Quick Start in Autodesk Fusion 360 for Inventor Users: An Old Dog Teaches New Tricks

JIM SWAIN: Hello. And welcome to Quick Start in Fusion 360 for Inventor users, or as I like to think of it, An old dog teaches some new tricks. My name is Jim Swain and I'm an Applications Consultant with Synergis Technologies. And by that, it means I do a lot of implementation and training. In the past previous lives I've been a design engineer, a test engineer, CAD administrator. I've even taught some plastic part design courses at a local community college.

Through all of that, I've been using CAD honestly since about 1982. So it's been a little while. With that in mind, and I will say that I've been using Inventor since it was introduced, I decided I was going to come up with this class. And the reason for it is about five, six years ago, I started exploring Fusion 360. And I found that Fusion 360 is very similar to Inventor and to other solid modelers that are out there.

But at the same time, it's different enough that it can be very, very frustrating, at least the way I was working on it, it was very frustrating. So what was giving me these problems? Really I boiled them down into about three main areas-- the file structure, meaning the components, the bodies that make up the actual designs; file organization such as projects, teams; and then how you bring the pieces together. As in Fusion, we have joints we don't have assembly constraints. That was a big jump.

Because of that, I developed this class and the official learning objectives are to understand common Fusion 360 design workflows; understand how to build assemblies without using assembly constraints; understand the relationship between sketches, bodies, and components; and then understand teams, project organization, and collaboration possibilities. So let's get started.

Fusion 360, Inventor, let's take a quick comparison, a very high level look at it. First of all, there's similarities. Both are parametric solid modelers. They also include surface modeling, mesh modeling, T-spline modeling. They have similar workflows for creating shapes, start with a sketch, develop it, constrain it, use that to create a feature, and then go back and repeat that add more and more features to your shape till you get what you're looking for.

Also for both of these drawings are separate files, separate from the parts and the assemblies. Projects are used to set up the search paths for the software to know where to look for components that are being brought together to make higher level components, parts coming in the sub-assemblies, sub-assemblies for higher level assemblies, and so on, and so on.

Now, let's look at some of the differences. So this is going to be looking at it from Fusion 360's point of view. And the first one really is the file organization. Inventor, storing on some kind of network, local drive, something along those lines. In Inventor, everything's inside the firewall. In Fusion, you're storing on the cloud. Now you're in the secure cloud, Amazon Web Services I believe is where things are, but high level of security but it's not inside your firewall.

In Fusion, you've got a single design file, whereas in Inventor you've got part files and then you also have assembly files. And both of those are called components typically in the Inventor workflow.

Also in Fusion, solid bodies are a lot more obvious than what you've got when you're working in Inventor. Inventor you are building solid bodies, but they're not really noticeable. They're tucked up in a folder, up in the browser. You may never notice it unless you specifically go and work on a multi solid body workflow.

In Fusion, the timeline is separate from the browser. The timeline is where you go to edit features such as extrusions or revolves. In Inventor and the other softwares I've seen, the browser is also the timeline. It's the history, that rolled into one. Whereas there are two separate jobs in Fusion 360, two separate tools.

The assembly structure is a little bit different in Fusion 360 in that you can have both internal and external components. In Inventor, you can only have external components that you're linking in as you build up your assembly structure. And also as I mentioned before, Fusion 360 you have joints. You do not have assembly constraints. And that was probably the first big tripping point for me.

Good news is once you get used to joints with Fusion 360, you can go back and apply that to the Inventor because Inventor has joints, has had them for well over a decade now. Now Fusion 360 is not as mature product as Inventor is. Inventor, they developed the frame generator over the years, routed systems such as tube and pipe, cable and wire harness.

Flip side though, Fusion 360 has built in electronic CAD, circuit board design. It has much more in the way of simulation tools compared to basic Inventor, has much more in the way of CAM, computer aided manufacturing tools, compared to Inventor. So a lot of similarities, but a lot of differences as well. And as I said before, it was those differences that tripped me up and caused me a lot of frustration in the early days I was using Fusion 360.

So let's start off by taking a look at the file organization. And by that I mean, how is it stored up in the cloud. So in Fusion 360 I'm going to use a file cabinet analogy. And Inventor, I'm just going to talk about Inventor because at this point I'm assuming you're used to it. I've been using Inventor, like I said, since the late '90s. So it should be a fairly familiar environment.

