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). 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).

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.

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

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:

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

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

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

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