How to Pattern Structural Components in SOLIDWORKS


The curve driven component pattern feature in SOLIDWORKS allows users to pattern assembly components along unique paths.

The video walkthrough above shows how this feature can be used to pattern support structures under a curved bridge, pattern links along a curved path for a chain or pattern steps to create a spiral stair case.

To use the curve driven component feature, users need to have a viable path for their pattern. In the video walkthrough above, a helical path is created along a pole.

To do this, users begin by opening the pole in a separate window. Next, we start a sketch on the face of the base of the pole, like the one shown below and in the video walkthrough.

This sketch will be a circle centered about the origin, then we’ll add a co-radial relation between the sketch and the edge of the pole.

To create the helix, we’ll navigate to the features tab on the command manager, select the “Curves” icon and click “Helix and Spiral.”

In the property manager, we’ll set the type to be defined by “Pitch and Revolution.” Under “Parameters,” we’ll set the pitch to 144 inches, the number of revolutions to one and the start angle to zero. The helix will be created after we click the green checkmark.

Users can now return to the original assembly and click rebuild. With the curve created, users can expand the “Linear Component Pattern” dropdown menu and select “Curve Driven Component Pattern.”

Users can see a preview of the pattern by first selecting the features to pattern, then activating the “Components to Pattern” selection box.

In the graphics area, we’ll select the step component and in the “Direction 1” group box, we’ll then click the “Pattern Direction Selection” box and select the helix from the Feature Manager Design Tree.

As soon as the path is selected, users can see a preview of the generated pattern, but the steps are not spaced or aligned properly.

To fix the spacing and alignment, users can make adjustments in the property manager. Users can begin by checking the “Equal spacing” check box and setting the number of instances to 20; however, the steps will still need to be wound around the pole.

To do this, users need to change the alignment. By default, the steps are aligned to the seed. Users can change the alignment to “Tangent to curve” to make the preview disappear and activate the “Face normal” selection box. Here, we’ll select the face on which the helix lies and you can see the steps now wind around the pole correctly.

Once the user clicks the green checkmark to complete the feature, a spiral staircase is created.

You can learn more about the new capabilities in SOLIDWORKS 2016 by signing up for a free membership.


About the Author


Sam Sanchez is an Applications Engineer with SolidProfessor and a CSWP. Sanchez is an alumni of UC San Diego, and in her free time enjoys 3D printing and hanging out with her dog Ruby. You can see more training videos on a wide range of CAD, CAM & BIM topics at www.solidprofessor.com.

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