In Fusion 360, I start off at the highest level with a team, if you want to think of a team as a file cabinet or a room full of file cabinets. And the reason why I use the idea of the room is you have to be invited into the room. So I can create a team. I can own a team. My account can own a single team. But I can be invited into many other teams. I have full control of my team. And as I said, I can invite anybody into it that I wish. I don't really have the equivalent at the Inventor level.

Projects, well projects with this file cabinet analogy, think of it in terms of the actual pull-out drawer in the file cabinet. In Inventor, projects, their main reason for being is to set up the search paths so that the software knows when you open up the assembly where to find all the parts and sub-assemblies that are needed for the assembly.

Both softwares have the ability to have folders. In Inventor, those folders are typically underneath the project files folder. So they're already part of the project search path, not always, but typically. In Fusion 360, the same thing. You have the project and then you'll put folders underneath to help organize your data, exact same purpose.

And then finally, call them components. In Inventor we've been calling components using that phrase for part files, for assembly files. Both have been called components. In Fusion 360, take that a little further. It's not only the part or assembly but the design file can be both. It can be just a part. It can be just an assembly.

But in Inventor, you've got the iProperties, same type of thing with the components within the design file in Fusion 360, also the analysis tools, also the CAM tools. So you have the body. You've got the metadata. All of that's held in that design file.

I like the visual of the file cabinet, so let me just hit it a little bit harder here. The Fusion team is the file cabinet itself. And you can lock it. You get to invite people into your team. Other people can invite you.

The project, it's a drawer in that file cabinet. You open up that drawer. Here's all the folders that are inside of there to help organize things. And projects can be set up where they're typically run as a closed project, so that you have to be invited into the project before you can see anything within that project.

Also right now in the educational market, in the educational accounts, folders can be set up to be very permission based. Think of setting up a classroom. You can have a project for a given class and then a folder for each student in that. And that student can only see the information in that particular folder that's assigned to them.

Similarly, you could have a folder set up for a small design group. And everybody in that design group can see only what's in that folder, not in other people's folder, so folder level permissions.

The design file, like I said, it holds the design data. So just to reiterate, folder level projects are only right now for the educational accounts. And the extra data includes the solid bodies, the CAM, the simulation, the bill of material information-- all of that in that envelope. And of course, all of that is stored up in the cloud. Bear in mind you're working at local but whenever you do a save, you're saving it up to the cloud at that point.

Now, I've got three sons. They all have different learning styles. So I just want to show the same type of information in a more organized chart form, where you've got Fusion team. Then you have projects where you're managing the data, and then folders to organize within there, and again, all in the cloud.

Now, how do we see this from the design point of view? Well, if I take a look at it from the design tool itself, and specifically I'm going to look at the data panel, which is that left-hand gray area. In fact here, there are the arrows pointing at the listing for the team, what team is currently active in that upper left-hand corner of the data panel.

If you don't see the data panel when you fire up Fusion 360, there is a tic-tac-toe button, Chiclet button, whatever you want to call it-- 3 by 3 square of little blocks in the upper left-hand corner. And you can click on that to turn on or hide the data panel.

I'm going to expand the look of the data panel so you get a better idea of what's going on. From here, I can see that I'm currently looking in a team called Jim Swain Edu Team. Just like Inventor, if you go to close a project file in Inventor, you need to shut down all of the open design files, all the parts, assemblies, drawings, et cetera.

You can't shift from one project to another project with any design files open in Inventor. Same thing applies here. I can't go from one team to another team with any design files open. I've got to close that cabinet drawer before I can open another one. Actually, I have to close it before I can leave the room, a little better.

The projects, there I'm currently in the Project AU 2023. And the project is that first level where with a commercial or hobby style of Fusion 360 account I can invite people and control who sees that. So invite into the team. Somebody must accept the team invitation. Then they can be invited and assigned roles within a given project.

Continuing down, there's a folder. This one is holding all the design files for the floor jack. Beneath it we've got the Inventor chassis files, locomotive, so on. And then design files, design files they might be down in the folder. And I recommend it. But here I've got some that are just sitting right at the project level, a little bit sloppy, but certainly allowed by the software.

