Quick Tool Parameters
Quick toolpaths are no longer available on the Mastercam ribbon. To create a new Quick toolpath, right-click the Toolpaths Manager and select Lathe toolpaths, Quick, Quick rough/finish/groove. You can also edit Quick toolpaths that already exist in part files. In addition, you can customize your Ribbon, Quick Access Toolbar, or Context Menu to contain Quick toolpaths using File, Options.
Use this tab to select a tool, set feeds and speeds, and set other general toolpath parameters. All lathe quick toolpaths share the same Quick tool parameters tab. Click on a sub-topic to learn more.
Use the large window to select a tool for the operation. There are three ways to access tools:
- The window by default displays all the tools that have been added to or are used in the current toolpath group. Select Show library tool to also display tools from the tool library. Click on a tool to use it in the operation.
- If the tool you want to use is not displayed, click Select library tool. This lets you choose tools from different tool libraries.
- Use the right-click menu to create an entirely new tool. The new tool definition will be stored only in the current toolpath group unless 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 can override any of them here by entering different values. Default parameters come from the tool definition, machine or control definition, or operation defaults. The machine group properties tell Mastercam where to get the default values for many of the parameters.
- To simplify the display, click Tool Filter to display only the tools from the library that meet filtering criteria.
- Use the right-click menu options to customize the display. If the tools are displayed as a list, click the column headers to sort the list. Reorder columns by dragging their headings.
- Double-click a tool to edit its tool definition or properties.
- 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 Machine Group Properties.
As soon as you select a tool, Mastercam inputs default feed rates and spindle speed. 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. See Calculating Feeds and Speeds from a Material: Lathe
Use the Machine Group Properties to tell Mastercam which type of default you prefer. You can override the defaults by entering different values.
Mastercam validates your feeds and speeds against the maximum and minimum values set in the machine definition. It warns you if you try to enter a value outside these limits and displays the proper range in yellow.
If you select a different machine for the toolpath group or import the operation into a file with a different machine, Mastercam validates the programmed valued against the values in the new machine definition. If the programmed values are out of range, they display in italics until you edit them.
The feed rate and spindle speed that you enter here are typically in effect for the entire operation. However, you can use the Change at Point feature to change them for specific moves. See Change at Point.
Click Coolant to select which types of coolant to activate or disable. The types of coolant options that are available to you are those which have been defined in the current machine definition.
If the button label appears in italics, then Mastercam has selected a default coolant option in response to a change in the machine definition. Click Coolant to verify or change it.
The label of this button can be changed in the machine definition.
The buttons at the bottom of the tab let you access many advanced toolpath options. These let you:
- Set home and reference positions See Home Positions and Reference Points for more information.
- Set values for miscellaneous or custom variables that have been defined for your control. See Miscellaneous Values for more information.
- Select machine axis combinations. These are used to select sets of axes or components when an axis is defined more than once for a machine. For example, different turret/spindle combinations on a lathe might implement the X-Z plane differently. Select From tool to have Mastercam scan the machine definition for axis combinations which are compatible with the selected tool. See Machine Axis Combinations: Machine Definition Manager.
Choose the checkbox in front of a button to activate a feature and click the button to set values for this operation. Some of these options might not be available if they are not supported by the current control definition.
Show library tools
Adds all the tools in the current tool library to the tool display window. Use Tool Filter to modify the list if there are too many tools to view conveniently.
The name of the current library displays on the right-click menu next to Tool manager.
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 use this feature to select a tool, Mastercam copies the tool definition to the current machine group so that it will be saved with the part. The tool will be listed in the tool display window where it can be selected for any operation in the machine group.
Tool filter
Select to activate the tool filter. The only tools that display in the tool list window are those which meet the filter criteria. Click Tool filter to change the criteria or display different tools.
When you select an axis combination for Mill-Turn toolpaths, the tool filter automatically filters the upper and lower turret tools based on the turret used by the axis combination.
Axis combination/Spindle origin
Select an axis combination. 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. You must define axis combinations 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.
Tool number
Shows the tool number used in the NC program. When Assign tool numbers sequentially in the Machine Group Properties is selected, Mastercam will number 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 set the Machine Group Properties to 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.
Station number
If you have only one tool loaded on a turret face, this assigns an auxiliary number used to define the turret face that the tool is loaded into. If you have multiple tools loaded on the same turret face, this assigns an auxiliary number to each tool position on that face. If Use station number to replace tool number is selected in the control definition, this number defaults to the operation's default tool number when you select a tool. Otherwise, this defaults to the station number value entered on the Parameters page of the Define Tool dialog box.
Offset number
Information about possible offsets required for each tool in the turret is stored in an offset register. Each offset register is given a one- or two-digit number. Enter a value that corresponds with the number of the offset register you want to use for the specified tool.
