Intersection Curves
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.
- 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:
-
With a part open, click Intersection Curve A 3D sketch opens (because you clicked
- 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. - 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.
- Click and measure the distance between the two sketched splines.