Turbocharge How You Design and Manage Large Assemblies in Autodesk Fusion 360

JACOB WEINSTOCK: Hello, and welcome to my presentation. The presentation is called "Turbocharge How You Design and Manage Large Assemblies in Fusion 360." My name is Jacob, and I'm a Manufacturing Data and Process Insights Engineer at Autodesk. So the three main class themes we're going to focus on is some large assembly basics; some modeling techniques, where I'm going to show you a live demo in Fusion; and then, collaboration.

And I'm going to show you some demos in Fusion Team and the Fusion Manage Extension, as well. So some of these concepts I'm going to be talking about and showing you how to do in Fusion, I actually used on a project we did internally Autodesk called Project Vesuvius. And you can see a picture of the large machine-looking thing there on the image.

This is a large 3D printer. And we had, I think, about 20 people working on the project. Some were designers. Some were manufacturing engineers. People did simulation, a whole broad range of team, broad team. And I think we had over 3,000 components in this assembly. And that included pre-bought components that we got off the shelves, some custom components, some electronics, et cetera.

So this is definitely a large assembly, I would say. And these techniques I'm going to be talking to you about are the ones that we tried to use when designing and managing this project. So the first question you might be asking yourself is, what is a large assembly? And the answer to that is, it depends. There's no strict dictionary definition of what a large assembly actually is.

I would say some of the key things that you might want to think about when saying what a large assembly is the number of components, the complexity of components. So for example, let's say you had 1,000 plain disks, that might not be as complicated as something with 50 very complex shapes with some generative shapes in there, et cetera.

So complexity of components also comes in. It might also depend on your industry. So for example, if you're a product designer working on radios, if there is any product designers doing that anymore, your assemblies might not be as large as someone who works in the automotive industry. And then, those assemblies might not be as large as the ones in aerospace or construction.

So sometimes, it depends on what type of projects you're naturally working on is what you would consider large processing power. So for example, if your PC is quite old, you might not have a good processor. So you might open an assembly with, let's just say, for example 50 components. And you might see some slight lag.

However, if someone had a very new computer with a great CPU and GPU, et cetera, you might be able to handle 500 components without noticing any lag. So that's another factor that it comes in. Also, the other obvious one is the physical size. Let's say you're working on a radio versus a whole building. The physical size of the building is much larger.

And that also could be considered a large assembly, based on size. My definition that I am going to give for the purpose of this presentation and the Fusion definition, I would say, the Fusion 360 definition is any assembly where performance is not noticeably decreased. So you might have an assembly opened, depending on your PC power, as I mentioned before, depending on the complexity of parts. If you're manipulating that assembly, moving it around, panning, zooming, et cetera and you notice some lag or some kind of stuttering, I would consider that a large assembly for your particular setup.

So what can we actually do to work more efficiently with these large assemblies? There are several techniques that we can employ that I'm going to talk to you about. Some of those are the way you actually modeled the components, put them together in an assembly. And then, also, perhaps not as a technical focused, but something about managing is if you're in a large team, like we were been working on that large 3D printer, how do you know who's working on what?

How do you know what the current version of the component is? And these things can be important, because if there's thousands of components, it's easy to forget the name of them. It's easy to forget who's working on what, when those parts are kind of due for manufacture, et cetera. So I'm going to go over some ways we can manage those inside Fusion Team and the Manage extension. Cool.

So the first thing I want to talk to you about is the difference between bottom-up modeling and top-down modeling. And you can see on the left there, a graphic on the bottom up. And the way this works is you would model each individual component in its own separate Fusion 360 file. So I've got the example here of three simple blocks.

And these are the simple examples I'm going to show you in Fusion. But they can be applied to any assembly, any number of components, any type of industry, et cetera. But I'm going to show you a simplified version for the purpose of the demonstration. And as I mentioned, you can model them individually and then put them together in a separate file to build the assembly.

The second variation is something called top-down modeling. And in this particular variation, you would model all the components in one file, rather than separately. And each one has its own advantage and disadvantage. The advantage of bottom-up modeling is, if you have several people working on the project, each person can work on the individual file.

However, a weakness might be, you might not be able to reference previous components to use in your current one, so things like dimensions, et cetera. With top-down modeling, you have the advantage that you can reference previous geometry. But because it's only one file, if you only have one person working on it at each time-- because in Fusion, right now, if you have a part open, that part becomes reserved.

So in other words, only one person can work on it and save. So there's advantages and disadvantages of each one. So I'm now going to switch to Fusion and show you how to do each one in the simple block example I've showed here. I'm going to show creating a new component and then adding it to the assembly. So if I switch to Fusion. Cool.

