Join Gabriel Corbett for an in-depth discussion in this video Building the rough enclosure shape, part of Sheet Metal with SOLIDWORKS: Enclosure Design Project.
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Before we get start building the enclosure, let's take a look at the final project. You can see here I've got a sheet metal enclosure that has a base and a cover. The cover's in green the base is dark gray or black. And you can see I can spin this thing around now. We're missing some of the hardware and we haven't added in kind of pims or the circuit board inside here, but this is just the basic enclosure shape and how we can design it. Now what makes this enclosure a little bit special is I have the ability to actually change this all based on equations. So what I can so is I can click on this part here, click on edit part, come over here to the equations.
And you can see I've got a few equations already set up here, so. W for width, h for height, l for length and then I got a couple of other variables that are based upon that or things like radius over here, foot width, tab width. Anyways, I can change any of these values I want, so up here; let's go ahead and change the width. Instead of being 6, let's go ahead and make it 3. And then instead of the length being 8, it's going to make that four, 'Kay, click OK. Go head and continue here. You can see the entire closure automatically changes sizes and scales, and beyond that notice the amount of little vent holes in the size actually.
Adjusted as well. So it's very powerful enclosure here. And if you design enclosure like this from the beginning, then you can kind of reuse that same shape and design multiple times over. And that is kind of the situation we are in right now, because you can see there's no holes for special deconnectors or anything like that. it's really just a basic enclosure that you can use for any number of projects. And I can scale and change the size of it as freely as I want. Now let's go back and change those values back again. Go back over here to collision values, click into here, let's type in six and this one here let's type in back in eight.
It's going to expand back out, there it is, okay. Now we're ready to get started so go ahead and close this down. Now I'm going to jump over to a basic sketch that I have open up already. And you can see here this is on the right plane. And I just have a couple lines laid out. And that's going to be the basis for our enclosure. Now I also like to sometimes just add a couple center lines into this design. Just to make sure and kind of visual the shape we're working with. Now, let's go ahead and add a couple dimensions. Now I could dimension from this side to this side, but I know that I'm going to be using some symmetry in my design, so I want to mirror these over, so really I'm only going to design one quarter of this enclosure and then use the Mirror command to build the full enclosure.
So in this case, I'm going to make use of the Double Dimensioning command. Click over here. And then click on this center line. It only works on center lines but as soon as I go past that center line, you can see that dimension doubles. That's exactly what I want. And over here I can type in that value. Now remember we just looked at the value and was six inches. Now I could easily type in six inches or in this case here, I could just click on the equals sign and then give it a value. So in this case here I'm going to say equal to w. Click OK and do you want to create a new global variable called W and i guess we do.
Now type in 6 inches and we have assigned that six inch value to the global variable W. Click OK then you could see there is little sigma in front of the six showing that equation driven then you are going do the same thing with the height. In this case here, I'm just going to say "equals H" and instead of clicking on enter, I can just click on this little global variable icon here, turn that into a variable, and then click in "1 inch." There it is. Okay. Now, all the lines are fully defined. Now I'm ready to create my base flange. So go over here to sheet metal, and click on base flange tab.
You can see I can drag that value out, if I need to. And of course, in here, we can also put in a value. In this case here, I'm going to say equals. Now, I could link to a global variable. We already have a couple. Or I can create my own. Now, this value here happens to be only half of the length of the enclosure. So we can say this is going to be, maybe. L, length half. Click on the icon, and this case here, we're going to say this is equal to 4. Now, we're going to go back and adjust that later, but in this case, we should be good to go.
So, there's four inches. That's the start of our enclosure. Now, notice, the origin is right there in the center of the design. And, I'm going to go up here to view and make sure I'm showing my origin, so I can keep track of where that origin is. Throughout my design. Now, let's continue on here and let's add a couple taps. So, I'm going to click on the top, go ahead and come over to sketch, start a sketch, I'm going to use a couple basic tools. First one is going to be the rectangle tool, click on the bottom corner here, just bring that up; click and then what I want to do is, because I'm going to want to add a lot of dimensions that aren't needed.
I just want to grab this point here and drag that up to that corner, and just snap that on there. Notice that turned black. Its fully defined. Now all we need here is just the length from here to here to def, fully define that rectangle. Let's go ahead and add a dimension from here to there, and in this case here, I'm going to call it tab width. So I'm going to say equals tab W. Set up the global variable and then give it a value .625. Okay. Looks good. And let's go ahead up to sheet metal.
Base flange tab. Just going to add that to our design. Great. Now a couple other thing we're going to need to do. We're going to add some radiuses. First, let's go up to features. Click on fill it. And in this case here, for the fill it variable. Let's go ahead and click on equals, and I'm going to say R. I'm going to create that variable and I'm going to say it's going to be 0.375. Great, click on this edge here, and this edge up here. Click OK. Great. Now, I've got these two edges filletted and they're looking pretty good. Anytime you want to go back and take a look at your variables, you can go right here to the equations or over here on the right you can always say right-click and say manage equations.
That's going to open up everything we've created so far. It also gives you the opportunity to create some equations ahead of time if you know you're going to use them. When you're happy with what you have, click okay. Now let's jump back over here. Start a sketch. And in this case, I'm going to go and start a sketch right on that corner right, because I want to make sure that's where that material's going to be coming down. Bring that down to this corner. And let's go grab a rectangle tool, so grab the rectangle. Start on that corner here, and I want us to create a little pole in the sheet metal, cause what I want to do is create a little tongue or a tab on the cover that's going to fit in to this hole, that's going to allow us to not use as many pieces of hardware.
The width of this; let's go ahead and define a width. Now anytime you're working with sheet metal, there's a few variables that are already pre-defined. So I'm going to say this is equal to global variable, there's always one called thickness; if you choose, if you're working inside of sheet metal. Choose thickness and then I'll just add a little bit to it, so thickness plus .020. So 20,000th of extra material above and beyond the thickness, and that's totally fine to build an equation right in the input bar. Click on enter. Now how about the width. Again let's add ourselves a center line so I can use that double dimensioning tool.
Come back up here. Click on this line here to that line there. And I know that my tongue width wants to be three quarters of an inch wide. So I'm going to say .75. Plus, and I probably want about 20,000 to either side, so I can say 0.02 plus 0.02 or I could have 0.040. The point is I want to illustrate here is you can use this as kind of a little bit of a calculator when you're building that. When you're happy with it, click OK. And it just does that math for you. Now, that math wasn't really that hard.
But sometimes, you're working on very complicated equations. And it's a real time saver to be able to type that right into the input bar and have it calculated out for you. Let's also add the hole in the corner. So, we want to have a hole that's going to be able to. Screw this enclosure down to the table or wall or wherever you'll be mounting it to, and let's go ahead and add that in right now. Now dimensioning, we can dimension things from the center line for some cases, but other times we want to dimension things from the outside edge. In this case here, we might be changing the size of that enclosure, so I want to make sure that I'm tying this in to the outside edge.
In this case, let's make it half-inch. And from our hole to the edge, let's make it 0.3, and then our hole diameter is going to be 0.25. That my change, so instead let's go ahead and change it and create a variable. So we'll call it Hole. And then we'll assign that variable 0.25. There it is, and let's go ahead and do a cut, so Features > Extruded Cut, and let's link to thickness, so it just cuts all the way through that sheet metal.
Click OK. Alright, we're looking pretty good here. Now, it's time to jump over and start working on the cover. Then we'll build an assembly and we can continue on developing both the parts at the same time in an in context assembly.
- 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