Join Gabriel Corbett for an in-depth discussion in this video Using the Jog feature, part of SOLIDWORKS: Sheet Metal Design.
A Jog feature is an offset in sheet metal. The most common use of this feature is to create an overlap of two parts or two edges. In this case here, I've got a formed sheet metal piece that have two edges that are kind of butting up against each other with a gap. What I want to do is add an offset that goes underneath this other flange, and then maybe extend this flange so, it covers. To do so, what I need to do is start a sketch on this top plane. Let's go ahead and click on Sketch, and click on Line. And this is a regular line, not a center line. Click on Spacebar, so, I'm looking straight down on that face.
And I'm going to make a line just across that part. And it just happened to be snapping across the origin, so, it defines where that's located. When you're happy with your sketch, go ahead and hit Escape, and then jump over here into the Sheet Metal tab and come up here to Jog. The first question is, which face is going to be fixed? In this case here, it's going to be this one. And as soon as I do that, I get a preview of what's going to be created. You can see that's way too big and going the wrong direction. So, we gotta fix this thing up a little bit. Number one is my offset distance. I really don't want is an offset that is just one material thickness. So, I type in 0.063.
You could see, it's looking better, but now it's still the wrong side. So, let's go ahead and flip the direction. So, it's on the inside. And actually when I am doing an offset, I ran into a little bit an issue because what happens is, there's two bends that actually create this offset. And they actually run into each other right here in this plane. So, at 90 degrees, it's to big of a bend to actually complete this offset. So, what I want to do is I want to start changing that angle to a smaller angle, so, you can see that flange starts moving up, up, up, up into the other flange.
And right about 60 degrees is the sweet spot. In fact, it goes a little bit past. So, 61 degrees will just give us a little gap right between the two faces, so, you have a nice flange with a nice overlap and nothing interferes. And while we're at it, because the two faces are actually touching, these two bends are touching, we can change this from 0.063 offset really to a 0.00 offset. And that'll be just fine. When you're happy with it, go ahead and click on OK. And you can see there's my flange, my offset looks good. Now, what we need to do is extend this face here so, it covers over the top of the offset. To do so, I'm going to click on that top face.
I'm going to start sketch and click on the Spacebar, look down straight on that part, and come up here to the Corner Rectangle tool. I'm going to click right on the edge, I'm going to snap there, and I'm going to snap right here to the beginning of that bend. I don't need any other dimensions there, because I'm snapping to two points. And that looks pretty good. Come over to Sheet Metal, use the Base FlangeTab tool, which is going to extend that face using a tab, click on OK. All the defaults are preset, because we're extending an existing Sheet Metal feature. Click on OK, and there we have it.
We have a nice overlap between the two parts. They're actually not touching, there's a small gap between the two. This perfect for spot welding. And if we wanted to, we could add some through holes. If we wanted to put some bolts or screws through there or rivets. We could use counter sunk screws if we need the two keep a nice flat surface. And we can put PEM fasteners or something like that on the backside to connect the two faces together. We're now going to jump over to 2.8.2, which is a flat plate. And it's going to demonstrate one more basic jog. If I click on the Jog feature from the beginning, it asks me for a planer face to sketch bend on. In this case here, I'm going to choose the top face, and it automatically puts me in the Sketch mode.
I'm going to choose the Regular Lline command, hit the Spacebar. So, I'm looking down at that, and I'm going to create a line from the inside of the part all the way to the other. Then I'm going to come up here hitting Escape to get out of that command. Grab the Dimension tool. Dimension from the line to the edge of the part. And in this case, I'm going to say 1.0, Enter. And that fully defines the line. Notice, it's black, fully defined, no other issues. And we're ready to create our jog. Go up here to Jog. And my fix face is going to be that same flat face, and they can see that there's my representation of the jog.
It's going to be a little preview of it. And I can change the size or height. And this time here, I'm going to make it a one inch jog. Instead of 60 degrees, let's go ahead and make it 90 degrees. And let's also look at the flange position here. You can see that it extends all the way out to the edge of the part. Notice that the part was this long and it still is this long. What that does is it adds a material to this jog to make sure it's the same length. That's controlled by this button here, Fix Projection Length. If I turn that off, notice that it sucks it way back, and it just takes up the existing material and makes the jog with it.
This is really handy though, because it always will add the correct amount of material to continue that part to the end. I can also play with the position of the jog. I can use the bend center line, I can use the material inside, material outside, or bend outside. Just to move that flange position around different places, depending on how I have that line defined originally and where I want that Jog feature to actually end up. When you're happy with all the features, I'm going to go back to the bend center line one, spin it around, and go ahead and click on the green check mark to finish the feature.
The jog feature is really a combination of two edge flanges, and some added features that control the length of the resulting flange. Jogs are great for creating off sets or strengthening edges.
- 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