Material Definition dialog box
Use the Material Definition dialog box to create and edit material definitions. Mastercam uses the information in this dialog to accurately calculate default spindle speeds and feed rates when the material is selected for a machine group.
When adjusting material speeds and feeds or defining new materials, you need to enter the following types of information:
- A base cutting speed for all operations using this material
- An override percentage of the base cutting speed for each operation type
- A base feed rate for all tool types
- An override percentage of the base feed rate for each tool type
- Additional override percentages for different tool materials (HSS, carbide, etc.)
Mastercam combines these parameters with information from the tool definition to calculate the most accurate possible feeds and speeds.
To edit a value in the Operation Type or Tool Type window, click on a line to select it, then click a second time on it so it becomes editable.
This dialog is slightly different between Mill/Router and Lathe. In general, the parameters in the top window are used to calculate spindle speed or CSS while the bottom window is used to calculate linear feed rates.
- Mastercam uses calculated feeds and speeds as defaults when you create a new toolpath. You can always override these values in the Toolpath parameters for a particular toolpath (Tool parameters for Mill/Router).
- The values in this dialog box are used when you select Feed Calculation—From material in the Tool Settings tab of the Machine Group Properties dialog box or From material in the Tool page of the Machine Group Setup function panel. Otherwise, Mastercam will read default feeds and speeds directly from the tool definition.
- Use the Feed section of the control definition to use inverse feed rates or to set units for rotary feed rates.
- Nesting operations ignore these parameters.
After you change a material definition, follow these steps to update the feeds and speeds for any operations which use the material.
- Select the operations in the Toolpaths Manager.
- Right-click and choose Edit selected operations, Recalculate feeds/speeds.
- Regenerate the operations.
Material name
Enter the name of the material you want to use.
ISO group
Select the ISO group value.
Base cutting speed
Enter a percentage by which the base cutting speed will be adjusted for the current toolpath type.
Operation list
Determines what percentage of the material's base cutting speed will be used for each operation type when using the specified material. It is calculated in surface feet or meters per minute. Change the percentage for a specific operation by double-clicking on the number found in front of the operation in the list box and entering a new value. The actual cutting speed is based on this percentage and the base cutting speed.
Base feed per tooth/revolution
Determines the base feed rate of the material you are defining. Mastercam uses this to calculate the default feed rate for an operation when this material is selected. Enter an adjustment percentage for each tool type in the window below. This value is material-specific and can be found in your Machinery's Handbook or tool catalog.
- For Lathe users, this value is a linear feed rate expressed as inches or millimeters per revolution.
- For Mill/Router users, this value sets how much material each tooth of a tool can remove per revolution as it rotates through the material.
If you choose Meters as the Output feed rate units option, the units are converted when the information is output to the NCI file. You should still enter the values in millimeters in this dialog box.
Tool type list
Determines what percentage of the base feed per revolution will be used for each tool type when using this material. Change the percentage for a specific tool type by double-clicking on the number found in front of the tool type in the list box and entering a new value.
The actual base feed per revolution is based on this percentage and the base cutting speed. For example, if the base feed per revolution is set to .01 inches/rev and the % of Base is set to 75 for OD roughing operations using the specified material, then the feed rate for all OD roughing operations will be .0075 inches per revolution.
Output feed rate units
Select the units in which Mastercam will output the feed rates it calculates from this data. Typically, you will maintain separate libraries for inch and metric materials. For metric libraries, even if you want to output the feed rate in meters, enter the base feed and speed values in millimeters; Mastercam will convert them automatically. Use the Feed section of the control definition to use inverse feed rates or to set units for rotary feed rates.
Comment
Enter any comments for this material.
Allowable tool materials
For each tool material, enter the following:
- Select the checkbox if tools or inserts made from this tool material will be allowed to cut this stock material.
- Enter an override percentage for the base cutting speed. Mastercam will multiply this by the override percentage for the operation type to further customize the default spindle speeds when the stock material is selected for an operation.
- Enter an override percentage for the base feed rate. Mastercam will multiply this by the override percentage for the tool type to further customize the default feed rate when the stock material is selected for an operation.
Use the arrow buttons to copy values from one column to another.
Reset
Resets the CS/SFM % and FPR/FPT % columns back to their original values.





