Tool page
Use the Tool page to select a tool, edit its properties, and enter feeds and speeds for tree-style toolpaths. This page is used for several different types of toolpaths, and not all features will be available for all toolpath types. Click a drop-down below to learn more.
The default values for many cutting and linking parameters are determined by the dimensions of the selected tool. When you select a new tool, Mastercam updates the values of these fields with new values. If you have manually edited these fields, your edited values will be replaced with the new defaults. You can also set Mastercam to lock in your manual values when you create an operation by using Lock Feedrates on the Toolpaths property page of the System Configuration dialog box.
Selecting a tool
Use the large window to select a tool for the operation. Use any of these techniques:
- Click a tool to use it in the operation. Tools that have been added to or are used in the current machine group are displayed. Used tools display with a check mark.
- Click Select tool from library. This lets you select a tool from the tool library, and select a different tool library if necessary.
- Click Create new tool. This button displays the Mill Tool Designer panel from which you can create a new tool.
- Click Select tool from library. This lets you select a tool from the tool library, and select a different tool library if necessary.
- Click Create new tool assembly. This button displays the Mill Assembly Designer panel from which you can create a new tool assembly.
- Use the right-click menu to create a new tool. The new tool definition will be stored in the current machine group only, 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 here by just typing in the desired values. Default values can come from the tool definition, machine or control definition, or operation defaults. The machine group properties tell Mastercam where to get many of the default values for this page.
- To simplify the display, choose Activate filter to show only the tools from the library that meet filtering criteria.
- Use right-click menu options to customize the display. If the tools are displayed as a list, click on column headers to sort the list. Reorder columns by dragging them.
- Double-click a tool to edit its tool definition, or use the right-click menu.
You can select a tool from the library just by entering its tool number if you have Search tool library set in your machine group properties.
Using aggregate tooling blocks and angled heads
Mastercam Mill, Router, and Mill-Turn support several types of aggregate tooling blocks:
-
Blocks with multiple live tooling stations
-
Block drills
-
Angled milling heads
For each product, right-click in the tool list window and select the appropriate command: Get angled head, Get aggregate, or Get block drill. However, the subsequent workflow is different for each product:
-
For Mill and Router, this opens the Aggregate dialog box, where you can select an aggregate tooling block and set tools in the block. See Selecting an Aggregate Head (Mill/Router) to learn more.
-
For Mill-Turn, this opens the Tool Setup Manager where you can select an angled milling head and load it onto the turret. See Angled Milling Heads and Milling Tool Locators (Mill-Turn) to learn more.
Feeds and speeds
As soon as you select a tool, Mastercam inputs default feed rates and spindle speed. You can get default values from either of two places:
- Read them directly from the tool definition.
- Dynamically calculate them from the material, operation type, and tool characteristics.
You can prevent this behavior for completed toolpaths by selecting Lock feedrates in the Toolpaths page of the System Configuration dialog box.
Use the machine group properties to tell Mastercam which type of default you prefer. You can always override a default value by simply typing in the value you want.
The default spindle direction comes from the tool definition. If you wish, you can override it with the Spindle direction drop-down.
Other ways to enter feeds and speeds
Besides the spindle speed and linear feed rate, Mastercam displays the cutting speed and feed per tooth. These fields are linked so that you can directly enter a cutting speed or feed per tooth and the other fields dynamically update.
You can also use the Feed/speed calculator to calculate different feeds and speeds by adjusting the tool and material characteristics. To access the calculator:
-
Select the Feed speed calculator icon from the top of the dialog box.
- Or choose it from right-click menu.
The feed rate and spindle speed that you enter in this page are typically in effect for the entire operation. However, you can use the Change at Point feature to change them for specific moves.
Feeds, speeds, and your machine definition
Mastercam validates your feeds and speeds against the maximum and minimum values set in the machine definition, and will warn you if you try to enter a value outside these limits. If this happens, it will display the proper range in yellow.
If you later select a different machine for the toolpath group or import the operation into a file with a different machine, Mastercam will validate the programmed value against the values in the new machine definition. If the programmed values are out of range, they will be displayed in italics until you edit them.
Configuring automatic tool inspection
Tool inspection is only available for 3D high speed toolpaths.
Inspection points can only be created at the end of a cut pass. Inspection points are not created along a cut even if the specified distance or time is reached.
