remove metal from the teeth of the work gear. Usually the cutter drives
the workpiece, which is free to rotate and is traversed past the cutter
parallel to the workpiece axis. Shaving requires less time than grinding,
but ordinarily it cannot be used on gears harder than approximately 400
HB (42 HRC).
Gear Grinding Machines for the grinding of spur and helical gears
utilize either a forming or a generating process. For form grinding, a
disk-type grinding wheel is dressed to the proper shape by a diamond
held on a special dressing attachment; for each number of teeth a special
index plate, with V-type notches on its periphery, is required. When
grinding helical gears, means for producing a helical motion of the
blank must be provided.
For grinding-generating, the grinding wheel may be a disk-type,
double-conical wheel with an axial section equivalent to the basic
rack of the gear system. A master gear, similar to the gear being ground,
is attached to the workpiece arbor and meshes with a master rack; the
generating roll is created by rolling the master gear in the stationary
rack.
Spiral bevel and hypoid gears can be ground on the machines on
which they are generated. The grinding wheel has the shape of a flaring
cup with a double-conical rim having a cross section equivalent to the
surface that is the envelope of the rotary cutter blades.
Gear Rolling The cold-rolling process is used for the finishing of
spur and helical gears for automatic transmissions and power tools; in
some cases it has replaced gear shaving. It differs from cutting in that
the metal is not removed in the form of chips but is displaced under
heavy pressure.
There are two main types of cold-rolling machines, namely, those
employing dies in the form of racks or gears that operate in a parallelaxis
relationship with the blank and those employing worm-type dies
that operate on axes at approximately 90° to the workpiece axis. The
dies, under pressure, create the tooth profiles by the plastic deformation
of the blank.
When racks are used, the process resembles thread rolling; with geartype
dies the blank can turn freely on a shaft between two dies, one
mounted on a fixed head and the other on a movable head. The dies have
the same number of teeth and are connected by gears to run in the same
direction at the same speed. In operation, the movable die presses the
blank into contact with the fixed die, and a conjugate profile is generated
on the blank. On some of these machines the blank can be fed
axially, and gears can be rolled in bar form to any convenient
length.
On machines employing worm-type dies, the two dies are diametrically
opposed on the blank and rotate in opposite directions. The speeds
of the blank and the dies are synchronized by change gears, like the
blank and the hob on a hobbing machine; the blank is fed axially between
the dies.
Although gears have been cold-rolled from solid blanks, most commercial
rolling is done as a finishing operation on fine-pitch, precut
gears.
PLANING AND SHAPING
Planers are used to rough and finish large flat surfaces, although arcs
and special forms can be made with proper tools and attachments. Surfaces
to be finished by scraping, such as ways and long dovetails and,
particularly, parts of machine tools, are, with few exceptions, planed.
With fixture

Additional comments :