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CAD software like SOLIDWORKS makes sheet metal design quick and cost effective. This course gets you up to speed with the sheet metal tools in SOLIDWORKS for designing parts and assemblies, and then takes you on a trip to the factory floor to see the final manufactured results. First, you'll learn to create base features, flanges, and bends that add strength and connections. Then find out how to flatten parts and add holes, cuts, and corners that are manufacturing ready, and use the Convert to Sheet Metal command to convert imported geometry into native sheet metal parts. Author Gabriel Corbett also shows you how to create assemblies from multiple parts, use the Pattern and Mirrors tools to effortlessly duplicate existing work, and then document and export your designs. Finally, take a tour of a sheet metal fabrication company and learn about the machinery and processes that occur during manufacturing.
The Split feature can be handy for separating a part into many pieces using a cut service. This tool can be used both for solid and sheet metal parts. Sometimes it's easier to design one part and then split that part into many pieces using the split feature as one of the final features in the part. To use the Split tool we need to create a surface first. If you're not familiar with the Surfacing tools that's okay, they're not too hard to use. But we do need to make sure we add in the Surfacing Tool Palette. First, let's go up to anyone of the available tabs, right click on it and make sure we turn on the Surfaces ribbon bar. As soon as it shows up we can go into Surfaces and we want to create an extrude surface.
However, before we do an extruded surface, we have to create a sketch to extrude. So let's go back over here. You can see that I have a sketch laid out on top of this part over here. Let's go ahead and edit that sketch. And take a look at what we have. So I've got a few different lines here, they're connecting. The one requirement is that all the lines extend past the end of the part or snap to one of the edges. But we can't have any lines that would stop, like, inside of here. They must all extend past the end of the part. Once we're happy with our sketch, exit out and we're ready to create that surface.
So we go up to Extruded Surface. Come down here, I'll choose that sketch and we can go up a little bit above the part. It's definitely fine to extend up past the part or below the part. But we want to make sure that either way we're cutting it completely through the part in both directions. That looks to me. Go ahead and click OK and there's our surface to cut. Next, we're going to go in and use the Split command. However if you look under the features tab, you might not see Split listed as one of the tools. So we need to go into Insert > Features, come down here to Split. When you choose Split, it's asking what's the trim tool, what are we going to use to trim out these individual parts? And that's that surface we just created. So, go ahead and choose the individual faces, this one, that one, that one, that one and that one.
And those will be all our tools to slice this part. When you're happy with what you have, you can then say Cut Part. And you can see that it creates all these individual bodies. And then any of the bodies you like, you can use the check mark here to select them. We can auto assign names or we can click on that part there. Double click on it and save out a body. Let's go ahead and put them in the Split folder. You can save out the bodies, and click on each one of those. I'm just going to use the default names. And when you're done with that, we can add a few other options as far as copying over the customer properties to those bodies.
And then click on OK. SolidWorks is going to go ahead and split up that part. Save out the individual bodies and there we have it. So now we have all these are in bodies. And we have the Split command is there, and if we go over to our file system, we can go and take a look. There's all the individual bodies. Let's go back over to SolidWorks. And I can now modify this, change it, I can always go back and re-split the bodies and save them out again. The Split feature is a nice way to design more complicated designs as one part and then use a simple surface to slice that part into individual pieces.
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