Toolpath Parameters: Mill/Router
Use the Toolpath parameters tab to select a tool, set feeds and speeds, and set other general parameters for milling and routing toolpaths. Click on a drop-down below to learn more.
Use the large window to select a tool for the operation. Use any of these techniques:
- The window displays all the tools that have been added to or are used in the current machine group. Click a tool to use it in the operation.
- If the tool you want is not displayed, choose Select library tool. Then select a different tool library.
- Use the right-click menu to create a new tool. The new tool definition is stored in the current machine group only if you choose to save it to a tool library.
When you select a tool, the other fields on the tab update with default values. You override any of them by typing in the values. Default parameters may come from the tool definition, machine or control definition, or operation defaults. The toolpath group properties tell Mastercam where to get the default values for many of the parameters.
- To simplify the display, choose Tool filter to display only the tools from the library that meet filtering criteria.
- Use right-click menu options to customize the display. If the tools display as a list, click on column headers to sort the list. Reorder columns by dragging them.
- Double-click a tool to edit its tool definition, or use the right-click menu.
- Let the mouse hover over a tool to see a larger picture of it.
You can select a tool from the library by entering its tool number if you have the Search tool library option set in your toolpath group properties.
As soon as you select a tool, Mastercam inputs default feed rates and spindle speed. To prevent this behavior for complete toolpaths, select Lock Feedrates in the Toolpaths page of the System Configuration dialog box. You can calculate the defaults in either of two ways:
- Read them directly from the tool definition.
- Dynamically calculate them from the material, operation type, and tool characteristics.
Use the machine group properties to tell Mastercam which type of default you prefer. Use the Feed/speed calculator from the right-click menu to calculate different values by adjusting the tool and material characteristics.
Use the Spindle direction drop-down to choose a rotation direction for the spindle (CCW/CW).
You can also enter separate values for plunging into the part or retracting from it, or you can choose to retract from the part with a rapid move.
Mastercam validates your feeds and speeds against the maximum and minimum values set in the machine definition, and warns you if you try to enter a value outside these limits. If this happens, Mastercam displays the proper range in yellow.
FPT (Feed per Tooth) values are related to feed rate values. SFM-CS (Surface feet per minute for inch, Cutting speed for metric) values are related to spindle speed values. If you change the value in one field, the related field value is automatically re-calculated and updated.
Click Coolant to turn on or off specific types of coolant for the operation. The types of coolant options that are available to you are those which have been defined in the current machine definition.
When any coolant option has been turned on, the button changes to include an asterisk:
You can configure Mastercam to select a coolant option when you select a tool. Each tool definition can include a default coolant selection; this is used for an operation if Use tool's step, peck, coolant is turned on in the Tool Settings tab of the Machine Group Properties dialog box or the Tools page of the Machine Group Setup function panel.
The label of this button itself can be changed in the machine definition.
The bottom area of the tab includes buttons to access many advanced toolpath options. These let you:
- Access rotary axis parameters. Select the checkbox to tell Mastercam that one of your axes is a rotary axis, and click the button to configure the rotary motion.
- Select different tool planes and origins, work offsets, or work coordinate systems.
- Set home and reference positions.
- Select canned text or set miscellaneous values that have been defined for your control.
Some options have a checkbox in front of the button. In these instances, select the checkbox to activate the feature, and click the button to review or set the specific values for this operation.
Some of these options might not be available if they are not supported by the current control definition. The names of options and fields on this page can also be customized with post text.
Not all options are available for all toolpaths.
Tool display window
Shows the tools available in the current machine group. Click a tool in this list to use it in the current operation. Right-click in this area to add tools to this list from a tool library, create a new tool, or change how this list is displayed.
Select library tool
Opens the Tool Selection dialog box so that you can select a tool from a tool library, or select a different tool library. When you select a tool, Mastercam copies the tool to the current machine group and saves it to the part. The tool is then listed in the tool display window where it can be selected for any operation in the machine group.
Tool filter
Opens the Tool List Filter dialog box to set filter criteria for finding tools.
Coolant
Opens the Coolant dialog box where you can select coolant options. The coolant options that are available to you are defined in the machine definition. When any of the coolant options are turned on, the button label will be marked with an asterisk.
- The name of this button and the title of the dialog box it opens are customizable in the Coolant command tab in the General Machine Parameters dialog box.
- Use the Change at Point feature to turn coolant on or off at specific points in the toolpath.
Tool diameter
Determines the diameter of the tool. This is the value that will be used to calculate Cutter compensation. Mastercam reads this value from the tool definition, but you can override it by entering a new value. To change the value stored in the tool definition, double-click the tool in the tool display window.