Use these options to force a retract move at set intervals so that your machine operator can inspect the tool. Mastercam only looks at the current operation when calculating when the tool should be inspected.
When the tool reaches an inspection point, it will retract and rapid off the part to the clearance plane according to the retract settings on the Linking parameters page. Once the inspection has been completed, the Linking parameters settings also determine how the tool returns to the part.
Parameters
Common toolpath dialog box controls
| Icon | Name | Description |
|---|---|---|
|
Detect (FBM Drill) | Analyzes the solid model and detects features based on the Feature Based Machining (FBM) operation's current parameters. View the results of all detected features and their machining information in the Features page. For more information, please refer to Detection States and Modes in FBM. |
|
Reselection is not available |
Hole Wizard features for a Wizard Holes operation can only be selected in Mastercam for SOLIDWORKS. Contact Mastercam for more information. NOTE
Mastercam for SOLIDWORKS is no longer supported starting with Mastercam 2024. |
|
Preview toolpath operations (FBM Drill/Wizard Holes) | Opens the Toolpath Operations Preview dialog box where you can view the list of operations FBM will generate using the current Features page list. |
|
Select default formulae file (3D high speed toolpaths) | Lets you select a different *.formula file, which Mastercam uses to calculate default values. |
|
Save parameters to defaults file | Makes the current toolpath settings the default for future toolpaths of this type. Saves the current values in the toolpath properties pages to the .mcam-defaults file specified in the machine group properties. |
|
Reload parameters from defaults file | Overwrites the current values in the toolpath properties pages with the toolpath's default parameters. These parameters are reloaded from the .mcam-defaults file specified in the machine group properties. |
|
Display graphical elements | Enables the display of graphical elements, such as plane labels and geometry colors. In 2D or 3D toolpaths Mastercam also has Display only elements on current page, Display plane labels, and Simplify plane display as options. |
|
Hide dialog | Minimizes the dialog box so that you can use other Mastercam functions, like changing your shading settings or the graphics window view. When finished, press [Esc] to maximize the dialog box. |
|
Tool Manager | Opens the Tool Manager. Use the Tool Manager to create and edit tool definitions and to work with tool libraries. When you close the Tool Manager, the toolpath dialog box will reappear just as you left it. |
|
Feed speed calculator | Opens the Feed & Speed Calculator dialog box where you can modify the calculated feed rate or spindle speed by adjusting the material and tool parameters. |
|
None |
Page window | This window displays all of the pages that are available to you, depending on the selected toolpath type. A green check mark indicates pages where data has changed in the current session. |
| None | Quick View Settings | This window summarizes key toolpath information from the Tool page, Coolant page, and Planes page. It updates automatically as you make changes to the different pages and is always visible. |
| None | Generate toolpath | When selected, automatically generates the toolpath when you click OK. For more information, refer to Accepting and Generating Toolpaths. |
|
OK | Generates the toolpath and closes the dialog box. If editing a toolpath, applies the changes and closes the dialog box. |
|
Apply | Applies your changes to the toolpath without closing the dialog box. |
|
Cancel | Closes the dialog box and cancels the toolpath creation. If editing a toolpath, any changes to the toolpath are discarded. |
Not all options are available for all toolpaths.
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.
Select tool from library
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.
Create new tool
Opens the Mill Tool Designer panel from which you can create a new tool.
Create new tool assembly
Opens the Mill Assembly Designer panel from which you can create a new tool assembly.
Filter settings
Opens the Tool List Filter dialog box. Use this dialog box to set filter criteria for finding tools.
Activate filter
Limits the list of displayed tools to only those that match the filter criteria. This can help you find tools quickly when many tools are displayed in the tool list. Click Filter settings to review or set the criteria.
Tool diameter
Determines the diameter of the tool. This is the value that will be used to calculate Cutter compensation. Mastercam reads this value from the tool definition, but you can override it by entering a new value. To change the value stored in the tool definition, double-click the tool in the tool display window.
If your control supports Wear compensation values, the Cutter compensation options let you adjust for wear without having to edit this value for each operation.
Corner radius
Displays the tool's current corner radius. This option is available only if your tool supports a corner radius. By default, Mastercam reads this value from the tool definition. Enter a new value here to override the tool definition value.
Tool name
Displays the name of the selected tool. Mastercam reads this value from the tool definition, but you can override it by entering a new name. If you enter a new name, it is stored with the operation and will not appear if you select the tool anywhere else. To change the name in the tool definition, double-click the tool in the tool display window.
