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SolidWorks is the world leader in 3D software for product development and design. Start creating manufacturing-ready parts and assemblies, as well as detailed drawings and bills of materials. In this course, author Gabriel Corbett shows how to create 2D sketches that will become the basis for your 3D models. You'll use the Extrude and Revolve tools to turn 2D sketches into 3D parts, then create more complex geometry with sweep and lofts. Then learn how to use the cut features to remove material and shape parts, and use mirroring, patterning, and scaling to modify parts. Next, you'll combine parts into movable assemblies and subassemblies. Finally, you'll create accurately annotated drawings, complete with itemized bills of materials that relate the final parts and assemblies to a manufacturer.
The real power of SolidWorks starts to shine when we link one part to another. If we think about assemblies as a whole instead of as individual parts, we can use one of the parts to drive the others. Think about a jar and a lid. Wouldn't it be nice if we made the jar bigger, and the lid would automatically change size to fit? We can. And we can do so much more. On the screen here, I have 1.4 assembly opened up, and this has got basically a jar, and the lid. First thing's first, we need to decide which part will be the driving part and which part will be the driven part.
In this case here, I'm going to use the jar itself as the driving part, so if I make that jar bigger, then the lid'll automatically adjust. So, you, you don't want to get into a state that you have components that are linked in a chain or in an infinite loop, that as one part changes the next part changes, then it goes all the way back to the original part. That can cause issues with parts linking to each other in a chain, and coming back to the original part. So it's always best to kind of pick one of your parts is going to be the part that's going to drive, most of the other parts and then build from there. To get started, let's take a look at this sketch here.
So I'm going to go ahead and open that up. And I'm going to say Open Part. And you can see it's a basic revolve. I'm going to go ahead and click on the plus, take a look at the sketch, and take a look at what's in there. So pretty straightforward sketch here. Just basically lines, and you can see we have three inch dimension. So that's the dimension we're going to want to change. And then we want the lid to automatically adjust. So in this case here, we're not going to actually touch this part, I just want to go through and show you what's in the sketch. I'm going to close that down, come back up here, back to the assembly. Say yes to the changes, and then open up the lid.
In this case here, I can open the part again, take a look at it. And inside of that sketch, you can see, again, I've got that three inch dimension here, defining the outside of the part, and everything else looks pretty standard. Okay, now is the tricky part. Instead of opening these parts individually, let's go ahead and open them them in context to the assembly. So this case, here, I want to change this part, based upon this part. So, right next to where I'd normally choose Open, I can also say Edit Part. As soon as I do that in the assembly, what happens is the original part over here, the jar turns clear transparent, and it shows me that I'm editing only the lid then I come down here to where the lid is take a look and notice the entire tree for that lid opens up just like we were looking at individually in the part, I can click on the revolve.
And I can open the sketch. So, the first thing's first. You need to determine where is the dimension that we want to drive from the other part. So in this case here, it's pretty simple because there's only one revolve in each part. But in this case, let's go ahead and choose sketch one and click on Edit Sketch. I'm going to click on the space bar to look normal to the part. And now, we've got this hard dimension here as three inches. What I need to do is get rid of that dimension right away. Click on that, hit Delete. And now, I have the ability to grab one of these lines and drag that out, and just double check that that's going to give you the right type of motion as the jar gets bigger, you basically want this to track, and do the exact same thing. Okay? Then instead of adding a hard dimension.
Let's put a dimension here in relationship to the base jar, and instead of the dimension, we can actually add a relationship as well. In this case here, I could take this little point or this line and make it co-incident to this line here. Let's try it out. Click on this line. Hold down Ctrl. Choose this line here. And I'll say, make co-linear. Now those two lines are going to be in line all the time and there's no hard dimension to finding it three. So if this jar gets bigger, theoretically, this lid should get bigger as well. When you're happy with your changes, go ahead and click on Exit Sketch. And you're noticing hey, the assembly didn't change at all.
What's going on here? Nothing changed. Well, here's the power. Let's go ahead and open this part now. Edit that part. Go down to that sketch. In this case here instead of the three inches, let's change it to six inches, 6.0, exit sketch. And then go back to the assembly and notice right away the lid automatically changed size to fit the exact same proportions. Auto update based upon that relationship between the two parts. Now this is only the beginning. You can make this extremely complicated, and you can have many, many different parts based upon one driving part, and you can have parts defined off of other parts and so on.
It can really get pretty complicated. But it really starts using the power of SolidWorks. External references can generate highly automated assemblies that really show the power of SolidWorks. Best practice is to have one main driving part, and have the others reference it. It is possible to create a circular reference, so make sure you think through what's driving what.
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