ALLAN`S MACHINING HANDBOOK

Transcription

Allan’s Machining Handbook Rev 1.6
5 December 2010
Allan’s
Machining Handbook
Allan Bester
Revision 1.6
December 2010
© Allan J Bester Dec 2002
0
5 December 2010
ALLAN’S MACHINING HANDBOOK
INDEX
Page
1.
Drilling Speeds & Feeds
………………………………………
2
2.
Lathe Turning: Cutting Speeds, Feeds, Depth of Cut ….……………
3
3.
Parting Off
……………………………………………………….
4
4.
Boring
……………………………………………………….
5
5.
Thread Specifications
……………………………………….
6
6.
Screwcutting in the Lathe
……………………………………….
14
7.
Reaming on the Lathe
……………………………………….
20
8.
Flycutting
……………………………………………………….
21
9.
Knurling
……………………………………………………….
22
10.
Milling in the Lathe ……………………………………………….
23
11.
Milling (Machine)
………………………………………………
24
12.
Gears & Gear Cutting
…………………………………………….
26
13.
Fits & Tolerances
……………………………………………….
30
14.
Keys & Keyways
……………………………………………….
33
15.
Silver Soldering
……………………………………………….
35
16.
Properties of Metals ……………………………………………….
37
17.
Bolts & Nuts ……………………………………………………….
40
18.
Formulae and Conversion Factors
……………………………….
42
1
1.
5 December 2010
DRILLING SPEEDS & FEEDS
Cutting speed is important in drilling. A relationship must be maintained between rate of
rotation, diameter of drill, rate of feed, form of drill point and clearances, lubrication of
cutting surfaces, and material of both drill and work. The cutting process is more complex
and the forces much greater when drilling than when turning, so that speeds are lower. It is
assumed that a suitable lubricant and coolant (water-soluble oils are preferred for drilling)
is used where appropriate, except for cast iron, brass and bronze. Plenty of cutting oil
greatly improves the drill action and makes it much less likely that the drill will heat,
expand, seize and break off in the work. Speeds and feeds for manual drilling (not power
downfeed) are selected on the basis of wishing to avoid resharpening of drill bits, and on
what feels comfortable, with reasonable chips emerging from the drill.
SPEEDS IN RPM FOR HSS DRILL BITS
Material
Aluminium
Brass, FCMS
Bronze, MS,
GM, cast iron
Stainless steel,
silver steel
Hard cast iron
1.0
20k
16k
10k
2.0
4.0
4600
3400
2500
Drill Diameter (mm)
6.0
8.0
10.0
4000
3100
2300
2500
1900
1450
1700
1260
1000
8.8k
3600
1700
1150
880
660
550
480
420
6.5k
1800
1000
650
500
400
330
280
240
12.0
1900
1250
800
14.0
1600
1050
700
16.0
1400
900
600
Notes:
1.
2.
When drilling in the lathe, reduce these speeds by 25% to 30% to allow for
the difficulty of chip clearance and coolant penetration down the hole.
Speeds should be reduced in holes after their depth exceeds eight times their
diameter.
SPEEDS IN FT/MIN FOR HSS DRILL BITS
Material
Aluminium, Brass
MS, Copper, GM, Bronze
Cast iron
Stainless steel, silver steel
Ft/min
300
85 - 100
70
60
2
2.
5 December 2010
LATHE TURNING: CUTTING SPEEDS, FEEDS, DEPTH OF CUT
For HSS cutters:
RPM = 12 x SFM
3,1416 x D
~
4 x SFM
D
RPM = 320 x CS (meters/min)
D (millimeters)
Material
Mild steel
Bronze
Silver steel
Stainless steel
Brass
Cast iron
Aluminium
Copper
FCMS
Average
CS
(ft/min)
80 – 100
80 – 100
40 – 70
20 – 40
100 – 200
50 – 80
200 – 300
100 – 120
100 – 120
Average
CS
(m/min)
24 – 30
24 – 30
12 – 21
6 – 12
30 – 60
15 – 24
60 – 90
30 – 36
30 – 36
where SFM = surface feet per minute
= cutting speed
RPM = spindle speed (revs per minute)
D = diameter of workpiece (inches)
where CS = cutting speed in meters/minute
D = diameter of workpiece (mm)
RPM (1”)
RPM
(10mm)
300 – 400
300 – 400
160 – 280
80 – 160
400 – 800
200 – 300
800–1200
400 – 480
400 – 480
750 – 950
750 – 50
350 – 650
190 – 350
950–1900
450 – 750
1900–2500
950–1150
950–1150
Screw
Cutting
(ft/min)
35
25
20
20
50
25
50
50
50
Coolant/
Lubricant
Oil
None
Oil
Oil
None
None
Paraffin
None
Oil
The above figures apply for dry cutting using HSS cutters. With coolant/lubricant, speeds
can be increased by 25-50%
Speeds for carbide-tipped bits can be 2 to 3 times the speeds for HSS bits.
The first number applies for heavy, roughing cuts, and the second number for fine finishing
cuts.
Speeds for parting off should be about half (1/2) to a quarter (1/4) that used for straight
turning. Feeds should be light but continuous.
Feed Rate:
The feed rate is usually expressed in terms of inches per rev (mm per rev).
For finishing, use a fine feed, 0,004” to 0,006” per revolution = 0,1 to 0,15mm per
revolution.
For finishing cuts on mild steel reduce the speed, and use very sharp round nose tool.
Depth of Cut:
General machining practice is to use depth of cut up to 5 times the rate of feed for
roughing.
3
3.
5 December 2010
PARTING OFF
Parting is the process of cutting off a piece of stock while it is being held in the lathe chuck
or collet. This process uses a specially shaped tool bit with a cutting edge similar to that of
a square-nosed tool bit. When parting, use plenty of coolant, such as a sulfurized cutting
oil (machine cast iron dry). Parting tools normally have a 5° side rake and no back rake
angles. The blades are sharpened by grinding the ends only. Parting is also used to cut off
stock, such as tubing, that is impractical to saw off with a power hacksaw.
Parting is also used to cut off work after other machining operations have been completed.
Parting tools can be of the forged type, inserted blade type, or ground from a standard tool
blank. In order for the tool to have maximum strength, the length of the cutting portion of
the blade should extend only enough to be slightly longer than half of the workpiece
diameter (able to reach the center of the work). Never attempt to part while the work is
mounted between centres.
Work that is to be parted should be held rigidly in a chuck or collet, with the area to be
parted as close to the holding device as possible. Always make the parting cut at a right
angle to the centerline of the work. Feed the tool bit into the revolving work with the cross
slide until the tool completely severs the work. Speeds for parting should be about half
that used for straight turning. Feeds should be light but continuous. If chatter occurs,
decrease the feed and speed, and check for loose lathe parts or a loose setup. The parting
tool should be positioned at center height unless cutting a piece that is over 25mm thick.
Thick pieces should have the cutting tool just slightly above center to account for the
stronger torque involved in parting. The length of the portion to be cut off can be
measured by using the micrometer carriage stop or by using layout lines scribed on the
workpiece. Always have the carriage locked down to the bed to reduce vibration and
chatter. Never try to catch the cutoff part in the hand; it will be hot and could burn.
The main requirements for successful parting are:
that the lathe mandrel bearings and slides be in good condition and well-adjusted,
that the tool be as rigid as possible with minimum tool overhang,
that parting should be done as near the chuck jaws as possible,
that adequate lubrication should get to the blade and cutting edge,
that the blade shape should encourage chip clearance and straight cutting (narrower at
the back than at the front), with a top-rake less than that normally used on a turning
tool for the same material,
that the turning speed is approximately one half of that normally used for ordinary
turning on the same material,
that the saddle is locked to the bed whilst parting,
that the tool should be at 90 degrees to the workpiece so it is not deflected to one side
or the other as the cut progresses,
that the tool is set exactly at centre height (slightly below for a front-mounted tool), and
that the feed is performed slowly by hand.
Ultimately, parting off should be performed using a rear tool-post, as designed by George
Thomas.
If the selected speed gives rise to chatter, then reduce the speed until chatter is eliminated.
Good quality leaded FCMS can be worked at higher speeds than for BMS. As the speed
for parting is determined by the outside diameter, it often pays to increase the speed
progressively as the diameter is reduced (for large diameters).
4
4.
5 December 2010
BORING
Boring provides a method to machine accurate holes which are truly parallel and of a size
for which there is no reamer available. The preferred setup consists of a boring bar with
inserted HSS bit mounted in a turret on the rear toolpost. The reason is that this position
offers the most rigid mounting and the tool can be adjusted for the minimum overhang
necessary to complete the job. Small holes are dealt with by one-piece boring tools held in
the same turret, or in the 4-way tool turret.
The accuracy of the bore is dependent upon the accuracy of the machine - in this case
particular attention should be paid to wear of the lathe bed, alignment of headstock spindle,
and correct adjustment of the carriage gib strips. If the lathe can turn parallel then it will
be able to bore a parallel hole. However, work mounted on the boring table and bored with
a between-centres boring bar will always produce a parallel bore - it might not be in the
right place or parallel with a datum surface of the work but the bore will be true.
The shape of the boring bit should offer adequate front clearance otherwise the tool will
rub and form a bell-mouth hole. Side and back clearances are similar to a knife tool.
There should be a slight negative approach angle to the tool bit so that facing of the bottom
of a blind hole is possible. It is important that large positive approach angles, and largeradius round-nosed bits be avoided, as these tool shapes tend to deflect the tool away from
the work - again leading to bell-mouth holes.
With a boring tool set up to cut on the nearside of the bore, it will be found that another
fine cut will be taken as the tool is withdrawn from the bore. If there is any amount of flex
in the tool, re-entering and withdrawing the tool again will produce yet more fine cuts. For
