Join Gabriel Corbett for an in-depth discussion in this video Looking at the Flange tool, part of Sheet Metal Design with SOLIDWORKS.
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The Flange tool is the same tool that we chose before to start a base, however this time we leave the sketch open. Instead of generating a flat part that's ready to add bends to, we start with a flange that's already bent. When laying out a sketch don't worry about adding in bend radiuses. The software will allow us to add these in later, so just start with a basic shape with hard corners. To get started, we need to start a sketch, and this time I'm going to choose a sketch from up here and I'm going to choose the top plane. From the top plane, it spins around so i'm looking straight at it and I'm good to go. This time I'm going to start with the line command.
And I'm a start right at the origin. Draw a line out to the right. And the length doesn't really matter in this case. I'm going to go about 4 inches. Click and go up, let's say about 2 inches and go over to the right. I'll say about 0.75 and the number doesn't exactly have to be correct. Just get, roughly there. When you're done, go ahead and just hit Escape, or you can continue adding more lines and more flanges as you go around. I'm going to hit Escape, takes me out of that tool, and I'm ready to create a flange. Let's go up to Sheet Metal, click on the tab, and click on Base Flange tab.
As soon as you do that, it spins it around 3-D and gives me a little representation of what's going to happen. I can click on this arrow here and drag it up or drag it down, your choice, and it gives you a little heads up display of how long that flange is going to be. I have it about 2 inches, click OK, and I can spin that around in 3-D, see what it's going to look like. And notice, even though I drew hard corners, or sharp corners, it actually adds in a bend radius, and that's determined by the Base Flange tab dialog box. So, under Direction 1, it's asking me how far do I want to go and what conditions.
So I have the 2 inches in there, and it's doing a blind condition, which means whatever value I want to type in is exactly how far we can go. We also have options for up to vertex, up to surface, offset from surface and mid-plane as well. Direction 2 allows me to create that same flange, go in the opposite direction, and same thing. I can type in a distance, and you can see that flange gets longer in that direction as well, but in this case here, I was just going to use the Direction 1 and come down here. I have the option to choose the thickness of the sheet metal, the bend radius, in this case here I'm going to type in 0.030, which is a very standard bend radius.
And I can choose the direction of where I want to have my flange. Notice if I zoom in here, that sketch is actually on the inside of that bend flange. If I click on this check box it swaps. It puts the entire sheet metal flange on the inside of the sketch, versus on the outside of the sketch. So you can switch between the two, depending on what type of design you're making. We cover this in the last movie a little bit, as far as the bend allowance and the K-Factors. K-Factor's great to start with, but it's not going to give you the correct size flat pattern. I always recommend using the bend deduction in getting that value from your sheet metal supplier.
But in this case here, we'll keep it as K-Factor, because K-Factor will always work. When you're happy with what your flange will look like. Go ahead and click on OK. And there you go, our first flange. And looks pretty good. Let me go ahead and turn off the shadows so we don't see that. And, we don't need the RealView graphics either. Those are nice for when you want to look at something that's real fancy on your screen and you want to maybe do a screen capture or something like that. But, in reality, those two features actually add some overhead to the computer and slow it down, so I generally turn them off when I'm working on sheet metal parts because things can get pretty complicated and you don't want to slow the computer down unnecessarily. Once you've created a flange, we can continue on here, or we can go back to that flange and modify it.
To change this flange, notice, I've got a feature called Base Flange 1. Now, if you've created several flanges, or if you've erased and started again, this could be Base Flange 2, 3, 4, doesn't really matter, as long as there's a base flange, you can click on the little plus next to it, expand it out, and you can see, there's the sketch. Sketch one that created that flange. And then here are the two bins used to actually bend that flange. And I can edit each one of these individually, if I needed to, to adjust the K factor, to adjust the bend deduction or any of the other features inside of there.
If I want to change the sketch, go ahead and click on Sketch 1, and notice this little pop-up window shows up. We choose that very first icon called Edit Sketch. I hit the space bar, that will bring up all the orientations available, I'm going to click on this one here called Normal To. So I'm looking straight at it and I can continue to add on, so I can make a bend this way, maybe one over to here. When you're done, hit Escape and I notice I can use any of the basic tools up here like lines and arcs to create the shape. But one condition though, is it needs to stay an open boundary and it cannot intersect itself. When you're happy with your shape, go ahead and exit out of the sketch. And, those extra bends will be added to your feature. If used correctly, and you can think about your design ahead of time, the flange tool can make your job much easier.
Any number of bends can be incorporated into one feature. However, simplicity is your friend. And remember, each bend adds cost and complexity.
- Understanding sheet metal fundamentals
- Creating base features
- Creating flanges and tabs
- Making hems and corner features
- Unfolding and folding parts
- Adding cuts across bends
- Adding welded corners
- Using the Forming tools
- Importing geometry
- Using the Convert to Sheet Metal command
- Making sheet metal drawings
- Exporting DWG and DXF files for laser cutting
- Building an assembly
- Creating parts in an assembly
- Creating flat patterns
- Using in-context design techniques
- Exporting parts