Calculating Feeds and Speeds from a Material: Mill/Router
Mastercam automatically takes tool and stock material into consideration when calculating speed and feed percentages needed for an operation. Use the Feed and Speed calculator to make adjustments.
The calculations and approaches are taken directly from the Machinist's Handbook (2000: Industrial Press)and based on the formulas described in the following sections. If you need to adjust these values (for example, to compensate for a hardened or softened material), or need to create a material that is not in the library, you can do so in the Material Definition dialog box.
Spindle speeds are based on the cutting speed (CS), which is calculated from the material’s base cutting speed in SFM multiplied by the Operation Type CS percentage multiplied by the tool’s CS percentage multiplied by the tool material's CS percentage.
CS = (material base CS value x operation type CS %) x tool CS % x tool material CS %
Most of these values are stored as part of the material definition and accessed in the Material Definition dialog box. The tool’s cutting speed % is specific to each tool and is read from the tool definition. You set this on the Parameters tab for the tool definition in the % of matl. cutting speed text box.
For example, aluminum has a base CS of 1000 SFM (surface feet/minute). Contour operations use 60% of this base value. The .500 inch diameter end mill assigned to the contour operation has its CS percentage at 80%. The end mill is constructed of titanium-coated carbide and has its CS percentage at 200%. The cutting speed for this material then equals 960 SFM using the following equation:
CS = (1000 x .60) x .80 x 2.0 = 960 SFM
For inch units, the CS value is then used to calculate the spindle speed (RPM) using the following equation:
Spindle speed = (3.82 x CS) / .50 (tool diameter)
For the aluminum example, the spindle speed for a 0.25 inch tool would be:
Spindle speed = (3.82 x 960) / .25 = 14,668.8 RPM
Feed rates are calculated in much the same way, starting with the material’s base feed per tooth (FPT) value multiplied by the Tool Type FPT percentage multiplied by the tool’s FPT percentage.
FPT = (material base FPT value x tool type FPT %) x tool FPT % x tool material FTP %
Set the tool FPT% on the Parameters tab for the tool definition in the % of matl. feed per rev text box.
For example, aluminum has a base FPT value of .008 inches/tooth. Contour operations use 75% of this base value. The 0.500 inch diameter end mill assigned to the contour operation has its FPT percentage at 90%. The end mill is constructed of titanium-coated carbide and has its FPT percentage at 200%. The FPT for this material then equals 0.0108 inches/tooth using the following equation:
FPT = (.008 x .75) x .90 x 2.0 = .0108 inches/tooth
The FPT value and the spindle speed (RPM) value are then used to calculate the feed rate (FEED) using the following equation:
FEED = (RPM x FPT) x Number of teeth
Using the previous examples for a 2-flute end mill:
FEED = 14,668.8 RPM x .0108 inches/tooth x 2 teeth = 316.8 inches/minute
When From material is selected in the Tool page of the Machine Group Setup function panel, and you select Calculate speed/feed in the Tool Wizard, the default plunge and retract rates are calculated at 50% of the feed rate.
You can adjust the calculations for a single operation with the Feed and Speed Calculatorr. This lets you recalculate the default feeds and speeds by changing different parameters and, optionally, saving them back to the materials definition.





