Intersection Curve

Intersection Curve 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. (See steps below.)

• 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.

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

1. With a part open, click Intersection Curve on the Sketch toolbar, or Tools, Sketch Tools, Intersection Curve.

   A 3D sketch opens (because you clicked 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.

   

3. Rotate the part, then click the opposite (inside) face of the part.

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, Measure and measure the distance between the two sketched splines.