Learn about adding in blank parts to an assembly and building complex assemblies from them.
- [Instructor] One of the best ways to build sheet metal assemblies is to create parts inside of the assembly. And we have a couple different ways we can do that. The first is to come up here to Assembly, Insert Components, and click on New Part. And what this will do is it'll create a new part in the assembly and that'll be a virtual part contained 100% inside of the assembly, and you can then save that up to the file system, but I actually prefer not to do it that way. What I'd like to do is actually create an individual part and then we'll bring that into the assembly. So to do that, come up here and click on New document, click on Part, click on OK.
Let's go ahead and File, Save As, and I'm gonna save that as 7.3.3, and save it in the chapter seven, 7.3 folder, click on Save, and now we have a blank part. Now this part does have three planes as well as an origin and that's all we need to do to bring that into the assembly. So click on Window, Tile Horizontally. You can see here's my assembly and here's my new blank part, and let's go ahead and just drag that directly into my assembly. Click on expand out, and now you can see here is that part even though you can't see anything 'cause it's a blank part, but I can still mate it together.
So down here I've got an origin of that part and I have an origin of the assembly. So go ahead and hold down Ctrl, select the origin of the assembly as well as the part, and click on Mate. Right and notice those slide together, and right over here we have this option for Align axes, and if you have that checked, that will automatically align all the axes and with one small mate, everything comes together. Click on OK, and now it's fully mated. All right, now we can start modifying that part in context. So you might want to actually close down the individual part, which is this one here, so just exit out of that one.
And now we have this part, here it is at the bottom. Let's go ahead and start modifying. So right over here, click on Edit Part. So now we're in the edit mode for that blank part, and we're gonna go ahead and create it. And I wanna choose the front plane, right, because we've already aligned those components, right there, that front plane is exactly where we need it, and start a sketch on that front plane. Here's my sketch, and let's start with the line command. Now I'm gonna spin this around so I'm looking at it normal, and I want to start with a center line actually, right at the origin. Bring that line all the way up to the top, and snap it there, then grab the line tool, and let's go ahead over here to this first point.
Then let's go ahead and create this arc. Let's see if we can't snap to this little corner here, and then come all the way down to right where it hits that top piece of sheet metal, right? So that is my line. Now notice there's no dimensions. I'm making a 100%, in-context relationships to the existing geometry so if this changes, all the parts will automatically update. At least this cover will update based upon the shape of these lines linked to the edges of the base sheet metal, all right? So now let's go ahead and create a feature, actually a sheet metal feature, so it's a Base Flange/Tab.
And how far do I wanna bring this out? Well, I wanna bring it all the way out to the front face here. So instead of saying Blind, I'd like to say Up To Surface. And the surface I want to choose is this front face. That way if the chassis gets deeper, my cover automatically gets deeper as well. All right? Everything else should be the same. Make sure that a material we're creating is on the outside of this, not on the inside, and the thickness is correct. In this case, I'm gonna make it 40-thousandths material just to match the base. The K-Factor and everything else is fine. Click OK, and there is a portion of our cover.
Now we're gonna use the mirror tool to mirror this over to the other side over here as well as to the other side on the back, but before we do that, let's make a couple other modifications to this piece of sheet metal. So click on this front face here. Start a sketch, and let's make a little tab. So I'm gonna start right at the origin. I'm gonna drag this down and snap to the bottom of the chassis. Then let's grab the Smart Dimension tool. Dimension from here, over to here, and give it about a 20-thousandths gap. All right, come back up here to Sheet Metal, and create a little tab. Click OK, and we've added that little tab so it sticks down in this little slot.
And maybe we'll radius one of the corners, so back over to Features, grab the Fillet command. 100-thousandths looks good, and let's fill up this little corner. All right, that looks pretty good. Now of course you can continue on adding holes or connections, but right now I just wanna illustrate how you can create a part in context, so let's go ahead and mirror this component over now. So click on Mirror. Now instead of using a traditional feature mirror, we want to actually mirror an entire body, so instead of the feature, which I don't want this one here, so get rid of that, come down here to Bodies to Mirror, and I wanna choose that entire body.
That brings all of those individual features over all with the one body. Click OK, and now let's do it one more time. So grab Mirror, and I didn't want to mirror that feature anyways, so that's okay, so click over here, Bodies to Mirror, I wanna choose the entire body, click OK, and now I have a full cover. All right, and now I can exit out of editing that part back into the assembly, and now you can see here we've got this nice in-context cover built within that assembly. Now let's go ahead and try to modify the base and see if that cover will follow along.
So open up this part right here. Now this part is controlled by equations, so if you click over here, I can say Manage Equations, and the width is three, let's go ahead and change that to four, and the height is 1.1, and let's go ahead and change that to three inches. All right? Click OK. This part automatically updates based upon those equations. Pretty handy. Let's head back over to the assembly, click on rebuild. Hey, look at that, awesome. So the cover automatically grew based upon the base of this assembly.
Everything works, and it's 100% in-context, so it's a really great way to design anything in sheet metal because you're basing everything on that one individual part, which is the base, and the cover, and the board, and the cutouts, and everything will follow and track everything based upon that, so it makes it really robust if you're making modifications to your design, everything will automatically track, and it will be a very clean design in Solidworks sheet metal.
First, review the sheet metal tools in SOLIDWORKS and the properties that make sheet metal unique: bend radius, K-factor, bend deduction, gauge thickness, and more. Then learn how to create basic parts, with base features, flanges, and bends that add strength and connections. Find out how to flatten parts and add holes, cuts, and corners that are manufacturing ready, and use the Convert to Sheet Metal command to convert imported geometry into native sheet metal parts. Gabriel also shows you how to create assemblies from multiple parts, use the Pattern and Mirrors tools to effortlessly duplicate existing work, and then document your designs with detailed sheet metal drawings. Watch the bonus videos to learn about the different machinery and processes that occur during manufacturing.
- Sheet metal tools in SOLIDWORKS
- Sheet metal manufacturing: Laser cutting, CNC machining, welding, and more
- Creating base features
- Creating flanges and tabs
- Making cuts and corners
- Using the Convert to Sheet Metal command
- Building multi-body parts
- Creating forming tools
- Forming across a bend
- Building an assembly
- Creating parts in an assembly
- Creating sheet metal drawings