Milling: Cutting Speeds & RPM Calculations

There are three factors that make up the cutting conditions; cutting speed, depth of cut, and feed rate. In this information sheet we will concentrate on feed rate factors and calculations. The table feed rate on milling machines is given in terms of inches per minute (IPM). Inches per minute is the rate at which the tool will advance into the work. The feed rate, that can be used, is determined by the speed of the rotation of the cutter (RPM), the number of cutting teeth on the cutter, and by the size of the chip that the cutter can withstand. The chip size is called the feed rate in inches per tooth or chip load (Figure 1).

Figure 1

The recommended values for chip load are based on the cutting tool material, the cutting tool size, and the hardness or machinability rating of the workpiece material. The recommended values for feed per tooth (chip load) can be found in charts in the Machinery’s Handbook, your textbook, and charts given to you by your tool salesperson. A typical feed in inches per tooth chart can be found in Table 2.

While the recommended feed rates found in these charts represent good fundamental machining practice, they are however only recommended values. Deviations from these recommended values may be necessary due to certain circumstances. Circumstances such as thin or frail part sizes. The feed rate used on small or thin work may need to be reduced. The work holding technique has a great deal to do with the feed rate. Setups, which lack rigidity, may require a slower feed rate. The configuration of the milling machine may also require an adjustment in the feed rate. Feed rates on C-Frame milling machines can be much heavier than those feed rates used on ram type milling machines.

When using large carbide face mills, the available horsepower and the rigidity of the machine spindle will always influence the feed rate.

Table 2. Recommended Feed in Inches per Tooth for High-Speed Steel Milling Cutters

Material	Hardness, Bhn	End Mills							Face Mills and Shell End Mills	Plain or Slab Mills	Side Mills	Form Relieved Cutters
		Depth of Cut .250"			Depth of Cut .050"
		Cutter Diameter			Cutter Diameter
		3/8	3/4	1 and up	1/8	3/8	3/4	1 and up
Feed per Tooth, Inch
Plain Carbon Steels, AISI 1010 to 1030	to 150 150 to 200	.002 .002	.004 .003	.006 .005	.001 .001	.003 .003	.006 .006	.008 .007	.012 .012	.008 .008	.008 .006	.004 .004
AISI B1111, B1112, B1113	140 to 180	.002	.004	.006	.001	.004	.006	.008	.012	.010	.008	.005
Plain Carbon Steels, AISI 1040 to 1095	120 to 180 180 to 220 220 to 300	.002 .002 .001	.004 .004 .002	.006 .005 .003	.001 .001 .0005	.003 .003 .002	.006 .006 .003	.008 .007 .004	.010 .012 .008	.008 .008 .004	.008 .006 .004	.004 .004 .003
All Alloy Steels Having .3% Carbon Content or Less	180 to 220 220 to 300 300 to 400	.002 .001 .0005	.004 .002 .002	.005 .003 .002	.001 .0005 .0003	.003 .002 .001	.006 .003 .002	.008 .004 .003	.010 .008 .004	.008 .005 .003	.008 .005 .003	.004 .003 .002
All Alloy Steels Having More Than .3% Carbon Content	180 to 200 220 to 300 300 to 400	.002 .001 .0005	.004 .002 .001	.005 .003 .002	.001 .0005 .0003	.003 .002 .001	.006 .003 .002	.008 .004 .003	.012 .008 .004	.008 .005 .003	.008 .005 .003	.004 .003 .002
Tool Steel	200 to 250 250 to 300	.002 .001	.004 .003	.005 .004	.001 .0005	.003 .001	.006 .002	.008 .003	.010 .004	.006 .004	.006 .004	.004 .003
Cast Iron	150 to 180 180 to 220 220 to 300	.003 .002 .002	.006 .005 .004	.008 .006 .005	.001 .001 .0005	.004 .003 .003	.007 .006 .005	.009 .007 .006	.014 .012 .006	.012 .010 .006	.009 .007 .006	.005 .004 .003
Zinc Alloys		.004	.008	.012	.002	.005	.008	.012	.020	.010	.010	.005
Brasses and Bronzes	100 to 150 150 to 250	.003 .002	.006 .004	.010 .006	.001 .0005	.004 .003	.008 .005	.010 .008	.014 .010	.008 .005	.008 .005	.004 .003
Free Cutting Brasses and Bronzes	80 to 100	.003	.008	.010	.001	.004	.008	.010	.014	.008	.008	.005
Cast Aluminum Alloy–as Cast		.003	.008	.010	.002	.003	.010	.012	.020	.010	.010	.005
Cast Aluminum Alloy–Hardened		.003	.006	.008	.001	.003	.008	.010	.012	.008	.008	.005
Wrought Aluminum Alloy–Cold Drawn		.003	.008	.010	.002	.003	.010	.012	.018	.010	.010	.005
Wrought Aluminum Alloy–Hardened		.003	.006	.008	.001	.003	.008	.010	.012	.008	.008	.005
Magnesium Alloys		.003	.008	.012	.002	.004	.010	.014	.020	.012	.012	.005
Ferritic Stainless Steel	135 to 185	.003	.004	.005	.001	.004	.006	.008	.012	.008	.008	.004
Austenitic Stainless Steel	135 to 185 185 to 275	.003 .002	.004 .003	.005 .005	.001 .0005	.004 .003	.006 .004	.008 .006	.012 .010	.008 .006	.008 .006	.004 .004
Martensitic Stainless Steel	135 to 185 185 to 225 225 to 300	.003 .003 .002	.005 .003 .002	.005 .005 .003	.001 .0005 .0005	.004 .004 .003	.006 .005 .003	.008 .006 .004	.012 .010 .008	.008 .006 .004	.008 .006 .003	.004 .004 .003
Plastics		.003	.008	.010	.002	.004	.010	.014	.020	.012	.012	.006

