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Autodesk Inventor Tips & Tricks

Control Inventor Splines with Spline Commands

Autodesk Inventor 2019
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by David Melvin, PE, TEDCF Publishing

This is the forth 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, Constraining Splines, and The Process of Drawing Splines Tips and Tricks, you might want to read them before proceeding.

In this short exercise you will learn how to use Spline Commands to control the shape of splines.

Create a Fully Constrained Spline Loop

Create fully constrained spline loop

If you’re not sure how to create a fully constrained spline loop, read The Process of Drawing Splines Tips and Tricks.

Fit Methods
You can use three different Fit Methods to fit the shape of splines through spline points. By default the Standard method is used, which provides a smooth transition through spline point, but it cannot be controlled by tension setting. The AutoCAD method is less smooth, but it can be controlled by tension settings. And the last setting is the Minimum Energy setting, which is just as smooth as the Standard setting, but this setting can be controlled by tension settings. It also creates the largest amount of data, which increases file size.

Fit Method Standard AutoCAD Minimum Energy

To access these methods, right click on the spline and select a Fit Method.

Bowties are used to define the shape of the spline near spline points, and they can take three forms: a Handle, a Handle and Curvature, and a Handle and Flat.

First we’ll add a Handle and dimension it. Right click on the top spline point and select Activate Handle.

Activate Handle

Once you select the command a handle is highlighted on the spline point.

Handle shown on spline point

The handle can be used to change and constrain the shape of the curve near the spline point. You can change the angle of the handle by dragging one of the grips, and if you do, be sure to add an angular dimension to control the angle. To keep the spline symmetrical, add a Horizontal constraint to it.

Dimension and horizontal constraint on handle

The length of the handle defines the relative length of the curve that is tangent to the handlebar. For this example, when you add a dimension to the length of the handle, the distance is .476. This is a unitless value that describes how closely the spline hugs the handle.

Dimension changes the length of the handle

Increasing this value increases the length of the tangent portion of the spline making the spline appear to hug the handlebar closer.

You can also define the radius of the spline near the spline point by changing the bowtie to a handle and curve. To do this, right click on the spline point and select Curvature.

Select the Curvature option

With this option you can control the radius of the tangent portion of the spline. The radial dimension in the following example is .467 inches. So this dimension uses standard units.

Radial dimensin on curvature curve

The last option consists of a handle and flat curve. Before you evoke this command, delete the radial dimension. Once you’ve done that, right click on the spline point and select Flat.


If you try to add a dimension to the flat curve you’ll find that you can only add a radial dimension.

Radius of Flat Spline Handle optoin shown

That’s because the Flat option essentially sets the radius of the curve approximately to infinity. In this case, it has the same effect as setting the radius of the Curvature option to 393.701. You can change this value back to .467 to have the same result as using the Curvature option. When you select the Flat option the Curvature option is automatically deselected. Likewise, when you select the Curvature option the Flat option is deselected.

Why is this important?
While splines are more difficult to define the exact size and shape than lines and arcs, knowing these commands give you more control over them. This will ultimately help you take more control over your solid models.