The extrude tool is one tool that I believe every single person who has ever played with or used SOLIDWORKS knows. It seems to be such a “basic” tool that I believe some of its capabilities get overlooked. The extrude feature has some very interesting functionality built in, and that is what this blog will cover.
Let’s start off by discussing the “From” option menu. The options in the “From” dropdown are often overlooked, if not completely unknown. You can use the “From” option to change where the extrusion is coming “From”, oddly enough. Every extrusion defaults to being “From” the sketch plane you created the geometry on, but you can specify a basic offset parameter using a distance, vertex or different plane/face.
In the screenshot below, you will see that the extrusion is created from a plane that was offset from the top (Red) face. Why create an offset plane when you can just create the offset directly in the extrude? Take a look below.
You can see the sketch was placed on the offset plane (Plane3). The plane was created by specifying an offset distance from the top (Red) face. I will show you how to create the offset directly in the Extrude!
As you can see, I placed my sketch on the very top (Red) face and, within the “From” options of the Extrude, I changed the parameter from Sketch Plane to Offset and inputted the 70mm offset dimension. Instead of creating an offset plane and using that to create the sketch, why not use the offset option within the “From” functionality? It saves you time and makes it easier…what’s not to like about that?
Whenever I teach an Essentials class, I always get asked about the dialog box under the End Condition selection. That is actually the direction of extrusion. By default, there is nothing selected in that box and the extrusion is just normal to the plane of the sketch. There are actually 10 different ways to make a directional selection. If you check out Catherine’s Tech Tip video she shows you all the different options.
To demo the feature, I will show the most common selection, which is a sketched line in the direction of the desired extrusion. This saves you from creating a sweep for such a basic profile that can be created using the Extrude. Check it out below.
The next thing I would like to talk about is the Thin Feature tool. The Thin Feature tool takes the sketched profile and creates a constant thickness in the sketch plane. One good example of this is a hollow tube. Instead of creating two circles in the sketch, you can just sketch one and then specify the thickness within the Extrude. I just have to activate the Thin Feature tool and input the thickness I want along with the direction (One-Direction, Two or Mid Plane).
When using the Thin Feature tool, you do not need to use a closed profile. It can be an open profile. You have to take a look at my screenshot below for one of my favorite examples of when to use a Thin Feature.
This is my favorite basic example of a Thin Feature because creating those rectangular profiles at an angle like that can get a bit tricky, but using the Thin Feature tool on a single line makes it a breeze. If you also noticed, I am actually within a Cut Extrude instead of a typical Extrude. These options not only apply to an Extrude but a Cut Extrude as well. The finished geometry is shown below.
Last but certainly not least is the Selection Contour dialog. The Selection Contour is a way to have multiple profiles within the same sketch, but choose to use a certain profile. When multiple profiles are within a sketch, SOLIDWORKS typically defaults to selecting the largest profile. To change the profile selected, you will want to delete the automatically selected profile and then select the profile(s) you want. If you select sketch entities (closed profiles), it will extrude the “contour”. If you select areas that are enclosed by sketch geometry, it will select “regions.”
Either of the two above techniques will result in the following extrusion.