Turning Speeds & Feeds - RPM
Calculations
|
There are rules and principles of cutting speeds and R.P.M. calculations that
apply to all metal cutting operations. The operating speed for all metal cutting
operations is based on the cutting tool material and the hardness of the
material to be cut. In this unit we will concentrate on cutting speeds for
single point tooling.
Cutting Speed for Turning |
Cutting speed is the speed at the outside edge of the part as it is
rotating. This is also known as surface speed. Surface speed, surface
footage, and surface area are all directly related. Two wheels can
illustrate this. Take two wheels, one wheel which is
three feet in diameter and the other wheel which is one foot in
diameter, roll each wheel one complete turn (Figure 1). |
![](http://its.fvtc.edu/MachShop2/Speeds/wheel.gif)
Figure 1 |
Which wheel traveled farther? The larger wheel traveled farther because it
has a larger circumference and has more surface area. Cutting speeds work on the
same principle. If two round pieces of different sizes are turning at the same
revolutions per minute (RPM), the larger piece has a greater surface speed.
Surface speed is measured in surface feet per minute (SFPM). All cutting speeds
work on the surface footage principle. Again, cutting speeds depend primarily on
the kind of material you are cutting and the kind of cutting tool you are using.
The hardness of the work material has a great deal to do with the recommended
cutting speed. The harder the work material, the slower the cutting speed. The
softer the work material, the faster the recommended cutting speed (Figure 2).
![](http://its.fvtc.edu/MachShop2/turnmach/incrCut.GIF)
Figure 2
The hardness of the cutting tool material has a great deal to do with the
recommended cutting speed. The harder the cutting tool material, the faster the
cutting speed (figure 3). The softer the cutting tool material, the slower the
recommended cutting speed.
![](http://its.fvtc.edu/MachShop2/turnmach/incrCut1.GIF)
Figure 3
The depth of the cut and the feed rate will also affect the cutting speed,
but not to as great an extent as the work hardness. These three factors, cutting
speed, feed rate and depth of cut, are known as cutting conditions. Cutting
conditions are determined by the machinability rating. Machinability is the
comparing of materials on their ability to be machined. From machinability
ratings we can derive recommended cutting speeds. Recommended cutting speeds are
given in charts. These charts can be found in your Machinery’s Handbook,
a textbook or in a chart given to you by your tool salesperson. In Table 4 you will
find a typical recommended cutting speed chart.
Table 4. Recommended Cutting Speeds in Feet per Minute
for Turning Ferrous and Nonferrous Metals*
Material |
Material Condition |
Hardness, Bhn |
Cutting Speed, fpm |
High-Speed Steel |
Carbide |
Free Machining, Plain Carbon Steels (Resulphurized)
AISI B1111, B1112, B1113,
1113, 1119, 1212, 1213 |
HR, A
CD |
100 to 150
150 to 200 |
160
180 |
500
600 |
AISI 1108, 1115, 1118, 1120, 1126 |
HR, A
CD |
100 to 150
150 to 200 |
140
150 |
450
500 |
AISI 1132, 1137, 1140, 1145, 1151 |
HR, A, N, CD
Q & T
Q & T
Q & T |
175 to 225
275 to 325
325 to 375
375 to 425 |
130
90
50
30 |
500
250
175
140 |
Plain Carbon Steels
AISI 1012, 1015, 1018, 1019,
1020, 1022, 1024, 1025 |
HR, A, N, CD
HR, A, N, CD
HR, A, N, CD
CD |
100 to 125
125 to 175
175 to 225
225 to 275 |
140
120
100
70 |
500
400
350
300 |
AISI 1027, 1029, 1030, 1032,
1035, 1037, 1040, 1043,
1045, 1047, 1050 |
HR, N, A, CD
HR, N, A, CD
N, CD, Q & T,
N, Q & T
Q & T
Q & T |
125 to 175
175 to 225
225 to 275
275 to 325
325 to 375
375 to 425 |
120
100
70
60
50
40 |
400
350
300
240
200
175 |
AISI 1055, 1060, 1065, 1070, 1074,
1080, 1085, 1090, 1095 |
HR, N, A, CD
HR, N, A, CD
N, CD, Q & T,
N, Q & T
Q & T
Q & T |
125 to 175
175 to 225
225 to 275
275 to 325
325 to 375
375 to 425 |
100
90
65
55
45
30 |
375
325
275
225
180
150 |
Free Machining Alloy Steels
(Resulphurized)
AISI 3140, 4140, 4150, 8640 |
HR, N, A, CD
HR, N, A, CD
Q & T
Q & T
Q & T |
175 to 200
200 to 250
250 to 300
300 to 375
375 to 425 |
125
100
70
60
40 |
450
400
325
225
150 |
Alloy Steels
AISI 1320, 2317, 2512, 2517, 3115,
3120, 3125, 3310, 3316, 4012,
4017, 4023, 4028, 4320, 4615,
4620, 4720, 4815, 4820, 5015,
5020, 5024, 5120, 6118, 6120,
6317, 6325, 6415, 8115, 8615,
8620, 8625, 8720, 8822, 9310,
9315 |
HR, A, CD
HR, A, N, CD
CD, N, Q & T
N, Q & T
N, Q & T
Q & T |
150 to 175
175 to 220
220 to 275
275 to 325
325 to 375
375 to 425 |
110
80
70
60
50
40 |
400
350
300
250
200
175 |
* Based upon a feed of .012 inch per revolution
and a depth of cut .125 inch. Symbols under Material Condition column,
designate: HR—Hot Rolled, A—Annealed, N—Normalized, CD—Cold Drawn or
Cold Rolled,
Q & T—Quenched and Tempered, AC—As Cast, ST & A—Solution Treated
and Aged.