this reason it is tricky to measure the progress of the boring operation and interpretation of
the readings of the micrometer collar requires some care. The best way of boring to a dead
size is to first make up a plug gauge, accurately turned beforehand to the correct diameter.
The gauge should incorporate various steps in diameter by which progress may be
assessed. A typical gauge for a 1" diameter hole would consist of 3 steps, the first 0.01"
undersize, the second 0.002" undersize, and the third exactly 1.000" diameter. Calipers
would be used to assess the hole size until the point where the first step will enter the bore;
the experienced machinist will then be able to gauge how much more needs to come off to
reach the 0.002" step - the less experienced would do well to take 0.001" cuts until the
second step enters the bore - at which point you will know there is less than 0.001" cut to
come off. Fine shavings can then be taken until the desired fit on the 1.000" portion is
achieved.
The same speeds recommended for straight turning should be used for straight boring.
Feeds for boring should be considerably smaller than feeds used for straight turning
because there is less rigidity in the setup. Decrease the depth of cut for each pass of the
tool bit for the same reason. It is often advisable to feed the cutter bit into the hole to the
desired depth and then reverse the feed and let the cutter bit move out of the hole without
changing the depth of feed. It is also good practice to take a free cut every several passes
to help eliminate bell mouthing of the workpiece. This practice will correct any
irregularities caused by the bit or boring tool bar springing because of the pressure applied
to the bit.
5
5.
THREAD SPECIFICATIONS
5.1
ISO Metric Thread Specifications:
5 December 2010
H = 0.866 x P
H/4 = 0.216 x P
H/8 = 0.108 x P
3/8 H = 0.325 x P
5/8 H = 0.541 x P
The IS0 Metric thread has a 60° included angle and a crest width that is 0,125 (1/8)
times the pitch, and the flat on the root of the thread is wider than the crest. The
root width of the ISO Metric thread is 0,250 (1/4) times the pitch. The (optional)
root radius is 0,1443 times the pitch.
Depth of thread = 0,6134P (for screws), where P = pitch
Core diameter = D – 1,227P (for screws), where D = nominal screw diameter
Depth of thread = 0,541P (for nuts)
Minor diameter = D–1,082P (for nuts)
Spark plug threads (metric) have an included angle of 60° with a crest and root
width that are 0,125 times the depth.
6
5.2
5 December 2010
Whitworth (BSW/BSF/BSP/ME/B.S Conduit) Thread Specifications:
Included angle of 55°, and root/crest widths that are 0,167 times the pitch (where
pitch = 1/tpi). The root/crest radius is 0,137 times the pitch. The Whitworth form,
therefore, is truncated by radii at root and crest (of value 0,16 times the pitch).
(The basic triangle height is 0,96 x P, whereas the thread depth is only 0,64 x P).
Depth of thread = 0,64P (inches) (for screws)
Core diameter = D – 1,28P (inches)
Minor diameter = D – 1,2P (for nuts)
For 40 tpi ME, thread height = 0,016”, core diameter = D – 0,032”
For 32 tpi ME, thread height = 0,020”, core diameter = D – 0,040”
5.3
BA (British Association) Thread Specifications:
Included angle of 47,5°, and root/crest widths that are 0,236P (where pitch = P =
1/tpi). The root/crest radius is 0,18 times the pitch – very heavily rounded at both
root and crest. Both the depth of thread and flank height for a given pitch are less
than for the Whitworth form. The root/crest truncation amounts to 0,268 times the
pitch.
Depth of thread = 0,6P (inches).
Pitch = 0,9N, where N = BA number – rounded off to nearest 0,01mm
Core diameter = D – 1,2P
Diameter of BA screw = D = 6P1,2, where P = pitch
7
5.4
5 December 2010
Unified (UNC & UNF) Thread Specifications:
The Unified thread has a 60° included angle and a crest width that is 0,125 (1/8)
times the pitch, and the flat on the root of the thread is a little wider than the crest.
Depth of thread = 0,6134P (for screws), where P = pitch
Core diameter = D – 1,227P (for screws), where D = nominal screw diameter
Flat at crest = 0,125P (for screws)
Minor diameter = D–1,082P (for nuts)
Flat at root = 0,125P (for nuts)
5.5
British Cycle (BSC) Thread Specifications:
Included angle of 60°, and root/crest widths that are 0,192 times the pitch (where
pitch = 1/tpi). The root/crest radius is 0,167 times the pitch. This form is also
truncated by radii at root and crest (of value 0,167 times the pitch), similar to the
Whitworth form.
5.6
British Standard Brass (BSB) Specifications:
This standard has a constant pitch equivalent to 26 tpi. Included angle of 55°, and
roots/crests that are 0,167 times the pitch (where pitch = 1/tpi). The root/crest
radius is 0,137 times the pitch.
Minor diameter = D – 1,2P (for nuts)
8
5.7
5 December 2010
ACME Thread Specifications:
The British & American standards are virtually identical. Included angle of 29°,
and basic thread height is P/2. Total thread height = P/2 + ½ the allowance
(allowance = 0.020” for < 10 tpi, and 0.010” for finer threads). The basic thread
thickness = P/2. The width of the flat crest = 0.3707P, and the width of the flat root
= 0.3707P – 0.259 x allowance.
For an 8 tpi ACME thread:
P = 1/8 = 0.125”
Total thread height = 0.0725”
Width of crest = 0.0463”
Basic thread height = P/2 = 0.0625”
Basic thread thickness = 0.0625”
Width of root = 0.0411”
Note that there is also a trapezoidal Metric thread.
5.8
Worm Thread Specifications:
Worm threads are used in worm gearing for the transmission of power between
shafts at right angles to each other. Consequently, worm threads differ on several
basic points from ACME threads; the principal difference being the angle between
the flanks of the thread which becomes significant as the helix angle increases. The
angle of the flanks of the worm thread is referred to as the “pressure angle” (1/2 of
the included angle). Note that a worm thread to mesh with a gear having a pressure
angle of 20 degrees will have an included angle of 40 degrees.
9
5 December 2010
A 29-degree worm thread (for a 14½ degree pressure angle gear) differs from the
ACME thread in three areas:
Depth of thread
Width of top of the tooth
Width of the bottom of the tooth
P = Pitch = 1/tpi = π/DP
Whole Depth of thread = 0,6866P
Working depth of thread = 0,6366P
Width of flat crest = 0,335P
Width of flat root = 0,31P = 0,31 x π/DP
Distance from crest to pitch line = A = 0,3184P = 1/DP
(Addendum)
Pitch diameter of worm = OD – 2A
Outside diameter of worm = OD = pitch diameter + 2A
Lead of worm = P x n (n = number of starts)
Lead Angle of worm = arc tan{
Lead of worm
}
Circumference of pitch circle
= arc tan{
nxP
}
(π x (OD – 2A)
= arc tan{
n x π/DP
}
(π x (OD – 2/DP)
= arc tan{
1
(n x DP x OD) – 2
}
Example: For a single start 20DP worm with a pressure angle of 14½º and an
OD of 0.75”,
Lead Angle
=
arc tan{
1
}
(DP x OD) – 2
=
arc tan{
1
}
(20 x 0.75) – 2
4.40º = 4º23’
=
The lead angle is the angle of thread with line at right angles to the worm axis,
and is also sometimes called the “gashing angle”. This is also the angle at
which the teeth in the worm wheel (gear) need to be gashed (roughed out) to
ensure that the worm axis will be exactly perpendicular to the axis of the worm
wheel.
10
5 December 2010
Gashing Angles for Single Start Worm Threads
TPI
DP
Outside Diameter of Worm (OD)
5
12.73
11.46
10.18
10
9.545
9
8
7.636
7
6.364
6
5.727
5.091
5
4
40
36
32
30
24
20
18
16
/8”
2º29’
2º47’
3º10’
3º14’
3º24’
3º39’
4º10’
4º23’
4º52’
5º26’
5º50”
6º10’
7º07’
7º17’
9º41’
¾”
2º02”
2º17’
2º36’
2º39’
2º47’
2º58’
3º23’
3º34’
3º56’
4º23’
4º42’
4º58’
5º42’
5º50’
7º40
7
/8”
1º44’
1º56’
2º12’
2º14’
2º21’
2º31’
2º51’
3º00’
3º19’
3º41’
3º56’
4º09’
4º45’
4º52’
6º20’
1”
1º30”
1º41’
1º54’
1º56’
2º02’
2º10’
2º28’
2º36’
2º51’
3º10’
3º23’
3º34’
4º05’
4º10’
5º24’
1 1/8”
1º20’
1º29’
1º41’
1º43’
1º48’
1º55’
2º10’
2º17’
2º31
2º47’
2º58’
3º08’
3º34’
3º39’
4º42’
1 ¼”
1º11’
1º20’
1º30’
1º32’
1º36’
1º43’
1º56’
2º02’
2º14’
2º29’
2º39’
2º47’
3º10’
3º14’
4º10’
1 3/8”
1º05’
1º12’
1º21’
1º23’
1º27’
1º33’
1º45’
1º50’
2º01’
2º14’
2º23’
2º31’
2º51’
2º55’
3º44’
1 ½”
0º59’
1º06’
1º14’
1º16’
1º20’
1º25’
1º36’
1º41’
1º50’
2º02’
2º10’
2º17’
2º36’
2º39’
3º23’
1 5/8”
0º54’
1º00’
1º08’
1º10’
1º13’
1º18’
1º28’
1º32’
1º41’
1º52’
2º00’
2º06’
2º23’
2º26’
3º06’
Note that the helix angle of the worm is the angle of the thread measured along the
axis of the worm. The lead angle is, therefore, 90º minus the helix angle.
The worm thread tool has an included angle of 29º for a standard pressure angle of
14½º. The width of the tool at the end is obtained as follows:
Width of tool = 0.31 x Circular Pitch = 0.31 x π/DP
For a 20 DP worm, width of tool = 0.31 x 3.1416/20 =0.0487” (1.237mm)
11
5.9
DIA.
Sizes
1/8”
5/32”
3/16”
7/32”
¼”
9/32”
5/16”
3/8”
7/16”
½”
9/16”
5/8”
11/16”
¾”
7/8”
15/16”
1”
1.1/8”
DIA.
Sizes
1/8”
5/32”
3/16”
7/32”
¼”
5/16”
3/8”
7/16”
½”
9/16”
5/8”
¾”
7/8”
1”
1.1/8”
5 December 2010
Tap Drill Sizes
BRITISH STANDARD WHITWORTH FORM THREADS (55º angle)
BSW
BSF
BSB
BSP
MODEL ENG
TPI Drill TPI Drill TPI Drill TPI
Drill
TPI
Drill
(mm)
(mm)
(mm)
(mm)
(mm)
40
2.6
28
8.8
40
2.6
32
3.2
40
3.3
24
3.7
32
4.0
32, 40
4.0, 4.1
24
4.5
26
4.7
40
4.9
20
5.1
26
5.4
26
5.4
19
11.8
32, 40
5.5, 5.6
20
5.8
26
6.2
26
5.8
32, 40
6.4, 6.5
18
6.5
22
6.8
26
7.0
32, 40
7.1, 7.3
16
7.9
20
8.3
26
8.5
19
15.3
14
9.3
18
9.8
26
10.0
12
10.5
16
11.2
26
11.5
14
19.0
12
12.0
16
12.7
26
13.0
11
13.5
14
14.0
26
14.8
14
21.0
11
15.0
14
15.8
26
16.5
10
16.5
12
17.0
26
18.0
14
24.5
9
19.3
11
20.0
26
21.0
14
28.0
9
20.8
11
21.5
26
8
22.0
10
23.0
26
24.2
11
31.0
7
25.0
9
26.0
26
UNC
TPI Drill
(mm)
20
18
16
14
13
12
11
10
9
8
7
5.1
6.6
8.0
9.5
11.0
12.2
13.5
16.5
19.5
22.0
25.0
AMERICAN NATIONAL FORM THREADS (60º angle)
UNF
NPT
UNS
DIA.
TPI Drill TPI Drill
TPI
Drill
Size
(mm)
(mm)
(mm)
#
27
8.5
40
2.6
0
32, 40
3.2, 3.3
1
32, 40
4.0, 4.0
2
24, 32
4.5, 4.8
3
28
5.5
18
11.0
24, 32