As I said before, you can have internal components. There you can see components listed in the browser. These happen to be part files for the caster, and the body, and the axle, swivel axle, but then an assembly component for the wheel assembly. That's my choice of names, not the software adding assembly.

I could also have external components. External components will show up as a link. This is what you're used to from Inventor, linking in those outside files into your assembly to build things. So Fusion 360, internal and external components can be brought together to complete your design.

I can also look at this purely from the web point of view, from the cloud, and go directly there. There's my team listing Jim Swain Edu Team, a little bit small to read there. What's big underneath it is the active project.

And then there's the folders, and the design files, and they're shown both in that left-hand area and also in that big central area. Folders show up as well as the different design files.

So in the actual product, the way this would look, and refresh. So here I am in Fusion 360 design tool. I've got these internal components. And there's the wheel assembly with the internal parts that made that up. But if I had a need to, I could certainly go and drag in another part. I'm not going to worry about where it's placed for right now. And you can see how that is showing the link to the outside.

I have the ability to edit in place just like with Inventor. And it will reach out and make the changes to the outside design file. But I don't really have a need for that. I'm also going to go and delete this right away. I don't want to have it cluttering up the design at this point.

To get out to the web, I've got the globe up here. Open it on the web. And that'll fire up a browser. So now I have to go over and get it from my browser. So let me drag that on over so I can see it on the screen. And I think it's behind. So let's go swing it in front.

That's a little bit lost. There we go. And here it is. So I'll pull that up. Again, here's the team that I'm currently in. Here's the project there. The project is also there. There's the folders and components in the data panel look again. Here it is in the main window. And if I hit the Home button here, I start seeing a list of all the projects that are going on.

So I'll go ahead and shrink that back out. OK, back to the slideshow.

The actual structure of the design files, so the sketches, the bodies, the components. Probably the first thing you went into when you started Fusion 360, you fired it up, started sketching, started making features. And then kind of said, what's going on here?

So in Fusion 360, first of all, you only have one design file. There's no part file. There's no assembly file, just a design file.f3d if you ever export it. In that design file you have components, bodies, metadata, data from the other workspaces like the CAM workspace, or the simulation workspace, or the animation. Think of it as exploded views. You also have any drawing files.

Compare that to Inventor, well in Inventor typically you're going to have things like part files, assembly files, project files, drawing files, exploded view files, presentation files. You can also have others-- design elements, iFeatures, that type of thing. So at a basic point of view, I'm getting one design file to do the work of parts, and assemblies, and exploded views, and then drawings are their own separate beast.

File size, by the way, still in Fusion 360, as I've explored it with this caster, much smaller in the Fusion world. Now, trying to organize things the right way, you are only in this class if you've already been frustrated. So how to avoid the frustration right off the bat? In a lot of online videos, blogs, and so on, people will talk about something called Rule 1. And here is what Rule 1 is.

In Rule 1, when you start a brand new design file, right now that's the swivel caster. I know brand new, and it's at version 4. Don't worry about it. The name is at the top, because I started a new design. Hit Save. It's also now at the top of the browser as well, that top browser note.

Right away, you've got a component. And actually, I'll be going through the workflow in just a minute for Rule 1. I got a little ahead of myself there. So the design file, you have components. And what I want you to do here is start noticing what is the active component.

So the active component is the one that's got the little bull's eye, the arrow is pointing to here. That is the piece that you are editing. If I bring another part in from the outside world, that external one, it gets added to in this case the caster body, and also the caster body is an assembly. You pay attention to where that bull's eye sits. That is a just good habit to get into.

If you get it wrong, catch it right away. Undo works fine. But pay attention to what has the active bull's eye. Then start building your volumes. You'll be working with bodies, just like you are in Inventor. But you're going to start with the component first.

Now something that's a little bit different, in Inventor I can only assign materials to a part file. I can do appearances to bodies, to faces, things like that. In Fusion 360, I can assign appearances just like in Inventor. But materials can be applied to bodies. It's a little bit unnerving I guess. It was hammered in my head for years that in a part file that's where the material is in Inventor.

Now, this is a little more flexible. I can start adding the material to a given body at that point, one there, or one there, different materials. I still think the best workflow is to keep the materials at the component level. Because that's what you're going to see at the bill of materials. So I think that follows through very nicely.

