Design Sheet Metal Parts in Fusion 360

Step 2: Create a Base Flange

A big part of our time in the Sheet Metal workspace will be spent adding flanges to the design. Flanges are basically sheet metal surfaces that are connected to other surfaces by bends in the material. To start our design, we will need to add a base flange. This flat piece of metal will be the starting point of our design and we will be adding other surfaces coming off the base flange to build the sheet metal part.

Creating a base flange starts with creating a sketch just like you would do in the Model workspace. This can be a simple rectangle or a more complex shape with cutouts, holes, or sides at irregular angles. For this tutorial, we will start with a sketch that will form the back of the servo bracket. The geometry of this base flange comes from the dimensions of the HS-5065MG servo.

To create a base flange, select the Flange command from the Create menu in the ribbon. This is a command we will be using quite a bit for this tutorial.

Then, using the Flange command, select the sketch profile for the part. Your selection will appear in the flange dialog box. You can also select a material to use for the base flange, a subject we will address further in the next step. After clicking OK, Fusion 360 will generate a flat body based on your sketch.

Step 3: Set up your Design Rules

You may have noticed that we never specified a thickness for the base flange. One of the significant differences between the Sheet Metal workspace and the Model workspace you are likely most familiar with is that when working with sheet metal, because we are using a sheet metal raw material, many of the geometrical attributes of the part are determined by the material selected, rather than having the user directly input the model geometry. In other words, unlike using extrude in the Model workspace, where you would specify the thickness by setting an extrusion distance, in the Sheet Metal workspace, the thickness of the material is determined by the Design Rules.

The Design Rules basically specify the properties of the sheet metal that will be used to make your part. This includes the thickness of the metal, along with some other useful properties like how sharp the bends in the material will be.

To adjust the design rules for the part, navigate to Sheet Metal Rules in the Modify section of the ribbon.

In the Sheet Metal Rules dialog box, you will find the material you selected for the base flange. If you hover the mouse over the name of the material, a little pencil icon will appear. Click this pencil icon to begin editing the sheet metal rules.

Then you will be presented with a second dialog box where you can edit, among other things, the thickness of the material. Sheet metal thickness is typically specified as a gauge, rather than a direct measurement as it is presented in Fusion 360. So, to figure out the thickness you want to use for the material, it is useful to refer to a chart of sheet metal specifications. Your sheet metal manufacturer or supplier should have a document detailing the availability of sheet metal gauges in different materials. For this project, I am using 18 gauge aluminum 5052, which is 1.02mm thick.

Once you are done, click Save. You will see the thickness of the base flange update.

Step 4:  Add Another Flange (Add a Bend)

Now that we have a base flange, the next step is to add more flanges to the design. Flanges are simply sheet metal surfaces connected to the base flange by bends in the material. You can picture this by imagining the process of making a sheet metal component. When the part is manufactured, the entire flat sheet metal shape will be bent by hand or by CNC bending tools to create the finished form. In Fusion 360, we will be able to toggle between the folded and flat design.

First, select the edge to which the next flange will connect. This can be any straight edge in the design. In the example part, I will be selecting the edge that will fold underneath the servo. Then, in the ribbon, select the Flange command from the Create menu just like we did when creating the base flange.

Then, in the Flange dialog box, input the length of the flange. This length is the distance between the edge you selected and the end of the new sheet metal surface.

You will notice that Fusion 360 automatically places a bend in the material, rather than creating a perpendicular surface like you would get when using the extrude command in the Model workspace. There are a couple options for the Bend Position. The default, and most common, option is an Inside position. With an inside bend position, the overall dimensions of the base flange stay the same; the flange is placed as if you extruded another surface from the base flange, only the software places a bend between the flanges as previously stated. The second most common option is the Outside position. When using this option, the new flange is placed off the end of the base flange. So, the overall dimensions of the base flange will increase in size by the thickness of the material.

You can repeat this process for however many flanges your design requires.

Step 5:  Unfold the Design

In the Sheet Metal workspace, you can fold and unfold the design in order to see the shape of raw sheet metal that will need to be cut in order to manufacture the part, and also to do more design work as we have been doing. Unfolding the design is also extremely important for adding additional geometries to the part, like holes, as we will see in the next step.

To unfold the design, select Unfold from the Modify menu.

The Unfold dialog box has two fields. The first designates the Stationary Entity. This is the surface that will remain stationary when the sheet metal part is unfolded. In most cases, you will want to select the base flange. Next you select the bends that will be unfolded in the Bends field. You do not necessarily need to unfold all the bends in your design, but I find it most useful to do so.

Pressing OK will produce a flat design from your sheet metal part that shows the shape that will need to be cut out of the sheet metal material itself in order to produce your part.

If you are following along with the example project this post, you will want to leave the design unfolded for now. But, when it comes time to re-fold the design later on, in order to return it to its three-dimensional shape, simply click the Refold button on the far right side of the ribbon.

Step 6:  Add Holes

Aside from seeing what our sheet metal part will look like in its raw form cut from a sheet of material, unfolding the design is also extremely important for adding additional features to the design, like holes or cutouts.

Take a look at this example of an issue that could occur if you tried to add things like holes without first unfolding the design. Let’s imaging you had a sheet metal part with a flange at a 45° angle to the base flange. Now you want a hole in that flange. You might use the same approach you would in the Model workflow, drawing a circle on one of the origin sides and extruding it through the material.

Take a look below at what that extrude does to the design once it is unfolded. You can see that this hole is not perpendicular to the material. Rather, it runs at an angle to the top and bottom surfaces. This creates a serious issue for manufacturing the part because, in addition to the fact that this features is likely not design the way you intended, it is impossible to manufacture on most sheet metal cutting tools.

So, to avoid this issue, it is always best to unfold the design. Then, once the material is a flat sheet, you can add holes using sketching/extrusion, or the hole tool. This guarantees that the holes run perpendicular to the surfaces of the sheet metal and show up correctly when the design is re-folded.

Once the design is re-folded, you will see the holes in the correct places on the part.

Step 7: Create a Drawing

When it comes time to get your sheet metal part made, it will be extremely useful to generate a drawing of the flattened part with a list of bends your manufacturer will need to perform. This way, your manufacturer will have all the information they will need to cut out the correct shape from the raw material, and they will also know where to place each bend, plus the angle for each bend.

To create this drawing, switch from the Sheet Metal workspace we have been using throughout this tutorial so far, and instead switch to the Drawing Workspace. When you hover over the Drawing workspace, select the option to create a drawing From Design.

Then you will be presented with a dialog box. The first field in the dialog, Representation, has two options: folded model and flat pattern. In this case, we will want to choose Flat Pattern.

A new tab will open in Fusion 360 with the Drawing workspace. Just like with a drawing of a model you might have created in the past, start by placing a base view for the drawing. In this case, the base view is of the flat metal sheet used to form the finished part. You can, and should, add dimensions to this drawing just like you would with other types of drawings.

One very important piece of information we will add to the drawing for working with sheet metal is a table of bends needed to form the final shape of the part. To insert a table into the drawing, click on the Table item inside the Tables menu in the ribbon.

The convenient feature is that Fusion 360 will automatically generate a table of bends in the design. You will notice that the table will automatically contain a row for each bend in the design. Additionally, on the drawing base view, you will notice that Fusion 360 automatically places a number next to each bend to identify that bend with the corresponding row in the table.