Sheet Metal with SolidWorks: Enclosure Design Project
Illustration by Richard Downs

Adding part drawings


Sheet Metal with SolidWorks: Enclosure Design Project

with Gabriel Corbett

Video: Adding part drawings

Now we have our top level assembly drawing complete. I'm going to choose the lynda template, click OK.

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Watch the Online Video Course Sheet Metal with SolidWorks: Enclosure Design Project
2h 31m Intermediate May 21, 2014

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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.

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
Gabriel Corbett

Adding part drawings

Now we have our top level assembly drawing complete. We now want to make drawings for our sub assemblies and individual parts. Now what I've done here is I've taken the assembly we had before, I rearranged it slightly, and I added the PEM standoff that we had individually in this assembly into a sub assembly, and I've rearranged it just slightly as you're talking about in the last movie. Now, I've added the cover, I finished off adding the descriptions, and now we're really ready to open up the individual sub assemblies and start making the drives from them.

I can do that directly from the build materials here which makes it really easy, so you notice I have this base assembly, which is the one I just created. I can right-click on it, and click on Open that assembly. And you can see it's just the base part here, with those four pieces of PEM hardware added into it. Now to create the assembly drawing, again come up here to File > Make Drawing from Assembly. I'm going to choose the lynda template, click OK. And bring in a view. So I'm going to bring in this Right view. It's my first view. Come up here with the top of it, and then I get another view over here, or actually just, probably just an isometric view.

Again it's bringing in some of the center lines and center marks. That's a default inside of the template and it works really great for some reasons and sometimes it doesn't. So depending on what kind of part you're making it can actually add some work, or if you have a lot of holes and you want to add center marks it's pretty great. So I have my Selection Bar turned on here, I'm going to turn on center marks and center lines, I'm just going to bring that around all those and delete them out, because I don't want them in the views here. Now, I'm going to go ahead and, and add the bill materials, so I'm going to say Insert > Tables > Bill Materials.

And turn my Selection Filter off, choose this view here, and chop top level's fine, and just bring that in. Now this bill of materials has the base, as well as that PEM standoff. I can adjust the size a little bit, I can rearrange, or change the height of the different rows, so it looks pretty uniform. And go from there. Now, I could make a separate drawing here of this base in a separate file, or I could add a sheet to my existing drawing here, and just add that data.

So a lot of times what I'll do, if I have a part which just has some pieces of hardware like a PEM pressed into it, and is not really a full assembly, it's just some additional hardware added on. I'll just add that drawing as a second sheet, so you don't have these multiple drawings and assemblies that are just assemblies of hardware, so it just kind of keeps things a little more compact and allows it to have its own file name. But it's just page two of top level assembly. So in this case here we'd just call out the different items using Annotation, so we'll go to Balloon, I would balloon out this item here, and zoom in here, and click on that PEM, and balloon those two out.

Then come down here to the bottom, click on Add Sheet. And for this one I want to make sure I got the file open, so I'm going to come down here to the assembly, and I'm going to open this part here. So, File > Open Part. There it is. Come back to that sheet, Sheet 2, go to View Layout > Model View, and make sure I'm picking that part, which is 6.2-1. Now, I could browse for it here, as another way to open it up. But, I prefer to just have it open. Click on that, and click on Next.

Click on Preview, and it'll show you which available views we have to bring this in at. And I could bring it in as isometric, or I can pick you know, just which one of these views is going to work out great. This one works pretty good for this situation. And I give you this dimension here and that one there. Okay, that looks pretty good, and I can give you this isometric. Again, sometimes we might want to have the center lines and center marks, unless we don't. In this view here looks great, but this one over here doesn't, so I'm going to turn Selection Filter on, and select out those for that one, get rid of them.

And down here I'll select those out and just in the bottom section, I'll leave it for the top. And turn that off. There's a couple of other little center lines here that I'm going to get rid of as well. Okay, now let's start doing some dimensioning. For the dimensioning, for most sheet metal parts, because there's so many little things in there, I find the best way to dimension those is under Smart Dimension. We're going to use either the Horizontal or Vertical Ordinate Dimension. So click on Horizontal. I'm going to choose this first edge over here on the left as my first dimension here.

And then I'm just start clicking on items that I want in my ordinate dimension. And you can see it was going across the part here. Now you notice I'm choosing the ones in the lower face here, you can also choose the ones on the upper. Right, so you pick one up here and trick goes right through both of them, so either way you want to do that. Again, pick up here. If you do pick the far one, it kind of hits them both at the same time. If you do it like this, you have the option to go back and add like a center line, showing that these two items are in line.

Do the same thing over here. So two different ways to do it depending on your preference there. And then same thing with the vertical. I'm going to choose this quantum face here, it's my 00 point, and I'm just going to click, click away and just add these items, to the order dimension going up. And looks like those are pretty close. Click there, click there, OK, looking pretty good. So, you hit Escape to close out the command and it'll auto drag it to the location you want. And you're going to come back under Indentation, you're going to say Smart Dimension, and we'll do some of these holes.

Right, so I can dimension amount in. When you dimension something like this it's only given me one of those holes. So you can also, as another option, you can go to Hole Callout, and that will give you a little bit more detail in that hole, especially if you're using a counter-sunk or counter-bored hole. I would definitely recommend using the Hole Callout versus just the regular dimension here. But either way you go, a great way to go to these, here I'm going to go back to the Hole Callout, callout those, and then you can come over here to the Dimension Text, and you can specify how many of those there are.

So in this case here, I've got four of those, so I'm going to say four and if you get a little warning here that says you're manually changing this, that's okay, just go ahead and click OK here, and click on Yes. I'm going to say 4x. I'll make it a small x. So 4x quarter inch. Looks good. Same thing over here. This ones four of those. So I'm going to say 4x. And, we're good to go there. I'll continue on here with it. Some more dimensions here. One thing I want to point out is I want to make sure I keep using the same location.

So in this case here I've got 0 0 on this lower quadrant here. So that's going to be this lower quadrant right here. And we want to choose one quadrant or one part of our design that's going to be our origin. And follow that through every one of our different views. And make sure always using that same quadrant. So again, so this is 0 here, would be in this corner here. So our 0 would start on this point and go that way, not that other way around. Just keep that in mind. And so, I'm going to wrap this one up as far as this view here, but I also want to jump back to going over it to the assembly here.

And look at it's drawing view which is the top level. Now when I go with something else like a part, with like the circuit board or the cover, I'm going to go back and do the exact same thing. I'm going to make a assembly drawing and then make sheet two of it. The drawing of the individual part, and this, they'll have a basic cover. Things like screws, circuit boards, RJ-45s, those are already existing parts, so in those ones we're just going to have a build materials calling out a reference drawing showing the screw maybe with a drawing that we got from McMaster-Carr or something like that.

Same thing with the circuit board. If it's not the shelf part, we're just going to say who the vendor is, what the part number is and how to buy it. So that's all going to go into that pillow materials, we can put all that together. We have one nice package, easy to work with and easy to build the parts or buy the parts as needed to complete your design.

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