Edit Common Parameters: Mill/Router dialog box
Use the Edit Common Parameters, Mill/Router 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.
The information in this topic is divided into several sections. Click on the drop-downs to learn more.
In the Toolpaths Manager, select the operations 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 select only operations from the active machine group, which is the machine group with the red insertion arrow in the Toolpaths Manager.
Use the checkboxes to activate the fields or settings to change. Use Select all or Deselect all to quickly toggle all the fields.
Then, for each field, enter or select the value to apply to the selected operations. When you are working with the cutting planes parameters, you can set several states in addition to the height of the plane:
- Select an option from the Use drop list to simulate activating or turning off retract and clearance planes. You can Enable or Disable the planes for all selected operations. Select No change to apply the value to only the operations where the plane is used.
- Select an option from the Abs/ drop list to set the type of value to Absolute or Incremental for all the selected operations. Select No change to write only the numerical value without changing its type.
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 of incompatibilities.
Clicking Cancel does not undo changes that have already been applied.
Use the Propagate feature to copy values from one operation to another. This is 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 that 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, and then click Propagate. Mastercam automatically 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.
- You can only edit toolpath and operation parameters. You cannot edit machine group properties or settings.
- When you return to the Toolpaths Manager you typically need to regenerate operations whose parameters have been changed.
Propagate
Select an operation in the list window, and click this button to load all of the fields with values from the selected operation.
Operation list
Displays the operations that have been selected in the Toolpaths Manager when you entered the Edit Common Parameters function. When you click Apply or OK, values from all the active fields are copied to the operations listed in the window.
Clearance
Sets the height at which the tool moves to and from the part. Select the checkbox to activate the clearance height. If it is not selected, the Retract value is used as the clearance plane. Click the button to set or change the height. You can select a point on the geometry or enter a value.
For Thread Mill toolpaths, Clearance sets the height that tool rapids to before and after cutting each thread. This is an absolute value.
For Multiaxis toolpaths and Drill toolpaths with multiaxis functionality enabled, Clearance is always an incremental distance from the current tool position.
For Model Chamfer toolpaths, Clearance is an absolute value from start and end. However, if there is a feature on the solid model that is higher than the entered Clearance value (shown as 1 below), Model Chamfer will instead use the entered Retract value (shown as 2 below) to clear it.
Retract
Sets the height that the tool moves up to before the next tool pass. Select the checkbox to activate the retract plane, and then click the button and select a point on the geometry or enter a value. The retract height should be set above the feed plane.
For Thread Mill toolpaths, Clearance sets the height that tool rapids to before and after cutting each thread. This is an absolute value.
For Multiaxis toolpaths and Drill toolpaths with multiaxis functionality enabled, Retract is an incremental distance from the current tool position.
For Model Chamfer toolpaths, the incremental value moves away from the current position and it is gouge checked against the selected solid model and the avoidance geometry. If the distance will gouge, Model Chamfer raises the value higher until it clears.
If you do not enter a Clearance height, the tool moves to the retract height between operations.
Feed plane
Sets the height that the tool rapids to before changing to the plunge rate to enter the part. The tool also moves to this height between operations if you do not enter both the Clearance height and the Retract height. Select the checkbox to activate the feed plane, and then click the button and select a point on the geometry or enter a value.
For Multiaxis toolpaths, Feed plane is an incremental distance from the current tool position.
For Model Chamfer toolpaths, Feed plane is an incremental distance above the next cut depth.
Top of stock
Sets the height of the material in the Z axis. Many other toolpath parameters are measured from this position in incremental mode, such as clearance, retract, and feed planes. Click Top of stock, and select a point on the geometry or enter a value. Incremental values are measured from the chained geometry.
Depth
Determines the final machining depth and the lowest depth that the tool descends into the stock. The default depth is the depth of the first chain selected. Click Depth, and select a point on the geometry or enter a value. Incremental values are relative to the chained geometry, not the top of stock.
