Working with Toolpath Defaults
When you create a new toolpath or other operation, Mastercam populates the fields on each tab or properties page with default values. These values are stored in a file with a .mcam-defaults extension. These defaults are specific for each type of operation; for example, a contour toolpath, a facing toolpath, or a feature based drill operation.
- The first time you create an operation of a specific type in a Mastercam session, the default values are read from the defaults file.
- Then, each time you create another operation of the same type, Mastercam uses the values from the previous operation.
For each type of toolpath, the defaults file stores a complete set of default values for all the tabs or properties pages where you need to enter information.
For example, even though the Toolpath parameters tab or Tool page are used for almost every operation, the defaults file stores different sets of values for each type of operation. The set of default values for each operation also includes values which you set from other dialog boxes, for example, lead in/out moves, tolerances, or gap settings.
You can quickly re-populate the toolpath parameters with values from the defaults file by right-clicking in the Toolpath parameters tab and choosing Reload parameters from defaults file or selecting Reload parameters from defaults file in the tree-style dialog box toolbar.
While many of the default toolpath settings are read from the defaults file, some—such as feeds and speeds, tool numbers and tool offsets— can be read from other places.
Select Files in the Toolpaths Manager to see which defaults file is being used and to select a new one.
After you select Files, you can either select a new defaults file or edit the current one.
Mastercam provides separate sets of default values for inch and metric operations, stored in separate defaults files. Mastercam also maintains separate defaults files for each product. Beyond that, you can create as many different defaults files as you wish. For example, you can create files with different default values for different machines in your shop so that when you select a machine and begin creating toolpaths, the proper defaults file is automatically loaded.
- Use the Files page in the Control Definition Manager to select the defaults file that will be loaded when a new machine group is created.
- In the System Configuration dialog box, you can select a primary defaults file for each Mastercam product. Mastercam uses this as the source for the default values if it cannot find the defaults file referenced in the control definition or machine group properties.
- When you switch between inch and metric operation, Mastercam automatically loads a defaults file in the proper units.
You can edit this file using the Machine Group Setup function panel or the Machine Group Properties dialog box, depending on the machine type. You can also save values to a defaults file while working on a toolpath or from the Control Definition Manager.
Follow these steps to edit a toolpath defaults file. This is a file with a .mcam-defaults extension that provides the initial values for new toolpath operations. Typically, you edit your toolpath defaults from the machine group properties, by following these steps. You can also save values to a defaults file while working on a toolpath or from the Control Definition Manager.
-
In the Toolpaths Manager, click Files under Properties.
-
Select the Edit button to open the Edit Operation Defaults dialog box.
or
Select Edit operation defaults in the Machine page to open the Edit Operation Defaults dialog box.
- If necessary, use the Browse at the top of the dialog box to select a defaults file from a different folder.
-
Edit default values for each type of operation by clicking Parameters.
- To add a new operation, right-click in the window and choose to create a new toolpath or choose Import to import an operation from another defaults file. New operations will be created at the insertion point, just like in the Toolpaths Manager.
-
To delete an operation, click on it, and press [Delete].
You can work on the operations list much like you can in the Toolpaths Manager. This means that you can access many different display options from the right-click menu; select multiple operations; and drag-and-drop operations within the list.
- The last defaults file that you worked on is set as the active defaults file for the machine group.
Mastercam also lets you save values to the active defaults file while you are creating or editing an operation. This lets you try out and test values while actually working on a toolpath, and then save the current parameter values as defaults as soon as you get them right.
If you are working in a tabbed toolpath dialog box, select the Toolpath parameters tab. Right-click and choose Save parameters to defaults file.
If you are working in a tree-style dialog box, select Save parameters to defaults file in the toolbar.
You can do this while creating an operation or editing an existing operation.
Mastercam allows you to create new toolpath defaults file. This is a file with a .mcam-defaults extension that provides the initial values for new toolpath operations.
Begin creating new defaults files from a machine definition already loaded in the Toolpaths Manager.
-
In the Toolpaths Manager, click Files for the machine group to open your machine group properties.
-
Depending on the machine type, select the Edit button in the Operation Defaults section or select Edit operation defaults to open the Edit Operation Defaults dialog box.
-
To create the new file, click Browse at the top of the Edit Operation Defaults dialog box to open the Select Operation Defaults File dialog box.
- Right-click the defaults file on which you want to base your new file, and choose Copy.
- Right-click in the window (not on a file name), and choose Paste.
-
Right-click the new copy of the defaults file, choose Rename, enter the new file name, and press [Enter].
When renaming your file, make sure not to change the file extension.
- Re-click the new file name. Make sure the new defaults file name appears in the File name field. If the correct file name does not display, click anywhere in the white area of the list of files, and re-select the correct file.
