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Real-world projects are vital to mastering SOLIDWORKS, and sheet metal enclosures are a perfect example of a typical project. Sheet metal enclosures house and protect circuitry, wiring, and other sensitive electronic parts and frequently require customization by a professional CAD designer. So take a firsthand walk through designing a sheet metal enclosure for circuit boards and panel-mounted connectors, as well as fans, power cords, and switches, with SOLIDWORKS. Gabriel Corbett covers the key techniques for working with in-context parts and assemblies that dynamically adjust based on the master part model. He'll show you how to use equations to drive the size of the box and calculate vent holes, work with circuit boards, and download connector components. Plus, learn how to add decals before prepping the final drawings for manufacturing.
Okay. Now that we have the basic shape roughed out, let's go ahead and add some tabs, corners and some connection points. To get started, let's create a little tab here so we can add a pin to the back of it, and a screw hole in the front so we're going to later put in a countersunk screw, to put this whole assembly together. Now, again, we've got four sides of this design that are all symmetrical. So, when we created both of these parts you noticed. We use the mirror commands. So, I want to roll back before the mirror and add that little tab in. So, first things, let open up the cover. So, I am going to say open part, and I am going to take the roll back bar here and just going to roll it back right before the two mirrors.
So, I only have that one corner of the part and look at the origin. Make sure the origin is here, so we want to be using, we're creating our tab on this little corner here. So keep track of that. And if you want to show that, I can go to View > Origin. So it just stays active so you kind of know where it is in the screen, so you're always making sure that you're putting the tabs in the correct location. Okay, first thing, come up to Sheet Metal, then go over to Edge Flange. And for my edge, I'm going to choose this bottom edge right here. And by default, it uses that entire edge. But I really don't want that entire edge.
I actually want only a portion of it. So that's where you come over here to Edit Flange Profile. Click on that. And then grab the corner, so I can drag these in. I can adjust this to size. Now, if you want to look at it straight on, you can click on it. I hit spacebar to bring it normal to it. Sometimes if you hit spacebar on your screen, you'll get up a little view orientation window that tells you the different options, and I always click on normal too, so either way you want to go. You also have a couple options up here at the top of the screen as far as how you want to look at it. But, first things, jump over here, add a couple dimensions. Now, I'm going to dimension to the outside edge, right, because.
If this enclosure is changing size, I want to make sure I'm always kind of staying close to that outside edge, not tied into the origin, or center. So in this case, let's just go ahead and say 0.75 inches. So we're pretty close. And for our width, I'm going to say 0.4. And our heighth, I'm going to say again, 0.4. That looks pretty good, and at this same point in time I can also add in the hole. So, just go ahead and snap a center line. So, I have a center line here to the center point. And then grab a circle, a center point circle and drag out a hole.
Now, for the size of the hole, I gotta get this data from the pin data sheet for the piece of fastener that I'm looking to put in. I know ahead of time that I need a 166 hole. So, I'm going to type in 0.166 and click okay. We will be looking at some of the data sheets of where to get that information in some of the following movies. And I'm going to say 0.2. Okay. There's our hole, there's our tab. And then come and say finish, and it creates that little tab. Now notice where that material ends up being. It's actually right flush with the edge of the part.
But if you remember, this cover actually covers over the edge of the part. It actually comes in a little bit. So, we need to recess this tab in slightly. So go back to the tab, edit the feature. And come over here to off-set. I don't want to off-set it out, I want to actually off-set it in. And as far as how far I want to off-set it in. I want to type in 050 which is the material thickness. And we got flange inside and click okay. Now that should put our tab just one material thickness inboard of where it needs to be.
Next I can add some fill its. So up to features. Go over here to fill it. And I guess round the corners off. So in this case, I'll say maybe 50 thousandths. Just so we don't have any sharp corners when we're building this in the final part. Click OK there. And then I might want to do the same thing down here in this corner here, and 50 thousandths so I can even make it 0.1 radius. Click OK. All right. Now, let's go back, roll this forward again. So I'm going to roll it forward using the history bar. And you can see because I added that before the mirrors, and we used a body mirror, it automatically propagates that to all four corners.