If your control supports Wear compensation values, the Cutter compensation options let you adjust for wear without having to edit this value for each operation.
Tool name
Displays the name of the selected tool. Mastercam reads this value from the tool definition, but you can override it by entering a new name. If you enter a new name, it is stored with the operation and will not appear if you select the tool anywhere else. To change the name in the tool definition, double-click the tool in the tool display window.
Tool number
Shows the tool number used in the NC program. When Assign tool numbers sequentially is selected in your machine group properties, Mastercam numbers the tools starting with 1, 2, and so on. When this option is deselected, Mastercam takes the tool number from the tool definition. You can also automatically check for duplicate tool numbers. You can override either method by entering a new number.
The post processor can associate the tool number with length and diameter offsets in the control. The control definition determines how Mastercam assigns the offsets for each tool.
Head number
Sets the spindle or head used on a machine tool with multiple spindles or heads. When set to -1, the head number parameter is not used. When Assign tool numbers sequentially in your machine group properties is deselected, the Head number parameter is set by the Station number set in the tool definition.
Corner radius
Displays the tool's current corner radius. This option is available only if your tool supports a corner radius. By default, Mastercam reads this value from the tool definition. Enter a new value here to override the tool definition value.
Length offset
Displays the current length offset associated with the Tool number. Mastercam reads and calculates this offset from the control definition. Enter a new value to override the control definition.
Diameter offset
Displays the current diameter offset associated with the Tool number. Mastercam reads and calculates this offset from the control definition. Enter a new value to override the control definition.
RCTF (Radial chip thinning factor)
Applies radial chip thinning calculations to the toolpath. This option is also automatically applied when the ISCAR HEM checkbox is selected for certain 2D and 3D toolpaths. The following toolpaths are supported:
- All 2D High Speed toolpaths
- Face
- Slot Mill
- Horizontal Area
- Dynamic OptiRough
- Area Roughing
- Circle Mill
- Surface Rough Pocket
- Surface Rough Parallel
Feed rate
Sets the rate (inches per minute or millimeters per minute) at which the tool moves through the part. In 2-axis machining (except drilling), the feed rate only applies to tool movements in the X and Y directions (or parallel to the tool plane) when the tool touches the material. In 3-axis machining, the feed rate is interpolated in the X, Y, and Z directions. For Drill toolpaths, the feed rate is measured along the drilling axis. Mastercam calculates a default value according to the settings in your machine group properties, but you can override this by typing in a new value.
FPT
Displays the amount of feed per tooth, based on the number of flutes in the tool definition.
Plunge rate
Sets the feed rate Mastercam uses when plunging into the part. Typically, this applies to tool movements in the negative Z direction only.
Force tool change
When the same tool is used in successive operations, this option replaces the null tool change in the NCI file with a tool change code, so that an event can be triggered between the two operations. The tool collision avoidance function assumes that the tool will go to the home position immediately after an operation with this option selected, even if the next operation uses the same tool.
Spindle direction
Sets the rotation direction for the selected tool as clockwise (CW) or counterclockwise (CCW). Mastercam displays a default value according to the value set in your machine group properties, but you can override this by an option here.
If the default feed rates are From defaults or User defined, entering a negative spindle speed for these defaults sets the Spindle direction to CCW; a positive value sets it to CW.
Spindle speed
Mastercam warns you if either the default or the value you type in is outside the range set in the machine definition.
CS (metric) / SFM (inch)
Displays the current cutting speed in surface feet per minute or surface meters per minute. By default, Mastercam reads this value from the tool definition. Enter a new value here to override the tool definition value.
Retract rate
Sets the feed rate Mastercam uses when pulling away from the part. Typically, this applies to tool movements in the positive Z direction only.
If the Use plunge, retract rate in gap option for Surface Rough and Surface Finish toolpaths (in the Gap settings dialog box) is selected, Mastercam always uses the Retract rate value for vertical gap motion even if Rapid retract is selected.
Force tool change
When the same tool is used in successive operations, this option replaces the null tool change in the NCI file with a tool change code, so that an event can be triggered between the two operations. The tool collision avoidance function assumes that the tool will go to the home position immediately after an operation with this option selected, even if the next operation uses the same tool.
Rapid retract
Select to retract from the part at the rapid rate set at the machine tool. If you do not select this option, Mastercam uses the programmed Retract rate.
If selected for a 3D high speed toolpath, the feed rate is used for exit and lead out motion. If deselected, the Retract rate is used for exit and lead out motion.
