machining process.pptx

MACHINING PROCESSES
Dr.M. Bala Theja,M.Tech,Ph.D
Associate Professor
Department of Mechanical Engineering

CONTENTS
• Introduction machining processes.
• General Design rules for machining.
• Dimensional Tolerances and surface roughness.
• Design For machining.
• Ease –redesigning of components for machining ease
with suitable examples.
• General design recommendations for machined parts.

INTRODUCTION
• Machining is the manufacturing process by which parts can
be produced to the desired dimensions and surface finish
from a blank by gradual removal of the excess material in the
form of chips with the help of a sharp cutting tool.
• Almost 90% of the all engineering components are subjected
to some kind of machining during manufacture for semi
finishing operations.
• It is very important to design those parts in such a way that
would lead to the increase in efficiency of the machining
process, enhancement of the tool life and reduction of the
overall cost of machining.
• To achieve these targets, a brief knowledge of various
machining processes is required.

CLASSIFICATION OF MACHINING
EROSION

DFM for economic production
• Manufacturing cost is the key for economic success of the product.
• Economic success depends on the profit margin on each unit sale and the
volume of the units sold.
• Profit margin and the sales volume depends on product quality.
• Successful design ensures high product quality while minimising the
manufacturing cost.
• DFM helps you to reduce the manufacturing cost without sacrificing the
product quality through the following:
• Simplicity of the product
• Standard materials and components
• Standard design of the product
• Specify liberal tolerances
• Use most machinable materials available in local market.
• Avoid secondary operations or finishing operations

DESIGN RULES FOR
MACHINING EASE
1. The amount of machining should be reduced, as far as
possible, by assigning size tolerances only for fits
between mating surfaces; all other elements should
have free dimensions. Parts may be obtained without
any machining if precise methods of blank manufacture
are applied.

2. Convenient and reliable locating surfaces should be
provided to set up work piece for machining. Whenever
possible, the measurement datum should be made to
coincide with the set-up datum surface by proper
dimensioning of the part drawing.
3. There should be sufficient rigidity of work piece so as to
eliminate significant deformation in the process of
machining.
4. Provisions should be made for conveniently advancing
rigid, high- production cutting tools to the surface being
machined. Difference in height between adjacent, rough
and machined surfaces should be sufficient, making
adjustment for the machining allowances, to enable the
cutting tools to clear the rough surface in its overtravel.

5. clearance recesses: Dimension A should be provided to
allow overtravel of cutting tool whenever it is necessary.

6.Parts should be designed so that several work pieces
can be set up to be machined simultaneously, as shown
in figure. The following considerations are important for
elementary surfaces of machine parts:

7. External surfaces of revolution, upset heads, flanges
and shoulders should be extensively applied to reduce
machining and to save metal.
8. It is advisable to retain the centre holes on the finished
components (shafts and similar parts ) that were
machined between centres.
9. The elements of the shank design should be unified ,
whenever possible, so that the same multiple tool set-
up can be employed in machining them, as illustrated
in Figure.

10. –A It is a good practice to provide a spherical convex surface with a flat end
surfaced.
10-B Minimize the use of different machine for a single part. Use single machine as far as possible
11. Holes: (a) through holes are to be used, wherever possible, because such
holes are much more simple to machine than blind holes. The form of blind
holes should correspond to the design of the tool to be employed in
machining for example, with the reamer or counter bore.

(b) Holes should not be located closer to a certain minimum
distance from an adjacent wall of the part: A ≥ D/2 + R.
This distance for holes accommodating fastening bolts
should be A ≥ Dn/2 + R. where Dn is the diameter of a
circle circumscribing the nut.

(c) Center distances of holes should be specified, by
considering the possibility of using multi spindle drilling
heads. For this purpose, the location and sizes of the
holes in flanges have to be unified. The number of holes
and their location in a flange should be designed so that
the holes can be drilled three or four spindle heads with
subsequent indexing.
(d) Holes to be drilled should have their top and bottom
surface square to the hole axis to prevent drill breakage.
(e) When several holes are located along the same axis, it is
good practice to reduce the diameter of each consequent
hole by an amount exceeding the machining allowance for
the preceding hole. This will enable a set-up to be used in
which all the holes are bored simulatenously.
(f) In drilling at the bottom of a slot, their diameter should be
less by 0.5-1mm than the slot width.

g) In stepped holes, maximum accuracy should be
specified for the through step.
h) Either a blind hole or a through hole should be
provided on the axis in the design of concave spherical
surfaces to avoid zero cutting speeds at the axis fig(a),
thus preventing damage to the tool point.
i) It is advisable to avoid recesses in holes that are to be
machined on single or multiple spindle drilling
machines since they complicate machining operations.
Machined recesses should also be avoided by using
cored recesses fig(b).

