Turning with Carbide: Cutting Speeds and Feeds

		Machine Shop Home

Introduction \| Adv Inspection \| SPC \| Carbide for Turning \| Adv. Lathe \| Adv. Milling \| Projects \| Tests

"Cutting Speeds, Feeds and Depth of Cut"

The turning operation is a combination of linear (tool) and rotational (workpiece) machine movements. The rate in IPR (inches/revolution) that the tool travels along or across the workpiece is referred to as the machine feed or the feed speed

Figure 1. Turning with a coated carbide insert.

The SFPM (surface feet/minute) or speed at which the part surface rotates is known as the cutting or surface speed. These two important criteria are selected to either maximize tool life and productivity or to balance them.

Selecting the Proper Cutting Speed

Cutting speed is determined primarily by the machinability of the material and the hardness of the cutting tool. Machinability describes the ease or difficulty with which a metal can be cut. The machinability of a material has a direct correlation with the material’s hardness, or its ability to resist penetration or deformation. There are a number of tests that measure a materials hardness, but the most common test for machinability and hardness is Brinnel. Brinnel or BHN is stated as a number: the higher the BHN number the harder the material. Different material structures pose different problems for the machinist. With the cutting tool type being equal, look at what happens to the cutting speed as the materials Brinnel hardness increases (see Figure 2, Cutting Speed Chart).

Material	Material Condition	Hardness, Bhn	Cutting Speed, fpm
Material	Material Condition	Hardness, Bhn	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

Figure 2. Chart of Cutting Speeds

The hardness or Grade of the cutting tool will also affect the cutting speed. By looking at the chart below (Figure 3), you can see that the six grades of Kennametal type inserts have significantly differing cutting speeds for the same hardness of workpiece material.

Figure 3. Carbide Grades and Cutting Speeds

The hardness of the coatings on the insert will also affect the cutting speeds that you select. To select the proper cutting speeds for the material and the tool, you will have to refer to the technical information that is supplied by the tooling companies.

Feedrate

Once the cutting speed is selected for a particular workpiece material and condition, the appropriate feed rate must be determined. When we establish feed rates for turning tools, the goal in roughing applications is to attain the maximum metal removal rate possible with the available part rigidity and machine horsepower. Selecting the proper feed and speed for roughing is a balancing act. The relationship to feed rates and speeds have a great deal of effect on the life of the cutting edge (see Figure 4).

Figure 4. Relationship of Speed to Feed

In finish turning operations, feed rates are established to produce the surface finish specified on the part blueprint. Feed in turning is measured in inches per revolution, or IPR. This represents the linear distance the tool moves in inches for each revolution of the part. Being that in turning operations you have a single cutting edge, feedrate will sometimes be expressed as the chip load. The feedrate can also expressed as the distance traveled in a single minute, or IPM (inches per minute). When establishing the feedrate for roughing operations, it is important not to over feed the nose radius of the insert. Generally, the feedrate for roughing should not be more than half the size of the nose radius. See the figure 5 chart below.

Nose Radius	.016	.031	.047	.062	.094
Feedrate	.005 - .010	.010 - .020	.014 - .028	.020 - .040	.028 - .062

Figure 5. Feed Rate and Nose Radius Selection for Roughing

Nose Radius, Feed Rate Selection, and Surface Finish

Nose radius and feed rate have the greatest impact on surface finish. To determine the feed rate required for a theoretical surface finish using a certain nose radius, refer to the chart in figure 6 below or charts found in your tool handbooks.

Figure 6. Nose Radius Selection and Surface Finish

Locate the required surface finish on the vertical axis.
Follow the horizontal line corresponding to the desired finish to where it intersects the diagonal line corresponding to the feed rate.
Project a line downward to the nose radius scale and read the required nose radius.
If the line falls between two values, choose the larger nose radius.
If no available nose radius will produce the required finish, the feed rate must be reduced.
Reverse the procedure to obtain the surface finish for a given feed rate and nose radius.

PRODUCTIVITY

Productivity in a turning operation can be improved by increasing the depth of cut, feed rate or cutting speed provided the appropriate level of machine horsepower is available. We will examine the effects of increased productivity on the cutting edge and work piece as these parameters are increased individually.

DEPTH OF CUT

Maximize the depth of cut amount. The easiest cutting parameter to adjust is the depth of cut. Doubling the depth of cut in a turning operation will double the metal removal rate without any increase in cutting temperature. The horsepower consumed will virtually double, but there will be no reduction in tool life (specific wear per inch of cutting edge length) assuming the cutting edge can withstand the added tangential cutting force. However, it is not always possible to increase the depth of cut to gain additional productivity, since there might not be any remaining material to remove.

FEED RATE

The feed rate is often very simple to alter, therefore, it is the second most likely parameter to increase to gain added productivity. Doubling the feed rate makes the actual chip twice as thick thus making it much more difficult to curl and bend. However, the tangential cutting force, cutting temperature and horsepower increase, but they aren't doubled. This occurs because the tool is cutting more efficiently and less power is being wasted in heat generation per cubic inch of material removed. Tool life is reduced, but not halved. The additional force impeded on the cutting edge often causes crater wear(Figure 7) of the top rake insert surface due to the increased temperature and friction generated during the cut. But, the cutting force per square inch of material removed (specific cutting force) is actually decreased.

Figure 7. Crater Wear

Obviously, if the feed is increased without monitoring the effect on the tool catastrophic failure of the insert will result when the chip becomes stronger than the cutting edge.