This blog post was inspired by a question I received via email. The question was about how to create a section view in an assembly.  There was a picture attached to the email that showed an assembly  that seemed to have been cut along two planes, but only partially, and  it appeared that one chunk  of the assembly had been removed to reveal the inside, while the rest of the assembly remained visible, similar to cutting a slice of a pie.  I was in a bit of a hurry, so I tried to explain myself really quickly, but then I thought that it was actually a very good question, and it may help a few other readers out there if I answer it here, as well.

For illustration purposes, I’m going to use this old model of a drill jig. Suppose I want to create a section view of this assembly by making a partial cut along the Front and Right planes and removing a section of the drill jig’s handle and  block, thus revealing the screw inside.  If I tried to use Section View  (from the Heads Up Toolbar in the Graphics Area or  from View, Display, Section View), it would slice all components in the assembly all along  a couple of planes parallel to the Front and Right planes, leaving just a piece of it, as you can see in the following image. That’s not really what the section view of the assembly in that picture was supposed to look like.

So, let’s try a different approach using Assembly Features.  First of all, I created a new configuration and called it Section View.  Now, on the assembly’s Top plane, I sketched a couple of lines right where I needed the cut for the section, as you can see in this image. Notice that this sketch in on the assembly’s Top plane, not at the part level.

Once my sketch was ready, I clicked on Assembly Features from the Assembly toolbar and selected Extruded Cut from the list to cut the components in the assembly using my sketch (you can also find this command from Insert, Assembly Feature, Cut, Extruded Cut).

Notice that this extrude cut command works pretty much in the same way it does for parts, but rest assure that the components themselves won’t be affected by this feature outside of the assembly. As a start condition, I decided to use offset, so the cut would begin a short distance from underneath the sketch plane. Under Direction 1, I reversed the direction to extrude trough all in the upward direction.  This way it won’t cut all through the bottom of the block, but only through the top. I used Feature Scope at the bottom of the Property Manager to select that only the handle and the block, but not the screw, would be affected by the cut. You can see all my selections in the following image.

Here in this other image you can see the section view that was created this way. In the Feature Manager, a new cut extrude feature has been added at the assembly level. This feature only exists inside the assembly; if you open your parts in a separate window, they’ll remain unchanged.