It does a lot of work with very little input. Go ahead and save that out, and then come back to our assembly. Back in the assembly, you can see that there's our little tabs, they look pretty nice. Now, I want to actually create a corresponding little tab that pops up here to fill in that little hole, so in this case, I'm going to edit this part, but instead of opening the part itself, I'm going to edit it inside of the context of this assembly, so click on the part and say, Edit Part. And come over here. I want to make sure that I'm rolling this back before those two features. Grab that bar.
Roll it back to there. And you can see it's actually on this back side here. So, in this case, let's click on that face. Let's click on sketch. Start a sketch, and then we use a rectangle tool. And I'm going to snap to the upper corner here, and we'll snap to the upper face of that. And then we're going to add a couple dimensions. In this case, 0.1 inches. So we're just going to give it 10 thousandths per side, of spacing. And that's going to automatically track. So if I move that tab around, it'll automatically adjust this tab, to be in the right location.
So we can see there it is. And go to Sheet Metal > Base Flange tab, and click okay. That's going to kind of autoalign all the parts. As needed. Hold on, let's go back. Now, that looks like a little bit too big of a gap, so we might have placed it in wrong there. So, let's take a look at that one more time. And yeah, we did. So actually, the 10 thousandths here, because I was looking at it on face is not actually the right dimension. So, let's go back to that again. And it's really this face here that I'm looking for. So, no problem. If you run into an issue like that, you can always kind of double check yourself.
Come back, adjust yourself. There it is. And again, delete this one here, hitting delete on your keyboard. Grab the dimension you want from there to there, .01. And accept that. And that looks a little better. That way you got a nice, tight fit. It auto kind of keys together and it makes a real slick design. Bring that assembly forward again, that auto-propagates all around, and go back to the assembly. The next thing we want to do is I want to add a counter-sunk screw to the front-side face of these two components. So, again, edit this part in context, add a part.
I want to be operating in this one quadrant here, so again I'm going to roll this back before the two mirror commands. Click on this one, come up to features. And come over here to the hole wizard. I'm going to be using a counter sunk screw. We're going to use a 100 degree, number four, normal fit. And up to necks is our end condition. And for our positions. Well, I don't want to really put in a real dimension. I want to just make it relative to wherever that hole is. In that back tab.
So I'm going to click on the wire frame mode. And then look normal to it. And just go ahead and snap to that center point. Notice I'm not adding any other dimensions, just snapping to the center point of where that corresponding hole is. That way if anything changes in my design, it'll automatically track and follow along. Click okay, and then go back to our assemblies, and we roll this, back forward. There it is, switch back to shaded with edges, and I got her holes, and the last thing we want to do in this movie is add this little tab.
Remember, we added this hole, but we haven't added a tab quite yet. So in that case, I can, I want to be editing the cover. But I don't want to roll all the way back, so let's go and edit the part. And let's roll this back to that point right there. Actually no, we'll take them both out and then we'll just do half for the tab. So click on this face here. Start a sketch, rectangle tool. Start right there at the origin, drag that out, snap to the bottom. Let's switch over to wire frame view. So I can see, here's the inside edge of where that hole's going to be.
And so I'm going to dimension directly to that. And I'm going to give it 20 thousandths in this case. From my tab, go back to sheet metal, base flange tab, click on okay. And that should have created that tab. Let's go back to the shaded view. So you can see there's the tab added to there. And let's add a little bit of a radius to this corner, fill it. And we'll fill it at 50 thousandths. Click OK. Roll this whole thing forward. That propagates to this side as well as the other side, and we've made all those adjustments we need.
Now that we've added the screw mounting flanges, the tabs and the screw holes, we're ready to move on to the next step.
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