Betcha Didn’t Know This: Extrude
There are some features in SolidWorks that don’t get much love. Some of these things are really amazing time savers, or help in getting you where you’re going more quickly and reliably. I’ll post a few of these in the coming weeks.
The small groove around the hood of this model would take a lot of noodling around if you had to do it manually, but the Extrude Surface feature has an option that makes it really easy. Just to make sure you understand what’s going on, you’ve got to start from a single face – so in the case of the car hood above, I drew a spline for the hood outline and offset it, then I used the Split Curve tool to break out the groove as a separate face.
Notice the “From” box at the top of the PropertyManager. You can extrude a surface from another surface instead of from the sketch plane. So this groove was extruded from the faces of the car hood.
If you look closely, there are some other options. You can extrude a blind distance, as always, which is what I did here. Plus, you can cap the end. The end cap is like using an offset of the “from” surface. Plus, you can delete the original faces (in this case, it means you can delete the “from” faces!!), and to top if all off, you can Knit the result.
Here’s another instance of the use of this feature in my Batmobile model from several years back.
To create those window insets without this automated feature, you’d have to:
- Offset the main surface
- create an edge or split or projected curve
- create a ruled surface for the offset
- Do a mutual trim
- Knit everything together
There’s actually a little more you have to know to make this work. First, select a non-planar face. You can’t get this to start from a 2d sketch. It can be a surface or a solid face. This actually works if you just hit the Surface Extrude button first, and then select the face.
Then you have to select a plane to define the direction. The plane normal is the direction of the extrude.
If you use this on a solid face, along with the Delete Original and Knit options, it will build another section of the solid, almost as if you had offset a surface and thickened it.
If you just do this on a surface, you can make a little indented box. Very cool. The following three images show the progression from a split out face to an built on box.
I think the Extrude From feature option is a real time saver when you have this kind of work to do. Do you have any examples of when you have used this function?