So the first example, I'm going to show you is the bottom-up example. So you can see on the left-hand side here, I've got a project where I have three individual blocks, and then another file for the assembly. So I'm going to basically create a new block and add it to that assembly using the bottom-up method. So it's very simple. Let's just create a sketch on this plane.

Let's create a rectangle. There we go. And let's do 50 by 50. Cool, very simple sketch. Let's extrude that 50 millimeters up. Cool. That's all we're going to do for the purpose of the demonstration. So let's save this into the correct folder. There we go. So let's save it in here. So you can see here, it's appeared in my browser view.

So I'm now going to open the assembly that I premade earlier, but I'm going to show you how to add a new component to this assembly. So it's as simple as clicking the assembly, dragging it in, letting it appear. And then, what we're going to do is, we're going to roughly move it into position. And then, we're going to put it into position properly. So to do that, you go to Assemble, Joint.

And then, let's click the bottom of the block. Whoops, click the bottom of the box. And then, click the top of this one. You see how the block moves down into the correct place. Cool. So now, we have an assembly with four separate components. And you can kind of see this if it saves. There we go, cool. So you can see here, we have these chains.

And that's basically showing that each component is referenced to a separate one. So that's the bottom-up method. I'm now going to show you the top-down method. And you can kind of see a difference, and the advantage, and disadvantage of each, and sort of decide yourself where you might see in the large assembly to use each one. So if I go back to my top-down method, cool, let's just close the previous one.

So you can see here, the differences. Instead of those chains linking each individual component, each block is created in a single file. And what that means is, if I create a sketch here on the top of this yellow one, I can actually project-- so pressing P and then clicking the top of the square-- project the previous block. So the advantage of this is, you can see how it's automatically got the size of that yellow block.

And if that yellow block were to change, it would then change the block on top. And that's not something you can do in the previous approach. So if I press Finish, I can now extrude that sketch. It's automatically selected it for me. So let's do it to 50 millimeters. Something key to look out for here is it's defaulted to join. But we want it to be a new component.

So if you open this window up, here, then press New Component, that's OK. Cool. Now, we have a new component in the window, here, we can see. And it's automatically in place. We don't have to place a joint. So as I said before, there is advantages and disadvantages to each approach. So to summarize the previous one, each person can work on each part and then combine them together, but you can't reference previous geometry. Whereas this approach, you can reference the geometry, but you only have one person working on it at one point.

So wouldn't it be great if there was-- I'm just going to say this. Wouldn't it be great if there was an approach that could combine the best of both worlds, where you could reference geometry-- so if that geometry changed, the subsequent geometry also changed, but you can also have individual people working on each component on their own. So if I switch back to my presentation, this third approach is something known as skeleton modeling.

So you can see the graphic here, we can see how you have this very basic skeleton model, which I'm going to show you, which is basically made up of sketches, and planes, and no 3D geometry. Is just a skeleton, so just sketches to position and outline the assembly you're making. You can then reference that skeleton model into individual parts and then combine them together afterwards.

So the advantage is, each person can work on the individual part. But there's still reference to a common geometry. So if I change back to Fusion. And you can see here. So the example I'm going to show you is almost finished. We're just going to add one more component. We're going to add, on this vise assembly, we're going to add another plate on this side.

So at first glance, you might think this is the same as the previous approach, with individual components imported in. However, the difference is, we have this skeleton model, which I'm going to open. So this is just a very basic sketch, or a few sketches, that define the shape and position of each component. So this would be something that's made and saved.

And then, if now, I created a blank component, I can come up here to Insert and then Insert Derive. Let's save it first. So let's call it Vise Plate. Save it in the right folder. Cool. So now, it's saying Select the Source. So this is where you would select that skeleton model I showed before. So here it is by skeleton, Select.

That's going to open up that previous component. And now, you select what you want to basically derive or import to this new file. So we want to import everything, basically. We're just going to import all of these different sketches, which I've named, just to make it clear what each one does. So I can do that. And then when I press OK, you see here how the sketch is imported into our vise plate component.

Excuse me. If this were to change when you would update this file, this would also change. So that's good about this approach, is it keeps a common reference that filters through to each individual component subsequently. Cool. Yes, I mentioned we're going to make that plate.

So this is kind of a side view of that plate we're going to make. So we're going to click Extrude. We're going to select that profile, here. Then, we're going to go-- instead of distance, we're going to go 2. Then, this sketch at the bottom here-- this one defines the width of the device. So again, if that were to change, it would subsequently change this extrude.