12. Threads:
(a) It is advisable to use an entering chamfer on
threaded holes.
(b) The number of incomplete threads cut with a tap in
a blind hole with no recess should be equal to three for
grey iron casting and five for steel parts
(c) A neck at the end of a thread is not required for
milled threads.
(d) Preferred thread standards should pertain, not only
to the machine under consideration, but to all the
threads used in the plant or branch of industry. Small
diameter threads(6mm and less) should be avoided if
they are cut.

13. Flat surfaces:
(a) The outline of a machined flat surface should
ensure, as far as possible, uniform and impact less chip
removal.
(b) The size of a machined flat surface should be in
accordance with the sizes of standard milling cutters,
i.e., the width of the surfaces should be unified to suit
the standard services of face mill diameters or the
widths of plain milling cutters.
(c) If no elements are provided for cutting tool
overtravel, the transition surfaces should correspond in
size and form to the cutting tool (See below figs)

14. FORMED SURFACES:
The radii of concave and convex surfaces should
correspond to those of standard convex and concave
milling cutters.
15. SLOTS AND RECESSES:
Whenever possible, through slots should be
employed. If through machining is possible, the end of
the slot should correspond to the radius of the cutter
The width and depth of slots should be specified
according to the sizes of standard side milling, viz. end
mills. The corner radii at the bottom of recess should be
the constraint for all around recess and should
correspond to the size

DIMENSIONAL TOLERANCE AND
SURFACE ROUGHNESS FOR
MACHINING PROCESSES

REDESIGN OF A PART FOR
EASY MACHINING
EXAMPLE: The following figure shows the initial design of
the shaft support bracket, which is bolted to a housing
to support a rotating shaft. Accurate machining is
needed for the bore with high tolerance in locating the
bore relative to the dowel.

EASY MACHINING
ANALYSIS: Initial design had the following features that
are difficult to machine:
• Different diameters for the dowels and bolt holes, which
requires tool change and loss of time
• The bore and oil hole are long relative to their diameter,
which require long processing steps.
• The is no obvious features on the outer surface to fix
the part and prevent rotation during machining.

EASY MACHINING
SOLUTION:
• For easy machining, the part was redesigned as shown
in Fig. 7.18:
• The dowels and bolt holes have the same diameter.
• The center of the bore has a larger diameter than the
ends to reduce length to be machined.
• The length of the oil hole is reduced.
• Flat surfaces were cast on outer surfaces for ease of
location while machining.

EASY MACHINING
CONCLUSION:
These changes reduced the machining time from
173 to 119 seconds, (33%). Quality is also better and
higher tolerances are possible.

MACHINING
OPERATIONS
PERFORMED
ON
LATHE

DESIGN RECOMMENDATIONS
FOR TURNING
A. STOCK SIZE AND SHAPE
1. The largest diameter of the component should be
taken as the diameter of the bar stock in order to
conserve material and save machining time.
2. Standard sizes and shapes of bar stock should be
used in preference to special diameters and shapes.
B. BASIC PART SHAPE COMPLEXITY
1. Keep the design of parts as simple as possible to
reduce the number of tool stations and gauging
processes required.
2. Use standard tools as much as possible by specifying
standard, common sizes of holes, screw threads,
knurls, slots, and so on.

FOR TURNING
C. AVOIDING SECONDARY OPERATIONS
1. The part should be complete when cut off from the
bar material.
2. Secondary operations such as slots and flats should
be small and performed when the part is held in the
pickoff attachment.
3. Internal surfaces and screw threads should be
located at one end so that they can be performed before
cutoff and without the need for rechucking

FOR TURNING

FOR TURNING
D. EXTERNAL FORMS
1. The length of the formed area should not exceed two
and half times the minimum WP diameter (Fig. Next
slide).
2. Sidewalls of grooves and other surfaces that are
perpendicular to the axis of the WP should have a slight
draft of 1/2° or more to prevent tool marks when the
tool is withdrawn (Fig. Next slide).
3. When turning from square or hexagonal stock, the
turned diameter is the distance between two opposite
flats of the stock. It is advisable to design turned parts
to be about 0.25 mm or smaller than the bar stock size.
4. Avoid deep narrow grooves and sharp corners.

