3D Modeling & CAD for Motorsport: Sweeps and Piping
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Sweeps and Piping
07.29
| 00:00 | - The sweep tool allows us to sweep a profile along a trajectory. |
| 00:04 | Think of it like the extrude tool, extruding a 2D profile to add depth, except now we have complete control over the shape of the depth we add, rather than just extruding in a straight line. |
| 00:16 | This means we need at least two sketches, the profile and the path on different planes. |
| 00:22 | The profile sketch will need to form a closed loop to create a solid, just like when we were using the extrude tool. |
| 00:28 | Without a closed loop we are only creating a surface which we'll eventually need to thicken to make solid anyway. |
| 00:36 | A closed loop isn't required for the path sketch and we can use either 2D or 3D sketches to define it. |
| 00:43 | As you can imagine, this tool is ideal for modelling motorsport and automotive components like roll cages, exhaust systems and other plumbing work like intercooler piping, although that's definitely not the limitation. |
| 00:56 | To get an idea for how this works, we'll start by sketching our profile as a circle with a 30 mm diameter on the right plane, centred on the origin point. |
| 01:06 | Let's now put a flat edge on the top of the circle, this is going to help us with visualising the sweep when we get to it. |
| 01:14 | Let's also use the offset modification tool here in the sketch toolbar to create a thin walled profile. |
| 01:20 | We'll make the wall thickness 2 mm and flip the offset direction so the profile we're creating is inside the original profile. |
| 01:29 | For our path, we'll sketch on the top plane, starting at the origin point as well, running perpendicular to the profile sketch. |
| 01:38 | Let's use the line tool for this, starting with a 100 mm straight line and then we just click, hold and drag to make an arc at a tangent, placing two in an S shape and a 100 mm straight line to finish. |
| 01:52 | Now onto the sweep tool, which can be found here in the create dropdown menu. |
| 01:56 | Or we can use quick key S to bring up the search function and search for sweep. |
| 02:01 | Leaving the type preference for now, we can select our profile and our path. |
| 02:05 | Note that we might need to make these sketches visible in our browser to do so. |
| 02:10 | And now we can see our sweep come to life. |
| 02:13 | The distance is actually a fraction of the path so 0.5 will sweep half of the sketch path and one will sweep the entire sketch path. |
| 02:22 | Looking at our orientation preferences, perpendicular keeps the profile or cross section perpendicular to the path along the whole trajectory. |
| 02:31 | Whereas parallel keeps the profile parallel to the original profile plane. |
| 02:36 | The important thing to note here is that perpendicular allows for taper and twist and parallel doesn't. |
| 02:43 | Taper angles, as the name suggests, tapers the sweep as it progresses along the path. |
| 02:49 | This doesn't work well with sweeps and we would usually get an error because the sweep would intersect itself. |
| 02:55 | Twist will rotate the profile along the trajectory, let's do 180° for example so the flat section starts on the top and finishes on the bottom. |
| 03:05 | Just like with the extrude tool, we have the same operation options to generate a new body or cut or intersect or join with existing bodies. |
| 03:13 | Looking back at the type preference, you can see that we have the option to use guide rails or surfaces. |
| 03:19 | Guide rails are open ended 2D sketches that can be used on the side of the sweep to guide its shape. |
| 03:25 | Guide surfaces work in the same way but you use a 3D surface to guide the sweep shape. |
| 03:31 | Sometimes the original output from the sweep tool, may be not exactly what we want so these guides can help us gain even more control over the shape of the sweep. |
| 03:40 | Let's go back now and look at how we can implement a guide rail and how it can be useful. |
| 03:46 | We'll start by clicking OK to execute our current model and then drag the cursor back before the sweep on the timeline. |
| 03:53 | We can start by making another sketch on the top plane in order to make a guide rail. |
| 03:58 | First we set the line type to construction and project the sketch for the path and the profile, except for the first straight section of the path because we'll be doing something different with this section soon. |
| 04:10 | Now we can take line type back off construction and offset the projected sketch by 15 mm on the inside. |
| 04:18 | Next let's connect the offset section to the profile with some different elements to illustrate how the guide rails work. |
| 04:25 | Just like we did earlier, we can use the line tool to create some extra arcs, making sure we finish at a tangent to the connecting curve. |
| 04:32 | OK so let's finish the sketch and then edit the sweep feature, changing the type to path plus guide rail. |
| 04:40 | If we select our new sketch as the guide rail, notice the twist preference is no longer available but the profile scaling preference is added. |
| 04:49 | Flicking between these options we can see the changes that it makes to the model. |
| 04:53 | As you can see, this is a really powerful tool for manipulating the surface of our sweep. |
| 04:59 | With some experimentation, you'll be able to model some really complex geometry. |
| 05:04 | Consider how this might be used to model an intake plenum or the expansion chamber for the exhaust or the two stroke motor. |
| 05:11 | Don't forget that there are always going to be manufacturing limitations to keep in mind like we discussed in the design fundamentals module. |
| 05:19 | Have a look back if you need a refresher on design for manufacture. |
| 05:23 | Before we finish up, let's take a quick look at another creation tool that's worth discussing in this module. |
| 05:30 | As although it's not part of the sweep tool, the idea is very similar. |
| 05:34 | This is the pipe tool which creates a pipe that follows a path. |
| 05:38 | Using this tool doesn't require a profile for the cross section, only a path or trajectory. |
| 05:44 | For the profile, we can choose from some simple and common section shapes, such as a circle, square or triangle. |
| 05:52 | Let's open our roll cage 3D sketch back up to have a quick look at how this works. |
| 05:57 | With the pipe tool selected, we first select the main hoop sketch for the path and use the circular cross section with 38.1 mm section size. |
| 06:07 | Then selecting the hollow preference, we can set the wall thickness to 2.6 mm. |
| 06:13 | These measurements are the metric equivalent to 1.75 inch by 0.12 inch DOM tubing commonly used for roll cages. |
| 06:24 | Now with the operation set to new body we can click OK to finish. |
| 06:28 | Then it's just a matter of repeating the same process for the A pillar bar using our other sketch and we can see our 3D model of the roll cage taking shape. |
| 06:38 | OK so to quickly recap this module, the sweep tool allows us to sweep a sketched profile along a sketched path. |
| 06:45 | To model a surface we can use an open sketch profile. |
| 06:49 | However, to generate a 3D solid, the sketch profile will need to form a closed loop. |
| 06:54 | Like the extrude tool, we can use the sweep tool to create a new body or join with or cut an existing body. |
| 07:03 | Using the taper twist guide rail and scaling functions can give us a lot of flexibility over the form of the sweep, just keep in mind that the part will need to be physically made and that comes with limitations on what's possible. |
| 07:16 | Circular tubing is commonly used in automotive applications and the pipe tool is a quick and easy way of sweeping circular and other basic sections along a path. |
