Suppressing Sketch Relations in SOLIDWORKS

Suppressing Sketch Relations in SOLIDWORKS

A few months ago, I ran across a discussion at a SOLIDWORKS user group meeting where someone asked me if it were possible to create part configurations where the same sketch segment could have two different sketch relations. I wasn’t sure if this was possible so I did some investigating. Much to my surprise, this is in fact possible! Here are some screen shots of this process in action.

To begin with, launch a new part and create a new configuration as well as renaming the default. I chose the following for my example as the descriptive names really teach the concept:

Next, make the Parallel configuration active and begin a new sketch. I then added some relations and size dimensions to this. In this case I chose to make this sketch line parallel to another sketch line.

Second, I chose to suppress this relation by accessing the Display/Delete Relations command from my Sketch Command Manager toolbar:

As this opens in the Property Manager area of my SOLIDWORKS workspace, I select the Parallel1 Relationship and make sure the Configuration option of “This Configuration” is selected with the Parallel Configuration name selected and verify that the Suppressed check box is empty:

A click of the Green Check to close this down. Exit the Sketch, and off to the Configuration Manager tab to activate the Angled Configuration:

Edit the same Sketch, and this time we go back to the Display/Delete Relations:

Now we pick the Parallel1 Relation but this time we want to specify “This Configuration” making sure the Angled Configuration name is selected and we will want to add a check to the Suppressed check box:

You will also see the name ‘Driven’ pop up above the Suppressed check box for your highlighted Relationship. Once you press the Green Check again to close this command down, you will see your sketch show as greyed out Parallel relations (suppressed now) and the top line in my example is under defined. To complete my example, I am going to add a new smart dimension to this sketch and enter in an angled value of 115 degrees. Be sure to only have this 115 for this Configuration only.

Finally, Exit this sketch and switch back to the Parallel configuration. Does it go back to Parallel? It should and just like that you can use Relations, Dimensions and Sketches to help configure your next part or concept model.

So, this is one example of how you can have multiple configurations in a model and have different relationships available to suppress or unsuppress. I hope you found this interesting and useful. I thank you for taking the time to read this Blog.

Brian Reel, Elite AE, CSWE
Senior Manager, Software Solutions
Computer Aided Technology, LLC