Cut Parameters: Contour
Use this page to enter cutting parameters for a Contour toolpath. Follow this general outline.
- Enter values for different cutting parameters and compensation options.
-
Select a Contour type from the drop-down list in the upper-right corner. Selecting a contour type activates additional parameters that display directly below the field. Use these fields to further refine the toolpath.
NOTEContour type fields do not display for Tab Cutoff toolpath cut parameters.
- Use the pages nested below the Cut parameters page to activate and configure advanced toolpath features.
You can create different types of Contour toolpaths. Refer to the Contour Toolpaths: 2D to learn more.
| 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 your Reseller for more information. |
|
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. |
|
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. |
|
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. |
Compensation type
Choose how you want to handle cutter compensation:
- Computer: Computes the compensated toolpath and does not output control codes for compensation.
- Control: Outputs control codes for compensation and does not compute the compensated toolpath.
- Wear: Computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are the same.
- Reverse wear: Computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are opposite.
- Off: Programs the tool tip directly on the chained geometry and does not output compensation codes.
The available options are determined by the active control definition.
Compensation direction
Offsets to the tool based on the selected direction. Choose one of the following:
- Left: The tool is allowed to travel to the left of the selected chains.
- Right: The tool is allowed to travel to the right of the selected chains.
If Compensation type is set to Off, Mastercam uses this setting to determine the orientation of other toolpath features such as multiple passes.
Tip compensation
Select whether the compensation point will be the center of the tool or the tip. Compensating to the center of the tool is frequently used with ball cutters where compensation is applied at the control.
Optimize cutter compensation in control
Eliminates arcs in the toolpath that are less than or equal to the radius of the tool and helps prevent gouging. Only available when Cutter compensation is set to Control.
Roll cutter around corners
Inserts arc moves around corners in the toolpath. Select None to guarantee all sharp corners, Sharp to only roll the tool around sharp corners (135 degrees or less), or All to roll the tool around all corners and create smooth tool movement. The radius of the arc moves equals the radius of the tool.
Infinite look ahead
Prevents the toolpath from crossing itself to protect against gouging.
Internal corner rounding radius
Creates smoother tool motion in sharp corners. Corner smoothing reduces tool wear and makes your tool motion more efficient.
External corner break radius
Enter a radius value to break external sharp corners defined within a chain to create a smooth, rounded corner.
This option will violate the defined chains and cut into the defined geometry.
Without an External corner break radius:
With an External corner break radius:
Maximum depth variance
Sets the amount that the Z value of the endpoints of 3D entities can be adjusted to make a smooth intersection during cutter compensation. A smaller value creates a more accurate representation of entities, but may insert an extra step move to meet an intersecting entity. A larger value means that Mastercam may not make the step move, but provides a less accurate representation of the entities' actual depth.
Stock to leave on walls
Sets the amount of stock on selected vertical machining geometry. Enter a positive value if you do not want to remove all stock or enter a negative value to remove more stock. If the machining geometry (or a portion of it) is not vertical, Mastercam interpolates a value between the Stock to leave on floors and Stock to leave on walls amounts.
Maintain sharp corners
Available only when a positive Stock to leave on walls value is entered. Rolls your tool around sharp corners while including the stock amount. The following images display how selecting this option affects your toolpath:
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.0.
-
Maintain sharp corners is not selected.
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.175.
-
Maintain sharp corners is not selected.
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.175.
-
Maintain sharp corners is selected.
Stock to leave on floors
Sets the amount of stock on selected horizontal machining geometry. Enter a positive value if you do not want to remove all stock or enter a negative value to remove more stock. If the machining geometry (or a portion of it) is not horizontal, Mastercam interpolates a value between the Stock to leave on floors and Stock to leave on walls amounts.
Contour type
Sets the type of Contour toolpath that Mastercam creates. Choose one of the following:
- 2D
- 2D chamfer
- 3D
- 3D chamfer
- Oscillate
- Ramp
- Remachining
You can choose only contour types that are compatible with the selected geometry for the toolpath. After you choose a contour type, Mastercam displays additional toolpath options below this field for the selected type.