So we're going to select the end of it. But we want it to go both sides, so we're going to go two sides, side two would go here. Cool. So that's basically created us the plate with the right width, and the right position, the right height, et cetera from that reference geometry. So I'm going to press OK. The plate also needs some holes in.

So this line here, this defines the position of those holes. So I'm going to create a sketch on this surface, here. I'm going to project that skeleton line, here, then draw two circles. So that's very obviously a very simple example. But as I mentioned, this approach can be used on very complex models. Even on subassemblies, which are then combined together to make a larger assembly.

Cool. So let's just extrude the holes. Nice. So we have the plate, there. So I'm going to save that. If I go back to the assembly component-- so now we want to basically import that vise into the assembly-- so very similar to-- where did I-- did I not save that in the right place? I didn't, did I? It doesn't matter.

Let's go here. Save it in the right place. It didn't matter, I'm just trying to keep this tidy. I did save it in the right place. I was talking rubbish. It doesn't matter. So this is the vise plate. So if I want to bring that in, I just again, select it, drag and drop, place it in. And you can see how it's in the correct place, and the holes are lined up to those holes here.

And these holes on this component were also driven from that skeleton sketch. So as I mentioned before, if that were to change, it would change both components at the same time. So this is the approach I would recommend if you can. I know it would take a bit of time to create that initial skeleton sketch. But in the long run, it will probably save you the hassle of having to change multiple components, going through hundreds of components, even.

And like I said, changing them individually, that would take quite a long time. Cool. Let's just save this and close out of some of these windows. So the next thing you might encounter with components that are a high face count is lag, basically. Especially if you have, let's say on this example, you have this gear. If you have to keep the gear as it is right now, fully modeled or modeled thread-- let's say you were 3D printing it, so you needed that thread there.

And you had, I don't know, 100 of them in your particular assembly, you could have a lot of faces. So the face count is the key thing with models, where if you have a high number of faces, you're going to experience slowness. So that's why I can see the turtle, here. So if it's just for representation purposes and not for actual-- like I said before, say you weren't 3D printing it, it was just a quick review of the design.

It would be handy to simplify this geometry into something that's representative, but not as high face count. So you can see how using this disk here, it only has four faces. So that's going to be much quicker to manipulate and pan around, et cetera, than the full model. So what are some of the ways or good ways to do this? Is if I go back to my Fusion 360, just close some of these out.

So if I go to-- here it is. So you can see, if I have one of these gears, it would be OK. But let's say, as I mentioned before, you had hundreds and hundreds, things are going to start to lag. So what are some of the good ways to simplify this but keep a reference to the actual component? So let's say this gear was changed to be a larger diameter or thicker, et cetera.

Thicker that way, how do we keep a nice reference to the simplified version but also have it simplified. So that's what I'm going to show you now. So again, we're going to make a new file. We're going to save it, let's call it gear, whoops, simple version. Save it in the right folder this time. So similar to the previous thing, we're going to go into and then derive.

And then, we're going to find the actual model. So this is that gear, there. And what I've done in this model beforehand is, I've just created a basic kind of doughnut-shaped sketch, which is projected from the tip of the gear, here that sort of purple you can hopefully see and also the inner threaded hole. So because they're projected, if they were to change size, the projected sketch would also then subsequently change size.

So always try and project, rather than just creating a sketch freehand. So we're going to derive that sketch, basically. But you can kind of see how we have the sketch selected. But how do we ensure that the thickness of the gear is also imported across? So to do that, we have created a parameter for-- we've created a parameter for that thickness.

So if you go in your Parameter window under Modify, you can see this Extrude1 distance. And I've renamed it gear thickness, just so I kind of know what it actually is. Then, I favorited it with the star. And you can see here how because it's favorited, it would appear at the top, just because that's the one we're going to be importing a reference to into this simplified version.

And so I'll just close this out. Let's do that process again. Now, you've seen the parameter. So Insert Derive. There we go. And Gear Select. Just save that because I made a change. Or I turned the sketch on, which is counting as a change. So we're going to import that sketch I mentioned before, we're also going to import our favorite parameters.

So if you drop down this here, pick favorites, it's going to import that thickness value into our simplified version. Then press OK. Cool. So let's turn the sketch on. So you can see there how we have the doughnut-shaped sketch. And I can-- just to remind myself, the parameter was called-- why hasn't it imported the parameter?

Let's do that again, it's fine. Insert, Derive, Gear, Select. Why isn't it doing it? Sketches, Favorites. Hopefully now, we should see-- nice. So we have that gear reference there, that 12 millimeter thickness. So I can favorite this, add it to the favorites on the simplified version.