Rapid retract
Select to retract from the part at the rapid rate set at the machine tool. If you do not select this option, Mastercam uses the programmed Retract rate.
If selected for a 3D high speed toolpath, the feed rate is used for exit and lead out motion. If deselected, the Retract rate is used for exit and lead out motion.
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.
Batch
-
To batch adds the current operation to a batch file for processing at a later time. Mastercam adds the toolpath to the Toolpaths Manager, but an NCI file is not generated until the batch is run.
When you select a Mastercam file for batch processing, all operations marked for batch processing are automatically loaded into the batch operations list.
- No batch stops all toolpath operations that have been set to batch on the Toolpath parameters tab from batch processing.
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.
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.
Planes
Select to set or change any of the following:
- the tool plane (Tplane) or work coordinate system used for the operation
- the Tplane or WCS origin
- the work offset associated with this operation.
For certain types of operations, you can also change the construction plane (Cplane).
Canned text
Click to open the Canned text dialog box to insert or review canned text commands in your NC program.
Home position
Sets the position on the machine tool where the tool returns for tool changes and at the end of the NC program. The default home position is determined by the active machine and control definition. Click Home position to override it for this operation.
NC name
Select to open the Enter new NC name dialog box where you can change the name of the resulting NC file.
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).
Head number
Sets the spindle or head used on a machine tool with multiple spindles or heads. When set to -1, the head number parameter is not used. When Assign tool numbers sequentially in your machine group properties is deselected, the Head number parameter is set by the Station number set in the tool definition.
Feed rate
Sets the rate (inches per minute or millimeters per minute) at which the tool moves through the part. In 2-axis machining (except drilling), the feed rate only applies to tool movements in the X and Y directions (or parallel to the tool plane) when the tool touches the material. In 3-axis machining, the feed rate is interpolated in the X, Y, and Z directions. For Drill toolpaths, the feed rate is measured along the drilling axis. Mastercam calculates a default value according to the settings in your machine group properties, but you can override this by typing in a new value.
Plunge rate
Sets the feed rate Mastercam uses when plunging into the part. Typically, this applies to tool movements in the negative Z direction only.
Length offset
Displays the current length offset associated with the Tool number. Mastercam reads and calculates this offset from the control definition. Enter a new value to override the control definition.
Diameter offset
Displays the current diameter offset associated with the Tool number. Mastercam reads and calculates this offset from the control definition. Enter a new value to override the control definition.
Retract rate
Sets the feed rate Mastercam uses when pulling away from the part. Typically, this applies to tool movements in the positive Z direction only.
If the Use plunge, retract rate in gap option for Surface Rough and Surface Finish toolpaths (in the Gap settings dialog box) is selected, Mastercam always uses the Retract rate value for vertical gap motion even if Rapid retract is selected.
Spindle speed
Mastercam warns you if either the default or the value you type in is outside the range set in the machine definition.
Spindle direction
Sets the rotation direction for the selected tool as clockwise (CW) or counterclockwise (CCW). Mastercam displays a default value according to the value set in your machine group properties, but you can override this by an option here.
If the default feed rates are From defaults or User defined, entering a negative spindle speed for these defaults sets the Spindle direction to CCW; a positive value sets it to CW.
Tool selection window
Chose the checkbox to activate the Tool selection window, which displays the tools used in the selected operations. Right-click in the window to edit existing tools. create new tools, access the Tool Manager or the Speed and Feed Calculator, and change how the tools are displayed (icon or details).
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 Tool List Filter dialog box to set filter criteria for finding tools.
Select all
Activates all the fields.
Deselect all
Makes all the fields inactive.
Create new tool
Use this option to 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
Use this option to edit the tool definition for the selected tool. The changes you make are stored in the machine group and do 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 machine group.
Feed/speed calculator
Use the calculator to calculate feeds and speeds including surface speed or feed per tooth.
View
Display the tools as large icons, small icons, or as a details list.





