Cutting Speed and Feed Rate

Cutting Speed and Feed Rate Settings

The cardinal rule in machining is to remove as much material as possible within the limits of machine capability. That is, to machine as quickly as possible. It is not so much a question of minimizing time wasted machining, but one of maximizing cutting tool life.

• Feedrates that are too low produce excessive heat which may cause premature failure of the cutting edge.
• Feedrates that are too high may cause the cutting edges to fracture or cause more catastrophic failure.
• Cutter speeds outside the recommended range may cause the cutting edges to experience buildup, wear excessively, crater, chip, or produce poor workpiece surface finish.

Cutting speed is the term used to express the velocity of the outside edge of the milling cutter (SFPM = surface feet per minute) as it cuts a specific material. Each material has an optimum range for its machinability with each cutting tool material (i.e. H.S.S., Carbide, etc.) Recommended cutting speeds are given in charts, usually as a range.

Feed rate (IPM = inches per minute) is the rate at which the cutting tool advances into the work. The allowable feed rate is governed by the cutter rotation speed (RPM), the number of cutting teeth on the cutter (called "flutes"), and by the size of the chip that the cutter can withstand (the chip load.)

Chip load (IPT = inches per tooth) is a measure of the chip thickness that one tooth can carve off of the workpiece. The recommended values for chip load are based on the cutting tool material, the cutting tool size, and the hardness of the workpiece material. The recommended values for feed per tooth are given in charts, usually as a range.

The formulae shown in the table bellow are used to compute the feedrate and cutter speed. The cut is assumed to be a slot of width equal to the tool diameter. The depth of the cut is specified in the tables that provide the SFPM and IPT values. As a rule-of-thumb do not bore deeper than the tool radius when making slots.

TERM	EQUATION	RESULT
Revolution Speed	RPM = 3.82 x SFPM ÷ D	Spindle RPM
Inches per Minute	IPM = RPM x IPT x (No. of Flutes)	Tool Travel Speed
Where: D: Tool diameter in inches SFPM: Surface Feet/Minute. Lookup in a table based on material being machined. IPT: Chip Load/tooth (feed per tooth in Inches Per Tooth). Lookup in a table. Remember that the feed rate and speed setting can only be used under ideal circumstances.

Alternatively, this MATLAB M-file may be used to compute feedrate and tool speed. (Note: This program returns different feed and speed values than those computed by hand using information on this page. The M-file uses a different set of tables for SFPM and IPT. This goes to show the variability of the RPM and IPM values.)

While the recommended feedrates found in charts represent good fundamental machining practice, they are however only recommended starting values. SFPM and IPT vary by material machined, material of the cutter, sharpness of cutter, type/amount of coolant used, depth of cut, milling machine horsepower, etc. Circumstances usually require deviation from these recommended values.

For instance,

• The feedrate used on small or thin work may need reducing.
• The work holding technique has a great deal to do with the feed rate. Setups lacking rigidity may require a lower feedrate.

Remember that using a chip load that is too small will cause excessive tool wear. Do not just set the feed rate low and think this is correct. A good rule of thumb is to start out at the low or mid range of chip load and increase the feedrate to the capacity of the machine tool, the setup, and the desired surface finish. Selecting the speed and feed for a job is an art and some judgment must be made based on common sense. For instance,

• Does the chip formation look good?
• Does the milling machine sound as if it is struggling?
• Does the finish look bad?

APPROXIMATE CUTTING SPEEDS (SFPM)
	H.S.S. Tooling	Carbide Tooling
Aluminum	400	1000
Brass	300	800
Cast Iron	80	350
Steel - Mild	100	450
Steel - Carbon	60	300
Steel - Stainless	40	200

APPROXIMATE CHIP LOAD (IPT) H.S.S. Tooling
1/32 to 3/32"	0.0002 - 0.0004"
1/8 to 3/16"	0.0002 - 0.001"
1/4 to 5/16"	0.0005 - 0.002"
3/8 to 1/2"	0.0005 - 0.003"
9/16 to 11/16"	0.0005 - 0.004"
3/4 to 15/16"	0.001 - 0.006"
1 to 3"	0.003 - 0.015"