So we have the name as Gear_Thickness_Ref, so it automatically adds the Ref to show that it's a referenced parameter, basically. So I'm just going to remember that, so Gear_Thickness_Ref. And then, go back to our sketch, here, Extrude. And instead of adding a distance, I'm going to-- just if I type G, it automatically will show me that favorited parameter.

So if I click that and press OK, you can see the line there. It's given me the 12 millimeter. So that's good. So that's showing that it's basically imported a reference to that previous extrusion thickness into this component. So if, let's just say, I save this and go back to this model-- if I were to go to my parameters and change it from 12 to, let's just say 15, for example, press OK.

Cool. So you can see how it's got slightly thicker, there, and I save. And then, here, it's given me this warning, which is fine. It's perfectly normal. It's basically saying that the derived import is out of date. So what we can do is, we can press that warning up here, give it a bit of time to think. And then, you can see how it's changed our thickness to what we changed it to in the actual component.

So that's the benefit of doing the derive as I showed on the previous demonstration, is it was always keep a reference to the actual component that you're working on. Great. So that's kind of showing you how to simplify a model. So so far, we've gone over different approaches for creating the assembly. We've gone over how to simplify models to speed up processing, because if you have a component with a large face count, you're going to experience some lag.

And the final thing I'm going to talk to you about-- I'll go back to my presentation-- is not something to do with modeling, or CAD, or design. It's more about how to manage the assembly and ensure that communication in the team is up to date and people know what they're doing, basically. Because if you have a lot of people working on the assembly, you have a lot of components on the assembly, it's easy to lose track of what needs to be changed and what needs to be made.

So for example, let's say you're making a component, but you need to specify a certain tolerance. And you want to inform the machinist on that tolerance in a nice way that he can go on and see and refer to when he's creating his CAM programming. How do we do that? So I'm going to show you a way to do that in a Fusion Team. So this is the webview of Fusion Team you can access in any browser as long as you're subscribed to Fusion Team.

I'm going to go back to that component I mentioned before, the assembly I mentioned before, the vise one we were working on. So if I open up the vise block, here, see a little preview, and I press View, it gives me this 3D preview in the browser. So an advantage of this is that someone, in theory, could view it from their phone. Let's say they're on the shop floor and they want to look quickly at a certain CAD file or a certain comment we're going to leave in a second, they don't actually have to have Fusion installed.

So let's say the designer wanted to specify the tolerance of this hole to the machinist in a way that's saved, and traceable, and will stay up to date is in this web view. We can come down here to the toolbar down here and press Comments and then Comment On Point. So you can basically specify the point you want to communicate. So I'm going to click that, and you get this crosshair.

So I'm going to choose this hole at the top, here. Then, I'm going to add a note to the machinists, I'm just going to give him a tolerance for the hole, just so he knows when it comes to machining, he needs to match that tolerance, there. So you can see, , when it comes back, I've added that comment at a certain time, at a certain date.

So what's good is that it shows a reference they can go back to. So we can also-- come on, there we go. Let's say the machinist has seen it. Obviously, I'm going to comment on my own comment. But in reality, it would be someone else. So let's say he's seen it, and he goes, "Thanks for the info," just to show that he's seen it.

So that's what's good about leaving comments in this web view is it will save them, and it will save who sent them, at what time, or what date, et cetera. So this is something that we did with that Vesuvius Project when we wanted to communicate certain tolerances and finishes on the components. But it can be used for anything-- say, if you want to, for example, test different variations of the same hole or something like that.

You might say to the machinist, machine three versions one with an 8 mil hole, one with a 10 millimeter hole, 12 millimeter hole, et cetera. So it's up to you how you want to use these comments. But they are there if you want to. Cool. So the second thing I'm going to show you is how to use a brief overview of the Fusion Manage extension.

So the reason you would use this Manage extension is it shows your team what stage of the design and manufacture process each component is at. Usually in companies, they go from a sort of design stage, to review stage, to a final review stage, and then finally, finally to an actual machining stage. So you want to basically certify throughout that process that the design is correct.

And you might also want to specify things like if a customer has requested a design change, how can you do that in a way that's documented in a nice, efficient way that everyone can see, and it's nice and traceable? So if I go to my Manage folder, here, I have this very basic threaded hexagon example. Again, this is just a basic example, but you can use it in any of your large assemblies, your complex assemblies.

So to access this Manage extension, if you come up to the top here, to the Manage tab, click that. And it's a very simple kind of toolbar. So the first thing you need to do is assign an item number. So this will basically create your component a unique number. So this is good if you want to reference a particular component.

