Explore the basic steps for creating a solid model.
- [Instructor] There are six basic steps used in almost every feature inside of SolidWorks. In this movie, we're going to be covering all the six steps and some examples of how to implement them. Step number one is to select a face or plane. When you first open up SolidWorks, there's really no geometry there, there's no faces there. We only have those three fundamental planes, so you need to choose one of those. Once you've created some geometry, then more than likely, you have some other faces that you can choose to continue building your model. The second step is to start a brand new sketch on one of those faces or those planes.
Step three is to draw geometry in that sketch, and we generally want to have an enclosed boundary for that geometry. Number four is to tie the geometry to the origin. Now, this is not required to create a solid. However, tying it to the geometry tells SolidWorks where it is in space and it's definitely highly recommended. Number five is to add relationships and dimensions defining the shape and size of your sketch. And finally, to create that feature. Now, let's jump over to SolidWorks and start working through the individual steps.
Okay, so step number one is to select a face or a plane. Now, I have a part opened up here and it's completely blank at this point in time. So, over here on the left, I've got the front plane, the top plane and the right plane, and I generally want to start a sketch on any one of those planes. There's a couple ways to do that. One is I can click on the plane itself and then go over here and click on sketch. Or you can go up here under the sketch ribbon bar and click on sketch, then it'll give you the option of choosing one of those planes. So over here, let's go ahead and choose the front plane.
Notice that spins around so we're looking directly at it, and now we can start creating some geometry. Step number two is to start that sketch, we just did that, so now we're in the sketch. Step number three is to draw some geometry. Now I'm going to go ahead and use the rectangle tool, right here, it's two-point rectangle. Click on the origin and drag something out. Notice these little green boxes that pop up over here. Those are called relationships and they're telling me that this line here is a vertical line, this line over here is a horizontal line, and over here, this line over here is tied into the origin with a coincident relationship.
If you don't like one of these things or they were added by accident, you can delete that relationship by clicking on it and hitting delete on your keyboard. Notice as soon as I do that, my sketch turns completely blue. I can also then move it around, 'cause it's no longer tied to the origin. There's three different colors inside of SolidWorks that are defining the lines. So, blue means it's undefined or under-defined, so I can drag it around, I can move things around, it's pretty easy to work with. Now, if I define something by snapping it or adding a relationship, notice these lines turn black, because they know where they are, they're tied into the origin and that's what we need to do in step number four is tie it in with the origin, so it knows where it is.
Now, these lines over here are still blue because I'm able to move them around. I can move 'em down here, I can move 'em up here, I can move things all around. That's where we get to step number five. That's where we want to add some dimensions. So, over here on your smart dimension, click on that. I might add a dimension from this side of the model all the way over here to this side, and then add the dimension of five inches. Now, this line over here turns black, because it's fully defined, it knows it's five inches from the other line. Let's continue doing that and go ahead and choose this top line here, choose a bottom line here, and let's place a three-inch dimension here, so 3.0, enter, and now all the lines are fully defined in black.
Now, if you add too many dimensions or you create a relationship that doesn't make any sense, you're going to get lines that are either yellow or red, so let's try that out to show you what exactly not to do. Over here, if I click on that line there, I can say, hey, I'd like to make this line, let's say it's going to be horizontal. Well, you can't have a line that's both horizontal as well as vertical, so you have a conflict. It's saying the item is unsolvable and there's conflicts. So that's generally a bad idea, so you either have to make this line vertical or horizontal. Problem is, if I try to make this line horizontal, it's going to mess up all the other pieces, so let's go ahead and delete that relationship.
Everything goes back to fully defined in black and we should be all set. So, we've got three different modes we can be in, we can be in the undefined mode, which is generally blue, we can be the fully defined, which is black, and then mode number three is the red or yellow, so conflicts and errors mode. We generally want to stay away from anything that's red or yellow, we definitely want to make sure our sketches are fully defined in black, and it's not a requirement 'cause you can obviously just make a drawing of fully undefined sketches, but most of the time, when you're working in SolidWorks, you're trying to define something that's going to be an exact size, that's why we want to tie it into the origin and give it hard dimensions.
Okay, step number six is going to be to create that feature, so we just have a basic rectangle here. If I hold down the middle mouse button, I can spin that feature around, notice there's no thickness to it, it's just a simple sketch. And now I'm going to go over here to features and I'm going to create either a boss extrude and drag that out. Or, if we didn't like that, you could also create a revolve, choose something to revolve it around, create, like, a little cylinder, like this. You could even create a sweep if you wanted to. You have a bunch of different options here, notice they are all available up here. Everything that's not available is automatically grayed out.
But in this case, I just want to create the extruded boss base, go ahead and drag something out and click on OK, and that is our first feature. Now we've used all six of those steps to create this feature, if I want to do another feature, I'm basically going to follow those same six steps. To give you an example, first I'm going to choose the top of this feature here. And I'm going to go through the steps one by one. So, the first step is selecting a face or plane. Now, I could choose one of those fundamental planes if I'd like to, but I already have this top surface, so go ahead and just choose that face.
Number two is start a sketch, so I can start a sketch by clicking on this little icon right here, it starts a sketch on that surface. I'm going to draw some geometry. I'd like to draw, maybe a circle. Let's draw it out here. Could I draw in 3D? Sure. Should I tie it in the origin? Absolutely. So, step number four is tie the geometry to the origin. So I'ma click my spacebar and I'ma spin it around. If you didn't get that, you probably got a view cube, and you can spin around normal to it. Then I'm going to add a dimension, so from the origin, which is up here, to this circle, I'm going to type in a dimension of three inches, and then, from this line over here, we'll say 2.5, and then define the size of the circle of 2.5 as well.
Everything shows up as fully defined in black lines, so we know everything is fully fine, which is great, and the next thing is going to be creating that feature. So, step by step, step one, we selected that face or plane, we did that. Step two is start a sketch. Step three is draw some geometry, did that. Step four is we tied that geometry to the origin. We added some dimensions for step number five, and finally, we're going to create that feature. So, this feature here, we have a few more options now, because we've kind of gone through these steps already.
So now I can do an extrude cut, for instance, and go ahead and cut a hole right through here. I'm going to type in blind and I'm going to say two inches. And there you have my second feature using those same six steps.
First, see how 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