Join Thom Tremblay for an in-depth discussion in this video Joining components, part of Fusion 360: Designing for Metal.
- [Instructor] It's important to understand how a multi-part design's components relate and connect to each other and what can move and what cannot. Joints allow you to test how a design will fit together. Fasteners which hold these components together are not something you should model, so we'll use a well-known catalog to bring in the purchased parts for the design as well. Opening the 01-03 design file we have the components of the assembly on the screen but not in the proper location.
We use joints to put them in place but before we do that I want to establish one of the components as being grounded so that its motion will not be allowed. I'll hover over the bottom component, right click and select Ground from the Context menu. Then from the assemble tool, I'll start the joint tool. We also see that there's a J shortcut key for joint. When I start the tool, the bottom component goes into a hidden mode. This is for two reasons.
One, it's grounded so it can't move, two, so it can't be selected as the first element, you should always select the part that will be moving or changing location to create a joint. This particular joint will be a bit more of a challenge. What we want to do is center the hinge portion of the top component on the hinge portion of the bottom component but there's no geometry here. Fusion has the ability to do a between two faces option where I can select two of the faces on the top component and then select an edge that will build an origin joint in the proper location as shown by the icon on the screen.
Once I've selected that, I can move to the bottom component and select a point on the face or in this case, in the middle of the cylindrical face for the second joint origin. I'll make that selection and the component will relocate. When it does, you'll get a shaking preview which shows that if one part moves, the other part moves. The way joints work is they automatically remove all degrees of freedom but you have the option through the dialog to change the motion type to release degrees of freedom.
Presently the rigid constraint removes all three translational and all three rotational degrees of freedom. By selecting revolute, it will release one of the rotational degrees of freedom allowing the top component to swing around the hinge. You have options including the ability to offset the position either through the dialog or by dragging the manipulators or you can even change which axis is freed up by the revolute joint.
In this case, everything is as I want it, so I'll select OK to place the joint. Take a look at what the assembly looks like now and it's exactly what I would expect including the ability to click and drag that top component. I'll continue to use the joint tool and it gives me an indication that one of the components has been moved. When I move the top component, I shifted it out of the position that was originally established.
I can capture this position which can be valuable at times but in this case I'll simply tell it to continue which will slightly shift the position of the top component and allow me to begin my selection. I'll select near the end of the pin and the end of the hole in the top component. It will slide it into position and you'll see that it's applying a revolute joint because that was the last thing that was applied. I'll change it to a rigid joint so that it's pressed into the top component.
Then click OK to finish the joint. The next thing I'd like to do is to locate the pin in the bottom component. The pin, however, was modeled exactly where I need it to be, so rather than moving things around or having to go through a lot of selection options, Fusion 360 has a great tool for when you design things right where they need to be even if there isn't as obvious a relationship as this pin and bottom component have, you can create what's called an as-built joint.
As-built joints allow you to use all the same options but the selection process is a little different. You simply select the components that you want to connect and then establish the motion type. Now, because I need this pin to be able to revolve, I'll select revolute and then I'll need to select a position. If I were to select this point, the pin would be allowed to revolve around this point which is not proper, so what I'll do is select one of the circular edges and we can see if I rotate this and play and animate the joint again that the hole spins past the opening, so I know that the motion is correct to allow the threaded hole to eventually align with the opening.
I'll click OK to place it and for now I'm all set. What I need to complete my design are two purchased components. I need a washer and a bolt but rather than modeling a washer and modeling a bolt, these are purchased items, so I want to make sure I'm getting the right geometry for what I can order. I'll go under the Insert pull down and select the Insert McMaster-Carr Component. When the McMaster-Carr Component library opens, you see there's a broad selection of options that are available.
Not all of them have 3D models but the most important ones do. There's also a great selection filter option, so I'll choose washers, see the wide variety of basic washers that are available and I can narrow by category. I can say that I want a flat washer, I want to use a metric system of measurement. I want a washer sized for an M5 and then I can choose a material or an OD. I'll select stainless steel and it will give me the options.
The type that I need is an 18-8. Here is the part number that I would use to order them but I can go to the product detail, move down, see the actual dimensions of the product and I can select a 3D step file, select Save and it will bring in a model of the geometry. I'll click OK to place the model in my design and now I'll apply a joint to that.
I'll press the J key, grab the circular edge and something I'd like to point out about adding joints is as you move over a face, you might see a large number of options. The triangles denote a midpoint, the circles denote a point, an endpoint or a junction. If we look closely we can see that there is a cross in the middle of the radius and there is a square at the centroid of the face.
If you have difficulty selecting the right thing, you can hold the command for Mac or control for Windows and it will isolate those options to only that face. So, here I'll select the centroid, it will relocate the washer but I don't want that to be a rigid joint. What I want to be able to do is have it move any way it wants along that face which is a planer relationship, so I'll select planer, click OK and it's located properly.
Next, I'll return to the McMaster-Carr library, go to Screws and Bolts, Socket Head, use the same filtering mechanisms for metric, M5. Then I can even change any of the specifications, including filtering down to length. So, here are the options that I have for length including one with the proper material. I'll select the part number again.
Once again choose the product detail and since I've already chosen 3D step as my standard, it will remember that and allow me to click Save to add the part to my assembly. The bolt will be dropped in place and I'll use the joint tool to locate it first, align it to the washer. You'll see that we're still using a planer constraint. I'll change that to a revolute joint and then use the flip option to put at the right direction.
I'll click OK to finish that joint and the next thing I want to do is a little more challenging. The browser in Fusion 360 allows us to change the visibility or the activity of any component. I'll simply turn the bottom component off, start the joint tool again, select a curved edge on the bolt and find the proper face on the hole in my pin and because I need this to be able to translate in and out of that hole, I need to change this from a revolute joint to a cylindrical joint so it can spin and move.
I'll click OK, the assembly will come back together, I'll turn the bottom back on and I can see how everything moves. Now, an additional option that I have when placing joints which are collected in the component that they're added to, I'll select that first revolute joint and use the additional option of controlling the range of motion. I'll tell it that it can start out at zero and move all the way to 180 degrees but that I normally want it to rest at zero.
Can animate how that would look and lock that in, so now if I grab this, I can lift it up. The behavior of the bolt will be a little out of the ordinary but it is proper and when I release, the top component will go right back into position and now I have my completed assembly. If you've done assembly modeling in other tools, joints might take a little getting used to. When you've adjusted though, be prepared to be asking yourself why you haven't already been or aren't able to use them in your other software.
- Setting up parameters
- Joining components
- Animating and rendering the design
- Testing alternative materials
- Creating the setup
- Publishing and posting the design