Did you know that you can configure sketch planes too?

Article by Alin Vargatu, CSWE updated June 6, 2011


Configurations are the perfect time savers when needing to create families of parts or assemblies. The items that are being configured most of the times are dimensions, features and components.

But did you know you can also configure equations, sketch constraints, external sketch relations, colors, end conditions and even sketch planes? Let’s take a look at the steps needed in configuring a sketch plane.

For exemplification, I am using a simple part (a box with a polygonal cut-extrude). Create 2 configurations (I called mine Cut on Top Face and Cut on Front Face (see Fig. 1).

As you can see, there is a hex cut on the top face of the box. My design intent is let this cut remain on the top face in the configuration with the same name (Cut on Top Face) and move it to the front face in the configuration Cut on the Front Face.

Fig. 1

Note: You probably noticed that finding amazing names for my configurations is not my strongest suit. I apologize for the lack of imagination.

You will also notice that when manually configuring any item,  the active configuration will be affected. Because of that I will first switch to the “Cut on Front Face” configuration, which is the one where the change will take effect.

What do we need to configure? The plane where Sketch2 has been… sketched on, of course. For that select Sketch 2 and from the in-context toolbar select Edit Sketch Plane as per Fig. 2.

Fig. 2

In the Sketch Plane Property Manager, make sure that the affected configuration is Cut on Front Face. Since this is the active configuration, I can choose “This configuration” option or select it directly under “Specify configurations(see Fig. 3). The latter is very useful when you need to affect multiple configurations. Now select the new face defining the sketch plane. In this example, it will be the front face.

Fig. 3

That’s it. The result is quite interesting. Take a look:

Fig. 4 Cut on the Front Face


Fig. 5 Cut on the Top Face

What do you think? Is this better than having 2 different features, one on each face (suppressed or resolved accordingly for each configuration)? What would you do and why?

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Alin Vargatu, CSWE

Alin is a SOLIDWORKS Elite Applications Engineer and an avid contributor to the SOLIDWORKS Community. Alin has presented multiple times at SOLIDWORKS World, Technical Summits, and User Group Meetings, while being very active on the SOLIDWORKS Forum.