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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.
If you have SolidWorks Premium or Professional, you have the option of using toolbox within SolidWorks. Toolbox provides thousands of hardware items that can be quickly added to your assembly. Let's go ahead and take a look. I have a little block here with some counter board holes in it for a 3/8-16 socket head cap screw. What I want to do is I want to build an assembly with some socket-head cap screws in this part here. So I'm going to go up to File > Make Assembly from Part, and start my first Assembly here. Bring that first block in.
There it is. And now I want to to add some hardware to this. Now, option one, I could go and design my own piece of hardware. No. Number two, I'm going to go ahead, and I can go to the internet, like McMaster-Carr, something like that, and I can find a source for that hardware. And download it, and that's a great way to go. And then third option would be to use the built in tool box within SolidWorks to download and use those files. We actually don't even need to download 'em. It just configures it locally on our system or on a shared network folder. We can use it locally here. To do so we need to make sure we add in toolbox.
So under Tools > Add Ins. And you can see all the different things we can add in here. And I want to come down here to Toolbox, or SolidWorks Toolbox, as well as SolidWorks Toolbox Browser. So go ahead and turn both of those on. And you might want to also turn those on, so they automatically start, when you start SolidWorks. Click OK. This should add a brand new label to the top of your screen. And also, over here in your Design Library, you should now have a folder called Toolbox. So if you click on the plus next to Toolbox, you can choose what system you want to use.
I'm going to use ANSI inch. And expand that out and here's a bunch of the things that I can download and use in my designs. I can use bearings, bolts and screws, keys, nuts, o rings, you name it, all kinds of great things in here I can use. In this case here I'm going to go to bolts and screws. I'm going to come down here to socket head cap screw There it is, and you can see I have several different types. I have a socket head button cap screw, a countersunk, a shoulder screw, or the regular socket head cap screw. Click and drag that item into your design. Very easy into your assembly.
It has to be an assembly, by the way, not an individual part, you have to be in the assembly mode. Now I can configure that component. So number one is what size do I want to use? In this case here I actually want a 3/8-16, so click on that. And then my length, I want that to be one inch long. I can click on the drive. I can have a hex. I can have a spline. I have a bunch of different choices there but I'm going to choose the hex. How long do I want it threaded? Do I want it fully-threaded or only a portion of it threaded? And then how do I want to display that item in my design? Do I want it simplified, do I want it cosmetic or schematic and notice if I change from one to the next it will add more detail or less detail to your design.
Generally, I prefer to not have too much detail in hardware because it just adds quite a lot of overhead to the system to be showing all that extra detail when you really don't need it. So I'm going to go over here and click on Simplified. To make that a little simpler. Here's the name it's going to be given it and you can overwrite that if you need to. When you're happy with everything you want, go ahead and click on the green check mark. And now you have that item in your assembly and notice it also shows up on your tool tip. You can then quickly go over here and start mating components together in your design, just by clicking, placing in these holes. Then come down here.
Place into the hole lower, and there you go. So quickly add that when you're done with it, hit Escape. If you have an item that wasn't made up properly in the beginning. You can always click on it, drag it around, and you can set up your mates for it, if you'd like. Put it all together, it makes it really simple way to quickly bring hardware into a design, drop it right into your assembly. It configures it on the fly, and you have access to it at all times. Without having to download it. One of the main drawbacks from using toolbox is there's no real part number assigned to that file. It's a generic part number that SolidWorks assigns and you can't go out and actually buy that part number.
You still have to figure out where that piece of hardware will be purchased from later on to then use in your design. Also, when using the toolbox with other users, it's best of have that toolbox on some type of a shared network server. That way, everybody has access to the same hardware. Toolbox is a great way to quickly add hardware to an assembly, but keep in mind, if we're going to be zipping up these files and sending them maybe to an outside vendor, we have to make sure we have to include that hardware in that assembly. So you might want to use the pack and go feature within SolidWorks to zip up all the individual files, including the hardware, and put it into one nice zip folder.
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