Swept 3D Parameters
Use this tab to enter the toolpath parameters for a swept 3D wireframe toolpath. This toolpath sweeps and/or blends one or more contours along one or more other contours.
- First, select a cutting direction, across the calculated surface or along it, and then enter the step sizes for each cutting pass.
- Then, select a cutting method. This determines the pattern that the tool will follow over the part surface. The 5-axis cutting methods will work only if 5-axis tool motion is supported in the current machine definition.
- Enter other toolpath dimensions and compensation options.
Along cut distance
Sets the distance between cuts in the along direction. Stepover is applied to the longest along boundary. This parameter determines surface smoothness. A smaller increment takes longer to process, but works well for more extreme surface curvatures. The more drastic the curvature on the part, the smaller the step size should be. On a fairly flat surface, a larger cutting distance may be used (for example, 0.150).
Across cut distance
Sets the distance between cuts in the across direction. Stepover is applied to the longest along boundary. This parameter determines surface smoothness. A smaller increment takes longer to process, but works well for more extreme surface curvatures. The more drastic the curvature on the part, the smaller the step size should be. On a fairly flat surface, a larger cutting distance may be used (for example, 0.150).
Cutting method
Sets the tool motion during the lofted toolpath. Select one of the following:
- Zigzag cutting forces the tool to stay down on the surface at all times and move back and forth across the part.
- One way cutting takes a pass, rapids up to a rapid plane, moves back to the beginning of the cut and takes another pass in the same direction. All passes are in the same direction.
- Circular cutting produces a spiral toolpath. This cutting method is normally used only in conjunction with constant Z cutting. Circular should be used only when the first and last along boundary are identical and the along boundary is closed.
- 5-axis cutting is used for 5-axis end cutting. This method outputs the normal vectors of the surface to the NCI file, which allows post processors supporting this format to produce NC code. Most posts do not support 5-axis cutting.
Stock to leave
Enter the amount of material to leave on the part model when the operation is finished.
Rapid depth (abs)
Sets the height from which the tool plunges at the rapid speed before it machines the part at the feed rate. The tool also retracts to this height when moving between toolpath segments. This parameter is an absolute value.
Compensation in computer
Generates a toolpath with compensation for the tool radius, but does not allow for tool wear adjustment at the control. Left and Right offset the tool by its radius; Off causes the tool to cut the center line of the geometry.
Tip compensation
Sets amount of offset to the tool's center or tip for bull-nose and ball (spherical) tools. Used for touching the tool off the part. For multiaxis toolpaths, tip compensation outputs the tool tip offset as either the tip or the corner radius distance from the tip.
Sync option
Lines up the across and along boundaries. Selecting Manual or Manual/density requires additional data input.
Along
Cuts in the along direction stepping over in the across direction.
Across
Cuts in the across direction stepping over in the along direction.
Rotate the across contour
Determines the across boundary's orientation when a single along boundary defines a 3D swept surface. Not available when you define two along boundaries.
Translate the across contour
Determines the across boundary's orientation when a single along boundary defines a 3D swept surface. Not available when you define two along boundaries.