5.3, 5.6
4
24
7.0
20, 32
6.7, 7.2
5
24
8.5
18
14.5
20
8.3
6
20
10.0
24
10.0
8
20
11.5
14
18.0
12, 24
10.5, 11.5
10
18
13.0
12
18
14.5
12
13.9
16
17.5
14
23.0
12
16.7
14
20.5
12
20.2
12
23.0 11.5 29.0
14
23.5
12
26.5
BSCon
TPI Drill
(mm)
18
11.5
18
14.2
16
16
17.5
20.6
16
23.8
UNC
TPI Drill
(mm)
64
56
48
40
40
32
32
24
24
1.55
1.80
2.1
2.3
2.6
2.8
3.4
3.8
4.5
UNF
TPI Drill
(mm)
80
1.25
72
1.55
64
1.85
56
2.15
48
2.4
44
2.7
40
2.9
36
3.5
32
4.1
28
4.6
12
5 December 2010
METRIC FORM THREADS (60º angle)
DIA
Sizes
(mm)
1.0
1.2
1.3
1.4
1.5
1.6
1.7
1.8
1.9
2.0
2.2
2.5
3.0
3.5
4.0
4.5
5.0
6.0
7.0
8.0
9.0
COARSE
Pitch
Drill
(mm)
0.25
0.8
0.25
1.0
0.28
1.05
0.3
1.1
0.3
1.2
0.35
1.3
0.35
1.35
0.35
1.5
0.39
1.55
0.4
1.65
0.45
1.8
0.45
2.1
0.5
2.5
0.6
2.9
0.7
3.3
0.75
3.8
0.8
4.2
1.0
5.0
1.0
6.0
1.25
6.8
1.25
7.8
METRIC FORM THREADS (60º angle)
FINE
Pitch
Drill
(mm)
(=14BA)
(=12BA)
(=11BA)
(=10BA)
(=9BA)
0.5
0.75
0.75
1.0
1.0
DIA
Sizes
(mm)
10
11
12
12
12
14
14
16
16
18
20
22
24
COARSE
Pitch
Drill
(mm)
1.5
8.5
1.5
9.5
1.75
10.2
2.0
12.0
2.0
14.0
2.5
2.5
2.5
3.0
15.5
17.5
19.5
21.0
FINE
Pitch
Drill
(mm)
1.0
9.0
1.0
10.0
1.0
11.0
1.25
10.8
1.5
10.5
1.25
12.8
1.5
12.5
1.0
15.0
1.5
14.5
1.5
16.5
1.5
18.5
2.0
20.0
2.0
22.0
4.5
5.3
6.3
7.0
8.0
Spark plug taps = M10x1, M12x1.25, M14x1.25, M18x1.5
Conduit taps = M16x1.5, M20x1.5, M25x1.5, M32x1.5, M50x1.5
BRITISH ASSOCIATION THREADS (47½ º)
No.
0
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
Dia.
(mm)
6.0
5.3
4.7
4.1
3.6
3.2
2.8
2.5
2.2
1.9
1.7
1.5
1.3
1.2
1.0
0.9
0.79
Pitch
(mm)
1.0
0.9
0.81
0.73
0.66
0.59
0.53
0.48
0.43
0.39
0.35
0.31
0.28
0.25
0.23
0.21
0.19
TPI
25.4
28.2
31.4
34.8
38.5
43.0
47.9
52.9
59.1
65.1
72.6
81.9
90.9
102.0
109.9
120.5
133.3
Drill
(mm)
5.1
4.5
4.0
3.4
3.0
2.7
2.4
2.1
1.85
1.6
1.4
1.25
1.1
1.0
0.8
0.75
0.65
BRITISH STD CYCLE (60º)
Sizes
TPI
1/8”
5/32”
3/16”
¼”
5/16”
3/8”
7/16”
½”
9/16”
9/16”
5/8”
5/8”
¾”
¾”
40
32
32
26
26
26
26
26
20
26
20
26
20
26
Drill
(mm)
2.7
3.3
4.1
5.6
7.2
8.7
10.3
11.9
13.1
13.5
14.5
15.0
17.8
18.2
13
5 December 2010
6.
SCREWCUTTING IN THE LATHE
6.1
Topslide Set-over Technique:
The set-over technique involves rotating the topslide to half the included thread
angle (say, 30° for a 60° thread) thus leaving the right hand cutting edge of the tool
(i.e., the trailing edge for normal RH threads) parallel to the right hand land of the
thread. In this situation the cut is put on exclusively with the topslide and the right
hand side of the tool does no cutting. This enables a top rake of about 7° to be
given the left hand cutting edge greatly improving the cutting action and hence the
finish on the work. This amount of top rake will have no significant effect on
thread form. It will be noticeable in using this method that the chips come away as
a clean curl of cut metal and that no burrs are thrown up onto the peaks of the
thread. A further modification involves setting the topslide over to about 1° less
than half thread angle, such that the trailing edge of the tool just shaves the right
hand land of the thread. This corrects a problem sometimes seen with drawn
phosphor bronze rod or stainless steel where scoring can appear on the right hand
land. Another solution to the problem is to apply the very last thou or two of cut
with the cross-slide (feed straight in) rather than the topslide. When feeding in at
an angle with the topslide, the movement indicated on the micrometer dial does not
represent the actual depth of cut. The true depth of cut can either be calculated or
read off a table.
OA = Thread depth
O
OB = Topslide feed
1/x = cos30deg
x
30deg
x = 1/cos30deg
A
B
AB is parallel to workpiece
The following steps apply:
First, establish the true depth of cut required.
Using the cross-slide, run the tool tip up to the work and zero it's micrometer dial.
Move the tool to the right of the work and wind the tool point in to the required
depth of cut using the cross-slide, then set the topslide micrometer dial to zero.
Back-out the tool point using the topslide only, move the tool to the left (back over
the work) and move the tool point in to just touch the work again.
Reset the cross-slide micrometer dial to zero.
Now, all cuts can be put on with the topslide, and when the dial reads zero you
know the correct depth of cut has been achieved. The cross-slide is only used to
retract the tool from the work for traversing, and returned to its zero setting ready
for the next cut.
14
5 December 2010
For Metric screwcutting, angle the topslide 30° from perpendicular to the workpiece
(equivalent to 60° from parallel with the workpiece). This is half the included angle of
the lathe cutting tool for metric threads. The correct depth of cut for the thread pitch
must be multiplied by a factor of 1,155, since the thread depth is achieved by
advancing the topslide feedscrew. The multiplication factor is derived from basic
trigonometry – the thread depth perpendicular to the workpiece translates to the
topslide feedscrew movement at 30° multiplied by cosine 30° (cos 30° = 0,866, and
1/cos 30° = 1,155).
For screwcutting BSW/BSF threads, angle the topslide 27,5° from perpendicular to the
workpiece (equivalent to 62,5° from parallel with the workpiece). This is half the
included angle of the lathe cutting tool for BSW/BSF threads. The correct depth of cut
for the thread pitch must be multiplied by a factor of 1,1274 (1/cos 27,5° = 1,1274).
Advance the topslide feedscrew by only 0,1 to 0,15mm each cycle.
6.2
Alternative to Topslide Setover:
As an alternative to setting the topslide over by half the included angle of the
thread, the topslide can be positioned parallel to the workpiece. The topslide
feedscrew must then be advanced by about half the amount that the cross slide
feedscrew is advanced (tan 30° ~ 0,5). This is the method preferred by M Cleeve.
6.3
Thread Depth:
For Metric screws, thread depth = d = pitch (mm) x 0,6134 (for rounded roots)
= pitch (mm) x 0,72 (for sharp roots)
For Metric nuts, thread depth = d = pitch (mm) x 0,5418 (for rounded roots)
For BSW/BSF screws, thread depth = d = pitch (inches) x 0,64 (for rounded roots)
= pitch (inches) x 0,8 (for sharp roots)
For BSW/BSF nuts, thread depth = d = pitch (inches) x 0,6 (for rounded roots)
Example 1: A Metric screw thread of 1,75mm pitch:
Thread depth = 1,75 x 0,6134 = 1,07mm for rounded roots
= 1,75 x 0,72 = 1,25mm for sharp roots
For a topslide setover of 30°, the foregoing depths must be multiplied by 1,155
to reflect the topslide feedscrew advance necessary. This results in a topslide
feedscrew advance of 1,25mm (1,45mm) for an actual thread depth of 1,07mm
(1,25mm).
Example 2: A Metric screw thread of 0,75mm pitch:
Thread depth
= 0,75 x 0,6134 = 0,460mm for rounded roots
= 0,75 x 0,72 = 0,54mm for sharp roots
15
5 December 2010
For a topslide setover of 30°, the foregoing depths must be multiplied by 1,155
to reflect the topslide feedscrew advance necessary. For example, 0,46 x 1,155
= 0,53mm topslide screw advance.
6.4
Tool Setting:
The thread-cutter bit must be positioned so that the centerline of the thread angle
ground on the bit is exactly perpendicular to the axis of the workpiece. The thread
setting gauge is placed against the workpiece and the cutter bit is adjusted on the
tool post so that its point fits snugly in the 60° (or 55°) angle notch of the gauge
6.5
Speeds and Lubrication:
As a rough guide, when threading ordinary mild steel with HSS tools, initially form
the threads at a speed of about one quarter (1/4) of those used to turn the diameter,
then reduce to about one sixth (1/6) for finishing cuts.
Soluble oil and water can be used for the initial stages of threading steels, but can
be substituted with neat cutting oil when taking half a thou (0,01mm) finishing cuts
at painfully slow speeds.
6.6
Method 1 for Metric Pitches:
For Metric pitches with an Imperial leadscrew thread, such as the Myford 8 tpi, it is
advisable to keep the carriage feed half nuts engaged throughout the process. For
short lengths of thread turn the lathe spindle by hand. The spindle (and leadscrew)
can be turned by hand in the forward direction as well as the reverse direction. Do
NOT disengage or try to reverse the leadscrew drive by using the tumbler reverse
mechanism – the alignment will be lost.
Take a light trial cut and check that the threads are of the correct pitch using a
metric screw pitch gauge. At the end of this trial cut, and any cut when metric
threading, turn off the lathe and back out the tool bit from the workpiece without
disengaging the half-nut-lever. Never disengage the lever until the metric thread is
cut to the proper pitch diameter, or the tool bit will have to be realigned and set for
chasing into the thread. After backing the tool bit out from the workpiece, traverse
the tool bit back to the starting point by reversing the lathe spindle direction while
leaving the half-nut lever engaged. If the correct pitch is being cut, continue to
machine the thread to the desired depth.
Note: If the tool bit needs to be realigned and chased into the thread due to
disengagement of the half-nut lever or having to remove the piece and start again,
then the lathe must be reset for threading. Start the lathe and with the tool bit clear
of the workpiece engage the lever. Allow the carriage to travel until the tool bit is
opposite any portion of the unfinished thread; and then turn off the lathe, leaving
the half nuts engaged. Now the tool bit can be set back into a thread groove by
advancing the cross slide and reference. Restart the lathe, and the tool bit should
follow the groove that was previously cut, as long as the half-nut lever stays
engaged.
16
6.7
5 December 2010
Method 2 for Metric Pitches:
An alternative method is to mark the top of the chuck as well as the leadscrew
handwheel when the half nuts are engaged at the beginning of the thread. Then
form a dead stop at the right hand end using the tailstock or a clamp on the lathe
