Creating a Multi-Axis Curve Engraving Operation

With this machining operation, you can manage letters and stripes engraving from 2.5 axis to 5 axis, and 3D guide contour engraving (5 axis trimming).

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

    It can be a single curve or a set or a join of curves (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 start and end points).
    • Plunges are optimized.
  3. Select the bottom surface.

    For letters and stripes:

    • The guide contour is projected on the surface.
    • The surface can be a plane (2.5 axis engraving).
    • The tool axis is always normal to the surface.

    For trimming:

    • The surface is generally the design part.
    • The tool axis is automatically modified if any collision with the design part is detected.

  4. Optional: Select limits (as start and end points) for each guide contour.
  5. Define the engraving depth (positive or negative).

    Engraving requires a positive engraving depth.

  6. From the Machining Strategy tab , select the Curve Engraving Mode: Letters, Stripes or Trimming.
    This choice impacts the tool path sequencing. Only the required parameters are proposed.
  7. Select the view direction.

    • This is mandatory to project the guide contour on the bottom surface.
    • For letters and stripes, it defines the propagation direction (from left to right, or vice-versa).
    • For stripes and trimming, a second arrow shows the direction of cut along the first stripe or guide contour.

      The default value is the direction of the first element in the set of curves.

      Click this arrow to invert the direction of cut.

  8. See Multi-Axis Curve Engraving for other machining parameters.

    Forced close contour and Closed contour overlap are available only for trimming.

  9. If you have selected Trimming, set required Tool Axis (fixed or normal to surface) and the Max lead and tilt angle.

    Notes:
    • For Letters, the Tool Axis is always normal to the surface.
    • For Stripes, the Tool Axis is normal to the surface when using an end mill tool, and normal to the surface with a 90° tilt when using a TSlotter.

  10. If you have selected Letters or Stripes, set the Compensation output, either No Compensation, or 3D radial (PQR).
  11. If using a NC Machine with engineering connections, go to the Machine Kinematics tab.

    See Machine Kinematics for more information.

  12. From the Tools tab, select a tool.

    Recommended tools for Letters and Stripes are:

    • End Mills
    • Face Mills
    • Conical Mills (including dovetail tools)
    • T-Slotters .

    For Trimming, Conical Mills with small ball end are commonly used.

  13. Go to the Feeds and Speeds tab to specify the feedrates and spindle speeds for the machining operation.
  14. Go to the Macros tab to specify the machining operation transition paths (approach and retract motion, for example).
  15. 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.