Kevin Kennedy: Welcome to “Fusion 360 Sheet Metal for Beginners!” This free course is brought to you by SendCutSend.com. We’ll look at utilizing Fusion 360’s sheet metal tools to create this Stainless Steel glove box holder. I was able to upload this Fusion 360 design in just a few minutes and three days later the laser-cut stainless steel was at my door. To get started, open the Fusion 360 demo file from the link below. This file includes a Box component that we’ll build the sheet metal around. Starting with a reference part is a great way to ensure your dimensions will work with the final object. We’ll start by creating a new Component for the Sheet Metal. Let’s first head to the Sheet Metal tab in the toolbar. It’s here that we’ll find all of the sheet metal tools. If we activate “New Component” from within the Sheet Metal tab, you will find that the component type defaults to a Sheet Metal Component. If you activate the New Component feature from anywhere else, simply select Sheet Metal from the type dropdown. Designating our component as a Sheet Metal type is required to assign a sheet metal rule. This will allow us to define the sheet metal thickness, K-factor, and additional information about the material. This glove box holder is a single-part design, so we’ll be using the Top-down modeling approach. In other words, all of our design will be within this file, so the default internal option will work. This ensures our component is created directly within our current file. For the component Name, I’ll type out “Stainless Steel Glove Box Holder.” By default, the parent option is applied to whichever component is active in the Browser. We’d like this to be the root or top-level component. Just note that you can clear this at any time, followed by selecting the desired component. “Activate” should remain checked, as we’d like to start working on this component once it’s created. Lastly, we need to define our sheet metal rule. This is what separates a sheet metal component from a Standard component. Sheet metal rules describe sheet metal characteristics and how the parts are manufactured. The Library folder includes pre-made Sheet Metal Rules, which applies the rules and parameters to the part. For example, I’ll start with the Stainless Steel inches option by selecting it. If I toggle the selection open, you’ll see the thickness, K-factor, and other conditions that make up the rule. Later on, we’ll take a look at creating a custom Sheet Metal rule. For now, let’s click OK to create the Sheet Metal Component. Note that Sheet Metal Components are differentiated in the Fusion 360 Browser via the folded sheet metal icon, while regular components are indicated with a gray cube. With our component active, we’re ready to start sketching. Nearly all sheet metal parts will start with a single face. In this case, I’d like to start by creating a flat face of sheet metal that is the same size as the box. We’ll then use that face as the starting point as we define each flange of the box. I’ll activate the “Create Sketch” feature and then I’ll select the bottom of the box since the full sheet metal face will cover the back or bottom of the box of gloves. I’d like to ensure the Sheet Metal part always adapts to the size of the box. In the Create dropdown of the Sketch tab, we’ll find the Project/Include folder, where we can select the Project command. The Project command allows us to select entities or 3D bodies and it will project the edges into our active sketch plane. We can select inside the rectangle to select all four edges at the same time. After clicking okay, you will see that we have four purple lines that are the same size as our box. Purple geometry lets us know that these sketch entities are “projected” and they’ll remain driven from the source. We’re now ready to activate the Flange feature from the Sheet Metal tab. The Flange feature allows us to turn closed sketch profiles into sheet metal faces by simply selecting within the closed profile. Looking at the model, we now have our first sheet metal face. In most workflows, you’ll use the Extrude command to create thickness. Instead, the Flange feature uses the thickness from our Statlines Steel Sheet Metal Rule that was selected per our component. Before clicking OK, we’ll want to look at the model from a side view to double-check that the Sheet Metal face is below the box. If it appears to interfere or take up the same space, we can choose the other side from the Thickness option. Note that in some cases you may find the symmetrical option to be helpful. This will center the Flange to the sketch entity, applying half the thickness in each direction. Let’s set this back to the original side. Lastly, we need to create a new 3D body, as we’ve already created our Sheet Metal Component. Had we not created the component first, we could select the New Component as the operation. After clicking OK, we have our first flange or sheet metal face, and we’re ready to build additional flanges off the four edges. I’ll view the model from the Home position, followed by reactivating the Flange feature. This time, we’ll select the upper edge of each length of the box. Remember that you can click and hold on top of an object, which will bring up the quick selection box. This will allow you to select edges, faces, or bodies, without having to reorient your model. Once they’re both selected, we’ll simply pull the blue directional arrow to the top. Notice how this automatically Extrudes the flange based on our selected edge and the direction. Because we’re working with the sheet metal tools, this will automatically apply our bend radius, thickness, and other details per our Sheet Metal Rule. For the height, I’ll type out 3.75 inches in the dialog. We’ll want to leave the angle set to 90 degrees, but note that you can adjust the angle in the dialog or by dragging the rotation