bed. This is to index the starting position when repeating the threading operation at
deeper and deeper feeds of the lathe tool. When the tool reaches the left hand end
of the workpiece, disengage the half nuts and traverse the carriage by using the
handwheel back to the right hand side stop. Once again, turn the spindle by hand
until both marks coincide, and then engage the half nuts.
6.8
Screwcutting Change Wheels:
For Imperial pitches:
Drivers =
Driven
Leadscrew TPI
Required TPI
For Metric pitches using an 8 tpi leadscrew:
Drivers =
Driven
4P x 50_
5
127
Pitch (mm) = P =
where P = pitch (mm)
Drivers x 127 x 5
Driven
50 4
=
Drivers x 127
Driven 40
Examples:
1.
For a pitch of 1,75mm,
30 – A – 38
35 – 50
(A = Any gear)
Pitch (mm) = 30/38 x 35/50 x 127/40 = 1,7546 mm
Or, for the same pitch,
30 – A – 35
45 – 70
Pitch (mm) = 30/35 x 45/70 x 127/40 = 1,74949 mm
2.
For a pitch of 0,75mm,
40 – 38
25 – 65
35 – 60
Pitch (mm) = 40/38 x 35/60 x 25/65 x 127/40 = 0,74983 mm
Or, for the same pitch,
30 – 60
20 – 55
65 – 50
Pitch (mm) = 30/60 x 65/50 x 20/55 x 127/40 = 0,7504545 mm
17
5 December 2010
SCREWCUTTING CHANGE GEAR TABLES FOR MYFORD SUPER 7
(WITH 8 T.P.I LEADSCREW)
IMPERIAL & UNC/F THREADS
T.P.I
4
5
6
7
8
9
10
11
12
14
16
18
19
20
22
24
25
26
28
32
36
40
44
48
52
54
60
64
72
80
88
96
104
112
120
4.456
6.366
8.913
12.73
Feed /Rev
Driver
0.125”
0.1111”
0.100”
0.0909”
0.0833”
0.0714”
0.0625”
0.0556”
0.0526”
0.0500”
0.0455”
0.0417”
0.0400”
0.0385”
0.0357”
0.0313”
0.0278”
0.025”
0.0227”
0.0208”
0.0192”
0.0185”
0.0167”
0.0156”
0.0139”
0.0125”
0.0114”
0.0104”
0.0096”
0.0089”
0.0083”
0.0058”
0.0043”
0.0037
14 DP
20 DP
28 DP
40 DP
40
40
40
40
35
40
40
40
40
20
20
20
40
20
20
20
40
20
30
30
30
30
20
20
20
20
20
35
25
25
30
30
20
25
20
20
20
20
45
40
A
20
First Stud
Driven Driver
A
A
A
A
A
A
A
A
20
40
A(60)
A(60)
A(60)
A(50)
A(70)
A(70)
A(70)
38
20
A(70)
A(70)
A(70)
50
30
A(70)
35
20
40
20
45
20
50
20
55
30
60
35
50
25
45
20
50
25
40
20
50
30
50
35
40
25
40
20
50
30
50
30
50
30
55
25
60
25
65
25
30
A
35
A
A
A
35
A
Second Stud
Driven Driver
A
A
A(55)
A
A(45)
A(50)
A(55)
A(55)
A(55)
A(50)
A(45)
A(55)
A(55)
A(55)
60
30
45
20
70
30
55
20
60
25
60
25
60
20
60
25
60
20
65
20
70
20
A
60
A
55
A
45
A
55
Leadscrew
20
25
30
35
70
45
50
55
60
35
40
45
50
50
55
60
75
65
60
60
60
60
60
70
65
60
75
70
60
75
75
75
65
70
75
65
75
75
50
50
50
50
18
5 December 2010
SCREWCUTTING CHANGE GEAR TABLES FOR MYFORD SUPER 7
(WITH 8 T.P.I LEADSCREW)
METRIC THREADS
Metric
Pitch
0.3
0.4
0.5
0.5
0.5
0.6
0.7
0.7
0.75
0.75
0.8
1.0
1.0
1.0
1.0
1.25
1.5
1.5
1.75
2.0
2.0
2.0
2.5
2.5
2.75
2.75
3.0
TPI
Driver
84.7
63.5
50.8
35
25
30
20
21
20
20
30
40
30
20
25
35
65
30
45
20
21
30
45
20
30
35
40
65
40
40
42.3
36.3
33.9
31.7
25.4
20.3
16.9
14.5
12.7
10.2
9.2
8.5
First Stud
Driven Driver
38
25
50
45
60
45
60
65
50
45
40
30
40
30
50
45
38
35
60
65
A
A
A
A
50
45
30
20
A
A
55
50
A
A
50
45
A
A
A
A
50
55
A
A
A
A
60
65
A
A
60
65
A
A
Second Stud
Driven Driver
65
20
55
20
55
25
50
20
40
20
65
40
75
55
35
20
60
25
50
20
55
45
55
45
40
30
50
20
25
21
40
25
50
65
A
A
35
45
55
50
A
A
25
21
40
45
A
A
A
A
A
A
50
65
Lead
Screw
75
65
65
55
60
75
50
70
65
55
65
65
75
55
40
65
55
40
70
65
35
40
50
55
75
50
55
Error
= 1 in
-4446
-1144
-1144
+3300
-1144
-466
-3430
-4446
+2200
-1144
-1144
+8000
+1650
-1144
+1650
-3430
-1144
-233
+8000
+660
+600
+600
+1650
BA THREADS
BA
0
1
2
3
4
5
6
7
8
9
10
Metric
Pitch
1.0
0.9
0.81
0.73
0.65
0.59
0.53
0.48
0.43
0.39
0.35
TPI
Driver
25.4
28.2
31.4
34.8
38.7
43.0
47.8
53.1
59.0
65.6
72.8
35
20
20
20
20
20
20
20
20
20
20
First Stud
Driven Driver
50
45
38
A
50
A
35
A
35
A
35
25
50
A
35
20
38
20
40
25
35
20
Second Stud
Driven Driver
40
30
A
35
A
35
A
20
A
20
55
50
A
25
38
30
50
45
60
38
40
25
Lead
Screw
75
65
55
50
55
70
60
60
70
65
65
TPI
25.4
28.2
31.4
35.0
38.5
43.1
48.0
53.2
59.1
65.7
72.8
19
7.
5 December 2010
REAMING ON THE LATHE
Reamers are used to finish drilled holes or bores quickly and accurately to a specified
diameter. When a hole is to be reamed, it must first be drilled or bored less than the
finished size, depending upon the diameter of the hole, since the reamer is not designed to
remove much material. Standard reamers have a tolerance of H7 (always slightly
oversize).
Reaming Allowance for most materials (steel, cast iron, copper, brass, bronze, aluminium)
Bore Diameter:
Allowance:
3 - 5mm
0.1 – 0.2mm
5.1 – 10mm
0.2 – 0.3mm
10.1 – 20mm
0.3 – 0.5mm
20.1 - 30mm
0.5 – 0.9mm
Parallel machine reamers only cut on the bevel lead, and parallel hand reamers which have
both bevel and taper leads may cut on both. Note that in neither case do the lands on the
body do any cutting
Reaming with a Machine Reamer
The workpiece is mounted in a chuck at the headstock spindle and the reamer is supported
by the tailstock. For the most accurate jobs in the lathe it is preferable to use a machine
reamer with a taper shank installed in the tailstock (of necessity the lathe must be
accurately aligned). Holding a reamer in a drill chuck of dubious accuracy will likely lead
to oversize and tapered bores. A better option is to mount a dead centre in the tailstock and
locate this in the female centre at the rear of the reamer, and use the tailstock handwheel to
push it through the work; a hand wrench or lathe dog attached to the shank of the reamer
will stop it rotating as it enters the bore.
The lathe speed for machine reaming should be approximately one-half (1/2) that used for
drilling. The reamer should be pushed through the work fairly quickly. This will reduce
the incidence of ridges forming in the bore. Where possible, the whole of the working part
of the reamer should enter the bore and then be backed out at the same rate with the spindle
still turning. Never reverse the direction of rotation with a reamer in the bore.
Reaming with a Hand Reamer
The workpiece is mounted to the headstock spindle in a chuck and the headstock spindle is
locked after the piece is accurately setup. The hand reamer is mounted in an adjustable tap
and reamer wrench and supported with the tailstock centre. As the wrench is revolved by
hand, the hand reamer is fed into the hole simultaneously by turning the tailstock
handwheel.
The reamer should be withdrawn from the hole carefully, turning it in the same direction as
when reaming. Never turn a reamer backward. Use copious amounts of cutting fluid for
reaming. Never use power with a hand reamer or the work could be ruined.
20
8.
5 December 2010
FLYCUTTING
Flycutting is a process whereby a single point cutting tool is swept across the workpiece
forming a flat-machined face. There are some advantages to flycutting compared to the
other forms of milling. Firstly, the cutter is far easier to sharpen than a multi-tooth cutter
such as an endmill. Secondly, the cutting action is very easy, requires less power and puts
less strain on the lathe. In addition, large areas can be flycut leaving an attractive finish.
The drawbacks are that metal removal is actually slower than when using an endmill; cuts
must be fine (typically 10 thou or 0,25mm for a small lathe) and the surface, though
appearing perfectly flat, is probably less flat than the equivalent surface generated by an
endmill. On finishing cuts the depth can be reduced to 5 thou (0,125mm).
To face large surfaces with an endmill it is best to chamfer the corners off the 4 teeth, this
will leave a better finish - a bit like adding a chamfer to the corner of a knife tool. When
you compare the surfaces generated by each method, the endmill leaves a striped finish,
and the flycutter a smooth finish. The reason lies in the fact that, to get a flat surface by
flycutting, the slide travel must be at exactly 90° to the axis of the cutter, and in lathes the
cross-slide is usually set to turn slightly concave. The long sweeping arc of the flycutter
exaggerates any off-square angle and so it will cut concave. This concavity is very much
reduced with an endmill because of the much shorter cutting arc. The difference is visible
if the flycut surface is rubbed on a faceplate with a touch of marking blue on it, and may be
significant if the surface in question is (for example) the bolting face of a cylinder head.
Another way it shows up is when taking a cut across a large casting it may be found that
the trailing arc of the cutter will take a thou or so more off than the leading arc. For many
other applications this effect is not significant, but it is as well to be aware of it.
Cutter bits are best ground up from HSS; the interrupted cuts typical of flycutting are not
very kind to carbide-tipped tools and they will likely chip. Having said that, carbide tipped
cutters can be used on cast iron, and the incidence of broken tips is very low. For very
large castings, use a tool mounted in a holder bolted to the catch plate (or it can even be
mounted on the largest faceplate).
An improvement over the single point tool is to mount two tools 180° apart, with one tool
sweeping a fractionally wider arc, and the other cutting 10 thou (0,25mm) deeper. This
way, the speed of metal removal is virtually doubled. Commercial 'facing cutters' for the
mill are no more than multi-tooth flycutters, often using 3 or 4 inserted bits.
The recommended spindle speed for flycutting using HSS cutters is half (1/2) that for
normal turning, and is given by the following formula:
RPM = 4 x CS (ft/min)
Cutter dia (inch)
= 320 x CS (metre/min)
cutter dia (mm)
Where CS = cutting speed (= 40 ft/min for MS, ie half of 80 ft/min)
Example – for a 2” diameter HSS cutter on mild steel, the spindle speed should not exceed
80 - 100 rpm, for a depth of cut of 0,25mm.
21
9.
5 December 2010
KNURLING
The knurling operation is started by determining the location and length of the knurl, and
then setting the machine for knurling. A slow speed is needed with a medium feed.
Commonly, the speed is set to 60 to 80 RPM, while the feed is best from 0.015” to 0.030”