All right, so swinging back to the workflow. Rule 1, start a new design file. Immediately create a component. Create that envelope to hold that information. And when you do it that way, the sketches will be part of that component. And you'll see what that's going to be like in just a minute. Activate the desired component. Well, actually that will take place automatically if you use the new Component button.

Create your sketches and features in that active component, and then repeat that to get the final shape that you're looking for, the final volume. As I said, this keeps the sketches, the bodies, within that component, much easier to troubleshoot. Down on the timeline, you can see down there that all the information is lined up nice across there. Also keep in mind that timelines where you need to go to edit the features, not in the browser like in Inventor. It's down on the timeline.

If you ignore it or as I like to say let's play a game called whose sketch is it anyway? If you ignore Rule 1, and you just start making sketches, making features, then the design file, that top node in the browser owns everything-- all the sketches, all the features. You can still make components. So it sounds like you can get out of jail free.

No, not free. Because all of those sketches and features are still owned by the design file itself. And even if you activate that piece like the caster body, you don't see anything. All you see is that a component was created. If you export that all you see is a base solid. So you set yourself up for not a fun situation, hard to tell who's sketch is controlling which feature on which body. Putting them in the separate components right from the beginning avoids all of that.

Now something that can also help you is in the inspection area, you can drop down the list and turn on what's called Display Component Colors. Actually if you hit n, Shift n, it will toggle that on or off. And what you'll see are pastel colors applied to all the components on your screen. I think there's about eight pastel colors. So you'll get some colors reused. But those colors will match up with those pieces in the browser, and it will also match up with those features down in the timeline. So it can be a really handy thing to tell who belongs to what.

You can toggle the colors on and off. You can't edit them. What you see is what you get. So it's like the driveway chalks my granddaughter likes playing with, very much like those actually. So let's take a look at that in the design tool.

I'll go and start a new design. I'll hit Save right away, because it's CAD, save early, save often. Just say-- there we go, saving it to that project. And you'll see it down here showing up in the browser. And that's the name now applied to the tab up in the application bar. It's also here. And immediately I go and hit New Component. I'm just going to leave it at Component 1. I'm not feeling all that creative with my names right now, so we'll leave it alone. Notice it's going to activate it right away.

Now I'm down in Component 1. Right away there's the bull's eye. It's got its own origin. When I start a sketch, and I'll just put it on the xy plane, and just draw something a little bit here, nothing real fancy. Similar sketch tools to what you're used to in Inventor, a little different look, but very similar.

And it's creating a brand new body in the browser. There's the component with its own origin. Currently one body, currently one sketch down in the timeline. I can edit the sketch. And I can also edit the feature.

When I want to go and do another component, activate the top level component, and then hit New Component. If I didn't activate the top level, Component 1 would all of a sudden turn into a sub-assembly. That's the clue. The icon changed from a single brick to the stack of bricks. Undo, activate this, and go on and sure, Component 2. That will work for now. Notice both of these are internal components.

I'll put my sketch on there. I don't think I'm going to impress anybody with my modeling skills today. There we go. And then maybe I change this material to, we'll just go to ABS. And if I go back and activate the top, now I see everything.

Down in the timeline, we've got Component 1 has got that kind of a peach color. Actually, rephrase that. That operation took place. The overall design file has the peach. So that was creating that first component. That took place at the top level. Once I was down in the yellow for Component 1, that's the work that was going on. Then I went back to the top level, created new component, and now in Component 2 it's that light blue.

Notice if I go into a given component, all I see in the timeline are those sketches and features that are used to make up that particular component. And also on the main screen, that component is the only one that's still full intensity, very much like edit plays in Inventor. Just all these are internal.

OK. Now as I said before, we don't have assembly constraints. So we better figure out what we do have. What we have are joints. Actually, we've got several flavors of joints that we can work with.

So let me go ahead and bring up it. Now, that's the list of the joints that are available-- Rigid, Revolute, Slider, Cylindrical, Pin in a Slot, more on that, Planar and Ball. What these do is they tell you what kind of motion is allowed. Rigid joint, OK, fixed no motion at all. Revolute, spin. Pin in a hole is an example of a revolute joint. Or an Inventor, it's the Insert assembly constraint has that same functionality.

Slider, you've got motion along one direction and in only one direction. Cylindrical, I've got motion along that direction but also rotation about that. It's like a garden gate latch. You can move it up, move it back, drop it down again.

