Creating and orientating SOLIDWORKS derived sketches

Let’s start with a question:

If you needed to translate a sketch 90°, let’s say from the Top Plane to the Front Plane and have those sketches update as one (linked), what would you do?

You could copy/paste the sketch, redefine relations, apply in-context relations, then proceed to link values with equations/global variables. This however can be time consuming for complex sketches. By now you must be asking yourself; “there MUST be a better way?”.

Enter the Derived Sketch!

SOLIDWORKS Derived Sketches are exact duplicates of the original sketch but retain a link to the original. They can however, only be placed, not changed.

Let’s start with initiating the Derived Sketch command. In order to do this, it needs some specific things pre-selected: Both the source sketch and the plane it will be copied to. With this done magically the Derived Sketch command (Insert > Derived Sketch) becomes selectable.

Once selected it will insert the source sketch onto the new plane. Now all that’s left to do is orientate it. To do this we will use the Modify Sketch command (Tools > Sketch Tools > Modify Sketch). This will cause your mouse icon to change and a black triad to appear.

Modify Sketch mouse icon

By using your left & right mouse buttons you can move / rotate the sketch manually, but notice how your mouse icon changes yet again when you scroll over this black triad. This triad allows you to mirror the sketch vertically, horizontally, or diagonally bases on the triads location.

Mirroring using Modify Sketch

Once in the proper orientation, all that’s left to do is lock it down with a few relations.

Fully defined Derived Sketch

Now we have a fully defined sketch that is linked to the source sketch, and denoted in your Feature Tree as derived.

Derived Sketch

No more worrying if your sketch has updated correctly! Happy sketching!