Cut Parameters: Waterline
Use the Cut Parameters page to configure the cutting passes for a Waterline toolpath. This is a finish toolpath which traces parallel contours on the drive surfaces with a constant Z spacing between them.
| 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. |
Closed contour direction
Orients the cutting direction of the closed contours. Closed contours contain continuous motion without a need for a retract or reversal of direction. Select one of the following options:
- Climb: Cuts in one direction with the tool rotating in the opposite direction of the tool motion.
- Conventional: Cuts in one direction with the tool rotating in the same direction as the tool motion.
- Climb Spiral: When machining a concave face, Mastercam cuts in one direction in a spiral pattern, with the tool rotating in the opposite direction of the tool motion. When machining a convex face, Mastercam cuts in one direction in a spiral pattern, with the tool rotating in the same direction as the tool motion.
- Conventional Spiral: When machining a concave face, Mastercam cuts in one direction in a spiral pattern, with the tool rotating in the same direction as the tool motion. When machining a convex face, Mastercam cuts in one direction in a spiral pattern, with the tool rotating in the opposite direction of the tool motion.
Open contour direction
Orients the cutting direction of the open contours. Select one of the following options:
- One Way: Cuts the open contour by taking a pass, moving up to the retract height, moving back to the beginning of the cut, and taking another pass in the same direction. All passes are in the same direction.
- Zigzag: Cuts each pass in the opposite direction to the previous pass. A short linking motion connects the two ends.
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.
Cut order
Controls the cut order Mastercam applies to different cutting passes in the toolpath. This can be set as:
- By depth: Select to machine all cut passes by Z-level.
- Optimize: Select to keep the tool in an area and keep it there until all cuts in the area are made.
Bottom to top
Machines from the bottom of the part to the top. This option respects the selected Cut order. The images below show a Waterline toolpath with Cut order set to Optimize. Notice the starting locations for both toolpaths.
| Bottom to top deselected | Bottom to top selected |
|---|---|
|
|
Stepdown (Passes)
Determines the Z spacing between adjacent cutting passes.
Add cuts
Adds cuts at shallow areas of the profile so that the toolpath does not have excessively large horizontal spacing between cutting passes.
Minimum stepdown
Sets the minimum distance between the added Z cuts in the shallow areas of the part.
Maximum profile stepover
Determines the maximum change in the surface profiles for two adjacent cutting passes. This represents the maximum value of the shortest horizontal distance between adjacent points on the two profiles.
For most applications, the Maximum profile stepover should be greater than the Stepdown. Otherwise, toolpath calculation time can increase significantly. If you think that your toolpath is taking too long to calculate, check to make sure that the Maximum profile stepover is greater than the Stepdown.
Critical depths
Select to customize the handling of flat areas when machining.
Type
Determines the type of flat area to be machined with a single Waterline contour.
-
Include flats: Includes flat areas when machining.
-
Include contact flats only: Includes and machines areas that make contact with the detected flat regions.
-
Flats only: Machines only flat areas.
-
Contact flats only: Machines only areas that make contact with the detected flat regions.
-
Include manual: Includes manually selected flat areas when machining. The manually selected points are highlighted below in yellow.
-
Include manual contact: Includes and machines manually selected flat areas that make contact with the detected flat regions. The manually selected points are highlighted below in yellow.
-
Manual only: Machines only the selected flat areas. The manually selected points are highlighted below in yellow.
-
Manual contact only: Machines manually selected flat areas that make contact with the detected flat regions. The manually selected points are highlighted below in yellow.
When using a Manual option, Mastercam places points in the graphics window to indicate your selections. If you deselect the points, they are removed from the part file. These points are reported in the Analyze, Statistics function.
Manual
Use the Select button to manually select a point at the depth you want to machine. Only available when Type is set to Include manual, Include manual contact, Manual only, or Manual contact only.
Extend
Expands the flat areas by the specified amount. Only available when Type is set to Contact flats only, Include contact flats, Manual contact only, and Include manual contact.
| Extend set to 0.0 | Extend set to 5.0 |
|---|---|
|
|
Corner rounding
Activates toolpath corner rounding, which replaces sharp corners with arcs for faster and smoother transitions in tool direction. Once you activate corner rounding, set the maximum radius, profile tolerance, and offset tolerance.
- Maximum radius: Enter the radius of the largest arc that you will allow Mastercam to insert to replace a corner. Larger arcs result in a smoother toolpath, but with greater deviation from the originally programmed toolpath.
- Profile tolerance: Represents the maximum distance that the outermost profile of a toolpath created with corner rounding can deviate from the original toolpath.
- Offset tolerance: Represents the maximum distance that a profile of a toolpath created with corner rounding can deviate from the original toolpath. This is the same measurement as the profile tolerance but is applied to all the profiles except the outermost one. This lets you maintain different tolerances for the first profile and subsequent profiles.