Tool angle
Click to open the Tool Angle dialog box where you can rotate the tool to a specific angle for the toolpath. It is only enabled if the active axis combination contains a compatible rotary axis, which is typically a B axis on a Mill-Turn machine.
Feed rate
Determines the speed at which the tool cuts along the toolpath. Enter a value in the text box and choose the calculation type:
- in/rev or mm/rev: Calculates the value in inches or millimeters per revolution.
- in/min or mm/min: Calculates the value in inches or millimeters per minute.
- micro-in or microns: Lets you enter a theoretical surface finish value in micro-inches, or microns. Surface finish refers to the depth of the grooves created on the surface of the part by the insert and is determined by several factors including the insert corner radius, coolant, machine vibration, and feed rate/revolution. The software converts the value you enter to a feed rate/revolution that will give you a surface finish close to the one entered. The feed rate calculation varies for different radius arcs, but is the same for linear moves. Since microns are very small units, the numbers entered in the feed rate text box will be relatively large.
Spindle speed
Determines the rotation speed of the spindle in revolutions per minute (RPM) or constant surface speed (CSS). Mastercam calculates a default value according to the machine group properties, but you can override this by typing in a new value. Mastercam warns you if either the default or the value you type in is outside the range set in the machine definition, (for lathes, it only does this if you are in RPM mode, not CSS mode).
Coolant
Click to open 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 through the Coolant commands tab in General Machine parameters.
- Use Change at Point to turn coolant on or off at specific points in the toolpath. This is not available for plunge and turn toolpaths.
Home position
Choose an option from the drop-down list to determine the home position.
- From Machine: uses the home position defined in the machine definition. This will update if you select different axis combinations.
- From tool: sets the home position based on the selected tool's defined home position. Select Setup tool in the Lathe Tools dialog box to define a tool's home position.
- User defined: lets you override either of the defaults. Click Define to enter the coordinates.
Define
Opens the Home Position dialog box. Use this to set a user-defined home position for this operation instead of using the machine or tool default position.
Force tool change
When the same tool is used in successive operations, this option causes a tool change code to be written to the NCI file instead of a null tool change. This allows special post-processor logic to be invoked between the two operations. Mastercam's tool collision avoidance function assumes that the tool will go to the home position immediately after an operation with Force tool change selected, even if the next operation uses the same tool.
To batch
Select to tag the toolpath for batch processing. If you select this option, the toolpath is added to the Toolpaths Manager, but an NCI file is not generated until the batch is run.
Update stock for this operation
Select to have Mastercam update the stock to show the material removed during this toolpath. If you edit the toolpath and change an option that does not affect the stock boundary, such as feed rate or spindle speed, deselect this option to save time regenerating the toolpath. If you select this option when editing a toolpath that has already been created, the stock for that operation and all operations after it are marked as invalid.
Regenerate subsequent operations
Select to have Mastercam mark as dirty all the operations that follow the current operation when the current operation is edited. If you make a change that does not affect the stock boundary, such as feed rate or spindle speed, then deselect this option to avoid having to regenerate the subsequent operations.
Run
Displays the toolpath without pausing until completed when you generate or regenerate it.
Step
Displays the toolpath one step at a time when you generate or regenerate it. Press [Enter] to advance to the next step, or [Esc] to run through the remainder of the toolpath continuously.
Misc values
Select to set the values of custom integer and/or real variables that have been defined for this machine. Click to review or change the values. This button can also be customized to launch an Add-In instead when it is clicked.
Reference point
A reference point is a location that the tool moves to between the home position and the start of the toolpath—the approach point, and another location that the tool moves to at the end of the toolpath before returning to the home position—the retract point. Select to use the currently programmed reference points, or click to set new reference points for this operation, or to apply default reference points from the current machine definition or axis combination.
You can store separate reference points for ID and OD work and Mastercam will select the proper ones.
- Create new tool: Create a new tool instead of selecting one from the list. The tool definition will be stored in the current toolpath group unless you save it to a library.
- Edit tool: Edit the tool definition for the selected tool. The changes you make will be stored in the toolpath group and will not affect future parts that use the tool unless you save the changes to a library.
- 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 toolpath group.
- Load tool on machine: Create 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.
- View: Display the tools as large icons, 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.
- Popup tool: A larger picture of the tool will popup if you let the mouse hover over an icon in the preview window. Select how long the mouse needs to hover before the larger picture pops up, or disable this feature.
- Save parameters: Save the current settings to your defaults file.
- Reload parameters: Overwrite the current values with the values from your defaults file.
- Re-initialize feeds and speeds: Reset feeds and speeds based on the tool settings definition in the tool library. This function works even if the Lock feedrates option in the Toolpaths page of the System Configuration dialog box is selected.





