Hi. In this short video, we're going to explore the capabilities of sheet metal within SOLIDWORKS or more specifically within the SOLIDWORKS online trial. If you want to follow along with this tutorial, you'll need to open up the complex sheet metal part five file from within the online trial. The easiest way to find this is probably by going to file and then checking the recent files, or picking browse recent documents and finding it from within there. If you can't see it immediately in either of those places, then just go ahead and go file open and browse to this location instead. Once you've got the part open, the first thing we'll do is to actually change the units to millimeters in the bottom right. And then we'll turn off the visibility of planes up at the top. Just to make the view a little bit clearer. Now to access the sheet metal commands, we'll need to turn on the sheet metal tab. When we can do this by right clicking on the command manager, locating tabs and selecting the option for sheet metal. The first feature will create is an edge flange. Select the edge flange command and then click and edge to start creating the edge flange, and then click a second time to define the direction and rough distance of the flange. Confirm the command and it'll be created, and I'll use the default bend radius that has already been set in this part. Sheet metal properties. Next, we'll define a custom profile for the flange. By editing the sketch that was created along with the edge flange. We can do this by expanding out the flange feature at the bottom of the tree, and then clicking and choosing to edit the sketch. Use spacebar to change the view, and then click the vertical relation and press delete to remove that. Remove the other relation here as well, and then just click and drag both of the edges inwards. And then use the centerline tool to add a horizontal centerline with one end attached to the origin. Deselect the centerline tool and then hold control and click the edges of the flange along with the centerline, and this should allow you to select all three at once. Once the selected, you should have the option to add a symmetric sketch relation, which will keep the edges symmetrical around the centerline. Now drag one of the corners inwards to angle the edges, and then just use the Smart Dimension tool to define the rest of the sketch. If you pause here, you can see the three dimensions that need to be added. Once you've completed that, leave the sketch and the flange shape will update. Following on from this, let's add another edge flange connected to our previous one for this edge flange. Let's set the angle to 50 degrees and length to 50mm. And for the flange position we'll choose to place the bend outside. Once that's all set just click the green tick to confirm the command. So far, we've added extra material to our sheet metal part with edge flanges By nature, these always introduce a new bend to the sheet metal part as well. If you want to add material to a sheet metal part without adding any bends, then you can use a tab feature instead. We'll add a tab feature onto our second edge flange here, and we can do this by selecting the face and then just starting a new sketch. Now we'll sketch out the profile of the tab. And to do this we'll use a series of lines and an arc. You can easily transition from a line to an arc while sketching by pressing A on your keyboard. Once you've drawn the main profile, finishing the rest of the sketch is fairly straightforward. We just need to add a circle to the center point, then use smart dimensions and a symmetric relation to fully define the sketch. Once the profile is fully defined, click the base flange tab feature and make sure that merge resolve is ticked so that the tab is combined with the existing part. The Sketch Bend feature allows you to add bend lines to a flat face of a sheet metal part. We'll use this to add a bend to our tab. Create a sketch on the tabs face, and then draw a line and add a 12 millimeter dimension between it and the whole center. When dimensioning, if you select the edge of a hole, it'll actually allow you to dimension to the center. So that should be straightforward. Now pick sketch, bend and click above the line to designate that as the fixed part of the model. Then just accept the command with the rest of the options. Set as default. Next, there are four edges that I want to round off, and we can use the fillet command to do so. Choose fillet and then set the Phillip radius to ten millimeters. And then click the two inner edges shown. Now if you confirm the command by pressing enter, you can press enter again to repeat the command. Let's do this just to finish the fillet command and start a new one. Now let's pick the two outer edges here and add ten millimeter fillets. Next let's take a look at the jog feature. Notice that one of the tabs on the side of the part is already had a jog feature applied to it. We're going to repeat this process to add a jog to both of the other tabs here. We can actually reuse the sketch that was created within the original jog. If you locate that in the tree and then expand it out, you can select the sketch and then right click to display it. Then let's start a new sketch on the face of the tab, and select the line in the original sketch and use Convert Entities to copy it. And then I'll reposition it. Just dragging it so it coincides with the tab or bend. Now we'll use the jog tool on the sheet metal tab, amending the jog offset values and position when necessary and selecting reverse direction if it's required to line up with the existing jog. Once you've done that for the first tab, just repeat the process again with the same values. To apply a jog to the remaining tab feature. When working with sheet metal, you can temporarily unfold bends, and this can be helpful when you're adding certain features. Next, I want to add a cut that goes across the bend between our first and second edge flange, and so we'll unfold it first to unfold the edge flange. Choose the unfold command. Select a fixed face which is the one highlighted, and then select the bend that you want to unfold. You can unfold all the bends at once by picking collect all bends. But as we only need to unfold this one bend, it's more efficient. From a performance perspective. Just to unfold what we need. Now we'll start to sketch and draw a centerline, locking onto the two midpoints on the bend edges. Then we'll use the slot tool with the center point slot selected to place a slot centered on the midpoint of the centerline dimension, and 15mm for the distance between the slots arcs and six millimeters for their radius. And we'll be ready to perform the cut. When creating the cut, choose to link the depth to the thickness of the sheet, as this will make it update. If we later change the sheet metal thickness, I'll ensure that the cut passes all the way through. Once you're happy with the cut, fold the part back to its original state by using the fold command. Finally, let's activate the flat pattern of our sheet metal component by using the flatten tool on the sheet metal tab. This will automatically create a derived configuration that displays the flat pattern of our sheet metal pop. If we press flatten again, it will actually return to its folded state. We can actually right click the face and choose to export straight to a DXF for manufacturing purposes. So that's the end of this quick introduction to sheet metal in SOLIDWORKS. I hope that's been helpful and that you'll find ways of using these tools during your time with the online trial.