(0,4 mm to 0,8 mm) per revolution of the spindle. The knurling tool must be set in the tool
post with the axis of the knurling head at center height and the face of the knurls parallel
with the work surface. Check that the rollers move freely and are in good cutting
condition; then oil the knurling tool cutting wheels where they contact the workpiece.
Bring the cutting wheels (rollers) up to the surface of the work with approx. ½ of the face
of the roller in contact with the work.
If the face of the roller is placed in this manner, the initial pressure that is required to start
the knurl will be lessened and the knurl may cut smoother. Apply oil generously over the
area to be knurled. Start the lathe while forcing the knurls into the work about 0.010”
(0,25 mm). As the impression starts to form, engage the carriage feed lever. Observe the
knurl for a few revolutions and shut off the machine. Check to see that the knurl is
tracking properly, and that it is not on a “double track”.
Reset the tool if needed; otherwise, move the carriage and tool back to the starting point
and lightly bring the tool back into the previously knurled portion. The rollers will align
themselves with the knurled impressions. Force the knurling tool into the work to a depth
of about 1/64” (0,4 mm) and simultaneously engage the carriage to feed toward the
headstock. Observe the knurling action and allow the tool to knurl to within 1/32” (0,8
mm) of the desired end of cut, and disengage the feed. Hand feed to the point where only
one-half of the knurling wheel is off the work, change the feed direction toward the
tailstock and force the tool deeper into the work.
Engage the carriage feed and cut back to the starting point. Stop the lathe and check the
knurl for completeness. Never allow the knurling tool to feed entirely off the end of the
work, or it could cause damage to the work or lathe centers. The knurl is complete when
the diamond shape (or straight knurl) is fully developed. Excessive knurling after the knurl
has formed will wear off the full knurl and ruin the work diameter. Move the tool away
from the work and shut off the lathe. Clean the knurl with a brush and then remove any
burrs with a file.
For a clamp-type knurling tool, the tool must be aligned at right angles to the work with the
knurls positioned equally above and below the work. The cross-slide is advanced to the
position where the knurls are a short distance away from the vertical centre line of the
work. The tool clamp is then tightened, the work rotated and the cross-slide advanced to
the point where both knurls are aligned with the vertical centre line of the work. This will
force the teeth of the knurls into the work without putting undue strain on either the work
or the knurling tool.
Special Knurling Precautions
Never stop the carriage while the tool is in contact with the work and the work is still
revolving as this will cause wear rings on the work surface. Check the operation to ensure
that the knurling tool is not forcing the work from the centre hole. Keep the work and
knurling tool well oiled during the operation. Never allow a brush or rag to come between
the rollers and the work or the knurl will be ruined.
22
10.
5 December 2010
MILLING IN THE LATHE
Note that the following information applies to milling operations using the lathe. For
milling machines, speeds and feeds can be increased considerably.
10.1
Speeds for End Mills & Slot Drills
The recommended speeds for end mills and slot drills are derived from the following
formula:
Speed = RPM ~ 4 x CS(ft/min)
D (inch)
~
320 x CS(metre/min)
D (mm)
Where CS = cutting speed for different materials, and D = diameter of end mill/slot drill
Cutting speeds for slot milling should generally be less than for peripheral milling
(profiling), since slot drills have fewer teeth than end mills. Slot milling feed rates should
accordingly also be less than for end mills running at the same speed.
Material
Mild steel, Gunmetal
Cast iron, Bronze
Stainless steel, Monel
Brass
Aluminium Alloy, Tufnol
Average
CS (ft/min)
50 - 80
45 - 60
30 - 35
80 - 100
100 - 200
Average
RPM
CS (m/min)
(1/4”)
16 - 24
800-1200
14 - 18
700-900
9 - 11
480-560
26 - 30
1300-1600
30 - 60
1600-3200
RPM
(10mm)
500-800
450-550
300-350
800-1000
1000-2000
From the foregoing it will be seen that cutting speeds are about half that used for turning
operations. These speeds are for dry cutting. With appropriate lubrication and cooling,
the speeds can be increased.
10.2
Feed Rate
Feed (IPM inch/minute) = No. of teeth (T) x chipload or feed per tooth (FPT) x RPM
Material
Mild Steel
Cast Iron
Bronze
Stainless steel
Brass
Aluminium
FPT
0.001” – 0.003”
0.001” – 0.004”
0.001” – 0.005”
0.0005” – 0.002”
0.003” – 0.005”
0.002” – 0.008”
IPM@300rpm (3T)
0,9 – 2,7 ipm
0,9 – 3,6 ipm
0,9 – 4,5 ipm
0,5 – 1,8 ipm
2,7 – 4,5 ipm
1,8 – 7,2 ipm
IPM@600rpm (3T)
1,8 – 5,4 ipm
1,8 – 7,2 ipm
1,8 – 9,0 ipm
1,0 – 3,6 ipm
5,4 – 9,0 ipm
3,6 – 14,5 ipm
A chipload of 0.002” is considered good practice, although this may be a bit heavy for a
light milling machine and for milling in the lathe.
Typical figures being 3 ¾ in/min (95 mm/min) for a 4-flute end mill rotating at 300 rpm
(chipload 0,003”), but less than 1 ½ in/min (38 mm/min) for a 2-flute slot drill rotating at
the same speed (chipload of 0,0025”).
23
10.3
5 December 2010
Depth and Width of Cut
For profile milling, the depth of cut should be between D/2 to D, and the width of cut
D/4 (at a push D/2), where D is the diameter of the end mill.
For slot milling the depth of cut can generally be D/4 to D/2. The greater the depth, the
slower the speed (rpm) should be.
It is advisable to start with a reduced depth of cut to compensate for any shortcomings in
the rigidity of the lathe and workholding arrangements.
10.4
Direction of Cut:
The work must always be traversed into the cut, so that the work and the teeth which are
cutting, approach one another.
If the work is traversed in the wrong direction (climb-milling), i.e. such that the work and
the cutting teeth are going in the same direction, the cutter drags the work into itself,
tearing out large lumps as each edge contacts the work, and spoiling the finish due to the
uneven rate of material removal.
When cutting slots with a slot drill, the situation is not quite the same since the cut is
occurring at the end of the slot rather than at the sides, and provided that the feed is
steadily applied and the cutter is within the work, the feed can be in either direction.
However, if a slot drill or end mill cuts out through the side of the workpiece, the slow and
steady feed of the work must continue until the mill or drill is completely clear of the work,
otherwise there is a high risk of the work moving too far between the arrival of successive
teeth and too heavy a cut being imposed. This is also likely to break off the cutting edge or
chip the teeth of the tool.
10.5
Cutting Slots:
An end mill, which usually has four teeth, will always cut a slot wider than the diameter of
the cutter, and the harder the cutter is worked, the wider will be the slot. This does not
hold true for a 2-tooth slot drill.
24
5 December 2010
11.
MILLING (MACHINE)
11.1
Speeds for End Mills & Slot Drills
The recommended speeds for end mills and slot drills in a milling machine are derived
from the following formula:
Speed = RPM ~ 4 x CS(ft/min)
D (inch)
~
320 x CS(metre/min)
D (mm)
Where CS = cutting speed for different materials, and D = diameter of end mill/slot drill
Cutting speeds for slot milling should generally be less than for peripheral milling
(profiling), since slot drills have fewer teeth than end mills. Slot milling feed rates should
accordingly also be less than for end mills running at the same speed.
Material
Mild steel, Gunmetal
Cast iron, Bronze
Stainless steel, Monel
Brass
Aluminium Alloy
Average CS
(ft/min)
60 - 80
45 - 60
30 - 35
80 - 100
120 - 160
Average CS
(m/min)
18 - 26
14 - 18
9 - 11
26 - 30
35 - 48
RPM
RPM
RPM
(1/4”)
(10mm)
(12mm)
950-1300
650-850
500-650
700-950
480-650
380-500
480-560
300-350
250-300
1300-1600 850-1000
650-850
1900-2500 1300-1700 1000-1300
These speeds are for dry cutting using HSS cutters. With appropriate lubrication and
cooling, the speeds can be increased. For roughing cuts, use a slower speed. For finishing
cuts, use a higher speed. For deeper cuts use a slower speed. The colour of the chip is a
good indicator of cutting speed. When using an HSS cutter, the chips should never be
brown or blue. Straw-coloured chips indicate the optimum/maximum cutting speed for the
specific cutting conditions.
These speeds also apply for depths of cut and widths of cut of up to ¼ of cutter diameter.
11.2
Feed Rate
Feed (IPM inch/minute) = No. of teeth (T) x chipload or feed per tooth (FPT) x RPM
Material
FPT
Mild Steel
Cast Iron
Bronze
Stainless steel
Brass
Aluminium
0.001” – 0.003”
0.001” – 0.004”
0.001” – 0.005”
0.0005” – 0.002”
0.003” – 0.005”
0.002” – 0.008”
IPM@300rpm
(3T)
0,9 – 2,7 ipm
0,9 – 3,6 ipm
0,9 – 4,5 ipm
0,5 – 1,8 ipm
2,7 – 4,5 ipm
1,8 – 7,2 ipm
IPM@600rpm
(3T)
1,8 – 5,4 ipm
1,8 – 7,2 ipm
1,8 – 9,0 ipm
1,0 – 3,6 ipm
5,4 – 9,0 ipm
3,6 – 14,5 ipm
IPM@600rpm
(4T)
2,4 – 7,2 ipm
2,4 – 9,6 ipm
2,4 – 12,0 ipm
1,2 – 4,8 ipm
7,2 – 12,0 ipm
4,8 – 19,2 ipm
A chipload of 0.002” is considered good practice for mild steel.
Typical figures being 3¾ in/min (95 mm/min) for a 4-flute end mill rotating at 300 rpm
(chipload 0,003”), but less than 1½ in/min (38 mm/min) for a 2-flute slot drill rotating at
the same speed (chipload of 0,0025”).
25
5 December 2010
12.
GEARS & GEAR CUTTING
12.1
Gear Theory
A gear is a toothed wheel which, when meshed with other gears, transmits motion
from one part of a mechanism to another. Of the many different types of gears, the
most common is the spur gear which consists of a wheel having teeth cut around its
