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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.
Much like linking to other parts in SolidWorks, we can have a layout sketch that drives a series of parts. SolidWorks has a built in layout function, or we can use standard sketches to lay out designs. To start using layouts, we need to create a layout in an assembly mode of SolidWorks. If you open up 14.2 Assembly, you can go ahead and see that I've actually created a layout sketch first, and I have one part already pre defined and designed off that layout. Now what I want to do is actually want to built out a secondary little frame bracket, it's going to build off that as well. Before we do that, let's go ahead and take a look at what the layout sketch has inside of it.
Notice I have a layout because I have this little four bar mechanism up here, this little wooden frame looking thing, that tells me I do have a layout derived in this assembly. So right-click on that Assembly. Come down here to Layout and take a look. You can see, if I click on the space bar and looking normal to it. That I've got a 24 inch circle to find. I've got a couple dimensions here, and I basically just have some lines defining that octagonal shape. That's all I really need to define this whole shape here. Go ahead and exit out of the layout sketch, come back to the assembly, and you can see I already have one part already defined from this.
So I have a sketch that's linked. And by the way, if you ever see these little arrows at the end, that means there's some kind of reference outside to some other part or some other sketch. So go ahead go to the Sketch. You can see I basically just got a few different lines. And then we off set these lines a little bit. And pretty basic, right. And that's all based upon those, there's no dimensions here. We're just referencing or converting the entities from that layout sketch to define that shape. The only dimension I do have is this quarter inch here, it's defining the thickness of that plate. Okay, go ahead and exit out.
And then come back to the assembly. Now, I want to put a new part in this assembly, so I have a couple of ways I can do that. One, I can go out and click on you know, New > Create a New Part, drag that part into the assembly. And it can be a blank part, there can be nothing in the part, that's totally fine. But the problem is that you make sure that you mate that part up. So, one way you can do that is you can mate the origin of the new part to the origin of the assembly, that brings it all together. That's a great way to do it. Or the other way you can do it is basically go over to insert components click on New part. What that will do is actually create a virtual component or virtual part within your assembly.
And make sure first before you do that though, you have actually a part name here. So 14.2.assembly. Make sure you save the assembly first so it's not just a new document when you open it up, because this part here will be created based upon that name. I can, if I want to save out this part here right-click on it and click on Save Part in External file, and I definitely recommend doing that sooner than later. Click on that, notice it's called Part2, and whatever path it's going to be stored in. In this case here, we're storing it in the Desktop.
So, I want to overwrite that path. So I'm going to go ahead and call it 14.2- 2 because I already have a -1. And make sure you're overriding that. And then click on, OK. And now I've saved that part out to the file system and it can be used and opened just like a regular part. But right now, that part is blank. So, let's go ahead and create something in it. So first things first, click on the part and make sure we're editing the part. I want to go and look at which plane to start drawing on. And it looks like the front plane is the one that I want. Go ahead and click on Sketch, start a sketch on that plane.
And we'll go ahead and choose the line command, but before we do that, let's first go ahead and convert a couple of these. We've already got lines behind the scenes in that layout sketch. Why not just use those? So click on this first line here, hold down Ctrl, pick on the second line here and convert those over. So convert entities brings them directly into the sketch here which is great. And we could do the same thing over here except those lines would extend too far so, I'm going to use the regular line command here. Snap to the end point and instead of going to the end let's just snap right here to this intersection of the inside of that plate and then come all the way down here.
So we enclose that shape. And just so you know, you see that little blue dot there I accidentally just double clicked too quick and it created another little line segment? Just delete that if It's a real common error to quickly double-click and it creates a smaller line segment and that'll screw up your drawings. So make sure that all of your points are clean points. And don't have any type of little artefacts like that. Anyways notice I'm snapping to the inside here so if this plate were to get thicker later on it would automatically update and be fine. I'm converting some entities here. All of this is based upon that layout sketch so there's no dimensions.
So, anything that's going to change in the layout sketch is automatically going to adjust in the sketch as well. Okay. When we're ready to create a feature, go over here to Features, Base Extrude. Type in a half of an inch, click OK, and there's our little bracket, okay. When you're ready get back over to the assembly. So exit out of this part. We're back in the assembly mode now. And what I want to do is I want to pattern these parts around. So I already have a pattern predefined, so I'm going to take this history bar, I'm going to roll it forward. And you can see I've already patterned this part here just by choosing the center align as my axis of rotation, and patterning that part around.
I created the axis just by grabbing the top plane and the right plane, coming up to reference geometry, and creating axis. Pretty quick. Okay? Now what we want to do is, edit that circular pattern. So come up here to Edit feature. And, go ahead and choose, notice I already have the 14.2 in there -1, and I want to add the 14.2- 2, so I'll just go ahead and click on that second item. It's going to add it to the pattern, click, Ok, and now you can see we got both those in the same pattern, looking pretty good.
Now let's go ahead and go back to the layout sketch and change the sketch and make sure that all the components are going to automatically change and move. So, right-click, Layout, and this case here, let's change it to 36. The layout sketch is going to change. Go ahead and exit out of the sketch. And notice that all the components automatically update. They change size based upon the layout sketch. And then the pattern automatically updates as well. I can also go ahead and choose a component maybe like this first one here, one.
And let's just play around, and say maybe instead of this being a quarter inch, what if we change it to a one inch. It gets a lot bigger. Update the sketch and notice that this component here also automatically updates. If I go back to that, exit out of that part, the secondary part, because we based upon the inside there, you can see there's a nice line. Defining where that is, because those automatically update based on the thickness of that material. If I want to go back, I can always go back here, edit the sketch back to the quarter inch. And notice again, it automatically updates based upon that.
It's all in-context modeling. It's a really great way to design things, because if you change one thing like a layout sketch, all the other components will automatically update. It's a very powerful way to work in SolidWorks. Layouts can be very helpful, and give the ability to derive a large amount of parts from the same layout sketch. It also creates a clear order of what's driving what, all by changing just one sketch.
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