Edit Common Parameters: Lathe
Use the Edit Common Parameters, Lathe dialog box to set values for one or more toolpath parameters for several operations at the same time. You can also use it to copy selected values from one operation to another. All the operations must be in the same machine group.
- You can only edit toolpath and operation parameters. You cannot edit machine group properties or settings.
- When you return to the Toolpaths Manager you may need to regenerate operations whose parameters have changed.
The information in this topic is divided into several sections. Click to read more.
In the Toolpaths Manager, select the operations whose values you want to change. When you change toolpath settings in the Edit Common parameters dialog box, Mastercam writes them to all the operations you select here.
- Press the [Ctrl] or [Shift] keys while clicking to select several operations.
- Click the group name to select all the operations.
You can only select operations from the active machine group where the red insertion arrow is located in the Toolpaths Manager.
Use the checkboxes to activate the fields or settings that you want to change. Click Enable all settings or Disable all settings to toggle the state of all fields:
Then, for each field, enter a value or click the button to make changes that you want to apply to the selected operations.
Click Apply to write the new values to the selected operations:
The dialog box stays open so that you can select a different set of operations and make other changes. Click Apply after each set of changes, or choose OK when you are done. Choosing OK also applies the current settings to the selected operations before closing this dialog box.
When you apply the changes, Mastercam automatically validates the new values against the machine definition for the selected machine group and notifies you if there are any incompatibilities.
Clicking Cancel will not undo changes that have already been applied.
Use the Propagate feature to copy values from one operation to another. This is very useful when you import an operation from a library and want to apply its values to operations in your current part file.
- While you are in the Toolpaths Manager, select one or more operations whose values you want to change and the operation which has the values you want to copy.
- Right-click in the Toolpaths Manager and choose Edit selected operations, Edit common parameters.
- Click on the source operation to select it, then click Propagate. Mastercam reads the values from that operation and loads them into all the fields.
- Use the checkboxes to activate the fields whose values you want to copy.
- Click OK or Apply to copy the values to the other operations.
Select the checkbox in front of each field, button, or option to activate it. The values that you enter for active fields will be copied to the operations when you click Apply or OK. If a field is inactive, its value will not be copied to any other operation.
Propagate
Select an operation in the list window and click this button to load all of the fields with values from the selected operations.
Maximum spindle speed
Enter a maximum spindle speed.
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 the Files tab of the Machine Group Properties.
Comments entered for FBM Mill and FBM Drill operations are copied to their generated toolpaths. For example, the same comment you enter for an FBM Drill operation appears in all of its generated drill cycles. This helps maintain a relationship between FBM "parent" and "child" operations.
Canned Text
Click to review or select canned text commands to insert in the tool change block for this operation.
Coolant
The name of this button and the title of the dialog box it opens are customizable through the Coolant commands tab of General Machine parameters.
Click to 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.
Use the Change at point feature to turn coolant on or off at specific points in the toolpath. This is not available for plunge and turn toolpaths.
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 when clicked.
NC name
Select to open the Enter New NC Name dialog box where you can change the name of the resulting NC file from the default file name.
Tool display
Use the tool display options 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 backplot feature, and do not affect it.
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
A reference point is a location that the tool moves to between the home position and the start of the toolpath, known as the approach point, and another location that the tool moves to at the end of the toolpath before returning to the home position, known as the retract point. Select to use the currently programmed reference points, or click the button to set new reference points for this operation or to apply default reference points from the current machine definition or axis combination. Mastercam Lathe lets you store separate reference points for ID and OD work and will automatically select the proper ones.
Filter
Select to eliminate unnecessary tool moves in the toolpath to create smoother movement. Click to configure toolpath filtering options.
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, so that special post-processor logic can 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 = On selected, even if the next operation uses the same tool.
Tool number
Shows the tool number used in the NC program. Select Assign tool numbers sequentially in the Machine group properties to have Mastercam number the tools starting with 1, 2, and so on. Deselect this option to have Mastercam take the tool number from the tool definition. You can also set the machine group properties to automatically check for duplicate tool numbers. Override either method by entering a new number here. The post processor associates 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 you select Use station number to replace tool number in the control definition, this number defaults to the operation's default tool number when you choose a tool. Otherwise, this defaults to the station number value entered on the Parameters page of the Define Tool dialog box.
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 updates if you select different axis combinations.
- User defined: Lets you override either of the defaults. Click Define to enter the coordinates.
- 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.
To batch
Select to automatically tag the toolpath for batch processing and choose To batch or No batch from the drop-down. 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.
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.





