3D Modeling & CAD for Motorsport: Assemble Joints and Constraints
Watch This Course
$199 USD
-OR-
Or
8 easy payments of only $24.88
Instant access. Easy checkout. No fees.
Learn more
Assemble Joints and Constraints
12.45
| 00:00 | - In automotive applications, there's a big variation in the way that parts fit together. |
| 00:04 | In just the suspension system along for example, we can have pin joints and ball joints at the connecting points between members. |
| 00:12 | These bushings and ball joints often have press fits. |
| 00:16 | We also have sliding joints like the damper and we have the spring clamped between the upper and lower seats. |
| 00:23 | The suspension arms themselves may be fabricated from a collection of parts welded together with rod ends threaded in. |
| 00:30 | My point is if we're modelling these assemblies in CAD to help us design components and analyse the system as a whole, then it's important we're also correctly modelling how these components will be joined to each other. |
| 00:43 | Thankfully our CAD software makes this possible with the use of what's called assembly constraints. |
| 00:49 | The idea here is that we're constraining components as they would be in real life. |
| 00:54 | Understandably if a component is intended to move, then modelling it as a rigid joint isn't going to be an accurate representation, which after all is really what we're trying to get out of CAD. |
| 01:05 | Having these constraints set up properly also helps add flexibility to modifications as well as the ability to more easily spot issues. |
| 01:14 | In Fusion 360 these assembly constraints are referred to as joins but be aware that in some other CAD programs these can be called mates. |
| 01:22 | In Solidworks for example we would add a series of mates, usually three, one for each dimension. |
| 01:30 | If we set three perpendicular faces of a cube to align with another three planes or faces of an existing object, we're removing degrees of freedom each time to fully constrain the cube's position. |
| 01:42 | To be clear, when we're talking about degrees of freedom, we have six, translation in the X, Y and Z directions and also rotation about these. |
| 01:50 | In Fusion 360, it's essentially just the same process but in reverse. |
| 01:55 | When we apply a joint between components, it locks down all degrees of freedom at once and then we can adjust the positions or release degrees of freedom to allow the movement required between the components. |
| 02:07 | Let's jump back into the exhaust assembly from our previous module to make sense of all of this. |
| 02:13 | Remember the third exhaust flange we had? It's an external component sitting in this somewhat useless position. |
| 02:20 | Let's say we wan to move that to the top of the exhaust tube, we could use the move tool, as with any of our components to specify the position of the part in space. |
| 02:31 | If we drag it up to around the top, we can't actually place it exactly where we want it though, with the tube against the bottom flange face. |
| 02:39 | With a bit of maths we could enter the desired Y distance value or use the point to point function to get it where we want. |
| 02:47 | Notice down the bottom of the move window, we have the option to capture position. |
| 02:51 | This means the position change would be captured on our timeline so we can come back to it. |
| 02:57 | If we don't click this, when we click OK, we have the position icons appear in our toolbar with capture position or revert which allows us to undo the position change. |
| 03:10 | So it's clear we can move components into their desired locations in different ways. |
| 03:15 | However this doesn't define the position or relationship to other components. |
| 03:19 | The component can easily be moved from its current position relative to the other component on purpose or by mistake. |
| 03:26 | Remember we always want to fully define our models to most accurately represent the real world scenario. |
| 03:33 | And to avoid unwanted errors creeping in. |
| 03:36 | And the joints are required to define relationships between components. |
| 03:41 | Therefore, since we haven't used any joints in our assembly so far, the position and relationship between them is not defined. |
| 03:49 | Before setting any joints, I recommend grounding at least one component. |
| 03:52 | This locks the position of that component in space, preventing it from moving. |
| 03:57 | Let's right click on our upper exhaust tube and select ground. |
| 04:01 | When opening the joint tool, we can see that there are two tabs, position and motion. |
| 04:06 | This is what we were talking about earlier. |
| 04:09 | The position tab defines the relative position between the components, creating a rigid joint between then by default. |
| 04:17 | By using the motion tab on the other hand, we can change this rigid joint to a range of other options, each one releasing some degrees of freedom and allowing movement between the components. |
| 04:29 | Starting back on the position tab, we need to place the joint origin point on each of our two components that we're making the joint between. |
| 04:36 | The joint origin defines the geometry that'll be used to relate the components. |
| 04:42 | Notice when we're selecting for component one, we can't select the grounded component which is the exhaust tube. |
| 04:49 | This is because we're actually defining the position of component one relative to component two. |
| 04:54 | Meaning that if for example we allow for degrees of freedom, component one will move relative to component two. |
| 05:01 | Since the exhaust tube is grounded, it can't move so it can only be component two. |
| 05:07 | As we move the cursor around the component to place the joint origin, we can see our snap points which are some of the key features of the geometry we might want to use, such as mid points, corners or the centre of curves. |
| 05:21 | Also notice how the joint origin, being the cursor, changes to different orientations depending on what plane we're trying to place it on. |
| 05:30 | This can make it a bit difficult to get it in the intended orientation. |
| 05:34 | The helpful tip here is to hover the cursor over the face desired and hold control on Windows or Command on Mac to stay on that face. |
| 05:43 | This can also be used for cylindrical surfaces and notice we get three options for the snap point, one at each end and one at the mid point. |
| 05:52 | If we can't manage to get the joint origin where we want it, we may want to change the mode setting from the default simple preference to between two planes or two edge intersection. |
| 06:03 | These are fairly self explanatory but it's of course a good idea to have a play with them to get a bit more familiar. |
