Learn about adding a strengthen rib across a bend in SOLIDWORKS.
- [Instructor] In this example, I'm gonna be showing you how to create a rib across a sheet metal bend. Now you can see here we have this little gusset that's been added to the sheet metal part, and that is created with a special form tool. So over here is the tool itself that creates that little rib. So how do we create this? So first things first, let's go ahead and create a new file which is exactly like this one here. So I'm gonna go ahead and start a new document, click on OK, and let's start a sketch. So I'm gonna choose the right plane, and let's go ahead and just draw a line starting at the origin and going up, over, down, back, and basically creating a little L shape.
Here it is. Let's make this line and this line over here both equal. Let's make this line here and this line here also equal. And add a couple dimensions here. So I wanna make this 1.25 and this one up here .125. All right, now let's do a feature, extrude. I wanna make this a midplane extrude, and I'm gonna make it one inch wide. All right, now let's use that same right plane which is in the middle of the part, start a sketch, and grabbing my line command, let's go ahead and just make a diagonal line here.
Snap back to the origin. Let's go ahead and make this line here and this line here equal. And then add one dimension here for one inch. All right, features, extrude. Let's make this one also a midplane, and .25 extrude. All right, so now we have the start of our gusset. I'd like to add a fillet, but instead of a regular fillet, I'd like to make a full round fillet. So my first face is gonna be this one, my second face is gonna be that one, and my third face is gonna be this guy over here.
Click OK and we've got a full round fillet. Now we need a couple more fillets. Now, this bottom fillet here needs to match what's on the outside of my sheet metal part. So let's head back over to my part itself and spin this thing around and take a look at this outside edge. So I'm gonna grab the measure tool and measure this outside edge. You can see it's .125, so that's exactly what we wanna put on the outside of my tool. So back to the tool. Here he is. Features, fillet, irregular fillet.
I'll make it .125 and grab these two inside corners here. Click OK. Now, as a separate feature, I wanna make the fillet around the outside, as well. I'm gonna choose this one here, keep it 1.25, and now we've got the tool exactly how we want it, but now we have to convert this into a sheet metal forming tool. So right up here is forming tool. My stopping face is gonna be this one right here. The faces to remove, I wanna remove everything else that is not the forming tool itself. So click on this face here, this one here, this guy over here, this front face, this guy, top, back, the bottom and the side.
All right, so we got everything else besides what's actually gonna form that little gusset, and my insertion point, I'm gonna go ahead and click on this one here. Right over here is the insertion point, and I like to actually put that at the origin here, so sometimes you have to get rid of this little relationship and then just drag that over here to the origin so it's right on the edge of the part and click OK, and now we've got ourselves a forming tool. All we need to do now is save this to the library. To do that, go over here to the library, come over under forming tools, ribs, and click on the little add to library plus.
We wanna choose this entire part, which is right here, and we wanna add that to the library, all right? So we wanna add it into ribs, and we can call it rib2. Click OK. Before we do that, we have to make sure we save our file, so let's go back. Go back, File, Save As. Let's go ahead and overwrite the existing tool, but we have it open. So right here is our existing tool. Let's close that down. Come over here, File, Save As. Let's overwrite the tool. You can name it something else if you'd like to, as well, but for right now, let's just overwrite it, replace that tool, and now we can add it to the library.
So go back over here to the library. Grab that entire tool. We can call it rib2. Click OK. And now it's in the library. All right, now let's go ahead and place that on our sheet metal part. So here's our sheet metal part. It already has that gusset. Let's get rid of that gusset for right now. So delete that out. All right, and let's go ahead and re-add that in with our new gusset. So over here under the library, here's our new rib2, and I wanna place it on this bottom surface, so drag and drop and place it over here.
Notice it's on the bottom surface but it's going the wrong direction. So let's change that 180. So I'm spinning it around, all right? And now let's go ahead and position that. So I wanna position it on my part, and I want this point right here to be right on the edge. Click OK. And now we've added that gusset right there to the corner going across that bend in my sheet metal part. So you can see it's a lotta work to get the original tool designed and built correctly, but once you have it, it's pretty easy just to drag it into your sheet metal piece and add that gusset to the sheet metal part quickly and easily.
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