What is an Intersection Curve?
Contents
An Intersection Curve is used to obtain the curve at different types of intersections. These intersections include:
- A plane and a surface/face.
- A plane and the entire surface or solid geometry.
- A surface and a face.
- A surface and the entire surface or solid geometry.
- Two surfaces.
Intersection curve entities obtained using the tool are fully defined as they have an existing relation of “At Intersection of two faces”. If you want to modify any of the intersection curve entities you have to delete that relation first.
How to create an Intersection Curve?
To obtain the intersection curves on a 3D sketch:
1. Click on the Intersection Curve present on the Sketch toolbar under Convert Entities or go to .
2. A 3D sketch will open and you will be greeted with the Intersection Curve PropertyManager.
3. Select the intersecting items and click OK.
4. The intersection curves will appear in the sketch. The Intersection Curves PropertyManager remains open and you can add more intersections if you want. When you are finished, click OK when the Select Entities box is empty to close the Intersection Curves PropertyManager.
You can now use this sketch in the same way that you use any other 2D sketch.
To obtain the intersection curves on a 2D sketch:
1. Click on the plane or 2D face first and then click on the Intersection Curve present on the Sketch toolbar under Convert Entities or go to .
2. A 2D sketch will open and you will be greeted with the Intersection Curve PropertyManager.
3. Select the items that are intersecting with your sketch plane and then click OK. The intersection curves will appear in the sketch.
You can now use this sketch in the same way that you use any other 2D sketch.
What are the uses of the Intersection Curve?
Intersection curves are usually used in the following ways:
1. These can be used to make cross-sections of a part. You can also measure the thickness of various cross-sections of a part if your part has a variable thickness.
In the above image, you can see that we obtained a cross-section of our rim with the Right Plane by selecting the Right-plane and the Solid Body that represents the rim. We can now use the Measure tool present in the Evaluate Toolbar or from Tools -> Evaluate -> Measure to measure the cross-section thickness of the rim.
2. They can be used to create paths or profiles for a sweep that represent the intersection of a plane and the part.
For example, let’s say, in the part shown below, we want to make a circular sweep around the whole Cupola but we want the circular sweep somewhat at the middle of its height.
One way is to create a plane at the desired height and then use the Convert Entities tool and select the outer edge to get our path.
But since the cupola has a curved shape we can’t use Convert Entities. As the converted entities do not lie on the surface. So instead we use the Intersection curves option to obtain the path for our sweep. Notice the difference between the two circles. The outer circle is created by the Convert Entities and the inner circle is created by the Intersection curve.
Now we can proceed with the Swept Boss/Base to make our sweep.
Tip: It is better to use Project curve rather than using Intersection Curves to especially create paths or profiles for a sweep as Project curves has a better compatibility for design changes. Read More…
3. Intersection tools also come in very handy when using Boundary or Loft features as they allow you to add tangency between your guide curves and existing surfaces.
Take a look at the below shape where we want to close the surface using the Boundary surface. So we make the desired guide curve but in order to achieve a smooth curvature, our guide curve needs to follow the tangency to the adjacent surface. So we use the plane on which our guide curve sketch is and use the Intersection Curves to get ourselves an intersection curve that we can use to make our guide curve tangent to.
Then we create the Boundary surface which is seamless to the previous surface.
