3D Modeling & CAD for Motorsport: Converting to Sheet Metal
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Converting to Sheet Metal
06.13
| 00:00 | - Sheet metal is commonly used in the automotive space, both in original equipment from the factory and also in aftermarket and custom fabricated components. |
| 00:09 | Think big parts like firewalls and fuel cells as well as smaller items like mounting brackets or tabs. |
| 00:16 | This all means that understanding how to effectively design sheet metal parts is critical. |
| 00:22 | I should point out that when we say sheet metal, I'm referring to metals like steel or aluminium formed into a thin sheet. |
| 00:30 | However the modelling skills in this module can also be used when working with polymer and composite materials like carbon fibre. |
| 00:38 | Due to sheet metal being relatively thin and having good formability, we can produce lightweight parts that have good strength characteristics at a fraction of the cost of machined billet. |
| 00:49 | As we saw in the solid modelling section of the course, our tools are generally based on the manufacturing techniques used to produce the end result so while solid modelling is most suited to machining on lathes and mills, Fusion 360's sheet metal modelling tools are based on the fabrication and manufacturing processes unique to sheet metal like bending and forming. |
| 01:12 | With that said, there are plenty of manufacturing processes that can be used on both solid and sheet metal parts and that means that we do see a good amount of crossover between the toolbars. |
| 01:23 | For example, the hole, fillet and chamfer tools, as well as our fundamental modelling tools like the construction of datums and sketches, are used in both types of design. |
| 01:34 | OK so let's jump back into Fusion 360 to take a closer look at our sheet metal toolbar. |
| 01:39 | As we can see, it's split into the same groups with create, modify, assemble, construct and so on. |
| 01:47 | We'll ignore the assemble group and the new component tool for now because we'll be diving into those in more detail soon. |
| 01:54 | Under the construct tab, we have the exact same tools used to create construction datums that we've already seen. |
| 02:01 | There's nothing new here, we still use datums for construction and references for modelling sheet metal just like we do with solids. |
| 02:08 | Starting under the create tab drop down list, we find the convert to sheet metal tool. |
| 02:14 | As the name implies, this allows us to convert a solid body into a sheet metal body as long as the solid body is of uniform thickness. |
| 02:22 | Having our model as a sheet metal body allows us to use the sheet metal modelling tools. |
| 02:27 | For example, we wouldn't be able to use the bend tool to create bends in a solid body and then be able to flatten these bends like we can with a sheet metal body. |
| 02:37 | Let's fire up a quick example to get a better feel for how this all operates. |
| 02:41 | As always, feel free to follow along with your own model. |
| 02:45 | We'll start by creating a simple sketch on the top plane of a rectangle 100 x 150 mm. |
| 02:51 | Let's now extrude this sketch by a distance of 5 mm, making a new body which we can see here in our browser. |
| 02:59 | Notice that this has the icon next to it that represents a solid body. |
| 03:03 | If we now select the convert to sheet metal tool, we're prompted to choose a base face as the source to infer the body thickness. |
| 03:12 | This is also known as a driving surface. |
| 03:15 | This just means that the thickness of the body perpendicular to the face will automatically become our sheet metal thickness. |
| 03:21 | But we can change this later if needed by coming back and editing our extrude distance. |
| 03:27 | For now, we'll just leave it at the 5 mm we originally defined with the extrude tool. |
| 03:31 | In Fusion 360 we're also given a set of sheet metal rules. |
| 03:35 | These rules are automatically applied as we create new features to ensure our designs are suitable for manufacture which is something we discussed in the design fundamentals section. |
| 03:47 | Feel free to check back if you need a refresher. |
| 03:49 | For example, one of the most common rules when bending sheet metal is that the internal radius should be at least equal to the thickness of the material in order to avoid the part fracturing or distorting. |
| 04:01 | Fusion 360 has a library of these current sheet metal rule sets to choose from and some of them vary with different material properties. |
| 04:10 | We need to apply a rule set when creating our first sheet metal body, be it while using the convert to sheet metal function, or if we use the flange tool which we'll touch on in an upcoming module. |
| 04:21 | After creating our sheet metal body, we can switch the rule from our browser if needed. |
| 04:25 | We can also edit these rules, set the default or create new rules for different materials if we know the properties. |
| 04:34 | This is done by selecting the sheet metal rules icon in the modify part of the toolbar here and right clicking on the rule. |
| 04:41 | Now one thing to note here is that we can choose to override these rules when using the sheet metal tool set in cases where they prevent us from modelling our design. |
| 04:50 | But we'll need to consider the manufacturing implications. |
| 04:54 | This is something we'll come back to in more detail soon so it's just something to keep in mind for now. |
| 05:00 | After completing the convert to sheet metal process, we can look at our bodies in the browser and see the icon for a sheet metal body is different to that of a solid body. |
| 05:09 | This was our first look into sheet metal modelling so let's recap. |
| 05:13 | We start with an extruded body from a sketch as our base. |
| 05:17 | Similar to how we'd often start solid modelling CAD work. |
| 05:20 | As long as the solid body is of uniform thickness, we can easily convert it into a sheet metal body of the same thickness to take advantage of the sheet metal specific toolset. |
| 05:33 | While creating our initial sheet metal body, we apply a set of sheet metal rules depending on our intended material. |
| 05:39 | These rules help us model our design with manufacturing limitations in mind and serve as reminders if we overlook certain aspects. |
| 05:48 | We can edit or create new rules if we understand the material properties that we plan to use or in some cases, we might choose to override these rules altogether. |
| 05:58 | The modelling skills and tools in this module could also be used for non metal sheet material, for example plastic or composite sheets, as long as we consider the different manufacturing processes involved. |
