This is the second in a series of Tips and Tricks that will show you how to create and use 2D and 3D Splines. If you haven’t read the Drawing 2D Splines Tips and Tricks, you might want to read it before proceeding.

In this short exercise you will learn how to add Spline Points to a spline, and then you’ll use Construction Lines to gain more control over the shape of the spline. First you’ll create a spline loop, and then you’ll modify it to create a fully constrained elliptical shape.

Create a Three Point Spline Loop.
Open a new standard part file, and then use the Spline command in the 2D Sketch Panel to create a Three Point Spline Loop.

1. Click the Spline command. 
2. Click three points in the graphics area. 
3. Double click the first point to create the spline.
4. Type the escape key to exit Spline mode.

Add a Spline Point.
The spline will have four spline points, which will define the size and shape of the elliptical shape.

1. Right click on the spline and select Insert Point.
2. Place your pointer over the spline on the location for the new point.
3. Click your left mouse button.
4. Drag the points so that they are about equally spaced.

Constrain the geometry.
As with all of your sketches, you need to fully constrain the geometry. You can add dimensions between spline points, but the best practice is to use construction lines, and then add dimensions to them. The construction lines will define the height and width of the ellipse.

1. Draw a construction line from the left point to the right point, and then add a Horizontal Constraint to the line.
2. Draw a construction line from the top point to the bottom point, and then add a Vertical Constraint to the line.
3. Add a Coincident Constrain to the node in the middle of the horizontal construction line to make the node coincident with the vertical line. Be sure not to select the node in the middle of the vertical line when you do this.
4. Add dimensions to the lines.
5. Use the Fix constraint to fix the location of the node on the bottom of the vertical construction line.

If all went well, the profile should look almost symmetrical and the sketch should be fully constrained. Click the Auto Dimension command to confirm that there are zero constraints required. If two constraints are required, chances are good that you didn’t fix the node on the bottom of the vertical construction line.

If you read my Tips and Ticks about Essential Templates, you know that the best practice is to use projected geometry to anchor your profiles to the sketch plane. In this example the spline was created first, so the sketch was anchored by using a Fixed constraint. A better approach would be to draw the construction lines first. One of the construction lines would be coincident with a projected node from the center point of the sketch, and both lines would be fully dimensioned and constrained. The final step would be to use the green snap dot to constrain the spline points to the nodes on the ends of the construction lines while you draw the spline. When you use this method the spline will be symmetrical.

Why is this important?
The example above demonstrates how splines can be malformed when you don’t use construction geometry before drawing the spline. Anytime you draw splines you should start with construction geometry.