periphery parallel to the axis and is employed to transmit motion between parallel
shafts.
Diametral Pitch (DP) indicates the number of teeth per inch of pitch circle
diameter – a gear of 1-inch pitch circle diameter with 24 teeth would have a
diametral pitch of 24.
Circular Pitch (CP) is the distance in inches between corresponding points on two
adjacent gear teeth measured along the pitch circle.
Module (M) is the reciprocal of the diametral pitch and is used to specify the pitch
of gears cut to metric dimensions.
Circular Pitch =
Diametral Pitch =
Module (metric) =
Pitch Diameter =
Centre Distance =
Outside Diameter =
Addendum =
Working Depth =
Whole Depth =
Lead =
CP = π/DP = 3,1416/DP
DP = π/CP = 3,1416/CP
M = 25,4/DP
Number of teeth/DP
(Total number of teeth in both gears)/2DP
(Number of teeth + 2)/DP
1/DP
2/DP
2,25/DP
CP x n (n = number of starts)
26
5 December 2010
27
12.2
5 December 2010
Gear Hobbing
Very satisfactory gears can be produced by the hobbing method. By this means, no
matter how many teeth are required on a gear, the correct involute form for that
number will be automatically produced. The teeth will always be the correct shape
as the appropriate involute curve is generate by the hobbing action. Only one cutter
is needed for each DP and pressure angle, and all the teeth are produced with just
one pass of the hob.
The hob is a cutting tool in the form of a thread or single start worm. The shape of
the thread is the rack shape of tooth profile that the hob will eventually produce.
The hob is provided with a series of gashes or flutes that form the cutting edges of
the hob where they meet the thread. When the hob is secured to a rotating spindle
and a gear blank is brought into contact with it, the hob will produce a series of
slots or teeth on the blank similar in shape to the teeth on the hob. Note that to cut
a spur gear with straight teeth, the hob will need to be angled to the gear blank at
the lead angle of the hob (see section on worm threads). The gear blank must be
gashed perpendicular to the plane of the blank (along the axis of the blank).
The width of the gash at the periphery of the hob should be about 0.4 times the
pitch of the flutes.
The approximate number of flutes in a hob can be determined by multiplying the
diameter of the hob by 3 and dividing this product by twice the linear pitch.
Table 12.1
DP
Cutting Tool Depth of Cut and Tip Width
Depth of Cut
Width of Tool Tip
14½° PA
20° PA
30° PA
16
0.135” (3.43mm)
1.55mm
1.14mm 0.38mm
18
0.120” (3.05mm)
1.37mm
1.02mm 0.33mm
20
0.108” (2.74mm)
1.24mm
0.94mm 0.30mm
24
0.090” (2.29mm)
1.04mm
0.76mm 0.25mm
30
0.072” (1.83mm)
0.84mm
0.64mm 0.23mm
32
0.067” (1.70mm)
0.76mm
0.58mm 0.20mm
36
0.060” (1.54mm)
0.69mm
0.53mm 0.18mm
40
0.054” (1.37mm)
0.64mm
0.48mm 0.15mm
Tip width = 0.732”/DP (20° PA) and 0.97”/DP (14½°PA)
Table 12.2
DP
16
18
20
24
Gear Trains for Selected DPs
Gear Train
55 x IDLER
35
55 x 40
35 x 45
55 x 40
35 x 50
55 x 40
35 x 60
DP
30
32
36
40
Gear train
55 x 40
35 x 75
55 x 30
35 x 60
55 x 20
35 x 45
55 x 20
35 x 50
28
5 December 2010
Notes:
1. The above data applies for an 8 tpi leadscrew
2. The top numbers reflect Drivers, and the lower numbers the Driven
gears
Table 12.3
DP
~ TPI
Mandrel
Gear
16
18
20
24
30
32
36
40
60
5.091
5.727
6.364
7.636
9.545
10.18
11.46
12.73
19.09
55T
40T
40T
40T
40T
20T
20T
20T
20T
Gear Hobbing Data (For a Lead Angle of 4.25°)
1st Stud
Driven Driver
Idle
Idle
Idle
Idle
75T
Idle
Idle
Idle
75T
(60T)
(50T)
(45T)
(45T)
55T
(50T)
(50T)
(45T)
55T
2nd Stud
Driven Driver
45T
50T
60T
Idle
40T
45T
50T
Idle
55T
55T
55T
(50T)
55T
55T
55T
(50T)
Lead
screw
35T
35T
35T
35T
35T
35T
35T
35T
35T
Hob
Dia
(mm)
24.9
22.1
20.1
16.5
13.2
12.5
11.2
9.9
6.6
Core
Dia
(mm)
17.5
15.8
14.0
11.7
9.4
8.9
7.9
5.8
4.6
Length
30
27
24
20
16
15
13
12
8
~TPI = 1/CP = DP/
29
13.
5 December 2010
FITS & TOLERANCES
When dealing with round holes and round shafts, it is common to consider the three types
of fit, viz:
Clearance
For a clearance fit, the hole diameter is larger than the shaft diameter, so that the shaft
can be moved through the hole axially and rotate freely.
Transition
The transition fit is size on size. The parts can be pushed or wrung together, but cannot
(easily) rotate after assembly.
Interference
For an interference fit, the hole diameter is smaller than the shaft diameter, and the
shaft must somehow be forced through the hole axially, and will not subsequently
rotate
For clearance and interference fits, the allowance is the difference between hole and shaft
diameters. It is positive for a clearance fit and negative for an interference fit. In the home
workshop one can make one component, measure it, add (or subtract) the necessary
allowance, and then carefully make the mating component to suit. In industry based on
mass production, this is not economically viable and it is necessary to allow some
variations in dimension which is called the “tolerance”.
Tubal Cain in “The Model Engineering Handbook”, has suggested the following system in
which the allowance equals a constant plus a variable amount based on diameter, for
shaft nominal diameters of 3 to 50mm:
Fit Class
Large clearance
Small clearance
Easy run
Normal run
Close run
Precision run
Slide
Push
Wheel keying
Drive
Force
Shrink
Example:
Constant
mm
inch
-0.076
-0.051
-0.038
-0.025
-0.015
-0.013
-0.008
-0.004
0
+0.008
+0.013
+0.013
-0.003
-0.002
-0.0015
-0.001
-0.0006
-0.0005
-0.0003
-0.00015
0
+0.0003
+0.0005
+0.0005
Variable Amount
(mm per
(inch per
mm dia)
inch dia)
-0.0050
-0.005
-0.0030
-0.003
-0.0023
-0.00225
-0.0015
-0.0015
-0.0008
-0.0008
-0.0007
-0.00065
-0.0005
-0.00045
-0.0004
-0.00035
0
0
+0.0005
+0.00045
+0.0008
+0.00075
+0.0015
+0.0015
For a 1” push fit the shaft must be 0.35+0.15 = 0.5 thou smaller than the
hole
30
5 December 2010
Interference Fits
For interference fits, the shaft is typically bigger than the hole and some means must be
adopted to fit the parts together. For press fits a lead-in taper on the shaft can facilitate
this, and for light press fits (e.g. dowel pins) a chamfer may be sufficient.
For shrink fits, the part with the hole is heated to expand the hole, and the shaft then
inserted. When it cools down, the hole contracts and grips the shaft. However, this may
introduce hoop stress in the hole part, and in extreme cases can lead to fracture.
An expansion fit is where the shaft temperature is reduced (by freezing) to cause it to
contract before inserting it in the hole at room temperature. When the shaft attains room
temperature, it grips the hole tightly.
A common rule of thumb states a difference of 0.001” per 1” of diameter for interference
fits.
Tolerances
ISO standard tolerances apply to all linear dimensions, eg diameter, width, length, etc.
There are 16 grades of tolerance for each size range, viz IT.1 to IT.16. Tables listing the
16 grades of tolerance for various sizes are readily available (DIN 7151).
Allowances
The tolerance determines the dimensional difference between two limits, but to establish
the various fits one refers to “allowances” or “deviations”.
A hole is described by the appropriate capital letter followed by a suffix number denoting
the tolerance grade, eg. H7.
A shaft is described by a small letter followed by a suffix number denoting the tolerance
grade, eg. p6.
A fit is described by the hole symbol followed by that of the shaft, eg H7 – p6 or H7/p6
The “standard hole” is H.
Typical Fits
Satisfactory clearance fits are obtained with the following combinations of holes & shafts:
Hole
H6
H7
H8
Shaft
g5, f6, e7
g6, f7, e8, d8/d9, c8/c9, b8/b9, a9
f8, e9, d10
Satisfactory interference fits are obtained with the following combinations of holes &
shafts:
Hole
H6
H7
H8
Shaft
n5 to x5
p6 to z6
s7 to z7
31
5 December 2010
ISO Recommendations
Tolerances in standard holes (millimetres)
H7
H8
Nominal
Diameters
High Limit
Low Limit
High Limit
Low Limit
2 Classes
0-3
3-6
6 - 10
10 - 18
18 - 30
30 - 50
50 - 80
80 - 120
+0.010
0.0
+0.014
0.0
+0.012
0.0
+0.018
0.0
+0.015
0.0
+0.022
0.0
+0.018
0.0
+0.027
0.0
+0.021
0.0
+0.033
0.0
+0.025
0.0
+0.039
0.0
+0.030
0.0
+0.046
0.0
+0.035
0.0
+0.054
0.0
Interference (drive fit) allowances on shafts for various fits
p6
Nominal
Diameters
High Limit
Low Limit
Tolerance
0-3
3-6
6 - 10
10 - 18
18 - 30
30 - 50
50 - 80
80 - 120
+0.012
+0.006
0.006
+0.020
+0.012
0.008
+0.024
+0.015
0.009
+0.029
+0.018
0.011
+0.035
+0.022
0.013
+0.042
+0.026
0.016
+0.051
+0.032
0.019
+0.059
+0.037
0.022
0-3
3-6
6 - 10
10 - 18
18 - 30
30 - 50
50 - 80
80 - 120
+0.006
+0.0
0.006
+0.009
+0.001
0.008
+0.010
+0.001
0.009
+0.012
+0.001
0.011
+0.015
+0.002
0.013
+0.018
+0.002
0.016
+0.021
+0.002
0.019
+0.025
+0.003
0.022
Transition (push fit)
k6
Nominal
Diameters
High Limit
Low Limit
Tolerance
Clearance (close running fit)
g6
Nominal
Diameters
High Limit
Low Limit
Tolerance
0-3
3-6
6 - 10
10 - 18
18 - 30
30 - 50
50 - 80
80 - 120
-0.002
-0.008
0.006
-0.004
-0.012
0.008
-0.005
-0.014
0.009
-0.006
-0.017
0.011
-0.007
-0.020
0.013
-0.009
-0.025
0.016
-0.010
-0.029
0.019
-0.012
-0.034
0.022
32
5 December 2010
14.
KEYS & KEYWAYS
14.1
Metric Parallel Keys & Keyways
Shaft Dia
(mm)
Key Size
Depth of
(mm)
Keyway into
WxH
Shaft (mm)
6–8
2x2
1.2
8 – 10
3x3
1.8
10 – 12
4x4
2.5
12 – 17
5x5
3.0
17 – 22
6x6
3.5
22 – 30
8x7
4.0
Length of key = 1.5 x shaft diameter
14.2
Key Size
Depth of
(in)
Keyway into
WxH
Shaft (in)
1/
1
¼-½
0.072
8 x /8
3
½-¾
/16 x 3/16
0.107
¾-1
¼x¼
0.142
5
1–1¼
/16 x 5/16
0.177
Length of key = 1.5 x shaft diameter
Depth of
Keyway into
Hub (in)
0.060
0.088
0.115
0.142
Std
Tolerances
(in)
+ 0.0006 – 0
Metric Taper Keys & Keyways (1 in 100)
Shaft Dia
(mm)
6–8
8 – 10
10 – 12
12 – 17
17 – 22
22 – 30
14.4
Std
Tolerances
(mm)
+ 0.1 - 0
+ 0.1 - 0
+ 0.1 - 0
+ 0.1 - 0
+ 0.1 - 0
+ 0.2 - 0
Imperial Parallel Keys & Keyways
Shaft Dia
(in)
14.3
Depth of
Keyway into
Hub (mm)
1.0
1.4
1.8
2.3
2.8
3.3
Key Size
(mm)
WxH
2x2
3x3
4x4
5x5
6x6
8x7
Depth of
Keyway into
Shaft (mm)
