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:
-
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).
Select the intersecting items:
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 Tools,
Measure and measure the distance between the two sketched splines.