Toolpath Parameters: Lathe
Use this tab to select a tool, set feeds and speeds, and set other general toolpath parameters. This tab is similar for most Lathe toolpaths. Use the large window to select a tool for the operation. Double-click a tool to edit its tool definition or properties. This includes setting it in a different turret, changing its mounting angle, or using it with a different spindle.
You can select a tool from the library by entering its tool number if you have Search tool library set in your Machine 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 the Lock feedrates option 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. You can override any of the defaults by entering different values.
The feed rate and spindle speed that you enter here are typically
in effect for the entire operation.
The bottom area of the tab includes many advanced toolpath options. Select the checkbox to activate a feature, and click the button to set values for this operation. Some options might not be available if they are not supported by the current control definition.
Many of the field and button labels on this tab can be customized and might differ from those listed here, or might be disabled.
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.
Show library tools
Adds all the tools in the current tool library to the tool display window. Use Filter to screen the list if there are too many tools to view conveniently. The name of the current library is displayed on the right-click menu.
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 Lathe Tool Filter dialog box to set filter criteria for finding tools.
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.
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.
Tool angles
Read-only. Displays the angle and orientation entered in the Tool Angle dialog box.
Turret index position
Sets the turret index position to which the tool is added.
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. Mastercam 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.
When you create a Lathe Thread toolpath, Mastercam automatically calculates the feed rate based on the value you enter for Lead (on the Thread shape parameters tab) and Spindle speed (on the Toolpath parameters tab).
Plunge feed rate
Select to activate the field and the feed rate calculation type, in/rev or mm/rev, in/min or mm/min, or micro-in or microns as described previously. Enter a plunge feed rate value by:
- Accepting the default value.
- Manually entering a custom value.
- Have Mastercam calculate the value based on 50% of the tool's feed rate by selecting Compute from material in the Parameters tab of the Define Tool dialog box.
Plunge rates are only applied if your operation includes plunges, and your plunge cutting method and parameters are set correctly in the Plunge Cut Parameters dialog box.
Spindle speed
Mastercam warns you if either the default or the value you type in is outside the range set in the machine definition.
Maximum spindle speed
Enter a value to determine the fastest speed that you will allow the part to turn. This value is always expressed in RPMs. For guidelines, refer to the documentation that came with your lathe machine.
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.
Home position
Displays the X and Z coordinates for the 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 - User Defined dialog box. Modify the settings in this dialog box to specify a new home position for this operation.
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.
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.
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/Spindle origin
Opens the Axis Combination/Spindle Origin 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. Axis combinations typically include a tool turret, spindle, and chuck. 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.
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.
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.
Stock update
Access the Stock Update Parameters dialog box to regenerate subsequent operations, define the operation's tool clearance, or use the default tool clearance defined in Job Setup. You can choose to keep either the part boundary, the stock boundary, or both boundaries after the part is cut off.
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).
Mastercam lets you store separate reference points for ID and OD work, and will automatically select the proper ones.
Canned text
Click to open the Canned text dialog box to insert or review canned text commands in your NC program.
Create new 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
Edit the tool definition for the selected tool. The changes you make are stored in the toolpath group and will not affect future parts which 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
Mill-Turn only. 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. Use this option to control how long the mouse needs to hover before the larger picture pops up.
Save parameters to default file
Make the current toolpath settings the default for future toolpaths of this type. The current values are saved to the .mcam-defaults file specified in the toolpath group properties.
Reload parameters from default file
Overwrite the current values with the values from your defaults file. These will be read from the .mcam-defaults file specified in the toolpath group properties.
Re-initialize feeds and speeds
Resets feeds and speeds based on the tool settings definition in the tool library. This function works even if Lock feedrates in the Toolpaths page of the System Configuration dialog box is selected.





