Create sheet metal parts

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Create sheet metal parts.

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In this video, we’ll create a flange, a bend, use Fold and Unfold and create a flat pattern.

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In Fusion 360, we want to get started with the supplied data set Sheet Metal Lever.

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This contains a single body and we're going to be creating a sheet metal lever that will attach to the area with this D shaped extrude.

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To get started, we first want to understand that sheet metal components can be designed in Fusion 360,

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but there are some requirements that we need to make sure that we do.

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The first of which is that a sheet metal part is going to be its own component.

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Now this can be done by creating a new empty component as a sheet metal component,

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or it will be automatically done when we use our first sheet metal tool.

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I'm going to start by going to Assemble and creating a new component and I want to make sure that the component is set to sheet metal.

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It's going to be internal.

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I'm going to rename component to be Handle and then I can determine which sheet metal rule I want to use.

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For this example I'm going to use this Steel (mm) Default and we're going to modify those parameters later.

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Once I do that, my design now contains Handle 1 component and you'll notice that the radio button is active,

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meaning we're currently working inside of this component.

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If we expand it, I have my sheet metal rules and I can modify these values by switching the rules to another value.

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Or I can navigate to my Sheet Metal tab, I can go to Modify and I can take a look at my sheet metal rules.

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Right now we have in this design and the thickness value of 2.5 mm.

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In the library we have our steel default.

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Notice on the right hand side, we can edit the rule or we can create a new rule based on this.

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I'm going to create a new rule based on this and instead of simply creating a copy of the original, I'm going to just put 3 mm in the title.

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Then I'm going to change the thickness value to be 3 mm.

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And I want to note that we have a couple other things that we can change but we will leave as default for this example.

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We can modify things like the K Factor and the way that the Miter/Rip and Seam gap is calculated.

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The K Factor will determine the position of the bend, internal to the sheet metal thickness.

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In most cases that K Factor value will be 0.44, meaning it's a little bit closer to the inside bend than the outside bend.

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We're going to save that and we're going to close, then we'll modify our sheet metal to include the new sheet metal value that we created.

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We’ll select steel 3 millimeters and you can see now our rule is going to create all of our sheet metal components as 3 millimeter thick steel.

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From here we're going to start by creating a sketch.

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When I select sketch, I want to select my XZ plane for this example and then I'm gonna slowly rotate.

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Go to Create Project/Include and Intersect, I'm going to bring in this face just as a reference, then go back to my front view.

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While it isn't strictly needed, it can be helpful to have that reference in place.

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So I'm going to start with a line.

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I'm going to begin dragging this up, I’m gonna slowly pan, drag this up into the right, place.

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And once I have those three sketch entities, I'm going to hit Escape to get off my Line tool.

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Next, we'll begin with dimensions and I'm going to go from this upper point to this point on the vertical line and make that a distance of 35 mm.

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I'm going to make the angle between these two 50 degree.

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And I want to make the overall height from the center of the shaft to this upper point, a distance of 165 mm.

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And I also want to have a 5 degree angle on this edge.

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There are a few other things that we need in order to fully define this,

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and one of those things could be the distance between this point and this point horizontally.

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In our case, I'll set that to 35 mm and this will give us a fully defined sketch.

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When we're creating sheet metal parts, the initial sketch for the flange can either be a closed profile sketch,

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or it can be an open profile like we've drawn here.

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There are some differences.

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And when we create sheet metal components like this, what we're actually doing is creating a thickness based off of that line.

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So when we go to Create and select Flange and we select the sketch, we begin dragging it,

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noting that it creates that 3 millimeter thick part based on the position of that line.

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We can choose which side that goes to or have it be symmetric based on our sketch line.

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In our case, it's going to be Side 1 and the direction is going to be Symmetric.

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In our case, we're going to set this distance value to 10 mm and this will be wide enough for the flange that were mounting to.

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We're going to say, OK, and now we've begun by creating that sheet metal component.