Comment
Enter comments for the toolpath. Comments help identify the operation in the Toolpaths Manager. These can be output in the NC file when you post if you select the proper option in your machine group properties.
Axis combination
Opens the Axis Combination dialog box to select an axis combination that has been defined for your machine. You need to select an axis combination if your machine tool has multiple definitions for the same axis. For example, a mill might have separate Z-axes defined for a quill and the table, or a lathe might have multiple axis definitions for different tool turret-spindle combinations. Axis combinations need to be defined in the machine definition before they can be selected here. Once you select an axis combination, its name displays on the button.
If your machine tool does not have any axis combinations, the default will be selected and you do not have to do anything.
To batch
Select to automatically tag the toolpath for batch processing and to add the toolpath to the Toolpaths Manager. An NCI file generates after the batch runs.
Miscellaneous values
Opens the Miscellaneous values dialog box to review or change the values of any custom integers and/or real variables that have been defined for this machine. This button can also be customized to launch an Add-In instead when it is clicked.
Home position
Sets the position on the machine tool where the tool returns for tool changes and at the end of the NC program. The default home position is determined by the active machine and control definition. Click Home position to override it for this operation.
Rotary axis
Opens the Rotary Axis dialog box. Sets parameters for rotary movement or axis substitution. This option is only available if your machine definition is configured to support rotary movement.
Tool display
Opens the Tool Display dialog box to control how Mastercam displays the toolpath when it is first created or regenerated. This lets you see a dynamic toolpath display, which previews tool positions when you first create the toolpath. These options are separate from Mastercam's simulation features and do not affect them.
Planes
Opens the Planes dialog box. You can change or set any of the following:
-
Tool plane (Tplane)
-
Work coordinate system used for the operation
-
The Tplane or WCS origin the work offset associated with this operation.
Reference point
Opens the Reference points dialog box to set reference points. A reference point is a location that the tool moves to between the home position and the start of the toolpath (approach point), and another location that the tool moves to at the end of the toolpath before returning to the home position (retract point).
Canned text
Click to open the Canned text dialog box to insert or review canned text commands in your NC program.
Create tool
Create a new tool instead of selecting one from the list. The tool definition is stored in the current toolpath group unless you save it to a library.
Edit tool
Use this option to edit the tool definition for the selected tool. The changes you make are stored in the machine group and do not affect future parts that use the tool, unless you save the changes to a library.
Edit projection
Lets you edit the projection value of tools and multiple holder assemblies (sometimes referred to as composite holders) using a graphical representation of the tool assembly in the graphics window.
Edit assembly names (Mill)
Opens the Assembly Names dialog box where you can edit the names for the assembly, holder, and tool names used in the assembly.
Get angled head (Mill) / Get aggregate (Router)
Opens the Aggregate dialog box, where you can select an aggregate tooling block and set tools in the block.
Tool Manager:
Displays the name of the current tool library, and opens the Tool Manager so that you can work with the library and the tools stored in the current machine group.
Load tool on machine
Creates a tool component in the machine definition based on the tool definition for the selected tool. Mastercam uses the tool setup information in Tool spindle and Tool locator components to properly position and orient the tool for simulation.
This feature is only used for Mill-Turn simulation. If you are not simulating these types of toolpaths, you do not need this function, and it will not be activated.
Save tool to a library
Lets you save one or more tool definitions to a library. You can select the tools from either the Part or Library window.
View
Display the tools as large icons, a list, or as a details list.
Arrange tools
Sort the tools by tool number or tool name. Use these options if you have the tools displayed as icons without any column headers.
Re-initialize speeds & feeds
Resets the values in the feeds and speeds fields based on the tool settings definition in the tool library.
These settings may also be based on the selected material or from values you defined in your machine group properties.
Feed speed calculator
Use the calculator to calculate feeds and speeds including surface speed or feed per tooth.
Search for cut parameters
Opens the Search Wizard in the stand-alone Tool Manager where you can enter conditions and parameters to filter the .tooldb file for cut parameters matching your search criteria.
Save parameters to defaults file
Use this option to make the current toolpath settings the default for future toolpaths of this type. The current values are saved to the defaults file specified in the machine group properties.
Reload parameters from defaults file
Overwrite the current values with the values from your defaults file. These are read from the defaults file specified in the machine group properties.
Get block drill (Router)
Opens the Drill Block Selection dialog box, where you can select a drill block and set the drills in the block. This is only available when you are creating or editing a block drilling toolpath.





