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 

You should calculate RPM & Feed whenever machining with a Mill, Drill or Lathe.  Experienced machinists often "fudge it" while manual machining, making changes based on the "feel" of the machine and the sound of the cut.  With CNC the RPM & Feeds need to be right before you hit the green button.

Definitions & Explinations
Cutting Speeds and Lathe Feed
Milling Machine Feed Rates
My Tests with Plastic
Quick RPM Table
Calculating RPM
Calculating Feed
Speed and Feed Links


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.  This "Ideal" cutting speed assumes sharp tools and flood coolant.  Adjustments need to be made for less than ideal cutting conditions.  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.

Feed Rate(Milling Machine) refers to how fast a milling-tool moves through the material being cut.  This is calculated using the Feed Per Tooth(FPT) to come up with the Inches Per Minute that a milling bit can move through a particular type of material.  Thus, a Four-Flute End-Mill will cut through material at twice the speed of a Two-Flute End Mill.  Feed Rates will decrease with dull tools, a lack of coolant, or deep cuts.

Feed Rate(Lathe) refers to how fast a lathe-tool should move through the material being cut.  This is calculated using the Feed Per Revolution for the particular material.  Lathe tools generally have only one tooth, so in most cases the FPT and FPR will be the same.  Feed rates will decrease with dull tools, a lack of coolant/lubrication, or deeper cuts.

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), round down to the 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). 

Approximate Material Cutting Speeds & Lathe Feed-Per-Revolution:
RPM and Feed Rates
Material Ballpark CS with High-Speed Tool Cutting Speed High-Speed Tool Cutting Speed Carbide Tool Feed/Rev
HSS Tool
Feed/Rev Carbide Tool
SAE 1020 - Low Carbon Steel 100  80-120  300-400  .002-.020 .006-.035 
SAE 1050 - High Carbon Steel 60  60-100  200  .002-.015 .006-.030 
Stainless Steel 100  100-120  240-300  .002-.005 .003-.006 
Aluminum  250  400-700  800-1000  .003-.030 .008-.045 
Brass & Bronze 200  110-300 600-1000 .003-.025 .008-.040 
Plastics*  250  200- 500 1000  .005-.050 .005-.050 
*Variation in Cutting-Speed & Feed-per-Revolution will exist with different alloys, procedures, tools & desired finishes.  Feed-Per-Revolution is also affected by the size of the lathe-tool, as well as the depth of cut.  The cutting speed and speed of plastics will vary greatly depending upon the type of plastic.
Link: Cutting Speeds by Specific Alloy

Approximate Feed Rates (Feed Per Tooth) for End Mills
Material .050" Depth of Cut .250" Depth of Cut
  1/8" 3/8" 1/2"   3/8" 3/4"
Plain Carbon Steels .0005-.001 .002-.003 .003-.004   .001-.002 .002-.004
High Carbon Steel .0003-.001 .001-.003 .002-.004   .0003-.001 .001-.004
Tool Steel .0005-.001 .001-.003 .002-.004   .001-.002 .003-.004
Cast Aluminum Alloy .002 .003 .005   .003 .008
Cast Aluminum -Hard .001 .003 .005   .003 .006
Brasses & Bronzes .0005-.001 .003-.004 .004-.006   .002-.003 .004-.006
Plastics *Much Variation .002 .004 .005   .003 .008
*Variation in Feed-per-Tooth exists with different Material Alloy Harness, Tool Qualities, Cutting Techniques and Desired Finishes.  Contact the manufacturer if precision is important.

Twist Drill Feeds (Feed per Revolution)

Drill Size Inches Drill Feed Inches Drill Size Metric Drill Feed Millimeter
1/8" and smaller 0.001" to 0.002 3mm and smaller .02mm to 0.05mm
1/8" to 1/4" 0.002" to 0.004" 3mm to 6mm 0.05mm to 0.10mm
1/4" to 1/2" 0.004" to 0.007" 6mm to 13mm 0.05mm to 0.10mm
1/2" to 1" 0.007" to 0.015" 13mm to 25mm 0.18mm to 0.38mm
1 to 1 1/2" 0.015 to 0.025" 25mm to 38mm 0.38mm to 0.63mm

Quick RPM/Spindle Rate Calculations: Lathe, Mill, Drill (HSS Cutter)
(RPM changes with Cutting Speed & Diameter)

Material 1/4" Dia 1/2" Dia 1" Dia 1 1/2" Dia 2" Dia
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)

Example #3 Use the information and RPM calculated in Example #2 for a Milling Machine, ball-parking the FPT(Feed per Tooth) of .005 (see table), and a cutting depth of .050"

Feed Rate = (2 x 2000 x .005) =  20 inches/minute  

Lathes: Cut/ Revolution and Thread/Inch.Lathes generally take Feed-Per-Tooth directly without conversion. (HAAS TL-1 Procedure Screen)

On lathes the Feed is generally expressed as Feed per Revolution.  In practical terms this is easy.  Input the Feed per Revolution for basic turning  As the RPM changes, so too will the movement of your lathe bit. 

Plastic on a CNC Lathe... a greenhorn's perspective
The following, with stock held in a 3-Jaw Chuck and using a sharp HSS lathe tool, worked for me.  Your results may differ. 
Acetel/Delrin - Turning at CS 325, Depth of Cut 0.035, Feed 0.015 - 0.010 Depth of Cut could be increased.  Slower Feed Rate gives smoother finish.  At 0.015 Feed Rate there were striations.
UMHW - Turning at CS 450, Feed 0.015 Nice finish.  Slower speeds produced a rougher finish.
UMHW - Part-Off at CS 250, Feed 0.01 Parted smoothly.
When turning plastic, taking too aggressive a cut can cause the plastic to deform and pull from a 3-Jaw chuck.  This has happened to me.  Also, I generally use lower-speeds and higher-feeds when drilling plastic, as heat builds up and begins to melt the inside of the hole.

Quick RPM Spindle Rate Table

Speed and Feed Links
Fox Valley Tech Feeds & Speeds
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