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.

Table 3.5: Milling Speed Data (SFM)
Mill Cutting Speeds (SFM) surface ft/min
Material	HSS	Carbide
Aluminum	600	800
Brass	175	175
Delrin	400	800
Polycarbonate	300	500
Stainless Steel (303)	80	300
Steel (4140)	70	350

Table 3.6: Drill Cycles Speed Data (SFM)
Drill Cutting Speeds (SFM) surface ft/min
Material	Drilling	C-Sink	Reamer	Tap
Aluminum	300	200	150	100
Brass	120	90	66	100
Delrin	150	100	75	100
Polycarbonate	240	160	120	100
Stainless Steel (303)	50	35	25	35
Steel (4140)	90	60	45	35

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.

Table 3.7: Feed Data (IPR)
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

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.

Table 3.8: Machining Parameters
Recommended Machining Parameters
Operation	Parameter	Value
All	Clearance Height	1.0 inch
All	Feed Height	.1 inches
All	Rapid Height	As needed to clear clamps and fixtures
Mill (Roughing)	Stepover (XY)	50-80% of tool dia.
Mill (Roughing)	Stepdown (Z)	25-50% of tool dia.
Drill	Peck Increment	.05 inches
Spot Drill	Dwell	.5 seconds

Table 3.9: Stock Allowances
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

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.