Creating a Multi-Axis Surface Engraving Operation

You can extract the boundaries of a surface or a set of surfaces and machine them.

  1. From the Surface Machining section of the action bar, click Multi-Axis Surface Engraving .
  2. From the Geometry tab , select the bottom surface.

    It can be one surface, or a set or join of faces, connected or not.

    • Each element to be engraved is completely machined before machining the next one.
    • The whole engraving is machined from left to right, or vice-versa (except if you define a start point).
    • Plunges are optimized.
  3. Select the guide contour.
    • After selecting the bottom surface, right-click the guide in the dialog box and select Extract Contour from Part: The free boundary of the bottom surface is automatically extracted and selected as guide contour.
    • Alternatively, select the contour manually.
  4. Optional: Define an offset on the contour:
    • Select Inside: The offset on the hard boundary is equal to the tool low diameter.
    • Or select On or Outside, and enter an offset value, if the guide contour contains soft elements.
  5. Optional: Select a start point.
  6. Define a positive engraving depth.
  7. Select the view direction.

    This is mandatory to project the guide contour on the bottom surface and define the side of the bottom surface to machine.

  8. Select a Tool path style (Helical, Back and Forth, Contour only).
  9. Optional: Clear the Always stay on bottom check box.
  10. See Multi-Axis Surface Engraving for other machining parameters.
  11. From the Radial tab, set the overlap Mode as Maximum distance or a Tool diameter ratio.
  12. If the Tool path style is Contour only, define the number of contouring paths (up to 4).
  13. Optional: If the Tool path style is Back and Forth, select the Contouring pass check box and enter the Contouring pass ratio.
  14. See Strategy Parameters for more information.
  15. If using a NC Machine with engineering connections, go to the Machine Kinematics tab.

    See Machine Kinematics for more information.

  16. From the Tools tab, select a tool.
    • End Mills
    • Conical Mills (including dovetail tools).
  17. Go to the Feeds and Speeds tab to specify the feedrates and spindle speeds for the machining operation.
  18. Go to the Macros tab to specify the machining operation transition paths (approach and retract motion, for example).
  19. Click Display or Simulate to check the validity of the machining operation.
    • The tool path is computed.
    • A progress indicator is displayed.
    • You can cancel the tool path computation at any moment before 100% completion.