Rather than just saying threaded hexagon, if you said the actual number, that's just more precise in your explanation to the machinists, just so they know what to actually work on. So let's click this. Cool. So it shows me the component that's in the Fusion file. So all I have to do is press Submit.

Generating me a number. Here we go. So it's given me part number 14. And it will basically just keep adding a number to the end of that item number until you reach the max. I'm not sure what happens. So you create your item number, that's the first thing we do. Then, we press Close.

Then, if we come up here to the Release section, you have two options-- the Quick Release or the Release with Change Order. So we can click here. I would recommend using this Change Order option. And I'll show you how that works. So if we click that-- and then, we're going to choose-- it automatically chooses the component we were just working on. And then, we're going to press Create Change Order.

Cool. So this is a window that's then displayed. So I'm going to give the example of-- on this threaded hexagon, let's say a design change needs to be done to change the thread from a M8 to a M10 thread. So that's something you might want to include in the title. So let's call it "M8 to M10 thread change."

So we have that. And then, the approvers-- because there's only myself in this Fusion Team, you're only going to see me. But if you had several people, you might have someone dedicated for the approval process. So you would choose them. But for this example, I'm just going to choose myself. Reason for change-- there's some built-in ones here that you can choose.

So I'm just going to choose functional fix, just for the purpose of this example. You can choose a description and priority, but these aren't required. Only the options with the red asterisks are required. So if you wanted to, you can add some information there. So this second stage here is who the change is going to be rooted to. So in other words, who's the person that's going to actually make this change?

So you can imagine, perhaps an engineering manager might do this approval process. And then, a designer might be the one that actually is informed that they need to make the change. So again, because it's only me and this team, I'm the only one that's displayed. But if you had multiple people, you would see each person.

And once you select them and press Save, they also get emailed just to prod them they have some work to do. So it would say basically, "M8 to M10 thread change," and it will provide them with a link to the component to work on. So we're going to press Save. Great so we created that change order. We'll just close that.

Then, the second part is this lifecycle dropdown. So either you can release it to the actual production or just a pre-production lifecycle process. But for this demonstration, I'm going to do the full release to production lifecycle. So I'm going to press that, press Save. Cool, so I've added that release to production lifecycle to that component.

So now, if we want to actually document the changes that have happened to the design, we can do that from the Fusion 360 Manage web interface. This is what you would see on the main dashboard. If I were to reload this, hopefully you're going to see change order come through. Cool. So you can see here, my outstanding work. So because I selected myself to make the actual change, I'm the one that gets informed of the change to make.

So I can click that. And you can see here all the information that we provided beforehand. And then, there are some options up here. The key one is the approval workflow. So right now, it's in this so-called open stage. So basically, it's been submitted to the Manage extension interface. So say if I wanted to start work on it or I've got around to doing the work, I would then hover my mouse. You can see here, as I'm hovering around, we're getting a blue highlight about what stage to go to.

So the stages are Open then Work, because then I would actually be making the changes. So let's do that. So if I hover my mouse over Submit to Work, then, you can leave some comments if you wanted to. But I'm just going to leave that blank. Cool. So now, you can see how the work box is highlighted.

So this is the stage where the designer would actually make the changes that have been asked of him. And then, if he wanted to, he could put it back to open. But usually, you would click this Submit to Review. So this would then submit the notification to that approval manager. So let's do that.

Cool. So now, we're in this review stage. You can see here on the right-hand side how the workflow history is updating after each button is clicked. And you see who's done what time. Again, because it's only me, you're only going to see my name. But in reality, there will be multiple people working on this, so you would see different people's names doing those workflow changes. So let's say now I'm the I'm the engineering manager.

I would then get a notification that something's been requested for me to review. So I would open the file Fusion-- or in Fusion Team, if I wanted to-- go over those changes the designers made. And either, if I'm not happy, say something doesn't look right. I can then click this Return to Open. And this would basically start the whole process again, where the project must be seen as open, the designer would have to do some work, and then back to review.

But if it all looks good and we're happy with the change that the customer has requested, I can press Approve and Close. In this stage, you have to add a comment. So I'm just going to say, "approved component," for example. Then we're going to go Approve. Cool. So now, we've gone through that process in your company. You can imagine how managing thousands of components, it's sometimes hard to track who's working on, at what time, and at what stage each component is, and if the changes are being submitted.

So using this Fusion 360 Manage interface, it's a great way to manage your large assemblies. So that is the end of my presentation. I hope you learned some good ways to both design technically and also manage your large assemblies. And you can take that away to your own company and hopefully improve your process. So thank you for listening.