If Contour type is set to 2D or 3D, the following parameter displays.
2D/3D contour type
Displays the type of selected chain and contour toolpath that is created, 2D or 3D. If the toolpath is based on 2D chains, this field is read-only. If 3D chains are selected for the toolpath, you can choose to change from a 3D to a 2D contour. To re-chain geometry for the toolpath, return to the Toolpath Type page, and use the chain geometry options.
If Contour type is set to 2D chamfer or 3D chamfer, the following parameters display.
Chamfer width
Defines the width from the chained geometry adjusted by the cut depth defined on the Linking Parameters page.
Top offset
Defines how far the full diameter of the tool is above the top rail of the chamfer.
Bottom offset
Defines how far the tip of the tool is from the bottom of the chamfer.
Depth
Defines the depth of the bottom of the chamfer when using a ball or bullnose tool.
Mastercam alerts you if the tool you selected for the toolpath is not wide enough to accommodate both the defined Chamfer width and Top offset.
If Contour type is set to Ramp, the following parameters display.
Angle
Ramps during depth cuts using a specified angle until the tool comes to the final depth.
Depth
Ramps during depth cuts by descending by a specified depth during each full ramp motion.
Plunge
Steps down directly between depth cuts.
Ramp angle
Sets the angle at which the depth cuts ramp descends before reaching the final contour depth. Available when you select the Angle option.
Ramp depth
Sets the depth at which each full motion of the depth cuts ramp descends before reaching the final contour depth. Available when you select the Depth or Plunge option.
One way ramping for open contours
Ramps in one direction and comes back at a constant Z level.
Make pass at final depth
Select to ramp to the toolpath depth, and then make a final pass without ramping. Deselect to continue the ramping motion throughout the entire toolpath.
Linearize helixes
Outputs helixes as a sequence of linear moves for controls that cannot process helixes.
Linearization tolerance
Used when converting helixes from curves to lines. Smaller tolerance values make more accurate toolpaths, but may take longer to generate and create a longer NC program.
If Contour type is set to Remachining, the following parameters display.
Previous operations
Determines remaining stock for remachining by calculating stock removed during all previous contour, pocket, circle mill, and facing operations in the Toolpaths Manager.
The previous operation
Determines remaining stock for remachining by calculating stock removed during the previous contour, pocket, circle mill, or facing operation in the Toolpaths Manager.
Roughing tool
Calculates the remaining stock based on the diameter and corner radius of a tool. Use this method to finish a toolpath without a previous operation.
- Diameter: Enter the roughing tool diameter.
Clearance
Extends the toolpath at the beginning and end to prevent cusps of material from being left behind. Enter the clearance as a percentage of the tool diameter or as an absolute value.
Remachining tolerance
Determines the accuracy of the toolpath and the stock display. A smaller value may result in longer processing time. Enter the tolerance as a percentage of the tool diameter (5% is recommended) or as an absolute value.
Display stock
Previews how much stock is removed during the roughing toolpath and the remachining or finishing toolpath, and how much stock is left after remachining.
If Contour type is set to Oscillate, the following parameters display.
Linear
Creates oscillation moves in the Z axis along the toolpath using a zig-zag linear motion.
High speed
Creates oscillation moves in the Z axis along the toolpath using a high speed (sine curve style) motion.
Maximum depth
Enter the maximum Z depth for the oscillation move. The Top of stock that you define in the Linking Parameters page sets the maximum Z height for the toolpath. However, the tool will not exceed the maximum Z depth that you specify in this field.
Distance along contour
Enter the distance you want Mastercam to move the tool in X or Y before changing direction in the Z axis.
If you edit the toolpath and modify the tool, Mastercam verifies that the flute length of the tool is sufficient. A warning message displays if the flute length is less than the overall oscillation distance.