slider. The Height datum allows us to define how the height is measured between faces. “Inner Faces” measures the flange height from the intersection of the inner faces, while “Outer Faces” measures the flange height from the intersection of the outer faces. Meanwhile, “Tangent to Bend” measures the flange height parallel to the flange face and tangent to the bend, as seen in the example illustration. In this case, I’ll set this to “Inner Faces,” as we’d like to include the 3 and ¾” inches for the depth of the box. The Bend Position is how we specify where to position the bend relative to the edges that we selected. You must think about the Bend Position, or the final size of your part may be incorrect. This is another reason why I recommend designing around an existing object when possible. With the Inside option, notice the flanges collide with the box. The outside option puts each flange on the outside of our original face, resulting in them being right against the box. The Adjacent option ensures that our bend radius starts at the edge of the selected face. I’ll choose this option as I’d like to leave sufficient room for the glove boxes while ensuring the bend radius doesn’t take away from the inner dimensions. Note that you can also choose tangent, which positions the bend tangent to the selected edge. At any time, we can also use the “Flip” button to flip the flanges in the other direction. The Miter Corners option overrides any rounded corners with sharp corners; however, this will not come into play until we create two or more flanges next to one another. Up to this point, all of our bend and corner rules are defined by our single sheet metal rule that’s tied to our Component. However, in some workflows, you may need a unique bend or corner rule. You can enable the Override Rules option, which then allows you to override many settings. In our selections at the top of the dialog, you will notice that each of our selected edges defaulted to the “Full Edge” option. In some cases, you may need Symmetric, Two Side, or Two Offset, each of which allows you to further define how much of the edge becomes a flange. When applicable, you’ll be able to define additional dimensions in the dialog, or by dragging the directional slider. With override unchecked, let’s click OK to create these flanges. Next, let’s create the four flanges that hold the front and bottom of the glove box. With the Flange feature, I’ll select the four inner edges of the previous flanges. I’ll make this 1.25 inches in height per the Outer Height Datum, as this time I know the measurement from the outside of the part. This time I’ll also set the Bend Position to the Adjacent option, which still leaves sufficient room for the box. Take note of the round Bend Relief in the corner where the two flanges meet. This shape is also defined in the sheet metal rules and will help prevent tearing and part deformation during the bending process. Note that this can be set to Round, Square, or Tear. Let’s click OK to confirm the four flanges. This front of the design should allow sufficient room for the gloves to be pulled out of the box. However, I’d like to ensure that the bottom has sufficient support, while also showing you a way to alter the flange size. At any time, you can edit your Flange features in the parametric timeline to alter their size. However, I’d like to extend only the bottom ones. We can instead use the Offset faces feature from the Modify dropdown of the Solid tab. After selecting the two inside faces, I’ll offset them to a distance of ¾” of an inch. We’ve now completed the overall Sheet Metal box with the flanges. At this point, we can finalize our design with rounded edges and some screw holes on the back. If I toggle open the Bodies folder of the Sheet Metal Component, you will see that the Sheet Metal body is also unique. Fortunately, Sheet Metal bodies still allow the use of some Solid Modeling commands, such as Chamfer and Fillet. After activating the Fillet command, I’ll take a minute to select all eight corner edges of each flange. Once selected, I’ll apply a ¼” round over, making sure the final product does not have any sharp edges. Be sure to click OK to confirm the fillet. We can now create some screw holes on the back to mount the holder. Oftentimes, working with an unfolded part will make it easier to sketch objects on the flanges of your design. In Fusion 360’s Sheet Metal tab, we can use the Unfold feature to unfold individual bends or all bends. It’s critical to note that Unfold is a different feature from “Create Flat Pattern,” which we’ll talk about later. With Unfold active, we first need to select a stationary face. Oftentimes, this will be the original face that you built the flanges from. We can then check “Unfold All Bends” which will automatically unfold all 6 of them. Otherwise, you can always select individual bends to unfold them. After clicking OK, you will see that our part is unfolded. The Unfold feature is recorded in the timeline, and we’re given the option in the toolbar to “Refold.” We can now hide the Box component, as well as any sketches that are turned on. This will make it easier to sketch directly on the flat object. I’ll right-click on the middle surface to “Create Sketch”. From here, I’d like to sketch out a keyhole slot that allows the glove holder to be mounted either vertically or horizontally. This can be done with Fusion 360’s native sketch tools or we could insert a premade SVG or DXF file that includes the keyhole pattern. I’ll go ahead and insert an SVG, which you can download from the link below this video. Before inserting the SVG, let’s set up some construction lines for its placement. I’d like to create a point of reference for both the top and bottom. I’ll start by creating two individual line segments. We can then use the Midpoint constraint. Select the endpoint of one