3D Modeling & CAD for Motorsport: Assembly Basics
Watch This Course
$199 USD $99.50 USD
-OR-
Or
8 easy payments of only $12.44
Instant access. Easy checkout. No fees.
Assembly Basics
13.18
| 00:00 | - When designing components in CAD that will interface with other components or parts of a vehicle, being able to create an assembly, allows us to analyse how the parts fit together. |
| 00:10 | Basically, every part on a vehicle fits with another in some way. |
| 00:15 | These could be simple examples like brackets to support a catch can in the engine bay or toe hooks mounted to the chassis, to more involved assemblies like multi link suspension systems. |
| 00:26 | Even if we're not using CAD software to design every part of an assembly and we're just designing one new part to fit with existing parts, it's still completely possible and usually beneficial to model these existing parts. |
| 00:40 | It's understandable to think this process of creating assemblies would come after modelling each part but there's generally going to be a fair amount of back and forth here, especially as parts and assemblies get more complex. |
| 00:53 | So it's much more efficient to model components and make changes while checking the assembly with other parts. |
| 00:59 | Having all these parts modelled is a great help for planning and being able to visualise parts together, giving us a better chance for optimising their function as a system. |
| 01:09 | As we've already discussed, Fusion 360 operates around a top down modelling approach as opposed to the bottom up approach we commonly see with other CAD software like Solidworks. |
| 01:20 | For nearly everything we've covered so far, this doesn't really make a difference, how we model features is the same or very similar between most programs. |
| 01:29 | When it comes to assemblies though, this is really where we find the key differences. |
| 01:34 | That's not to say the fundamentals behind all of this aren't the same, they are, it's just two different ways of doing the same thing. |
| 01:41 | Let's quickly revisit the meaning of these approaches before going any further. |
| 01:45 | Bottom up is where we model our parts separately and then bring them together in an assembly once they're created. |
| 01:53 | That means that when we want to make changes to the parts of our assembly, we must go back to the individual parts and modify them separately. |
| 02:01 | With top down in Fusion 360, we can do this all from one file, meaning we can create new components, model them and assemble them together at the same time. |
| 02:10 | This allows us to make modifications to individual components more quickly and see the effects of the changes to the assembly as we do so. |
| 02:19 | Our Fusion 360 files used for modelling are referred to as designs so a single design might contain one component or multiple components in which case it's essentially an assembly. |
| 02:31 | In the previous modules you likely noticed the new component function either in the toolbar or when using our create functions under the operation preference. |
| 02:40 | There are two types of components we can create inside a design, internal or external. |
| 02:46 | As the name suggests, an internal component exists only in the current design whereas an external component exists externally under its own file and is then referenced in the current design. |
| 02:59 | The advantage of an internal component is that it doesn't exist elsewhere so when moving files around, references don't get broken. |
| 03:07 | External components however do make it easier for us to use the same component in other designs. |
| 03:14 | If we create a new component using the operation preference inside our creation tools like extrude for example, it'll automatically be an internal component. |
| 03:24 | On the flipside, if we use the new component function in the toolbar, we have the option of internal or external. |
| 03:32 | Let's work through an example to help explain all of this. |
| 03:35 | We'll be using some skills that we've already learned so if you're hazy on the finer details, make sure you jump back to the relevant module for a refresher. |
| 03:43 | Pulling up our exhaust flange example from earlier, consider an assembly of a section of an exhaust system with four parts. |
| 03:51 | Two identical flanges that connect together and a length of exhaust tube coming off each flange. |
| 03:57 | Our design file currently has one component and one body shown in the browser. |
| 04:03 | In the timeline, we can see this sketch and extrude used to make the flange. |
| 04:07 | We'll quickly save this as a new file under the name exhaust assembly so we aren't changing the original flange design file. |
| 04:16 | We do this because we want to keep this as a single component file so it's easy to use elsewhere. |
| 04:22 | For the next step we can use the mirror tool that we learnt about in the earlier solid modelling basics section, let's set the type to bodies and select our only existing body. |
| 04:31 | For the mirror plane, we can select the bottom face which is also the top origin plane in this case. |
| 04:37 | For operation, let's select new body. |
| 04:41 | So now we have two bodies in our browser but our design file still thinks there's only one component. |
| 04:47 | If we right click on body two in the browser, we can create a new component from this body. |
| 04:53 | Notice how our browser changes, the icon at the top now shows that we have an assembly. |
| 04:59 | In our current state, our second flange is its own internal component with its own origin and bodies but the original flange is actually still grouped under the overall assembly which makes things a bit confusing. |
| 05:14 | To organise the browser better, let's also create a component from the original body. |
| 05:18 | To experiment with this a bit more, let's first make sure the assembly is activated. |
| 05:23 | By opening the data panel, we can right click on the design file for the flange before we saved it as an assembly and then insert it into our current design. |
| 05:32 | Let's drag it up about 50 mm to separate it from the other bodies just for clarity. |
| 05:38 | Don't worry too much about this step right now, we'll be covering it in the next modue. |
| 05:43 | This is an external component, shown by the chain link icon here that links it to the original design file. |
| 05:50 | If we had that file open in another window and modified it, the component in the assembly can be updated to reflect that change as well. |
| 05:59 | This doesn't happen automatically though so we need to prompt Fusion 360 to make the update. |
| 06:05 | If an external component isn't the most recent version, meaning changes have been made and saved, but these aren't captured in the assembly file, we get this warning with a yellow exclamation mark over the chain link icon. |
| 06:18 | Clicking this icon above the toolbar will update all out of date external components whereas clicking the individual icon for just the component will update only that component. |
