Speeds & Feeds
Modern milling cutters capable of operating at higher feeds and speeds, and moving more cubic inches of metal per minute, require greater machine rigidity and more power.
Therefore it is important to determine that enough power is available to handle the desired depth and width of cut at the higher feeds and speeds.
T= Number of teeth in cutter
D= Cutter diameter in inches
RPM= Revolutions per minute
SFM= Surface feet per minute
F= Feed in inches per minute
f= Feed per tooth in inches
W= Width of cut
d= Depth of cut
HP= Motor horsepower
C= Machinability constant
Machinability constant values for various materials are based on removing one cubic inch of metal per minute per horsepower with 60% power efficiency at the spindle nose and a 25% allowance for cutter dulling.
Aluminum, Magnesium, Dural – 4.0 plus
Brass – 2.5
Soft Bronze, Copper – 2.0
Cast Iron – 1.5
Steel up to 150 Brinell, Malleable Iron – 0.75
Steel, 300 Brinell, Hard Bronze – 0.6
Steel, 400 Brinell – 0.5
Speeds & Feeds – Carbide
In conventional milling, the cutter revolves opposite to the direction of table feed. Therefore the width of the chip starts at zero and increases to a maximum at the end of the cut. This can lead to accelerated tool wear under some conditions – conventional milling is recommended for hot rolled steel, surface hardened materials and steels with a surface scale. In climb milling, the cutter revolves in the same direction as the table feed. The tooth meets the work at the top of the cut, producing the thickest part of the chip first. In horizontal applications the resultant force created by climb milling can act as a clamping force, acting toward the machine table. It is important to make sure that the machine tool has no leadscrew backlash. Normally climb milling improves product surface finish and increases tool life.
Advantages of Climb Milling
Longer Tool Life: Since the chips produced are deposited behind the cutter, tool life can be substantially increased.
Ease of Fixturing: Climb milling exerts a downward clamping force on the workpiece and not an upward force as in conventional milling, which results in simplified fixturing.
Improved Surface Finish: Since the chips are not carried by the cutter, less likelihood of marring the machined surface.
Lower Power Requirements: A higher rake angle can be utilized, lowering power consumption.
Better Chip Evacuation: Easier and faster chip removal since chips are deposited behind the cutter.
Drill Time Formula
Speeds & Feeds – Formula
|Revolutions per minute (RPM)||SFM||(SFM x 12) / (Diameter of drill x 3.1416)|
|Surface feet per minute (SFM)||RPM||(Diameter of drill x RPM x 3.1416) / 12|
|Feed rate per RPM (FR)||SFM and FM||(Diameter of drill x FM x 3.1416) / (SFM x 12)|
|Feed rate per RPM (FR)||RPM and FM||FM / RPM|
|Feed rate per minute (FM)||FR and RPM||RPM x FR|
|SFM||RPM and drill dia.||.26 x RPM x drill diameter|
|RPM||SFM and drill dia.||3.8 x (SFM / drill diameter)|
|Aluminum and Aluminum Alloys||150-300|
|Brass and Bronze (free cutting)||150-300|
|Brass and Bronze (high tensile)||70-120|
|Cast Iron (soft)||80-120|
|Cast Iron (medium)||60-90|
|Cast Iron (hard)||30-70|
|Nickel Base Alloys||20-50|
|Plastic and Related Materials||100-200|
*Surface feet per minute
Drilling Time Formula
Time (Minutes) = Travel(in.) / RPM x Feed (per rev.)
Travel = Sum of: Depth of Hole, 1/3 Drill Diameter, Approach Clearance, Over Travel (through cavities) / Total Travel (in.)
Drill Speeds (Steel)
|Alloyed – under 200 B.H.||60-90|
|Alloyed – 200 – 300 B.H.||40-70|
|Alloyed – over 300 B.H.||20-30|
|Cast and Forged||40-70|
|Heat Treated – 35 – 40 R.C.||30-40|
|Heat Treated – 40 – 45 R.C.||20-30|
|Heat Treated – over 45 R.C.||10-20|
|Mild – .2 – .3 Carbon||70-100|
|Mild – .4 – .5 Carbon||50-80|
|Stainless – 300 Series||20-50|
|Stainless – 400 Series||30-70|
|Tool – over 1.0 Carbon||40-60|
*Surface feet per minute
|Diameter (in.)||Light Feeds||Heavy Feeds|
|1/8||.0005 – .0010||.0015|
|3/16||.0010 – .0015||.0020|
|1/4||.0015 – .0020||.0025|
|5/16||.0020 – .0025||.0030|
|7/16||.0025 – .0030||.0035|
|1/2||.0035 – .0040||.0045|
|5/8||.0045 – .0050||.0055|
|3/4||.0055 – .0060||.0065|
The above are suggested ranges. Due to many variable in an operation, more optimum speed may be established through trial.
TiN – General purpose coating for Steels, Stainless Steels and Inconel. Excellent wear characteristics in roughing applications.
TiCN – High performance in Die and Mold Steels, Hardened Materials, Steels and Stainless Steel. Ability to run at increased Feeds and Speeds over TiN coated tools.
TiALN – Best results in Dry Milling applications at high temperatures. Works well in Hardened Materials, Titanium Alloys, Stainless Steels, Cast Irons, Graphite and HSM applications.