Pin Slot, yeah, it really is what you're hoping for. I'd like to see that one back in Inventor, to be honest with you. Planar, I always think of it as the air hockey puck. It can move in x and y. It can rotate in x and y. It just can't rotate off or lift off. Yeah, I know air hockey pucks do all the time, but still at a perfect world.

And then Ball joint, it's your hip, again, in a perfect world, three axes of rotation, and that's what it allows. So joints open up an allowed motion between components. That's the short and sweet of it.

Pin Slot, again, that's we're going to take a look at that. That's worth it right there. Now, if you've already built things in the right position in space, you happen to build the piece right on top of the other piece and it doesn't need to be shifted or anything, what you can do is what's called an as-built joint. You can say, hey, it's where it needs, especially for a rigid joint, it is where it is. Fix it.

What that implies is I can use one joint to do the work of what normally would be three assembly constraints, mating a face, maybe doing a flush on the end, and then a flush on the other side, three constraints, one rigid joint, same thing. If they're already in the right position, perfect.

If they're not already in the right position, in Fusion 360 we have a move tool. You can probably guess how that works, and an align line tool. And if you've ever used the align tool in good old AutoCAD, it feels a lot like that. Take this. Move it, swing it around, get it where I need it, and then hopefully I can use it as-built joint right then and there.

With the as-built, you get to pick which joint type you want. Again, it could be Rigid, it could be Slider. It could be any of those. A lot of times I'm using it for a rigid connection though. And there is a technique which is used heavily, and that's putting a rigid as-built joint between typically your first component and that top level in the browser. And what that does is the function of grounding.

Now I'll say that Fusion 360 does have the ability to right click on a component and ground it. Use this instead. And there's a great video online for it. You can do a search on YouTube for Fusion 360 grounding versus rigid as-built joint. I think that's the search that gets you there.

And it shows how. If it's just a standalone assembly, you can use grounding. That's fine. But if that gets put into another assembly, the fact that something's grounded doesn't mean that it can't move overall. The origin of the part can't shift compared to the origin of the design file. Whereas the rigid as-built joint between a component and that top level basically locks the origins together. If one moves, the other moves, end of story. You don't have to worry about it. So just get in that habit right away.

If you have a group of things that are already in the right position. You don't have to make rigid as-built groups between all of them. You just tell them to be part of a rigid group. And it basically grabs them all together and they have to move together. That's it. It's like putting in a series of rigid as-builts.

Now just a word of caution, advice, whatever you want to think of it as. With joints, the first thing you pick will then be moved to the second thing you pick. So if you do a planar joint, the first one will move to be on the second, and then move like that. So as you can imagine, if something is already grounded or has that rigid as-built to the top level design file, it can't be the first thing you pick. The software won't let you. It will yell at you. So the first pick goes to the second.

The other thing is when you're doing a joint, you are creating a coordinate system right then and there. It's not really called a UCS, for user coordinate system. It's a JCS for joint coordinate system. But you'll see a little tiny XYZ triad, RGB, red green blue triad, where that origin is that it picks. Pay attention to that because the translations for a slider or the rotations for a revolute take place about that z-axis. So keep an eye on the blue axes when you're placing those.

All right, let's take a look at these. So kicking back over to the design tool, right now this one's free to move. So the first thing I need to do, that one's going to be my fixed piece. I clicked in space to clear the selection. Just it's a habit I have. So I'm going to do an as-built joint. It's going to be a rigid as-built joint. It's going to be between that and that.

If you want to preview the motion, yeah, that's the preview. OK, that's it. This is now locked in space. It can't move. So now if I want to go and do a more typical joint, if I go and grab that-- well first of all, if I go to get it-- I caught that by surprise a little. But if I ground it, it will not let me grab it. Yeah. See it's grayed out if it's grounded. You also get the pushpin. Still go with the rigid joint. You want that very first one in there.

And you can rename the joints too. Not now, because I'm in the middle of the other command. So let's see. I'm going to go and edit this. And I'll put a sketch on here and put a big circle on the top. Now, I'm going to mention this later on.

If you do a capture position, it actually adds something to the timeline down there. And a key to performance is going to keep that timeline as short as possible. So I'm not going to worry about that. I'm going to just go ahead and let it revert back to the original. And I'll make this a little bit bigger to make it very obvious what's going on. I'm not going to worry about a dimension. And I'm going to drag it down and tell it to go all the way through.

