3D Mill and Router Toolpaths
Mastercam includes several 3D toolpaths. These toolpaths are classified as either high speed or surface rough/finish toolpaths. These types of toolpaths work best on organic, mold/die, or 3D shaped parts.
In some cases, you may want to use a Surface Rough or Finish toolpath instead of a high speed toolpath. Here are some of the reasons you may prefer to use them.
- Some types of tool motion, such as plunge roughing, are not supported by or are unsuitable for high speed machining.
- Your application or your machine tool is not appropriate for the higher feed rates associated with high speed toolpaths. The high speed toolpaths tend to create more retract moves, for example.
- The toolpaths may have options and parameters that are not in the high speed versions, such as more options for entering/exiting the part.
High Speed
3D high speed toolpaths (HST) are a set of machining strategies specially designed to produce the smoothest, most efficient tool motions when machining surface models or solid faces. Mastercam uses two main techniques to achieve this:
- Each cutting pass can be configured with advanced corner rounding and toolpath refinement techniques to reduce the impact of corners, sharp angles, and other discontinuities. These parameters help maintain a constant load on the tool, reduce machining time, and improve machined surface quality.
- An advanced suite of linking tools lets you optimize the transitions between cutting passes and the lead in/out to each cutting pass.
3D high speed toolpaths also extend Mastercam’s gouge-checking capabilities to include the tool holder. Use the Holder page to define custom holder shapes and save them in holder libraries.
Another difference between high speed toolpaths and Mastercam's other toolpaths is how they use defaults. Most toolpaths read default values from the .mcam-defaults file for each operation type. High speed toolpaths dynamically calculate default values based on the selected tool. Whenever you select a new tool for an operation, Mastercam updates the toolpath parameters.
3D high speed toolpaths support both roughing and finishing operations. The following toolpaths are available:
To select geometry for a 3D high speed toolpath, you use the Toolpath Control and the Model Geometry pages in the toolpath dialog box to set machining regions, avoidance, and containment boundaries. These pages are accessed after you select the toolpath type. You can change the toolpath type at any time during creation.
Use the Model Geometry page to select machining and avoidance regions. You can have multiple machining and avoidance regions, each with a separate stock to leave on walls or floors amount. For more information about the parameters on the Model Geometry page, refer to the Model Geometry Help topic.
Use the Toolpath Control page to select containment boundaries and set other containment parameters. Tool containment boundaries are used to control the tool's position around the boundary that you define. The boundary is a closed set of wireframe curves which enclose the area to be machined. For more information about the parameters on the Toolpath Control page, refer to the Toolpath Control Help topic.
Surface Rough and Finish
Mastercam Surface Rough and Surface Finish toolpaths drive the tool over the selected geometry. Surface Rough toolpaths typically use larger tools, multiple stepovers, and multiple stepdowns to quickly remove larger volumes of stock and leave an even amount of stock for finishing. Surface Finish toolpaths typically finish a part down to the drive geometry (or to the stock to leave amount if one is specified).
Both Surface Rough and Finish toolpaths use the same method to select geometry. You can customize how and when Mastercam prompts for toolpath geometry in the Toolpaths page of the System Configuration dialog box. Mastercam prompts for machining geometry, avoidance geometry, and a tool containment boundary for each surface toolpath type.
In your Mastercam configuration file settings, you can choose to automatically use all non-machining regions as avoidance regions.
Depending on the toolpath type, additional geometry may be optionally selected, such as a starting point, a radial center point, or curves. These entities, usually separate from the part, provide Mastercam with additional information about how you want the tool motion created and will improve the final toolpath results.
If you do select avoidance regions, and then select a toolpath strategy that does not support them, Mastercam automatically treats the avoidance regions as additional machining regions.