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.
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.
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.
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.
Tool inspection/change
Enables tool inspection, which establishes points during operations where the machine can be programmed to a specific position and stopped to allow you to perform tool inspections.
RCTF (Radial chip thinning factor)
Applies radial chip thinning calculations to the toolpath. This option is also automatically applied when the ISCAR HEM checkbox is selected for certain 2D and 3D toolpaths. The following toolpaths are supported:
- All 2D High Speed toolpaths
- Face
- Slot Mill
- Horizontal Area
- Dynamic OptiRough
- Area Roughing
- Circle Mill
- Surface Rough Pocket
- Surface Rough Parallel
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.
FPT
Displays the amount of feed per tooth, based on the number of flutes in the tool definition.
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.
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.
Safety zone enabled
Indicates that a safety zone is selected.
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.
CS (metric) / SFM (inch)
Displays the current cutting speed in surface feet per minute or surface meters per minute. By default, Mastercam reads this value from the tool definition. Enter a new value here to override the tool definition value.
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.
Tool edge feed rate
Calculates feed rates from the tangential edge of the tool, rather than from the tool center line.
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.
Comment
Enter a Comment to 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.
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.
ISCAR HEM
Activates the ISCAR HEM (High Efficiency Machining) options. By selecting this option, the RCTF (radial chip thinning factor) option is automatically applied.
This field displays only when an ISCAR CHATTERFREE tool is selected for a Dynamic Milling or Dynamic OptiRough toolpath.
Recalculate values
Only avaialble when Automatically calculate HST defaults is selected in the Toolpaths page of the System Configuration dialog box. Updates the cutting and linking parameters based on the current tool dimensions. In this way, you can control when values are updated.
HEM Factor
Adjusts the ISCAR tool's feed rate and spindle speed values to achieve maximum speed and efficiency. Enter a value in the field or use the slider positioned directly above the field to adjust it. You can enter a value from 1 up to 5, depending on the selected machine and tool configuration. Mastercam displays the corresponding feed rate and spindle speed values below the field.
When you enter the maximum HEM Factor allowed by the machine and tool configuration, Mastercam displays a message marked with an asterisk and marks the threshold value in the same manner. This field is available only when the following conditions exist:
- An ISCAR CHATTERFREE tool is selected for a Dynamic Milling or Dynamic OptiRough toolpath
- The ISCAR HEM checkbox in the Tool page is selected
Turret index position
Sets the turret index position to which the tool is added.
Right-click menu options
Select tool from library
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.
Create tool
Opens the Tool Wizard to create a new tool. The tool definition will be stored in the current toolpath group. It will also be stored in the current library if you are creating it within a library.
Edit tool
Opens the Tool Wizard where you can edit the tool. The changes you make will be stored in the machine group and will not affect future parts which use the tool unless you save the changes to a library.
Edit projection
Lets you edit the projection value of tools and multiple holder assemblies (sometimes referred to as composite holders) using a graphical representation of the tool assembly in the graphics window.
Edit assembly names
Opens the Assembly Names dialog box where you can edit the names for the assembly, holder, and tool names used in the assembly.
Get angled head (Mill, Mill-Turn) / Get aggregate (Router):
-
For Mill and Router, opens the Aggregate dialog box, where you can select an aggregate tooling block and set tools in the block. See Selecting an Aggregate Head (Mill/Router) to learn more.
-
For Mill-Turn, opens the Tool Setup Manager where you can select an angled head and load it onto the turret. See Angled Milling Heads and Milling Tool Locators (Mill-Turn) to learn more.
Get block drill
Opens the Drill Block Selection dialog box, where you can selecting a drill block.
Save tool to library
Saves the currently used tools into a .tooldb file.
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.
View
Display the tools as large icons, small icons, 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.
Re-initialize speeds and feeds
Resets the values in the feeds and speeds fields (shown below) based on the tool settings definition in the tool library. These settings may also be reset based on the selected material or from values you defined earlier in your machine group properties.
Feed/speed calculator
Use the calculator to calculate feeds and speeds including surface speed or feed per tooth.
Search for cut parameters
Opens the stand-alone Tool Manager where you can enter search conditions and parameters to filter the .tooldb file for cut parameters matching your search criteria.
