Cutting Data

Tables on the following pages provide basic speed, feed and cutting data for some of the materials commonly used for prototypes. Use the tool manufacturer's data instead whenever it is available.

Mill Cutting Speeds (SFM) surface ft/min

Material

HSS

Carbide

Aluminum600800
Brass175175
Delrin400800
Polycarbonate300500
Stainless Steel (303)80300
Steel (4140)70350

Table 3.5: Milling Speed Data (SFM)

Drill Cutting Speeds (SFM) surface ft/min

Material

Drilling

C-Sink

Reamer

Tap

Aluminum300200150100
Brass1209066100
Delrin15010075100
Polycarbonate240160120100
Stainless Steel (303)50352535
Steel (4140)90604535

Table 3.6: Drill Cycles Speed Data (SFM)

Never use tools that have been used to machine metal to cut plastic. The sharp edge of the tool will be compromised and cutting performance and finish will suffer. A good practice is to keep two sets of tools: one for plastic and one for metal.

High speed steel cutters work best for plastics. Carbide cutters work better for aluminum and other metals.

Cutting Feeds (IPR) in/rev

Operation

Tool Diameter Range (in)

 <.125.125-.25.25-.5.5-1.>1.

Milling

Aluminum

.002.002.005.006.007

Brass

.001.002.002.004.005

Delrin

.002.002.005.006.007

Polycarbonate

.001.003.006.008.009

Stainless Steel (303)

.0005.001.002.003.004

Steel (4140)

.0005.0005.001.002.003
 

Drilling

.002.004.005.010.015
 

Reaming

.005.007.009.012.015

Table 3.7: Feed Data (IPR)

Best Practice Machining Parameters

Best practice machining parameters for prototype and short-production milling are different than for mass production. Production machining is obsessed with minimizing run time and maximizing tool life because even small improvements per part can result in significant cost savings.

Prototype and short run production seeks to maximize reliability. Obviously, it does not make sense to risk breaking a tool or scrapping a part trying to save a few seconds if only making a few parts.

Tables 3.8 and 3.9 on the following pages list recommended machining parameters for prototypes. The values are relatively conservative and work well for materials and tool types listed on the previous pages.

For materials or tools not listed, consult cutting data from the tool manufacturer.

Recommended Machining Parameters

OperationParameterValue
AllClearance Height1.0 inch
AllFeed Height.1 inches
AllRapid HeightAs needed to clear clamps and fixtures
Mill (Roughing)Stepover (XY)50-80% of tool dia.
Mill (Roughing)Stepdown (Z)25-50% of tool dia.
DrillPeck Increment.05 inches
Spot DrillDwell.5 seconds

Table 3.8: Machining Parameters

Stock Finish Allowances (inches)

Operation

Tool Diameter Range (in)

 <.125.125-.25.25-.5.5-1.>1.

Milling (XY)

.001.005.015.020.020

Milling (Z)

.001.002.005.005.005

Reaming

.005.010.012.020.030

Table 3.9: Stock Allowances

Troubleshooting Speed/Feed Problems

Do not make the mistake of thinking that the only option when encountering a machining problem is to reduce feed rate. Sometimes that is the worst thing to do and decreasing speed and increasing feed may be a better option.

Be methodical. When a problem occurs, stop. Analyze what is happening, draw on all available resources, and then devise a solution to correct the problem. The Machinery's Handbook (Industrial Press Inc, 2008, New York, NY, ISBN: 978-8311-2800-5) contains extensive information about diagnosing and correcting cutting tool problems. This book is an essential reference for anyone using machine tools.