Learn how to turn basic 2D sketches into 3D objects.
- [Speaker] The Extrude feature is one of the biggest workhorses inside of SolidWorks. We use that pretty much all the time to create majority of the geometry you're probably going to be designing inside of SolidWorks. It basically takes a sketch with an enclosed boundary and it just defines how far we want to pull that into a 3D space. To get started, let's go ahead and just create a sketch, I'm going to choose the top plane here and let's just create some geometry, how about a circle? Hook a circle on the origin and go ahead and just click on Extruded Boss/Base under the Features menu and go ahead and choose the Extruded Boss/Base under the Features tab and then go ahead and just drag that up.
Now we have a couple options here, I can click on this arrow and drag it up if I want to and notice I get this little in context ruler that kind of shows up where I'm dragging or just type in a value here. So let's type in 3.0. Now again this is pretty straight forward but we have a few more options inside of the Boss Extrude feature. Under here, we have the option to flip it. So we want to go the other direction, we can easily flip it either way and we have a whole list here of other ways we can create this feature. So the most basic is just a Blind, so blindly go for three inches in the direction up.
The next one's Up To Vertex but the problem is there's no vertexes to be up to, we'd have to have a more complex geometry to have that so we'll be getting to that one in a little bit. Same thing with Up To Surface, there's no surfaces right now in our model so we can't use that. Same thing with this Offset From Surface. Again, no surfaces so we can't use it but we'll be getting into this in the future. Same thing up here is Up To Body. So we've got a lot of these options we can't really use quite yet but we will be using them very, very soon. The last one is Mid Plane and we can use that one so we're going to go inch and a half up, inch and a half down for three inches total 'cause we're going on the Mid Plane.
Okay so we'll go ahead and use that one there. Now we've got this Front Plane over here, we get a Top Plane, actually let's go back to that sketch, let's click on the sketch and edit the sketch. Instead of being right there at the center, let's go ahead and just kind of drag this one over here to the right and I want to be centered so I'm going to use a Centerline and just kind of snap that feature right over there and to be good, SolidWorks designer's supposed to add a dimension of six and over here let's add a dimension of six again and then exit out and you could see there's my shape.
Now I've got this Right Plane right here so I can define a new sketch on that plane. Go over to Sketch, click on Sketch and then let's go ahead and click Normal to it so I'm looking right at that side of the cylinder and let's go ahead and create a Rectangle. So I'm going to draw a Rectangle out this way and that way, that's pretty good and if I want to center it, if I didn't use the Centerpoint Rectangle, I could always use a Centerline. Click from one point down to the other point and click on that centerpoint of the origin and then click on the line by holding down control and let's add a relationship that says make that the midpoint.
Now I can change the size if I want to but it's always centered on that part. Okay let's add a couple dimensions. I could add dimension from this side up to the top or I can also add it to the top of the cylinder no problem. I always want that to be a half inch from the top of the cylinder. If the cylinder grows, this feature will also grow. Same thing over here. If I want to snap that to the outside here, I could say .50 no problem. You can start adding dimensions to other features inside of your SolidWorks model. Now when I go over to Features, I'm going to go back to Extruded Boss/Base, I can go blindly but in this case here, I could also go Through All if I wanted to extend that pass to this other part here.
Now I can say Up To Next so I'm going to Extrude up to this surface the next thing it sees so you got that option here. Up To Vertex, there's no real vertexes here but you could try clicking on some stuff, we're not really going to find a vertex. We need to have like a point to get a vertex so I have to come back to that one. Over here, Up To Surface, I can choose this surface here, that would work. I can also choose any other surfaces that happen to be in the part but in this case here, it's one surface that goes around the outside of the part so it doesn't matter where you pick it's always going to be the same surface. I can also do this one called Offset From Surface.
So I'm going to say hey I'd like to choose this surface right here and then give it an offset. Right now, notice nothing shows up because it's got this 5.68 in there. Let's get rid of that and type in .25 and now I've got a smaller offset and it makes sense. So I have quarter inch away from that surface so that's a pretty good way to do that and it works really nice. A couple other ones are Up To Body so I can choose this body right here, same thing it comes up to that body and you can also say Mid Plane which we already looked at. So I'm going to try this one Offset From Surface, choose that surface, quarter inch away that looks pretty good, click on Okay and there's my second feature and kind of we've looked a little bit more into how we can create those shapes.
Now for fun because these are linked together based upon that sketch, let's go ahead and change the original design. Over here, let's make that one eight inches, that's a little bit bigger, exit out, notice everything updates automatically and let's change the height of it instead of three inches, let's make it nine inches, click Okay. And notice, this feature changed as well because 'member, we linked this sketch directly to the height half inch from the top and half inch from the side.
So automatically if the main cylinder grew, so did the secondary feature because we're linking them together. That's a parametric modeling feature. So those are the basics for using the Extrude command. There's a bunch of different options of how you can extrude things up to and depending on the geometry that you have, you have a lot more options as far as how you want to extrude something up to something else. Maybe it's a surface, maybe it's a plane, maybe it's another body, we have a whole bunch of options inside of there and again, the Extrude feature inside of SolidWorks is pretty much one of the most used and real workhorse features inside of our modeling tools we have available to us.
First, see how to how to use the sketch tools to create two-dimensional sketches that become the foundation for 3D objects. Next, look at extruding and revolving 3D features; creating complex objects using the Sweep, Loft, and Surface tools; and modifying parts. Learn how to create uniform holes with the Hole Wizard, and explore more advanced modeling techniques using equations, mirroring, and pattern tools. Then review best practices for putting parts together in assemblies and building robust structures. The course wraps up tips for creating detailed drawings that relate the final parts and assemblies to a manufacturer, complete with an itemized bill of materials and drawing notes.
- Working with templates
- Creating sketches
- Extruding and revolving features
- Applying materials
- Sketching lines, shapes, and polygons
- Trimming, extending, and transforming geometry
- Adding fillets and chamfers
- Working with planes and coordinates
- Creating patterns
- Modeling advanced parts
- Making holes
- Designing with blocks
- Building assemblies
- Mating parts
- Linking sketches
- Using design tables
- Creating part and assembly drawings
- Creating dimensions
- Adding annotations