Section Views with Surfaces

This works, but may not be an ideal solution. Create surface offset
copies of all your relevant surfaces. Create a new plane, relative to what
you want your view to be. Trim all of your offset surfaces to that plane.

 

Even though SolidWorks will display a sectioned view of a surface in a
part viewport, the same is not true for a drawing.

There needs to be some thickness to the surface. So, if you can create
a solid by inserting a Boss/Base / Thicken with the selected surface
(even as little as .001", for example), then the thin solid can be
sectioned and shown in the drawing.

Once the side view (or section) exists in the drawing, the edges which
make up the contours of the surface (along the original face, prior to
thickening) can be selected and converted - on edge - into the view.

After the entity conversion, the Thickened Surface feature can be
selected from the drawing view's Feature Manager and the body hidden.

This will leave just the zero thickness surface edge entities...

Per O. Hoel

 

Hello,
I am trying to create multiple section views of a surface model in a drawing
and/or part file, but I am having some problems. I have no problem in
either mode with a solid model, but when I try it with a surface, it says
that I cannot get a section view of an empty model (in the drawing file). I
realize that I probably shouldn't be able to see anything (since I'm
essentially viewing a zero-thickness surface on edge), but I was wondering
if there was any way I could sort of "turn on" the edges of the surfaces at
various cross-sections so they would be visible. Any ideas? Thanks a lot.

-Ryan

 

Alright, I ended up adding that boss (through thickening by 0.001") since
that was easier on my end, and it worked great. I was able to get the
several cross-sections I needed. They turned out beautifully. Thanks a lot
for the help.

-Ryan