1.2
1.8
2.5
3.0
3.5
4.0
Depth of
Keyway into
Hub (mm)
0.5
0.9
1.2
1.7
2.2
2.4
Std
Tolerances
(mm)
+ 0.1 - 0
+ 0.1 - 0
+ 0.1 - 0
+ 0.1 - 0
+ 0.2 - 0
+ 0.2 - 0
Imperial Taper Keys & Keyways (1 in 100)
Shaft Dia
(in)
¼-½
½-¾
¾-1
1–1¼
Key Size
(in)
WxH
1/
1
8 x /8
3
/16 x 3/16
¼x¼
5
/16 x 5/16
Depth of
Keyway into
Shaft (in)
0.072
0.107
0.142
0.177
Depth of
Keyway into
Hub (in)
0.039
0.067
0.094
0.121
Std
Tolerances
(in)
+ 0.0006 – 0
33
14.5
5 December 2010
Woodruff Keys & Keyways
Key
No.
202
203
303
403
204
304
404
305
405
505
406
506
606
Size W x
Dia (in)
1
/16 x ¼
/16 x 3/8
3
/32 x 3/8
1
/8 x 3/8
1
/16 x 1/2
3
/32 x 1/2
1
/8 x 1/2
3
/32 x 5/8
1
/8 x 5/8
5
/32 x 5/8
1
/8 x 3/4
5
/32 x 3/4
3
/16 x 3/4
1
Key Dia
Max – Min
(in)
Depth of
Key
Max – Min
(in)
Depth of
Keyway in
Shaft (in)
Depth of
Keyway in
Hub (in)
0.268 – 0.250
0.375 – 0.370
0.375 – 0.370
0.375 – 0.370
0.500 – 0.490
0.500 – 0.490
0.500 – 0.490
0.625 – 0.615
0.625 – 0.615
0.625 – 0.615
0.750 – 0.740
0.750 – 0.740
0.750 – 0.740
0.104 – 0.099
0.171 – 0.166
0.171 – 0.166
0.171 – 0.166
0.203 – 0.198
0.203 – 0.198
0.203 – 0.198
0.250 – 0.245
0.250 – 0.245
0.250 – 0.245
0.313 – 0.308
0.313 – 0.308
0.313 – 0.308
0.0778 – 0.0728
0.135 – 0.140
0.119 – 0.124
0.104 – 0.109
0.167 – 0.172
0.151 – 0.156
0.136 – 0.141
0.198 – 0.203
0.182 – 0.187
0.167 – 0.172
0.246 – 0.251
0.230 – 0.235
0.214 – 0.219
0.0372 – 0.0322
0.042 – 0.047
0.057 – 0.062
0.073 – 0.078
0.042 – 0.047
0.057 – 0.062
0.073 – 0.078
0.057 – 0.062
0.073 – 0.078
0.089 – 0.094
0.073 – 0.078
0.089 – 0.094
0.104 – 0.109
The cutter number is the same as the key number. The last 2 digits give the
nominal diameter in 1/8ths of an inch, and the first digit gives the nominal width in
1/32s of an inch. The key should be a tight fit to the shaft and a close fit to the hub.
There should be a clearance of from 0.007” to 0.010” between the flat top of the
key and the root of the slot in the hub.
14.6
14.7
Metric Woodruff Keys (DIN 6888)
DIN
Size
2 x 3.7
2.5 x 3.7
3 x 3.7
W x Dia
(mm)
2 x 10.5
2.5 x 10.5
3 x 10.5
2x5
2.5 x 5
3x5
4x5
2 x 13.5
2.5 x 13.5
3 x 13.5
4 x 13.5
DIN
Size
2 x 6.5
2.5 x 6.5
3 x 6.5
4 x 6.5
W x Dia
(mm)
2 x 16.5
2.5 x 16.5
3 x 16.5
4 x 16.5
3 x 7.5
4 x 7.5
5 x 7.5
6 x 7.5
3 x 19.5
4 x 19.5
5 x 19.5
6 x 19.5
General Key Issues
Material for keys = 070M20 or EN3 (not less than 550 N/mm2 tensile strength).
Generally speaking, the shear strength of a material can be found by multiplying
the tensile strength by 0.8.
34
15.
5 December 2010
SILVER SOLDERING
The secret of silver soldering is to fulfill the following criteria:
Close-fitting joint prior to soldering.
Make sure the work is CLEAN before starting.
Flux the work thoroughly (using the right flux).
Use the correct amount of heat.
Use the correct amount of solder (and size of rod) for the job.
Apply the solder at the correct time and place.
Control the flow of the solder.
There are several grades of silver solder, and some flow more easily than others (it is the
silver that provides the free-flowing characteristics). However, silver solder is not good
good at gap-filling – this is opposite to that other useful property it has which is to creep
into every nook and cranny. Because of this the joint needs to be close – not more than 5
thou (0,13mm) preferably – but an interference fit is not only not required, it is to be
positively avoided. Edges of joints can be chamfered to provide better access for the
solder, and joint faces may be scored to encourage flow in a certain direction. Neither of
these are really necessary for small fittings though. If it is necessary to fill a larger gap it’s
quite simple to jam in fresh cut slivers of copper or brass sheet before soldering, filed flat
afterwards and you would never know the gap was there.
It is absolutely essential that the joint faces be quite clean and oil-free to obtain a sound
joint. The solder will not flow across nor bind to a dirty or oxidised metal surface. All
joint faces should be cleaned with emery and/or wire wool to brighten the metal surface;
fresh-machined surfaces are best, but if there is oil there it’s best to use a solvent to remove
it. Jobs that require more than one soldering operation will need to be pickled in an acid
bath to remove traces of old flux before the second part of the job is tackled. Dilute
sulphuric acid is probably the best pickle for brass and copper work, but it is not the safest.
Citric acid and some other mixtures can also be used, but are slower in action and tend to
have other drawbacks that sulphuric avoids. For small fittings it’s less of a danger using
sulphuric acid as the quantities are small, but dunking large hot chunks of metal into
sulphuric acid can ruin your day if you’re not careful. Be particularly careful with hollow
parts (tubes or items with bores), as these can cause the acid to shoot out in a jet a
considerable distance. Always wear eye protection, and wear rubber gloves and aprons
etc.
Different fluxes are recommended for different silver solders. Most are based on borax
(boracic acid being the active ingredient) but the temperature at which they work, and the
length of time they will work for once the metal gets hot will vary. Most are sold as a
white powder to be mixed with water to a creamy paste for application. When using
Easyflo #1 (AG1) and Easyflo #2 (AG2) silver solders from Johnson Matthey, use Easyflo
flux powder. This has an indefinite shelf life. Mix flux with water and drop of Sunlight
liquid to creamy consistency. Use Tippex or chalk to “mask” solder. Caustic soda in
warm water will dissolve flux.
Make sure all joint faces are thoroughly coated and dribble some extra along the joints to
make a fillet to be sure. The first application of heat should be gentle to vapourise the
water leaving the flux intact and in place, then gradually increase the heat until it melts.
A large amount of heat is needed to make the solder flow correctly, and whilst this is easy
to apply to small fittings it’s much more of a problem where larger items are concerned.
35
5 December 2010
For large items it’s very useful to have a purpose-built brazing hearth complete with
firebricks as the work can then be insulated to some extent thus retaining the heat where
it’s needed. For small jobs a hand-held can of propane (not butane as the calorific value is
much lower) with a screw-on burner is adequate. Larger jobs, however, require some sort
of brazing torch with a larger heat output (e.g. those made by Sievert). Oxy-acetylene or
oxy-propane gear is really for the specialist and not really suitable in novice hands for
silver soldering; special techniques are needed to manipulate the highly localised heat to
prevent burning of both solder and parent metal.
The first sign of nearing the required temperature is when the flux turns to a brown sticky
goo, it will change from this appearance to a light-amber mobile liquid as the correct
temperature is reached and it will seem to crawl all over the surface of the metal. In this
state it is able to remove any oxidation from the metal and keep it bright. When this
temperature has been reached, then move the flame away from the work and just touch the
silver solder rod to the joint; it should immediately melt and flash around – if it doesn’t
then the work is not hot enough. On NO account should the silver solder rod be poking
into the flame whilst you are applying heat; not only is it likely to melt and a blob will fall
off and stick just where you don’t want it, but you are likely to end up with an unsound
joint through lack of heat even when it appears to flow. It is the hot work that should melt
the solder.
Silver solder is available in different sized rods. For small fittings 1 mm wire is
wonderful; it is easy to apply small amounts of solder in the precise place it’s needed.
Larger work can use sticks up to 2,5 mm or larger. Johnson Matthey supply Easyflo #1
(=AG1 = 50% silver, red painted tip) and Easyflo #2 (=AG2 = 42% silver, black painted
tip) rods in 600mm lengths (at R1900/kg).
If the joint gap is correct very little solder is required and any excess will do nothing useful
and just look ugly. You can also buy ground silver solder and flux as a paste, and this can
be applied to the joint and simply heated – useful for joints in fittings that would be
difficult to reach otherwise. You can do something similar with the fine solder wire if you
snip a length off and wrap it round the joint before heating, but if you do this put the solder
on first and cover it well with flux, then heat the work indirectly – i.e., don’t blast the
flame at the silver solder, but to one side of the joint. When it’s hot enough the solder will
melt and flow normally.
36
16.
PROPERTIES OF METALS
16.1
Strengths of Materials
5 December 2010
EN1A = 220M07 = Free-cutting mild steel EN1B = 240M07= Free-cutting mild steel
EN1A (leaded) = same as above, with lead EN8M = 212M44 = free-cutting carbon steel
EN24 = 817M40
Material
Spec
UTS
Yield
Elong
E
Shear
Density
BS 970
Tons/in2
Tons/in2
(%) Lbs/in2 Tons/in2
g/cc
2
2
6
2
(New)
(N/mm )
(N/mm )
x 10
(N/mm )
Cast iron
17
16-19
7.20
(260)
Freecutting EN1A
28 (min)
21
12
30
19
7.86
MS Bright
220M07
(430)
(325)
(295)
Freecutting EN1A
23 (min)
14
27
30
15
7.86
Hot rolled
220M07
(360)
(220)
(230)
20 Carbon
EN3A
32 (min)
24
17
30
21
7.86
Bright
070M20
(500)
(370)
(325)
20 Carbon
EN3A
28 (min)
14
26
30
19
7.86
Hot rolled
070M20
(430)
(220)
(295)
40 Carbon
EN8
40
31
13
30
27
7.86
Steel Bright 080M40
(620)
(480)
(420)
40 Carbon
EN8
35
18
21
30
23
7.86
Steel
080M40
(540)
(280)
(360)
Hot rolled
55 Carbon
EN9
45
40
10
30
30
7.86
Steel Bright 070M55
(700)
(620)
(460)
55 Carbon
EN9
40
30
10
30
27
7.86
Steel
070M55
(620)
(460)
(420)
Hot rolled
Silver steel Stubs
40-60
35-50
20-35
30
7.83
(620-920)
(540-770)
Cast Brass
8.42
Drawn
CZ109
23
8
45
14
8.20
60/40 Brass
(360)
(124)
(215)
Gunmetal
BS 1400
17-20
8-12
13-25
16
8.84
