Toolpath Parameters: Mill-Turn
Use this tab to select a tool, set feeds and speeds, and set other general toolpath parameters. This tab is very similar for most Mill-Turn Turning toolpaths. Click on a sub-topic below 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 tools to also display tools from the tool library. Click 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 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 by just typing in the desired 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 detailed list, click on column headers to sort the list. Reorder columns by dragging their headings.
- 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.
- Hover the mouse over a tool to see a larger picture of it.
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.
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 you later 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 Change at Point to change them for specific moves.
Use the Feed page in the control definition to configure the feed rate units, inverse feed rates, or other advanced options.
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.
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.
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.
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.
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.
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.
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.
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.
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.
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.





