Intersection Curves

Intersection Curve Tool_Intersection_Curve_Sketch.gif opens a sketch and creates a sketched curve at the following kinds of intersections:
  • A plane and a surface or a model face.
  • Two surfaces.
  • A surface and a model face.
  • A plane and the entire part.
  • A surface and the entire part.
You can use the resulting sketched intersection curve in the same way that you use any sketched curve, including the following tasks:
  • Measure thickness at various cross sections of a part.
  • Create sweep paths that represent the intersection of a plane and the part.
  • Make sections out of imported solids to create parametric parts.
To use the sketched curve to extrude a feature, the sketch that opens must be a 2D sketch. Other tasks can be performed using a 3D sketch.
  • To open a 2D sketch, select the plane first then click Intersection Curve.
  • To open a 3D sketch, click Intersection Curve first then select the plane.

Sketching Intersection Curves

You can use intersection curves to measure the thickness of a cross section of a part.

To measure the thickness of a cross section of a part:

  1. With a part open, click Intersection Curve Tool_Intersection_Curve_Sketch.gif on the Sketch toolbar, or Tools > Sketch Tools > Intersection Curve.
    A 3D sketch opens (because you clicked Tool_Intersection_Curve_Sketch.gif before selecting a plane).
  2. Select the intersecting items:
    • Select a plane that intersects a face of the part.
    • Click the face of the part.
    A sketched spline appears at the intersection of the plane and the top face.
  3. Rotate the part, then click the opposite (inside) face of the part.
    Another sketched spline appears on the inside face.
    You can also select the part in the FeatureManager design tree. A sketched spline appears on every face where the plane intersects.
  4. Click Tools > Evaluate > Measure and measure the distance between the two sketched splines.