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Next I want to use my Modify Fillet tool and I want to create a fillet on each of these edges.

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Going to select the bottom ones as well and note that we have an option to use a Fillet Full round.

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If we use Full Round, it allows us to select specific faces.

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And in this case, you'll notice that as I go through this selection, different selections will give me different fillets.

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So when we're creating these full round fillets, we need to make sure that it works in our specific instance.

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For this example, since I'm creating a sheet metal part and I want to fillet the top and bottom edges at the same time,

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I'm going to add a manual fillet and it's not going to be a full round.

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I'm going to add a value of 5 mm to simply round off those corners.

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The next thing I need to do is remove this D shaped area from the center of my sheet metal part.

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This can be done by creating a sketch based off of that face.

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To do this, I'm going to hide my sheet metal body temporarily and I'm going to start a new sketch on the face of this part.

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We're going to right click and use Create Sketch.

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This will automatically give us that inside profile.

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And one of the reasons that we're not doing this based on the face selection is because that face has a hole in the center of it.

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We can bring back the body and we can use extrude holding down the left mouse button looking for that profile.

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We can begin to drag it and set the distance Through All,

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and noting that objects to cut, we want to make sure that we exclude the original body and we're only removing it from our handle.

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Now that we've removed that geometry gives us a way to mount our sheet metal handle onto that existing shaft.

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Any changes we make earlier in the design will be parametrically updated and won't affect that extrude cut.

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The next thing that we want to do is we want to create a cut that goes through the center of the handle.

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In order to do that, we need to Unfold and Fold the design.

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We can simply create a sketch in an extrude cut.

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But because the handle is at an angle, the cut edges will not stay normal to the direction of the sheet metal.

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This means that it can be problematic to fabricate.

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So we're going to go to Modify and we're going to select Unfold.

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When we do this, we need to select our stationary entity which will be this portion of the design.

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And notice that it automatically collects those bends.

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We're going to unfold all bends and we're going to say, OK.

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Next, from a right view, I want to create a new sketch and I'm going to start by selecting this face and creating that sketch.

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I'm going to use my Create and I'm going to select a sketch slot.

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I'm going to use center to center and simply going to drag it down, begin dragging the diameter and then I want to use some constraints.

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I'm going to set this endpoint vertical with the origin and then using my dimension tool, I'm going to give it an overall height of 125 mm.

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Going to give it a distance from the origin of 35 mm and I want to give it a radius or diameter value.

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In this case, I'm going to set the radius to 5 mm and then we'll finish the sketch.

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Use extrude to remove this and make sure that we cut all the way through this part.

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Once again we want to double check our objects to cut, to make sure we're not removing from any other geometry.

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And to make sure that this can update easily, I'm going to select Through All in case I change the thickness of the sheet metal part later.

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Now that we've created that cut and we know that all the sides of the cut are normal, we can re fold those faces.

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So this is a great way for us to create this complex geometry, knowing that it can be manufactured later.

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There are many other things that we can do with sheet metal parts such as use that create flanges and bends to create more complex sheet metal parts.

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But the last step that we're going to explore is something called a flat pattern.

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The flat pattern is the next stage in creating a detailed drawing or exporting this for manufacture.

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So under the Create drop-down, we want to make sure that we create a flat pattern.

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Once again, we need to select a stationary face and we'll say, OK.

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A flat pattern is generated and it gives us a position of the bends as well as the internal and external bend lines.

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We can select Export as a DXF from here.

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Or we can even select this, right click and create a new detailed drawing of this flat pattern.

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Once we finish the flat pattern, now we can see that is included in the browser and we can activate it at any time.

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Some of the things that we did, such as creating the extrude cut could be done at the flat pattern stage.

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But if you want to see them in the bent design, you want to make sure that you use the option to unfold and refold those designs.

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From here I'm going to activate the top level of this design and go back to a home view that I want to make sure that I save this before moving on.