line and the edge of the 3D body and then we’ll repeat this for the other side. I’ll also apply an equal constraint to both of these lines. This will allow us to dimension only one line while keeping them the same length. With the dimension tool, I’ll make this half an inch, so we know our slot is at least half an inch away from the edge. Although it’s not required, we can also turn both of these lines into construction lines. Simply hit the escape key to clear all commands, select a line, and select construction in the Sketch palette. Construction lines are denoted by the dashed lines. We can now insert the keyhole slot SVG file from the Insert dropdown, followed by Insert SVG. Insert from My Computer, followed by selecting the SVG file. The overall placement is not critical at this point. For now, I’ll simply move to the middle of the body and I’ll rotate this 90 degrees, to ensure it’s symmetrical. After clicking OK, you’ll see that SVG geometry is green, which means that it’s locked with the Fixed constraint. We’ll need to click and drag over the entire SVG, followed by selecting the Unfix constraint in the toolbar. The line geometry will then turn blue, letting us know that it’s not constrained. I’ll clear all commands with Escape, and then click and drag over all the sketch entities. This time, we can use the Move command from the Modify dropdown. Using the Point to Point move type, we can simply select the top of the arc and the endpoint of our reference line to move this keyhole design into the desired position. Notice we can also create a copy. This works out well in this case as we need a second one for the bottom. After selecting “Create Copy,” I’ll click OK. To Move this second slot into place, we’ll need to first create a sketch point on the bottom so we have something to reference. Once complete, we can once again use the Point to Point Move Type to reposition the slot. Now that both keyhole slots are in place, we can shift-click the inside of each closed-profile before activating the Extrude command. We’ll want to Extrude cut this, while also setting the Extent Type to “All” so this will always cut through the 3D body, even if we change our thickness per the Sheet Metal Rule. At this point, we can “Refold” the faces of our sheet metal component. As you can see this makes Fusion 360 extremely flexible and powerful when designing for sheet metal, allowing us to design in both a flat and finished mode. The design of our Stainless Steel Glove box holder is now complete; however, we need to confirm the sheet metal details, including the thickness. Let’s take a look at creating a Custom Sheet Metal Rule in Fusion 360. We’ll also look at how the existing Glove Box holder adapts when switching rules. After Browsing the available materials on SendCutSend’s website, I decided to go with “304 Stainless Steel” with a thickness of 18 gauge, or .048 inches. Under the Modify dropdown of the Sheet Metal Tab, you will find the Sheet Metal Rules. This dialog includes any rules used “In This Design” as well as a Library of pre-made rules. While hovering over any of these rules, you will find that we can create a “New Rule” while starting with the existing info. Let’s create a New Rule from the Stainless Steel inches. For starters, I recommend that you always rename your rule so it’s clear what it represents. In this case, I’ll change it to “Stainless Steel 18 Gauge.” Most important, the Thickness of 18 gauge is .048 inches. The second option is the K-factor or the ratio between the "neutral axis" of a bent part and the thickness of the material. The "neutral axis" is where the material doesn't elongate or compress during the bend. The K-factor of this 18 gauge is approximately .4. The bending process and other variables may affect the k-factor, so we can leave this to the default of .44. Lastly, you will see we can define the “Miter/Rip/Seam Gap.” Notice the default input contains the thickness variable. This will derive the value from our thickness input above. Experienced Sheet Metal users can also toggle open the Bend Conditions and Corner Conditions. Notice the Relief Shape can be set to Round, Straight, or Tear. Now that we’ve filled out the desired rules, we can click OK to save this new Sheet Metal Rule. If created in the “In this design” section, we can right-click to copy it to our Library folder. We can close this dialog and head to the Fusion 360 Browser to apply this rule. At this point, we’ve only created a new rule. Our design still includes the original Sheet Metal Rule. With a Sheet Metal Component toggled open, we can simply select “Switch Rule” that appears while hovering over our rule. From here, we simply select the newly desired rule in the dialog. Before I select the “Stainless Steel 18 gauge” rule and click OK, I want you to take note of the current thickness of the sheet metal. Watch as it changes when I apply this new Sheet Metal rule. You’ll see that our Sheet Metal part automatically adapts to the new Thickness and bend parameters contained in the Sheet Metal Rule. Custom Sheet Metal rules can be a great way to check or generate designs in multiple thicknesses, which can be extremely helpful in the prototyping process. It’s important to note that we can Switch Sheet Metal Rules at any time throughout the design process, as long as we have a Sheet Metal Component. In the Sheet Metal Rules Dialog, you will also find that you can right-click on rules in the Library folder, and set one as a default. This will apply the Sheet Metal rule to any newly created Design files that contain Sheet Metal Components. We can also edit existing rules, delete, or create new rules at any time throughout the design process. Now that our sheet metal part is complete and set to the desired thickness, we can turn it into a flat pattern for manufacturing. A sheet metal part starts as a flat piece of