Radial Toolpaths: 3D
Use the 3D High Speed Radial toolpath to create cutting passes that radiate outwards from a central point. This machining strategy is most effective on areas with shallow curved surfaces and circular areas. Since the stepover between each pass is a 2D value calculated in the XY plane only, the cuts might not be appropriate for steep areas. This is especially true when the steep contour is perpendicular to the cutting direction. In such areas a Waterline, Spiral, or Hybrid toolpath might produce better results.
To define the machining zone, enter the radius of the circle to be machined and the coordinates of its center point, in the Cut Parameters page. Mastercam projects this circle onto your selected drive surfaces and calculates the toolpath within this area.
To select the radius or center point coordinate based on geometry in your part file, right-click in the desired field and choose a value from the short cut menu.
You can also limit the machining zone by specifying a starting and ending angle in the Cut Parameters page. The start and end angle are positive values measured from the X-positive axis. The following pictures show some examples of toolpaths created by different angle spans.
| Toolpath Output | Start and End Angle Amounts |
|---|---|
|
Start angle = 0, End angle = 90 |
|
Start angle = 80, End angle = 200 |
|
Start angle = 0, End angle = 360 |
Specify the stepover between cutting passes in either of two ways:
- Entering a 2D stepover distance
- Specifying a maximum scallop height
The two fields are linked so that when you change one value, the other automatically updates. The stepover is calculated at the outer radius of the machining zone as entered in the Cut Parameters page.
The stepover and scallop height are based on what the cutting pass would theoretically be at the radius entered in the Outer radius field:
This is true even if the toolpath never actually extends to this radius; for example, if the outer radius extends past the boundaries of your drive surfaces.
One problem that can occur with Radial toolpaths is overmachining in the area where the cutting passes converge. In these cases, you can restrict the tool motion by specifying an inner radius. Mastercam will not calculate cutting passes for the area of the circle inside this radius.