SAE 660
(270-360)
(150-170)
Cast
20
2.58
Aluminium
(310)
Wrought Al
2.69
Bronze (Al)
7.78
Copper
(210-240)
8.81
Phosphor
23-32
11-18
6-25
Bronze
(360-500)
(170-280)
1.
2.
As purchased, the steel is typically in the “Bright Drawn” condition, where the tensile strength is
increased and the ductility (elongation) reduced.
For steels in the “Hot Rolled” or “Normalised” condition, the tensile strength is decreased and the
ductility increased.
37
16.2
5 December 2010
Interpreting BS 970/1972
First 3 Digits:
000 to 199 = Plain Carbon steel
200 to 240 = Freecutting versions of plain carbon steels
300 to 499 = Stainless and Valve steels
500 to 999 = Alloy steels (NOT stainless)
From 000 to 249 the 2nd and 3rd digits carry some more information:
Plain Carbon Steels: indicate 100 x Manganese content, eg 112 = 0.12% Mn
Freecutting steels:
indicate sulphur content, eg 212 = 0.12% sulphur
Middle Letter:
M = mechanical properties
A = chemical properties
H = will Harden to specified limits in BS 970
S = stainless steel
Last 2 digits:
100 x % carbon (> 1.0% the figures will always be 99)
Examples:
070M20 = plain carbon steel, 0.2% Mn, to BS 970
mechanical properties, with 0.2% carbon (= EN3)
220M07 = freecutting steel, 0.2% sulphur, to BS 970
mechanical properties, with 0.07% carbon (= EN1A)
16.3
Strength Formulae
Stress = Force (N)/Area (m2)
Strain = Change in length (m)/Original length (m)
Young’s Modulus = E = Stress/Strain (N/ m2)
Force = Mass (kg) x g (m/s2)
1 N/m2 = 1 Pascal
16.4
(For MS, E ~ 207 GPa)
(g = 9.81 m/s2)
1 N/mm2 = 1 MPa = 145 psi
1 psi = 0.0069 N/mm2
Chemical Properties
EN1A
Carbon %
Mn %
Sulphur %
Phos %
Lead
Silicon
Cr
Copper
Sn
Zn
Ni
0-0.15
0.9-1.3
.25-.35
0-0.07
0.15-0.35
0-0.1
EN3A
EN8
.15-.25
0.4-0.9
0-0.06
0-0.06
.35-.45
0.6-1.0
0-0.06
0-0.06
.05-.35
.05-.35
Silver
Steel
1.1-1.2
.25-.45
0-0.035
0-0.035
Stainless
Steel 304
0.08
2
0.03
0.045
0-0.4
.35-.50
0.75
18 - 20
8 – 10.5
Gunmetal
Phosphor
Bronze
0-0.15
6-8
0.5-1.0
0-0.25
81-85
6-7
2-4
0-0.5
Remain
10-11.5
0-0.05
0-0.1
38
16.5
D
mm
8
10
12
13
15
16
19
20
22
16.6
5 December 2010
Weight of Round Barstock (kg/metre)
Steel
0.396
0.620
0.892
1.047
1.394
1.587
2.237
2.479
2.999
Cast
iron
0.359
0.562
0.809
0.950
1.264
1.439
2.029
2.248
2.720
Brass
0.644
0.927
1.088
1.449
1.649
2.325
2.576
3.116
GM
0.694
1.000
1.173
1.562
1.778
2.506
2.778
3.360
D
mm
25
27
30
35
40
45
50
55
60
Steel
3.873
4.500
5.577
7.591
9.918
12.545
15.488
18.747
22.305
Cast
Iron
3.513
4.081
5.058
6.885
8.996
11.378
14.048
17.003
20.231
Brass
GM
4.025
4.340
5.796
7.889
10.304
13.041
16.101
19.482
23.181
6.249
8.505
11.108
14.059
17.353
21.004
24.991
Normalising
Cold-rolled steels (“bright” steels) may require normalising to relieve the internal
stresses pent-up in the material from the compressive action of the forming process.
Machining away parts of the material will release these stresses and produce
distortion. Normalising is carried out by heating to a bright red (viewed in subdued
light), then allowing to cool naturally in still air. The ideal way of doing this is to
suspend the part by an iron wire which will facilitate both its removal from the
flame and suspension for cooling. Normalised steel will also machine better.
16.7
Annealing
Annealing is required to “soften” a previously hardened high-carbon steel,
carburised (case-hardened) steel or even chilled cast iron, to allow subsequent
machining to be carried out. Annealing is similar to normalising, but requires
extremely slow cooling to ensure that no residual hardness remains in a hardened
ferrous metal. This is typically achieved by placing the metal item in a coal fire to
achieve red heat, and leaving the item in the fire until the fire dies and cools down
completely.
39
17.
BOLTS & NUTS
17.1
Bolt Strengths
5 December 2010
Bolt strengths (metric system) for carbon steel are expressed in terms of product
classes as follows:
Class 8.8 = 800 MPa UTS and Yield = % of UTS = 640 MPa
Class 4.6 = 400 MPa UTS and Yield = 240 MPa
Ultimate Tensile Stress = theoretical minimum point at which the material will
fracture (N/mm2 (MPa))
Yield Stress = theoretical point of stress beyond which the material loses its
elasticity and becomes permanently stretched (N/mm2 (MPa)).
Proof Load Stress = the minimum point prior to permanent elongation and the test
point for actual proof load testing (N/mm2 (MPa)). The proof load stress is
typically 80-90% of the yield stress
There are two common types of stainless steel fasteners: corrosion-resistant
stainless steel, ASTM 304 (a.k.a. 18-8) or DIN/ISO A2, and acid-resistant stainless
steel, ASTM 316 or DIN/ISO A4. A2 is by far the most prevalent material, and is
what is normally supplied for stainless metric fasteners. There are three typical
property classes (strengths) for stainless steel fasteners in the metric system: 50, 70,
and 80. The class equals the tensile strength (in MPa or N/mm2) divided by 10.
The metric property class is a dash (-) number after the alloy designator. For
example, a screw marked A2-70 is a 304 stainless steel screw with a 700 N/mm2
tensile strength. Both alloys come in all property classes, but A2-70 and A4-80 are
the most common.
Thread galling can occur when using bolts and nuts of the same grade stainless
steel. This can be prevented by using A2 bolts with A4 nuts (or vice versa), or by
using a thread lubricant such as CopaSlip.
In the case of nuts, the marking consists of a single number, and if this number
matches, or is higher than, the first number on the bolt, then the nut is strong
enough.
17.2
Coatings
Automotive bolts are usually made from mild steel, alloy steel or stainless steel. A
plain black finish, known as black oiled, is the best from a strength and preload
point of view, because any form of plating may cause (hydrogen) embrittlement
unless the bolts are treated after plating. This is especially true of chromium
plating applied to high-alloy steels, and such bolts should not normally be used in
high-stress applications. However, unplated bolts will rust, so bolts are often
coated with a very thin layer of zinc or cadmium, followed by a chromate coating
to lock-in the finish. Such treatment is less harmful on steels of grade 8.8 and less,
which is why coated bolts are often of a lower strength grade than black bolts.
40
5 December 2010
The plating also affects the friction between the bolt and the joint surfaces, so the
recommended torque values will change. Whenever you change from a black bolt
to a coated bolt you should find out what the torque should be. For example, zinc
plating increases the friction by up to 40 per cent, and stainless steel doubles the
frictional coefficient, but cadmium plating reduces the friction by about 25 per cent.
Note that hydrogen embrittlement can be treated/reduced by baking the work in an
oven at 200 deg C overnight.
17.3
Thread Lubrication
Thread lubrication is another variable that needs to be considered, and for highstress applications one should follow the instructions in the workshop manual. In
general, a light oil or a good anaerobic coating (thread locking compound) will
reduce the required torque values by about 10 per cent, but special anti-seize
lubricants may mean a reduction of about 20 per cent.
17.4
Bolt Tensioning
As a general rule, the bolted joint is designed with sufficient numbers and sizes of
fasteners to apply the required clamp load at 65 - 70% of the fastener proof load, ie
well below the yield point of the fastener. Note that gasketed or soft compound
joint components significantly alter this.
17.5
Factors of Safety
Use FoS = 6 for impact loads
Use FoS = 2 for normal loads
41
5 December 2010
18.
FORMULAE AND CONVERSION FACTORS
18.1
Length
18.2
18.3
1 inch = 25.4 mm
1 thou” = 0.0254 mm
0.1 mm = 4 thou”
1 mm = 40 thou”
Weight/Mass
1 pound = 0.4536 kilogram
1 kilogram = 2.2 pound
2240 pounds = 1 ton
1 ton = 1016.05 kilogram
1000 kilogram = 1 tonne
1 tonne = 2204.6 pound
Volume
1 inch3 = 16.4 cm3
18.4
Pressure
Pressure = Force (N)/Area (mm2)
1 pound/in2 = 145 MPa (N/mm2)
100 kPa = 14 psi
1 bar = 0.1 N/ mm2 = 100 kPa
1 MPa = 1 N/mm2
Atmospheric pressure = 101.306 kN/m2 absolute = 10,33m head of water
Gauge pressure = absolute pressure – atmospheric pressure
18.5
Force
1 N = 0.22481 lbf
1 N = 9.81 kgf ( = 1 kg x 9.81 m/s2)
100 kgf = 981 N
18.6
18.7
Stress
1 tonf/in2 = 15.444 N/mm2
1 lbf/in2 = 0.0069 N/mm2
1 N/mm2 = 0.06475 tonf/in2
1 N/mm2 = 145.038 lbf/in2
Heat, Work & Energy
1 horsepower = 0.746 kW
1 kW = 1.34 horsepower
1 BTU = 1055 joule
1 kW = 1000 J/sec
1 joule = 1 Nm
42
18.8
18.9
5 December 2010
Torque
1 lbf ft x 1.356 = 1 Nm
1 Nm x 0.7376 = 1 lbf ft
1 kgf m x 9.807 = 1 Nm
1 lbf ft x 0.138 = 1 kgf m
Temperature
t oF = 5/9 (t - 32) oC
0 oC = 273.15 oK
t oC = (32 + 1.8t) oF
18.10 Density
Mass density = ρ (rho) = mass/volume = kg/m3
Specific weight = weight/volume = ρ x g, where g = 9.81 m/s2
Specific gravity = relative density = ρ substance / ρ water (ρ water =
1000kg/m3 at 4 ° C)
18.11 Airy Points
The Airy Points of a bar are equidistant from each end of the bar and separated by a
distance of 0,577L, where L is the length of the bar. Supporting at these points
ensures the end faces of a length of bar are parallel, a necessary condition for
accurate measurement.
In supporting a long straight edge, it is necessary to ensure minimum deflection –
in this case the points of suspension are at 0,554L.
18.12 Pi
= 22/7 = 355/113
18.13 Metric Conversion Tables
43
5 December 2010
44

ALLAN`S MACHINING HANDBOOK

Transcription

Similar documents

“The Cask of Amontillado” by Edgar Allan Poe from Charters, Ann

Scaredy Cat - Total Flyfisher Magazine

CAMPING** Gennes - Camping Au Bord de Loire

Robison Anton Thread Colo on Anton Thread Colors - Tommys T

ARTISTIC STITCHES, INC. Robison Anton Thread Colors

Leasing Procedures

Working with the Media

Log Max 5000D - Biomass Innovation Centre

important - Pro-Bolt

Shultz Machine