The lathe R.P.M. must be set so that the single point cutting tool will be
operating at the correct cutting speed. To set the proper speed we need to
calculate the proper revolution per minute or RPM setting. We stated earlier
that cutting speed or surface speed would change with the size of the part. So
to keep the surface speed the same for each size part we must use a formula that
includes the diameter of the part to calculate the proper RPM to maintain the
proper surface footage.
Calculating RPM
![](http://its.fvtc.edu/MachShop2/images/Top.gif) |
The RPM setting depends on the cutting speed and the diameter of the
part. The RPM setting will change with the diameter of the part. As the diameter
of the part gets smaller, the RPM must increase to maintain the recommended
surface footage. Again, take the case of the wheel. Think of the part as a wheel
and the cutting speed as a distance. A larger wheel (part) will need to turn
fewer revolutions per minute to cover the same distance in the same amount of
time than a smaller wheel (part). Therefore, to maintain the recommended cutting
speed, larger diameter parts must be run at slower speeds than a smaller
diameter part.
The lathe must be set so that the part will be operating at the proper
surface speed. Spindle speed settings on the lathe are done in RPMs. To
calculate the proper RPM for the tool and the workpiece, we must use the
following formula:
![](http://its.fvtc.edu/MachShop2/Speeds/RPM1.GIF)
This simplified version of the RPM formula is the most common formula used in
machine shops. This RPM formula can be used for other machining operations as
well.
Let's put this formula to work in calculating the RPM for the machining
example below. Use the recommended cutting speed charts in Table 4.
A cut is to be made with a high-speed steel (HSS) tool on a 2-inch diameter
piece of 1018 steel with a brinnel hardness of 200. Calculate the RPM setting to
perform this cut.
Cutting Speed = 100 (fpm)
Diameter of part = 2.0
![](http://its.fvtc.edu/MachShop2/Speeds/Rpm2.GIF)
Since the available spindle speed settings are generally not infinitely
variable, the machine cannot be set precisely to the calculated RPM setting.
Some judgment must be made in selecting the speed to use. Try to get to the
speed which is nearest to the calculated RPM, but if you can’t, consider these
conditions. Are you roughing or finishing? If you are roughing, go slower. If
you are finishing, go faster. What is your depth of cut? If it is a deep cut, go
to the slower RPM setting. Is the setup very rigid? Go slower for setups that
lack a great deal of rigidity. Are you using coolant? You may be able to go to
the faster of the two settings if you are using coolant. The greatest indicator
of cutting speed is the color of the chip. When using a high-speed steel cutter,
the chips should never be turning brown or blue. Straw-colored chips
indicate that you are on the maximum edge of the cutting speed for your cutting
conditions. When using carbide, chip colors can range from amber to blue, but
never black. A dark purple color will indicate that you are on the maximum edge
of your cutting conditions. Carbide cutting tools are covered in much greater
detail in other sections of your learning materials.
Let’s try more examples.
A cut is to be taken with a (HSS) turning tool on a 0.75 inch piece of 1045
steel with a brinnel hardness of 300. Calculate the RPM setting to perform this
cut.
Cutting Speed = 60 (fpm)
Diameter of part = 0.75
![](http://its.fvtc.edu/MachShop2/Speeds/Rpm3.GIF)
A 1-inch (HSS) drill is used on a 4-inch diameter piece of 1012 steel with a
brinnel hardness of 100. Calculate the RPM setting to perform this drilling
operation.
Cutting Speed = 140 (fpm)
Diameter of the drill = 1.00
![](http://its.fvtc.edu/MachShop2/Speeds/Rpm4.GIF)
Note that in the R.P.M. calculation, we used the diameter of the drill and not
the workpiece. This was done because the cutting takes place at the diameter of
the drill, not on the outside diameter of the workpiece.
A turning operation is to be done on a 3.00-inch piece of 4140-alloy steel
with a brinnel hardness of 200. A carbide turning tool is to be used. Calculate
the RPM setting to perform this cut.
Cutting Speed = 400 (avg.
fpm)
Diameter of part = 3.00
![](http://its.fvtc.edu/MachShop2/Speeds/RPM5.GIF)
Top
![](http://its.fvtc.edu/MachShop2/images/Top.gif)
|