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Adding vents to the design


From:

Sheet Metal with SOLIDWORKS: Enclosure Design Project

with Gabriel Corbett

Video: Adding vents to the design

It's now time to add the vents to the design. I want to open up just the cover piece. So, you can see here, we have the sub-assembly here, and assigned to that sub-assembly is this part, which is the cover. Go ahead and click on Open Part, and there's just the cover piece. Now, what I want to do is just add the vents along this edge, here, but I want to roll it back prior to those two Mirror commands, so I'm only seeing this one quarter, so we get the benefit of using that Mirror command and using the Mirror Body, which is going to propagate those events to all four sides.
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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

Adding vents to the design

It's now time to add the vents to the design. I want to open up just the cover piece. So, you can see here, we have the sub-assembly here, and assigned to that sub-assembly is this part, which is the cover. Go ahead and click on Open Part, and there's just the cover piece. Now, what I want to do is just add the vents along this edge, here, but I want to roll it back prior to those two Mirror commands, so I'm only seeing this one quarter, so we get the benefit of using that Mirror command and using the Mirror Body, which is going to propagate those events to all four sides.

Starting at the top, start a sketch. And, I want to draw a rectangle, which is going to be my vent hole. And, my vent is going to be roughly down here. We'll make it a little bit over-sized at first. I'm going to click on this edge here, and I'm going to click on this edge here. I'm going to make those two co-linear. And then, I want to make sure that this vent's kind of on-center. So, I'm going to add a point to the center point of this line, here, and I'm going to drag that point and snap it right to the edge of the enclosure. Add a couple of dimensions. I'm going to type in 0.1 for the width of the vent and 0.65 for the length of the vent.

Go over to Features, click on Extrude Cut. Now, I want to extrude this into the material. 0.65 is the correct value, but if it wasn't, I could automatically change that. Click OK, and it cuts it into the material. Now, take that same cut, and we're going to pattern it across the part, so we don't have to keep doing that work. Click on Linear Pattern. As far as the direction, let's go ahead and select this edge, here, but any edge going in the correct direction would work just fine. You could use this edge here, or this edge down here, doesn't really matter.

And then, our Features to Pattern is going to be that cut we just added. And, this is going in the wrong direction, so let's go ahead and flip that over, so it's going the correct direction. My spacing wants to be quarter inch and I want 11 instances of that cut. Click OK, and there they are. Roll this thing back forward, and you can see it automatically propagates all the way through because we're using that Body to Mirror command. And, there we have it. Now, if we want to take this to the next level, we can set it up so we have an equation that actually determines how many of these vents there are, based upon the size of the enclosure.

To do that, I need to start with a little sketch. Again, let's roll this back, before the Mirror command. Click on this face, here. Start that sketch. And, I'm just going to use the center line. Start at the origin, and bring that out to the edge. Go ahead and add a dimension on that. And, SolidWorks is asking us, do we want to make this a driven dimension, and we do because this length is actually determined from the assembly and built upon the base part. So, click OK. Now, come over here to Equations, and we want to start building a couple equations. So, click on Add > New Variable.

In this one, I'm going to say it's spacing, and I'm going to make that equal to 0.25 inches. And, I'm going to make another variable directly below that called count. This time I'm going to make it equal to this value, here, which I'm just going to click in the window. Notice, I'm selecting that, so it's D1@sketch9 minus, I'm going to say, quarter inch. I really don't want to start these events right at the edge, I want a little spacing before the end of the part. So, that's going to subtract a little space before the edge of the part. That's going to be my quarter inch.

And then, I want to divide that. So, I'm going to make a little parentheses around this. Go back and add one to the front. I'm going to divide that by the spacing. So, here's the spacing, here. I can click here and just type in spacing. You can see, it adds the equation, it's saying I have 11.2 instances of that cut. Well, it's kind of hard to have a 0.2 of a whole, so we really want to like to round that number down. We can easily do that by adding an INT, making that an integer, and then adding the closed parentheses at the end.

And, by the way, there's a bunch of different features, or functions you can add when you're looking at things, just by selecting here from the drop-down. Take a look at those, they're pretty handy. Now, it equates to 11 exactly. Click on OK. Now, we have a couple different equations that we've added in here. We just need to go back and those to our design. Go to the Linear Pattern. Exit out of this sketch. Go back to that Linear Pattern. Click on Edit Feature. Now, up here where it says the 0.25 for spacing, instead of a hard number, let's go ahead and make that equal to, grab a global variable, and click on Spacing, and then as far as our count, again, click As Equal To > Global Variables, then come down here to count.

Click OK, and now it's equation driven, so if I change the size of the enclosure or the cover, the length will decrease, and the amount of holes we're going to put in there is going to decrease, as well. Adding vents and using equations is a great way to develop complicated design that can rapidly change and adapt as the design progresses.

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