| 06:09 | Alternatively we can also create our own joint origins using the joint origin tool under the assembly drop down list. |
| 06:16 | This gives us a bit more flexibility with where we position the joint origin on each specific component. |
| 06:23 | Back to the joint tool, let's select our joint origins for our example. |
| 06:27 | With component one being the external component flange, we want this at the centre of the inner diameter on the bottom face. |
| 06:35 | So let's either click on the edge of the diameter or the cylinder and use the command or control keys to help. |
| 06:42 | With component two being the exhuast tube, we use a similar method to select the centre of the diameter on the top face, these joint origins will then coincide. |
| 06:52 | From there we can change the angle, rotating the flange on the top of the tube, or if we want to offset the position for some reason, we can do that with the X, Y and Z components. |
| 07:03 | All of which change the joint alignment. |
| 07:06 | Also since there are technically two ways that a pair of planes can align, we can flip the component over the joint origin. |
| 07:14 | We don't need to do that in this case but sometimes this can be useful if the components align and one is up the wrong way by default. |
| 07:22 | Moving onto the motion tab, we can change our joint type. |
| 07:26 | For each type, Fusion 360 provides a quick animation so we can visualise the allowed motion. |
| 07:32 | By default it's set to rigid as this is the most common type that gets used. |
| 07:37 | Obviously this doesn't allow for any motion. |
| 07:40 | Revolute releases the constraint on rotation about one axis and allows component one, being the flange to rotate about the joint origin. |
| 07:51 | To be clear, with all these joint types we're looking at, we can change the axis we want the motion around, or in some cases along. |
| 08:00 | For example, slider allows for motion along one axis. |
| 08:04 | Cylindrical allows for motion along one axis and rotation around the same axis. |
| 08:10 | Whereas pin slot allows for motion along one axis but rotation around another. |
| 08:15 | Planar allows for translation along two axes or in other words a plane. |
| 08:21 | And also rotation around the axis perpendicular to these. |
| 08:25 | And finally we have ball. |
| 08:27 | This represents a ball joint and allows for rotation around two axes, defining these rotations as pitch and yaw. |
| 08:35 | Choosing the right one of these for our application is important so it's worth experimenting with them and seeing how they work. |
| 08:42 | If we do end up realising that we've chosen the wrong type, it's not the end of the world though because we can always go back and change it as we progress through the model. |
| 08:52 | Let's now finish up with our example, since the flange would be welded in place, a rigid joint makes the most sense. |
| 08:59 | After finishing we can see our joints are now in the browser and we can show, hide or edit from here. |
| 09:07 | As expected, the joint is also here in our timeline. |
| 09:10 | Moving on, in our toolbar under joints we also have as built joints. |
| 09:15 | This works in a very similar way to regular joints, the difference being that with as built joints, components maintain their current positions. |
| 09:24 | It makes things a bit more simple when the components are already in their correct place, like what we have with the rest of our assembly. |
| 09:33 | Use of the joint origin is also a bit easier since the components are already where we need them. |
| 09:38 | We just need to select the joint origin that's common to both components rather than one for each. |
| 09:44 | In our case, we won't need a joint origin at all for the tube and upper internal flange, since we'll use a rigid joint with no movement. |
| 09:53 | Next we also have the ability to create a rigid group and we'll use that for the rest of our assembly. |
| 09:59 | This just locks the position of all the selected components relative to each other. |
| 10:04 | So if we ever move one or create a joint after this, they'll all maintain their relative position and move together. |
| 10:12 | Let's just choose both the internal component flanges and the lower exhaust tube since one of these flanges is joined to the upper tube which is also joined to the external component flange. |
| 10:24 | Now if we unground the upper tube and move any component, we can see that they all move together as a rigid group. |
| 10:31 | Finally let's look at a recent addition to Fusion 360, the tangent relationship. |
| 10:37 | As you might recall, we discussed the tangent constraint for our sketches as well as our datum planes. |
| 10:43 | As a refresher, this refers to a plane, straight line or even a curve that just touches another curve but if extended along the same trajectory, doesn't pass through it. |
| 10:54 | This is the same for our assemblies and we can add a tangent relationship between the flat or curved face of one component and the curved face of another. |
| 11:04 | This is a fairly simple tool which will usually need to be used with other joints or rigid groups to fully constrain the components. |
| 11:12 | It can be quite useful though, especially when working with tubing and sheet metal which as we know is common in performance automotive applications. |
| 11:21 | And that wraps up the fundamental knowledge required for assemblies in Fusion 360 so let's quickly recap this module. |
| 11:29 | Assembly constraints in Fusion 360 are referred to as joints. |
| 11:34 | These are a way of defining the position and motion of components relative to one another. |
| 11:38 | I recommend grounding one component to lock its position in space first. |
| 11:44 | This way we can clearly see how other components move relative to it. |
| 11:48 | We can them make the joint between two components, specifying the joint origin for each component. |
| 11:55 | These points will coincide and become the point that defines the geometry that relates the components. |
| 12:02 | For example, the components will rotate about this point relative to one another. |
| 12:07 | From here, we can define the position of the component and specify the joint type, of which there are quite a few to choose from. |
| 12:15 | Each releases certain degrees of freedom for different motion around or along axes that we choose. |
| 12:22 | As built joints are very similar, but work with the current positions of the components, making the process of placing the joint origin a bit more simple. |
| 12:31 | If our components are already where we need them to be relative to one another, and we don't want any relative movement, then forming a rigid groove is a nice and quick way to lock them all together. |