| 06:30 | We could also right click to break the link if we wanted and it would become an internal component. |
| 06:35 | Notice that if we activate each component by clicking the dot next to it in the browser, the timeline changes to show the history of creating just that component. |
| 06:45 | For the internal components, we only see the create new component from body process but for the external component, the timeline still has the sketch and extrude used to make the part in the first place. |
| 06:58 | If we activate the entire assembly, we can still see the original sketch in extrude used to make the internal components. |
| 07:06 | If for example we wanted to modify the size of the bolt holes from 11 mm to 13 mm, we need to edit this sketch, in which case both internal components would change as they both reference it. |
| 07:20 | The external component doesn't change though because these are no longer the same sketches. |
| 07:25 | Also notice for the external component we have this edit in place icon. |
| 07:30 | As the name suggests, this allows us to edit the component in place inside this assembly rather than opening the component's own design file. |
| 07:39 | If we select edit in place, we can see our model space change with the blue border. |
| 07:45 | Up the top of the screen we can choose if we want the edit in place to be associative or not. |
| 07:49 | This means we can make references to other components in the assembly and those references will be captured in an assembly context inside the external component's own design file. |
| 08:01 | For example, if we delete the bolt hold dimension and reference the recently modified bolt hole for the internal component, we can see this assembly context in the browser. |
| 08:11 | After saving, we can look at the design file for the external component and see these changes carried over. |
| 08:18 | We can edit the context from here as well or to make this file independent again we might consider breaking the link. |
| 08:25 | A quick thing to note here is Fusion 360 won't allow us to create new components from sheet metal bodies, this isn't really an issue though, we just need to use them as external components in our designs and we can still use the edit in place function. |
| 08:40 | OK so let's head back to our assembly and hide the external flange component. |
| 08:44 | We'll make a new component making sure our assembly is activated first so that a new component isn't added within another component but to our top level instead. |
| 08:55 | If we select the external setting in the pop up window rather than internal, it'll of course be an external component and can be used again elsewhere if we wanted to. |
| 09:06 | Let's select standard type rather than sheet metal as our new part won't be made from sheet metal or need any specific sheet metal modelling tools. |
| 09:14 | The activate preference here simply means that the new component will be activated when created so we can go straight into modelling it using the edit in place function. |
| 09:24 | We'll sketch on the top plane and with the edit in place set to associative, we'll use the project tool to use the internal diameter of the flange for our sketch profile and also offset this to make another circle with a 2 mm larger radius. |
| 09:39 | If we finish this sketch we can now make an extrude of the profile. |
| 09:44 | Let's make the start point the upper face of our top flange and the extrude can be 200 mm long. |
| 09:50 | New body is a good setting for the operation preference here because this is the first body in this component anyway. |
| 09:57 | We can now click OK to finish the extrude and then end the edit in place. |
| 10:03 | Now that we have one of the sections of the exhaust tube we need to save this external component, renaming it first to something more appropriate. |
| 10:10 | Let's now find the design file for this component in the data panel, right click and insert it into the assembly. |
| 10:19 | This is going to require positioning the component though which is something we'll cover in the next module. |
| 10:25 | A simpler way for now is to just use the mirror tool and mirror the component through the top plane. |
| 10:31 | Notice that this new component is an internal component, that's because we made it with a create tool, the same idea as the extrudes. |
| 10:38 | This isn't really a problem though because it references the external component so if I were to change the length to 300 mm using the edit in place function, we can see the internal component also changes. |
| 10:51 | To illustrate one more consideration before we move on, let's hide the lower of the two flanges and show the external component flange that we had earlier. |
| 11:01 | With the assembly activated, we'll sketch a small circle on the top plane to cut through our flanges using the extrude tool to cut in both directions. |
| 11:11 | We'll set the extent preference to through all. |
| 11:14 | If we then show our lower flange we can see that the operation didn't cut it because it'll only cut components that are visible. |
| 11:21 | Note that it also didn't cut our external component flange and that's because this can only be modified using the edit in place function. |
| 11:30 | If just cutting through one flange was our intention, then we're better off activating that specific component rather than the entire assembly and performing the modification. |
| 11:40 | That way, it'll be included in the timeline for that individual component rather than the assembly and if we want to change that feature further down the track, it won't cause us any headaches showing and hiding other components. |
| 11:54 | We've covered a lot of ground in this module so let's have a little recap of the main points. |
| 11:59 | First, understand that working with assemblies might not be required for every CAD job but it's a really powerful tool to help us define how parts will fit together before we manufacture them. |
| 12:10 | Since Fusion 360 is tailored to a top down approach, we have the benefit of being able to create, modify and assemble components all within one design file. |
| 12:21 | While this allows us to make modifications quickly and more efficiently, there are some considerations we need to take to make sure we can make the intended changes. |
| 12:30 | Components used in our assemblies can be internal or external. |
| 12:35 | Internal components only exist in the assembly whereas external components have their own design file, making them more suitable to use in multiple different assemblies. |
| 12:45 | We can still modify external components within our assembly using the edit in place function and can choose to make those changes associative. |
| 12:54 | Meaning that we can make references to other components. |
| 12:58 | These references are then captured in the external components file as assembly context. |
| 13:04 | When making any changes to internal components we need to be careful what component is actually activated and what components are visible because this has a significant effect on the outcome. |
