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Video: Designing the cover

Once we have the base part roughed out, now we're ready to get started with a cover. What I'd like to do is build a part that is built in context around the base part. So any changes to the base will automatically be reflected in the cover. And it'll auto-scale to size. To do so, let's go ahead, and first take a look at the finished part. You can see here, I've got the cover and the base together. And there's our cover. And then I jump over here and look at the cover itself. You can see I've got a big, long radius bend here. I've got a little tabs here we're going to be adding later. And then I've got a series of vent holes along the edges.
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Watch the Online Video Course Sheet Metal with SOLIDWORKS: Enclosure Design Project
2h 31m Intermediate May 21, 2014

Viewers: in countries Watching now:

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.

Topics include:
  • Working with the Base and Flange tools
  • Building the rough enclosure shape
  • Designing the cover
  • Adding vents
  • Adding components
  • Cutting holes for connectors
  • Adding graphics
  • Making assembly drawings
Subject:
CAD
Software:
SOLIDWORKS
Author:
Gabriel Corbett

Designing the cover

Once we have the base part roughed out, now we're ready to get started with a cover. What I'd like to do is build a part that is built in context around the base part. So any changes to the base will automatically be reflected in the cover. And it'll auto-scale to size. To do so, let's go ahead, and first take a look at the finished part. You can see here, I've got the cover and the base together. And there's our cover. And then I jump over here and look at the cover itself. You can see I've got a big, long radius bend here. I've got a little tabs here we're going to be adding later. And then I've got a series of vent holes along the edges.

So you can start with that. Let's go up here to New > Start a Part and click OK. Now that I have a part open, I could start a sketch and start creating some lines to create that shape. However, what I really like to do is do that in context in my assembly. So first, let's go up to File. We're going to save as 2.2-2. Save that and let's build an assembly. So, I can go up to New > Assembly, click on OK. And then, my starting part of my assembly wants to be this 2.2-1, which is that base piece.

Click on that and click OK. That comes in, the origin notice is right here in the center of the part, and the origin of that part itself, again is in the same spot. Now, go to Window > Tile Horizontally, and you can see all our parts. The 2.2-2 is right here, and I'm going to bring that in. So you're saying, well, there's nothing in there, how am I going to bring that part in? Well. Don't worry let's just go ahead and click on it and drag it in. Now, that part should be in here; you can see it here, so let's go ahead and expand out the assembly. And while we're at it, let's go ahead and save the assembly, so go click on File > Save As and I call this one 2.2.

Click on Save. Now you can see here I've got two parts in the assembly, the dash one and the dash two. And the dash two is just floating around in space, and there's nothing in it. So first things is we actually want to mate that to the assembly. So click here and let's find that origin; you can see the origin's right over here. And I want to bring the origin right in to where the other origins are, so I can click on Ctrl on my keyboard. Click on Origin, and then click on Mate. What that will do is bring this two origins together.

We'll click on this little check mark or make sure it's checked, called Align Axes. That aligns both your x, y, and z axes, so that you have all those lined up. And with one single mate, you fully define that part. Click on the green check mark. Okay, now I've got a part who's mated, and he's ready to go. Let's start building the part. First, let's click on the part itself 2.2-2 and come up here to Edit Part. Now I'm editing the part, I want to create some lines. So first things first, I need to find a plane to draw on. Now, inside of my part here I've the front plane, which is right there where we need it.

That's good. Or the top plane or the right plane. In this case here, I want to have something that's going to come out and over here, so let's start and use that front plane. Start a sketch. And then create some lines. Now there's a couple different ways I can use to create lines here. One, I can click on these lines here which going to be the outside and I could convert those over, I could bring those into my sketch. And that does work really well, and so let's go ahead and do that with a couple of these. So let's convert 'em over. And then create a line. I'm going to create a line from here over to here.

Now one issue you have if you do convert all the lines is sometimes this line when you start mirroring the enclosure over, will continue on. So I want to make sure that I'm stopping that line right here at the origin. All right, so it's always going to stop. I'm going to use the center line, and then down here, I also want to make sure that I've got a continuation of that line down at the base. Okay? Looking pretty good and jump over here to Sheet Metal. Click on Base Flange Tab. You can see this gives us a little preview of what we're going to get. First, I want to go the other direction, and I want to make sure that I'm getting that curve on the right direction.

You can see this one is on the inside. So let's flip that over so it's going in reverse on the outside. Make sure you're using the same exact material that you were before, and we are. And then our length, how far do we want to go? So I can drag this out here; I can type in a value. But, instead of doing that, let's go ahead and click on Up to Surface. Which surface, this one right here. That way, whenever the base part moves around, you can see the covers going to automatically adjust to the right length. If you're happy with that, click on OK.

Great. Exit on the assembly, and now we're ready to continue on. This so also a great time to use the Mirror command. So, let's go ahead and open up each one of these parts. Open the part, go over here to Features, click on Mirror. Click on Mirror Face or Plane, I'm going to choose this plane over here, and then by default, it normally choose features mirror, but in this case here, I want to use bodies to mirror, bodies. I want everything here. I don't want just one of those features. I don't want just that hole or that tab. I want everything that went into creating that whole body right there. I choose the body, click OK, mirror that over, and then do the exact same thing over here on the bottom.

Features, Mirror. If you get a warning like this, don't worry about it, just click OK. Make sure you're choosing, not a feature but a body. Choose that body and click OK. So there that is and click on Save and then come back to our assembly, which is here. Just click Okay, because there's a couple of little issues that we're looking at, saying, hey, there's an issue with that sketch. Let's go see what that is. Jump over here, look at the sketch. It's saying, well hey, that point we connected to earlier is no longer there.

Sometimes you run into issues like this when you're working with in-context; especially when you using mirror commands. They're generally really easy to fix, just click on that point there, get rid of that, because that was an end point, and now it's not; now it's an mid point, no big deal, exit out of that. And we're already editing this part here, so go head up to Features > Mirror, select this face, bodies to mirror that entire thing, okay? And then, again, choose this face right here, Mirror.

Bodies to mirror, let's use that entire thing. Click OK. Go back over here, see what's going on here. Again, that's causing a little bit of issue, so you want to make sure that nothing's really wrong here. Click on that one down there. That looks like it's maybe causing the problem. Let's go back and look at that again. This is basic problem solving you're going to have to do, generally when you're working in these kind of designs, and it just happened to, maybe have a little of an issue, but we want to make sure we're snapping right to the origin. And might just have to snap it a couple of times, turns black, exit out, and we're looking pretty good.

Okay, that's the covering conduct. So we're going to come back and continue on with that cover in the next couple movies and build it a little further, but that's the basic cover, and that's the basic shape of our enclosure. By designing parts that always fit together, we eliminate many of the issues in repetitive work associated with part changes. And by the way, there's always going to be changes. Utilize this power of in-context modeling. It will really pay off in the long run.

There are currently no FAQs about Sheet Metal with SOLIDWORKS: Enclosure Design Project.

 
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