FOR TURNING
E. UNDERCUTS
1. Avoid angular undercuts and use undercuts obtainable
with traverse or axial tool movements.
2. External grooves are machined more economically than
internal recesses.
F. HOLES
1. The bottom shape of blind holes should be that made
by a standard drill point(Fig. Next slide).
G. SCREW THREADS
1. Avoid the formations of burrs in threaded parts (Fig.
Next slide).

FOR TURNING
H. KNURLS
1. Knurled width should be narrow (≤WP diameter).
2. Specify the approximate number of teeth per inch,
type of knurl, general size, and use of knurl.
I. SHARP CORNERS
1. Avoid sharp corners (external and internal) as they
cause weakness or more costly fabrication of form tools.
2. Provide a commercial corner break of 0.4 mm by 45°.
3. An internal sharp corner can be made by providing
an undercut at the corner

FOR TURNING
J. SPHERICAL ENDS
1. Design the radius of the spherical end to be larger
than the radius of the adjoining cylindrical surface

FOR TURNING
K. SLOTS AND FLATS
1. Slots are produced with a concave surface at the
bottom or end (milling cutter radius)

FOR TURNING
L. MARKING
1. Position impression marking so that roller
marking tools can be used.

FOR DRILLING
A. DRILLING
1. The drill entry surface should be perpendicular to the
drill bit to avoid starting problems and to ensure proper
location.
2. The exit surface of the drill should be perpendicular
to the axis of the drill to avoid drill breakage when
leaving the hole .

FOR DRILLING
3. For straightness requirements, avoid interrupted cuts
to avoid drill deflection and breakage (Fig).
4. Use standard drill sizes whenever possible.
5. Through holes are preferable than blind holes, as they
provide easier clearance for tools and chips.
6. Blind holes should not have flat bottoms because they
require a secondary machining operation and cause
problems during reaming.

FOR DRILLING
7. Avoid deep holes (over three times diameter) because of
chip clearance problems and the possibility of
straightness errors (Figure).
8. Avoid designing parts with very small holes if they are
not truly necessary (3 mm is the desirable minimum
diameter).
9. If large holes are required, it is desirable to have cored
holes (casting) in the WP before drilling.

FOR DRILLING
10. If the part requires several drilled holes, dimension
them from the same surface to simplify fixturing.

FOR DRILLING
11. Rectangular rather than angular coordinates should
be used to designate hole locations (Figure).
12. Design parts so that all can be drilled from one side or
from the fewest number of sides.

FOR DRILLING
13. Design parts so that there is a room for the drill
bushing near the surface where the drilled hole to be
started (Figure).
14. Standardize the size of holes, fasteners, and screw
threads as much as possible.

FOR DRILLING
15. For multiple-drilling operations, the designer should
bear in mind that there are limitations as to how closely
two simultaneously drilled holes can be spaced (for 6
mm diameter or less, spacing should not be less than
19 mm center to center).

FOR REAMING
1. Even when using guide bushing, do not depend on
reaming to correct location or alignment discrepancies
unless the discrepancies are very small.
2. Avoid intersecting drilled and reamed holes to prevent
tool breakage and burr removal problems (Figure).
3. If blind holes require reaming, increase the drilled
depth to provide room for chips (Figure).

FOR BORING
1. During boring, avoid designing holes with interrupted
surfaces, as they cause out-of roundness errors and
tool wear.
2. Avoid designing holes with a depth-to-diameter ratio of
over 4:1 or 5:1 to avoid inaccuracies caused by boring-
bar deflection. This ratio becomes 8:1 for carbide boring
bars.
3. For larger depth-to-diameter ratios, consider the use of
stepped diameters to limit the depth of a bored surface.

FOR BORING
4. Use through holes whenever possible.
5. If the hole must be blind, allow the rough hole to be
deeper than the bored hole by ¼ hole diameter.
6. Use boring only when the accuracy requirements are
essential.
7. Do not specify bored-hole tolerances unless necessary.
8. The bored part must be rigid so that deflection or
vibrations caused by the cutting forces are reduced.

