Creating Combined Curves

This task shows you how to create combined curves, that is a curve resulting from the intersection of the extrusion of two curves.

Open the Combine1.CATPart document.
Display the Project-Combine sub-toolbar by clicking and holding the arrow from the Projection icon.

  1. Click Combine .

    The Combine Definition dialog box appears.

  2. Choose the combine type: normal or along directions.

    • Normal: the virtual extrusion are computed as normal to the curve planes

    • Along directions: specify the extrusion direction for each curve (Direction1 and Direction2 respectively).

    Normal Type

  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 represent 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.

    Along Directions Type

  5. 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:

  6. Click OK to create the element.

    The curve (identified as Combine.xxx) is added to the specification tree.
     
    The Nearest solution option, allows to automatically create the curve closest to the first selected curve, in case there are several possible combined curves.