Feed Rate Calculations-The feed rate in inches per tooth must be converted into feed rate in inches per minute (IPM) before you can make the feed rate setting on the machine. The formula for converting feed rate in inches per tooth into inches per minute is as follows:

Feed Rate (in./min.) = RPM x Chip load x # Teeth

This simplified version of the feed rate formula is used in most machine shops. Again, it should be pointed out that these feed rates setting can only be used under ideal circumstances. You will typically be given a range of chip load factors to use. A good rule

of thumb is to start out at the low range or average feed per tooth factor and increase the feed rate to the capacity of the machine tool, the setup, and the desired surface finish. It must also be mentioned that using a chip load that is too small will cause excessive tool wear so don’t just set the feed rate low and think this is correct.

Let’s try some feed rate calculations. Follow along using the recommended feed rate charts in figure 2.

A four flute 0.500 inch high speed steel (HSS) end milling cutter is to be used on a piece of 1018 steel with a brinnel hardness of 200. The closest RPM setting to perform this cut is 750 rpm. Look up the feed per tooth in the charts and calculate the feed rate in inches per minute.

RPM = 750

Feed in inches per tooth (chip load) = 0.004 avg.

Number of teeth (flutes) = 4

Feed (in. / min.) = RPM x Chip Load (CL) x # Teeth (flutes)
Feed (in. / min.) = 750 x 0.004 x 4
Feed = 12 in. / min.

Since the available feed rate settings are generally not infinitely variable, the machine cannot be set precisely to the calculated feed rate setting. Some judgment must be made in selecting the feed rate to use. Try to get to the feed rate that is nearest to the calculated amount, but if you can’t, consider the following conditions. What are your surface finish requirements? A larger feed rate will leave a rougher finish. What is your depth of cut? If it is a deep cut, go to the slower feed 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.

Lets try another examples, but this time we must first calculate the RPM.

A two flute, .250 inch high speed steel (HSS) end milling cutter is to be used on a piece of 8620 alloy steel with a brinnel hardness of 300. Calculate the RPM setting first to perform this cut using the average (avg.) cutting speed factor found in the chart in figure 2. Also, calculate the feed rate in inches per minute using the average (avg.) feed in inches per tooth factor found in the chart in figure 2.

RPM = 320

Feed in inches per tooth (chip load) = 0.008 avg.

Number of teeth (flutes) = 2

Feed (in. / min.) = RPM x Chip Load (CL) x # Teeth (flutes)
Feed (in. / min.) = 320 x 0.008 x 2
Feed = 5.12 in. / min.

Top

		Machine Shop Home

Introduction \| Safety \| Milling Machines \| Speeds/Feeds \| Cutting Tools \| Broaching \| Projects \| Tests