Join Gabriel Corbett for an in-depth discussion in this video Revolve, part of Cert Prep: Certified SOLIDWORKS Associate.
- To create revolve features, we want to make sure that we have a center line as well as a sketch. All it needs to be is one closed feature, goes all the way around, and we need a center line to revolve around. A couple things I want to point out while we're here. If you're adding dimensions to a drawing, I want to sometimes use what's called a double dimension that makes it a lot easier to input the exact values you might be getting from the exam. So to do that, so for instance, this is going to be 250 millimeter diameter, and not radius, so notice it goes as a double dimension. So I'm going to delete that for right now and go back.
If I had to make a dimension from the top here to the bottom, it only gives me the option of the 125. But instead, if I were to give a dimension from the top to a center line, on this side here, it's 125, but as soon as I pass over the center line, notice it switches over to the double dimension, or the full diameter of that, so if I want the diameter, all I have to do is dimension from something to a center line. Now it has to be a center line to get that feature, so kind of handy there. And same thing if I want to do the same width. I can click on the center line, create a new center line there, and then make a dimension from this outside edge to that center line, So I'm going to delete that 30 and then add a dimension from here to the center line and get that double dimension, 60, and click OK.
Again, add a few other dimensions here. From here to this point. Obviously, I can type in 30 right here, but if I got rid of that, I can also do the same thing here, from that point to that center line, and type in a 60, so that's double dimensioning, and a lot of times, you're going to be getting diameters, not radiuses, so it's easy to put those full values in. Couple more dimensions here, I'm just going to type in real quick. Make that 15, make this 45. All right, now I'm ready to revolve.
Now, couple options here, when I go to Revolve, Features, Revolve, it's going to ask me what do I want to revolve around? Now I can revolve around this right here, or delete that out of there. I can revolve around this one right here. So two completely different parts, depending on what I revolve around, so keep in mind what we're going to revolve around. In this case here, I want to revolve around this axis. Click OK, and then notice I only designed half the part, because it's symmetrical. So that's why I'm going to use that Mirror feature, mirror about a face, and I'm going to use the body to mirror.
Mirror that body, click OK, that's my completed part. So that's a real quick way to revolve. Make sure you can use those double dimensions. They really help out in the exam, and make sure we also can link to some equations, values that we want to, to make that a lot simpler. To do that, I'm going to go back here. This 250, double click it, and just say equal to, and I'll say, let's say for instance, A, and make a global variable, make it 250, click OK. Now that's an equation driven dimension, and if I want to change it, I can just go up to my equations over here, look at A, modify it, and the part will automatically update.
So a real quick way to make modifications, and that's the Revolve feature.
Along the way, he'll cover creating effective sketches, using equations to modify parts, weighing parts, building assemblies, assigning the correct materials and units, and creating drawing views. At the end of the course, there are two sample exams to practice what you've learned.
- CSWA requirements review
- Working with sketch entities (Line, Circle, Rectangle, and Arc)
- Making offset, convert, and construction lines
- Reviewing the boss and cut features
- Sweeps and lofts
- Smoothing corners with Fillet and Chamfer
- Creating linear and circular patterns
- Dimensioning techniques
- Setting mass properties
- Selecting and using materials
- Inserting components
- Setting up reference geometry
- Establishing standard drawing views
- Annotating your drawings