Real quick and dirty, putting that piece in there. Now when I go back to the top, I can go and make a joint between that, and you can see the coordinate system jumping into the center, and that. And tell it that it's going to be a revolute. You can see the little glyph showing the preview of how it works.

As far as the pin and slot, there we go. I go and open this. Here's an example of one of those in place. Oh, let me go and grab another one of these. I'll take that fastener. We now in Fusion have a fastener library and I'm taking advantage of it here. So copy and paste that, and I'll drag this over here to get it out of the way.

And for the joint, for the first one I'll pick-- by the way I'm using a 3D mouse for doing this smooth motion. And I browsed across this. I scrubbed across that circle and there's the top of it. And there it's previewing what the rotation is going to be. And better tell to use the pin slot, there we go.

And for the alignment then, what I'm going to do is, let's see. Pin slot, hex bolt, oh, this is just the initial position of it. You can see how I can spin that around, which really won't buy me anything here. So rotating about that local z-axis, yep, sliding along the local-- no, let's go and do a custom. I'm going to use that as my custom direction. And there we go. And I could further go and set up limits, have it go from-- I don't know-- linear limits from 0 to 1 inch.

And you can see how now it's moving along there. Plus it can still spin in there. I definitely would like to have that available in Inventor as well. OK, moving on, and yes, just old habits. I'll save. I'll close this off.

Collaboration, wow, that went by quick. So what you can do with Fusion 360 is very easily you can do small group collaboration. Basically any number of people can open a file. You'll see a little glyph down in the data panel. You also see the glyph at the top of the browser. And there'll be a single initial for whoever it is that has it reserved.

You'll also have a two-letter glyph up on the top up in the application bar, so a little more information there. Anybody can have it open. But only one person can be editing at a time. And what'll happen is you'll get a little white dot on whoever's got the editing. So whoever starts editing first, I'll keep one and call it a token. They've grabbed that token. They're holding on to it. If I look at this from another assembly point of view, here's an assembly using those casters. And it shows that I have it reserved. I'm making a change.

I still have that reserved. When I do a Save, that's going to release the token. If somebody else wants to start an edit, they will then be grabbing that token they will have it till they do a Save. So you can work in a collaborative environment. Well, I've used it mostly in small groups.

To help with that, break things apart, just like you would in Inventor where you've got sub-assemblies. OK, it's a separate file. We'll do that here in Fusion too. Take that piece or that caster assembly, and save it out as another file, and then bring it in so it's an external component. The chair base, when I get around to finishing it, do the same thing.

The chair body, right now all we have is a bottom cushion. But as I build the arms and so on, make those separate design files, and then bring them together into a master level assembly. And that way people can be working. Everybody can have that master level open. But they can be working on things and seeing what's going on.

So that brings us now to basically how do I recommend running Fusion 360. Well it's going to start off follow Rule 1. Rule 1 says, when you start a new design, save the file. Give it a name, Workflow Example, great name.

Then go and create a new component right away. There's the icon off of the tool bar. Then the panel pops up. Give it some kind of name, JSPart123. It's going to be activated immediately. It's going to be a child of whatever was highlighted when you hit the New Component button, which was this brand new design file, so new component right off the bat.

Then go create your sketches and features in that active component. And then that component owns those sketches, owns those features, as well as the bodies and all the other information. If you ever save that out, that information goes with it. Repeat as much as you need to. Sketches features do you get that part the way you want, and then bring things together to make your assemblies.

And as a reminder, create a rigid as-built joint between your first component and the top level of the assembly. If you want to ground it too, great. Belt and suspenders both do the same job keeping the pants up. Sometimes one is better than the other. Do them both, nothing wrong with that.

I've got a few minutes left here. So let's take a look at just some other suggestions, things I've picked up watching other people run Fusion 360, things I learned beating my head against a wall. Not an expansive list, just some things that I think will help you.

So first of all, go into Preferences. Go up to where your icon is at the very top, and click on it. Here you can see that picture of myself. When I click on it, my preferences are right underneath it. That's great. No matter what device I log in on, my preferences follow my logging in. In the Preferences, just take a good, long look at all the different options. Some things I've done, I changed my up to be Z being up.

