SOLIDWORKS: Tips & Tricks

- [Instructor] For this tip, we're going to be looking and learning more about the intersecting command, or the Intersect command. Now we've already touched on this a little bit on some previous tips and tricks, but I want to dive a little bit deeper and really give you an understanding of what goes into using this tool. So right over here you can see I already have a plane, which is down here, which is going to be a planar surface. And I want to create one more surface that slices through my part. So I'm going to go ahead and choose the Front Plane over here, start a sketch, and I'm going to start with a line. Going to click normal to my part, snap to that endpoint there. Go a little bit past my part, that's fine, because I'm going to be creating a surface here. Come over here to Surfaces, Extruded Surface, let's go ahead and choose the Mid Plane. And let's just make sure that is at least bigger than my part. Click on OK and there's my surface. Okay, now let's go over to the Intersect command. It's under Features and here I have it under Intersect. If you have a different user interface, no big deal, come up here and type in inter, I-N-T-E-R, and guess what, we get Intersect right there, bam. Choose Intersect, and notice over here, I can choose Solids, Surfaces, or Planes to intersect. So notice I have a few planes already. So I have this one here which is the the Front Plane, choose that, sure. How about the surface over here? Sure, how about this guy here? A couple solids, let's do everything we have, why not? All right, now, I have a bunch of options. So I can create intersecting regions. I can create internal regions. I can create both of those, which is probably the best option there. And if you happen to have a surface body, you can cap planar openings on surfaces. So a bunch of cool things you can do here. But before we do any of those things, let's go ahead and choose Intersect, right? And what that does is it takes those surfaces and it slices up our model into all these little pieces. So each one of those could then be used for something else or we could save it as an individual file, delete it, whatever you want to do, just allows you do chop up your existing solid, or multiple solids, into a whole bunch of different pieces. So here they all are, regions one through 12, great. And if you didn't want one of those, you can just click on the box and it just removes that one. But if you like all of them, go ahead and click on OK. Now notice down here at the bottom though is Merge result is there. And it's turned on by default. I'm not sure what SOLIDWORKS was thinking here because normally you're going to take something, you're going to chop it all back into pieces, or chop it all up into pieces, and then merge them all back together? It makes no sense. So why would you want to automatically have this turned on? It makes no sense. But let's just see what happens. Click over here and we get back to pretty much what we had before. So that was pretty useless. Let's go ahead and try it one more time with that unchecked. Come down to the bottom, uncheck merge result, and now we have a whole bunch of pieces, pretty cool. So right over here on my Solid Bodies, you can see they're all here. If you want to go back to that feature itself, Intersect, one more time, I could also say, hey, let's go ahead and consume those surfaces. So I'm done with them. I've used them to cut up my model. I don't need them anymore. Let's consume them and so we don't see them anymore. And now you can see it's all looking quite a bit prettier. Now each one of those is its own body, right? I can use that body, or each one of these things as its own little piece. Right, so all these things have been sliced up. And if you wanted to, of course, you could save this out. So right-click on it and say Insert into New Part, if you wanted to. A whole bunch of things you can do. But anyways, those are the basics and some cool tips and tricks for using the Intersect command to slice up your model into multiple pieces.