FOR MILLING
1. Sharp inside and outside corners should be avoided.
2. The part should be easily clamped.
3. Machined surfaces should be accessible.
4. Easily machined material should be specified.
5. Design should be as simple as possible.

ADDITIONAL RECOMMENDATIONS
FOR MILLING
1. The product design should permit the use of standard
cutter shapes and sizes rather than special ones

FOR MILLING
2. The product design should permit manufacturing
preference as much as possible to determine the radius
where two milled surfaces intersect or where profile
milling is involved

FOR MILLING
3. When small flat surface is required, the product design
should permit the use of spot facing, which is quicker
than face milling

FOR MILLING
4. When spot faces are specified for casting, provide a low
boss for the surface to be machined.

FOR MILLING
5. When the outside surfaces intersect and a sharp corner
is not desirable, the product design should allow a bevel
or chamfer rather than rounding

FOR MILLING
6. When form-milling or machining rails, do not blend the
formed surface to an existing milled surface

FOR MILLING
7. Keyway design should permit the keyway cutter to
travel parallel to the center axis of the shaft and form
its own radius at the end

FOR MILLING
8. A design that requires the milling of surfaces adjacent
to a shoulder should provide clearance to the cutter
path (Fig).
9. A product design that avoids the necessity of milling at
parting lines, fl ash areas, and weldments will generally
extend the cutter life.

FOR MILLING
10. For more economical machining, the product design
should allow staking so that a milled surface can be
incorporated into a number of parts in one gang milling
operation

FOR MILLING
11. The most economical designs are those that require
the minimum number of operations.
12. The product design should provide clearance to allow
the use of larger-size cutters rather than small-size
ones to permit high removal rates.
13. In end-milling slots, the depth should not exceed the
diameter of the cutter (fig)

FOR MILLING

DESIGN RECOMMENDATIONS FOR
SHAPING, PLANING AND SLOTING
1. It is preferable to put machined surfaces in the same
plane to reduce the number of operations required.
2. Avoid multiple surfaces that are not parallel to the
direction of tool reciprocation, which would need
additional setups.
3. Avoid contoured surfaces unless a tracer attachment is
available and then specify gentle contours and generous
radii as much as possible.
4. Design parts so that they can be easily clamped to the
worktable and are rigid enough to withstand defl ection
during machining

5. With shapers and slotters, it is possible to cut to within
6 mm of an obstruction or the end of a blind hole. If
possible, allow a relived portion at the end of the
machined surface.

6. For thin, flat WPs that require surface machining, allow
sufficient stock for a stress-relieving operation between
rough and finish machining or, if possible, rough
machine equal amounts from both sides to allow 0.4
mm for finish machining on both sides.
7. The minimum size of hole in which a keyway or a slot
can be machined with a slotter or a shaper is about
25.54 mm.
8. Because of the lack of rigidity of long cutting tool
extensions, it is not feasible to machine a slot longer
than four times the hole diameter.

FOR THREAD CUTTING
1. Provide a space (1.5–19 mm) for the thread cutting tool
2. Keep the thread as short as possible, which machines
quicker and provides longer tool life.

FOR THREAD CUTTING
3. Allow chip clearance space when cutting internal
threads (through holes are best)
4. Include a chamfer at the top and the end of external
threads and a countersink at the top and the end of
internal threads.

FOR THREAD CUTTING
5. Consider the use of a reduced height thread form,
which machines more easily
6. The surface of the starting thread must be flat and
perpendicular to the thread’s center axis.

FOR THREAD CUTTING
7. Avoid slots, cross holes, and fl ats that intersect with
the cut threads.
8. When cross holes are unavoidable, consider
countersinking of such cross holes.
9. Do not specify closer tolerances than required (class 2
is commonly satisfactory).
10. Ground threads should be provided with corners of
0.25 mm at the root.
11. The length of center less ground threads should be
larger than the thread diameter.

FOR THREAD CUTTING
12. Coarse threads are more economical to produce and
assemble faster than fine threads.
13. Tubular parts must have a wall thickness that
withstands the cutting forces.

machining process.pptx

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Similar to machining process.pptx

Similar to machining process.pptx (20)

More from Dr.M BALA THEJA

More from Dr.M BALA THEJA (18)

Recently uploaded

Recently uploaded (20)

machining process.pptx