Creating Combined Curves

You can create combined curves using the Combine command. Combined curve is a curve resulting from the intersection of the extrusion of two curves.

This task shows you how to:

Before you begin: Create a 3D shape containing two curves.

Create a Normal Combined Curve

You can create a 3D curve by combining two planar curves lying on a different planes.The virtual extrusion is computed as normal to the curve planes.

  1. Click Combine in the Wireframe toolbar (Project-Combine sub-toolbar).

    The Combine Definition dialog box appears.

  2. In the Combine type list, select Normal.

  3. Successively select the two curves to be combined.





    Using the Normal type, the combine curve is the intersection curve between the extrusion of the selected curves in virtual perpendicular planes.

    This illustration represents the virtual extrusions, allowing the creation of the intersection curve that results in the combine curve.



  4. Click OK to create the element.

    The curve (identified as Combine.xxx) is added to the specification tree.

Create a Combined Curve Along Directions

You can create a combined curve along specified directions. You need to specify the extrusion direction for each curve (Direction1 and Direction2 respectively).

  1. Click Combine .

    The Combine Definition dialog box appears.

  2. In the Combine type list, select Along directions.

  3. Successively select the two curves to be combined and a direction for each curve.





    Using the Along directions type, the combine curve is the intersection curve between the extrusion of the selected curves along the selected directions, as illustrated here:



  4. Click OK to create the element.

    The curve (identified as Combine.xxx) is added to the specification tree.

Important: Select the Nearest solution check box to automatically create the curve closest to the first selected curve, in case there are several possible combined curves.