metal with a consistent thickness. With that in mind, we need to get a flat pattern from our final 3D model. Fortunately, Fusion 360 makes this process easy and efficient. To start, it’s critical to note that Fusion 360’s “Unfold” feature is different from “Create Flat Pattern.” Unfold, allows us to select individual or all flanges to unfold, with the intention that we need to sketch or create features across existing flanges. Contrary, “Create Flat Pattern” will unfold our design while allowing us to quickly create additional details included in a flat pattern that will not be shown in the 3-dimensional model. After activating the “Create Flat Pattern” feature, we’re prompted to select the “stationary face.” This should be the face that all flanges are folded from. In our case, this is the back face. Once selected, we can click OK. The “Create Flat Pattern” feature also differs because it shows us bend lines, bend zones, centerlines, and the shape of the entire part with all bends flattened and bend factors considered. It’s important to note that you can only create one flat pattern for each Sheet Metal body. Notice how we’re placed in a Flat Pattern contextual mode. Our Fusion 360 Browser is now limited to this flat pattern. At any time, we can select “Finish Flat Pattern” to return to the Folded Part. Flat Pattern is not recorded in our timeline, as it will always generate a pattern on the latest design. You will see that it’s instead listed as an object in our Browser. If for some reason you need to delete the Flat Pattern, you can simply right-click, followed by delete. To return to the flat pattern, we simply need to activate the Flat Pattern in the Browser, just as we would with a Fusion 360 component. When in the Flat Pattern environment, you will also notice a new folder nested within the bodies folder in the Browser. The Bend Lines folder includes our bend or “Extent” lines and our “Center Lines.” This allows us to toggle their visibility at any time. One of the reasons this is important is the fact that we can also use the Solid and Surface modeling tools to alter our flat pattern. Again, it’s critical to call out that any changes you make will be parametric and recorded in the timeline; however, they will only display in this Flat Pattern Mode. This is the key difference between Flat Patterns and the Unfold feature. If you’d like changes to only affect your flat pattern, then create them in the Flat Pattern mode. If you’d like to design across flanges that affect both the flat part and the 3-dimensional model, then you’ll want to create them while your part is unfolded. Lastly, you will find that Flat Patterns need to be updated if the Sheet Metal design is changed. For example, I’ll head to the Folded Part, and I’ll simply alter the height of one of the Flange features. After altering the Flange feature, you will see a warning icon in the Browser noting that the Flat Pattern does not correspond with the latest version of the sheet metal design. Simply right-click on the Flat Pattern in the Browser and select “Update Flat Pattern.” We can then reactivate the Flat Pattern and it will now include the latest version of the design. In summary, Fusion 360 makes working with Sheet Metal parts and flat patterns an efficient and easy process, allowing you to quickly prepare metal parts for the laser cutter. It’s also important to note that the Document Units of the Flat Pattern, found under the Document Settings in the Browser, are unique from the Design file units. Be sure to update your desired unit of measure if your default is different from the Design file. This is especially important before exporting your Flat Pattern to a DXF File. Exporting a DXF from Fusion 360’s Flat Pattern mode has some advantages and disadvantages, particularly for laser cutting. For starters, the DXF will include all outer profiles, interior profiles, bend center lines, bend extend lines, and any text, which will all be assigned to different layers within the DXF file. With the Flat Pattern active in the Fusion 360 Browser, we can simply select “Export Flat Pattern as DXF.” You will then see the option to “Convert Splines to Polylines.” Polylines are line segments strung together, which makes them much simpler. We highly recommended using this option as polylines are more widely accepted and provide more consistent results across software packages. After checking the option, we can also define the tolerance. This will specify the maximum allowable deviation between the polylines and the original splines. Leaving this to the default is often sufficient. After clicking OK, we’re presented with another dialog where we can define the File name and location. Click Save once you’ve filled out the name and location. I also recommend opening your DXF in a graphics program, such as Adobe Illustrator, or reopen the DXF in a new Fusion 360 file to ensure everything was included in the Export. The only real disadvantage to this Flat Pattern Export is that it will always include the bend lines and we have no choice to exclude them. However, you may choose to remove them in a graphics program to not confuse them with the outer contour lines, if you don’t plan to have the part bent. To summarize, leveraging Fusion 360’s sheet metal features is a great way to design for sheet metal manufacturing while providing flexible workflows. Creating custom Sheet Metal Rules allows you to design specific to the material and bend processes you’re working with. Finally, exporting the Flat Pattern as a DXF is a quick and easy way to get a flat pattern for laser cutting. Be sure to check out SendCutSend.com for high-quality custom laser cut and CNC parts with a super-fast turnaround, including metals, wood, and composite materials to choose from. [Upbeat Music] Then, check out our playlist on Learning Fusion 360 for Laser Cutting. [End Upbeat Music]