- Click OK.
- If prompted to save changes to your original defaults library, click No.
-
Edit the new defaults library as necessary.
You can also empty the new file and start with a blank file by choosing Delete all operations from the toolbar.
- When finished, click OK twice to save your changes and return to the Toolpaths Manager.
Alternatively, you can create new toolpath default files through the Control Definition Manager. Choose Control Definition Manager from the Machine tab, and make your edits. Click Save current selection to create the new file.
Certain types of default values are handled specially or have advanced, specialized configuration options. Click on the drop-downs below to learn more.
Mastercam's Multiaxis toolpaths have hard-coded defaults and formulas that are not stored in the defaults file.
Many cutting and linking parameters for high speed toolpaths are based on the selected tool. This means that, even though you can store default values in your .defaults file, many of the values will be overwritten as soon as you select a tool.
Mastercam gives you additional options for default feed rates and spindle speeds. You can:
- Treat them like other toolpath defaults. This means you set default feeds and speeds for each operation type and save them to a defaults file.
- Read default values from the tool definition.
- Dynamically calculate default values based on the operation type, stock material, and the specific tool that you selected.
Use the Tool Settings tab on the Machine Group Properties dialog box (Lathe) or the Tools page of the Machine Group Setup function panel (Mill or Router) to tell Mastercam your preference.
Because the coolant options that are available for any operation are defined in the active machine definition, consider your default values carefully if you will be using custom coolant options. If the default coolant options in the defaults file are custom settings that are not supported by the active machine definition, Mastercam attempts to match them to the options that are available, but there is no guarantee that this will be successful or meaningful. If you will be using custom coolant options, consider creating a machine-specific defaults file.
Mastercam lets you define your own custom variables. Users can enter specific values for these variables when creating a toolpath on the Miscellaneous Values dialog box. Use the Misc int in the Control Definition Manager to tell Mastercam where to get the default values for these variables. You can either read them from the defaults file on a per-operation basis, or from the control definition (which stores them in the post). Use the control definition to read them from the post if you want them to be the same for all operations using that control or post. Read them from the defaults file if your custom variables only apply to specific operations.
You can choose to use modal defaults for these parameters. This means that once you set a value for any toolpath, Mastercam will continue to reuse that value as the default for the next toolpath, even if the next toolpath is a different type. For example, if you know that every toolpath will have to clear a 6-inch fixture, you can switch to modal defaults as part of your job setup in the machine group properties, and then enter a retract height of 6.5 inches for the first toolpath. Every successive toolpath that you create will be preset to a clearance height of 6.5 inches. Once you change it, the new value will become the default for the next toolpath. Select the Tool Settings tab on the Machine Group Properties dialog box (Lathe) or the Tools page of the Machine Group Setup function panel (Mill or Router) to set your preferences.
For certain types of cutting parameters, you can choose to read default values from the tool definition instead of the defaults file. These include the step sizes for milling tools; peck depths for drills; and coolant selection. Select the Use tool's step, peck, coolant option on the Tool Settings tab on the Machine Group Properties dialog box (Lathe) or the Tools page of the Machine Group Setup function panel (Mill or Router) to
Default home positions and reference points are both stored in the machine definition as part of the axis combination settings. For sophisticated machines with multiple axis combinations, this lets you set specific defaults for each one. The Machine Axis Combinations dialog box in the Machine Definition Manager sets defaults for both home and reference positions, but they're implemented slightly differently:
For home positions, you can choose whether to use the axis combination default or an operation-specific default, stored in the .mcam-defaults file. For lathes, you can also choose a default home position from the tool definition. Use the Tool page in the Control Definition Manager to select which default to use. No matter where the default comes from, the user can override it on the Toolpath parameters tab.
For reference positions, the only defaults are stored with the axis combination. You cannot create operation-specific defaults. You can still override the default on the Toolpath parameters tab. Reference points can be completely disabled in the Control Definition Manager on the Tool page.
Whenever you select a tool for a toolpath, Mastercam assigns it a tool number. This tool number gets output in the tool change block in the NC program when you post the operation. You can choose where this default tool number comes from. Use the Tool Settings tab on the Machine Group Properties dialog box (Lathe) or the Tools page of the Machine Group Setup function panel (Mill or Router) to tell Mastercam to number the tools sequentially, or to read the value from the tool definition.
For tool length, diameter, and back offsets, use the Tool page in the Control Definition Manager to tell Mastercam whether to calculate them from the tool number, or simply read them from the tool definition.
Default tool and material libraries (including insert and holder catalogs for lathes) are set in the machine definition. Use the Tool/material libraries tab in the General Machine Parameters dialog box to select these.
Operation-level defaults for these settings are not supported.