I found I was doing a lot of stuff where I was building off the floor and up, tables, chairs, that kind of thing. So Z-up seemed to work really well. That doesn't mean it's a hard and fast rule. It's just the way your default is. If I'm doing something where XY should be the front plane and Z coming out, that's fine. Right click on the View cube, just like you do in Inventor to change who's front and who's top. Same applies here.

In the Design tab, turn off allowing 3D sketching. The reason for that is if you've got lines that almost touch and you try and drag one, if 3D sketching is on, you may pull it up when you're trying to pull it over, and you never get a valid region to make an extrusion. No, you're trying to drag it here. You want it to stay on the 2D plane. You can always, when you make a new sketch, turn on a little check for 3D sketch. I'll show you that in just a moment. But by default, keep them as 2D sketches. That might even be the default setting these days.

On the Drawing tab, sorry Drawing node in the left-hand side, I keep thinking tabs from Inventor. You can set up what you're drafting standard is, ANSI, ISO. What your default sheet size is, 11 by 17. What your line weights, what your textiles, what your dimension settings are, two decimal place, three decimal place, setting up your defaults.

Set your default material. You may have noticed mine came in, it comes in as brass, different. The out-of-the-box is steel. I got tired of the gray. So I changed my default material to brass. I also set my default units to be inches. I can change any given file anytime I want to a different unit. There's a node, let me show you real quick here in the design tool, document settings.

And for a regular design environment, this is where you would change your default units. This document settings will have different meanings depending on what your workspace is that you're in. But for document settings in design workspace, that's where I set my units.

And way at the bottom, preview features. Take a look in there. That stuff that's not released for prime time. But you can explore. Things that have been in there that I've enjoyed exploring-- plastic part modeling, the simulation tools for injection molding, there's advanced CAM features in there that are in there as they work the bugs out. They get feedback from us, the users. And when it's ready to go it's put into the main product.

The timeline, the more efficient you can be in the timeline, the faster, the better performance you have, the faster software is going to run. So things like doing a pattern instead of inserting a half dozen bolts, avoiding those capture positions. They're just adding spots on the timeline.

Use coloring. That can help you figure out what components are what. Is that a separate body is that a component? What did I do here? Using coloring, that was the one that just, wow, why is it all the same color? Oh, yes. I forgot Rule 1 when I started the file. Everything's in the same component. It's all one color. You can't do a joint unless it's a separate component, can't do an exploded view, can't do a tweak unless it's a separate component. So that separation by components is very important.

Features, pay attention. All the way at the bottom, in fact, sometimes it falls off my screen. If you're doing something like a hole or a cut style of extrusion, or even joints, but I notice it mostly on cuts, there'll be a listing says objects to cut. And if you expand that, it'll say what components and what bodies are being cut. I've seen some coming up for fillets, chamfers, like I said, holes going through everything, or just only a single component. You can turn on and off the check boxes there to control where things are going, what they're affecting.

Make sure you keep track of who's the active component. Again, you're going to see it with the bull's eye, and it's the red arrow is pointing to it there. But also then down on the timeline, you will only see the features for what the active component is. If you're on that top design, you see everything. But as you get down and activate lower level pieces, you only see the data for that piece.

Components, there is a tool called Duplicate with Joints. If I placed that bolt right on the end arc of that slot, I could have then used this tool to quickly put another one, another one, another one, in other openings, other holes, other ends of the slots, that kind of thing. It duplicates the component and the joint that's holding it in place. But you have the chance to pick a new origin for the joint to receive it. So you pick one hole, and then you pick another hole, and then you pick another hole, and you got three bolts in three different holes.

Now, there's times the pattern would be easier but this is a really nice tool when you have just awkward spacings and such. You can always upload Inventor models. I didn't mention here, but you can go out to Mcmaster-Carr and download STEP models. You don't have to give up what you've already done. That's kind of nice, because you can use Fusion for doing the simulation or the CAM end of things for what you've already done in Inventor.

But you may find that some of this modeling, especially a conceptual design phase, is easier with Fusion 360. That's actually the route I went. I was using it originally for doing simulation, and then found that I wanted to try something. I want to try a new mouse, or I want to try a new design for something else. And that quick experimentation phase was easier in Fusion than it was in Inventor. Now, that's also where I ran into the first case of what is Rule 1. Hmm, maybe I should have used it. Oh, well.