SouthBayMachine.com

Integrated Design - Advanced Manufacturing

Machine tools are dangerous and may cause great injury.  This information was collected from a variety of sources, is neither complete nor verified, and is of a general nature for theoretical study only.  Any attempt to duplicate the operations described should be done with the guidance and supervision of a qualified instructor who will teach the appropriate safety skills and fill in the missing details.  Follow this link for Statements of Warning, Limitation & Responsibility.

Cutting Speed & Feed Rates 

Know a material's Cutting Speed to calculate your RPM.Cutting Speed(CS) of a material is the ideal number of Feet-per-Minute that the tool-bit should pass over the work-piece.  Different materials (High-Carbon/Low-Carbon Steels, Aluminums, Different kinds of Plastics) have different Cutting Speeds and can be worked/cut at different rates.  In addition, some tools or processes (like threading, knurling, or cutting-off) will need to be worked at slower speeds than the Cutting Speed would indicate.

Diameter refers to the diameter of whatever is spinning: work-piece(Lathe) or cutting tool-bit(Mill/Drill).  *As the diameter gets bigger use a slower RPM.

RPM(Revolutions Per-Minute) is the turning speed of whatever is spinning: On a Lathe this is the work-piece.  On a Mill or a Drill it is the cutting-tool.  *Using Cutting Speed and Diameter you can calculate RPM as shown further down on this page.
When calculating spindle speed(RPM), choose the closest slower speed option offered by your Lathe/Milling Machine/Drill.  Operations like Threading, Knurling, or Parting-off, require much slower speeds (Generally 1/3 to 1/4 Calculated RPM for Threading, Knurling & Parting-off). 

General Cutting Speeds & Feed-Per-Tooth for Calculating RPM and Feed Rates
Material Ballpark CS with High-Speed Tool Cutting Speed High-Speed Tool Cutting Speed Carbide Tool Feed per Tooth
SAE 1020 - Low Carbon Steel 100  80-120  300-400  .003-.007 
SAE 1050 - High Carbon Steel 60  60-100  200  .003-.007 
Stainless Steel 100  100-120  240-300  .002-.005 
Aluminum  250  400-700  800-1000  .007-.018 
Brass & Bronze 200  110-300 600-1000 .003-.008 
Plastics  500  500 1000  .003-.015 
*Variation in Cutting-Speed & Feed-per-Tooth will exist with different alloys, procedures, tools & desired finishes.  Contact the manufacturer if precision is important.
 Link: Cutting Speeds by Specific Alloy

Quick RPM/Spindle Rate Calculations: Lathe, Mill, Drill
 (RPM changes with Cutting Speed & Diameter)
Diameter 1/4 Inch 1/2 Inch 1 Inch 1.5 Inch 2 Inch
Low-Carbon Steel 1600 RPM 800 RPM 400 RPM 267 RPM 200 RPM
High-Carbon Steel 960 480 240 160 120
Aluminum 4000 2000 1000 667 500
Brass & Bronze 3200 1600 800 533 400
* RPM Spindle Speed Examples calculated using Ballpark Cutting Speeds with High-Speed Steel cutting tools

Calculating RPM

Lathes, Milling Machines, Drills
RPM (Turning Spindle Speed) of the cutting tool or work piece is calculated as follows:

RPM = (Cutting Speed x 4)/Diameter

RPM = Spindle Speed
Cutting Speed = Cutting Speed for the material being cut/worked.
Diameter = The Diameter of whatever is turning.

Example #1 Calculate RPM for turning a 1 inch diameter piece of Low-Carbon Steel with a Cutting Speed of 100 on a Lathe. (Double-check CS table)

RPM = (100 x 4)/1 = 400 RPM

Example #2 Calculate RPM (Spindle Speed) for a 1/2 inch High-Speed-Steel 2 Flute End-Mill cutting Aluminum with a CS of 250 on a Milling Machine

RPM = (250 x 4)/.5 = 2000 RPM  

Example Feed on Kent CNC Milling Machine "Inches Per Minute"Calculating Feed Rates

Aluminum spinning at 400 RPM with an Automatic Feed Rate of .0071Link: Machine Shop Feed Rates Explained

Milling & Drilling
The Feed Rate in "INCHES Per MINUTE" is determined by multiplying the number of cutting teeth by the RPM, multiplying that product by the Feed per Tooth, and dividing by 3.  The calculation is as follows:

Feed Rate = (Number of Cutting Teeth x RPM x Feed Per Tooth)/3

Example #3 Use the information and RPM calculated in Example #2 for a Milling Machine, ball-parking the FPT(Feed per Tooth) at .010(see table).

Feed Rate = (2 x 2000 x .010)/3 =  13.3 inches/minute  Lathes: Cut/ Revolution and Thread/Inch.Lathes generally take Feed-Per-Tooth directly without conversion. (HAAS TL-1 Procedure Screen)

Lathes
 On lathes the Feed is generally expressed a the amount of Feed per Revolution.  In practical terms this is easy.  Just use the Feed per Tooth(shown on the Feed & Speed Table) for basic turning. 


Quick RPM Spindle Rate Table

Link - Suggested Cutting Speeds
Link - More Cutting Speed Charts
Link - Pierce College Cutting Speed & Feed 

Automatic Milling Speed CalculatorReccomended Feed & Speed Charts for Roughing or Finishing






Top of Page



copyright 2009