Autodesk Fusion 360: Sheet Metal Parts, from Sketch to Nesting and Production

HELGE BRETTSCHNEIDER: Hello. And welcome to my Autodesk Fusion 360 sheet metal parts from sketch to nesting and production session. My name is Helge Brettschneider. I'm from the EMEA team of the Autodesk for CAD/Cam, which means, in the end of the day, Fusion 360.

So just a little bit of housekeeping up front here-- as you know, as Autodesk employee, we sometimes work on confidential products. So just to ensure that you know that you not always the [INAUDIBLE]-- so there is this little safe harbor statement so that you know that when I make a statement that it's not appropriate and in the moment because it's confidential-- it's important that you know that this is something you should keep for yourself.

Let's get started on that. So ideas-- I have a couple ideas every day. But the thing is when you think on something, you think you have several stages. You have the rough idea. You might give first sketches. And then you continue your journey.

And when you reach something that is really usable, you transfer it into a product. And that's just the same when you are in your making environment, like Fusion 360 is used in a lot of maker spaces and something like that or in companies that are having design environment and CAD and production, CAD and CAM in-house. So Fusion is covering all of these areas. And this is what is the same with the ideas. You have different stages you have to combine them. And this is what this session is about.

We take a brief journey from the design space over the CAM planning, which is nesting. And then we come to the final stage of production. This, obviously, means that we have quite a lot of points that we cover. We will maybe not cover every single detail. But if it is necessary for the whole process, we definitely will go into details of that specific information.

So let's get started in the design environment. In the design environment, we have the first stop, which are the sheet metal groups. Different to the solid modeling environment, the sheet metal section of solid model, so it's a little bit different because we have here the capability or the opportunity to standardize things. For instance since we work with flat material, the material thickness is a point that we can standardize. K factor is also a point that we can standardize, and also band radius and band relief.

Fusion 360 provides you a couple of predefined standards for these sheet metal rules. As you can see here, the sheet metal in millimeters or stainless steel-- same definitions also available in inches. So this means you don't have to come up with every detail by yourself, you can start from one of these predefined roots and bring them in the specific values that you want to have here. OK, next one.

What is the K factor? The K factor is something that is very important here in that situation because since we work with flat material that gets into a press break and get a deformation, so this deformation needs to be calculated in our model, and therefore, we have an imaginary neutral fiber. The standard neutral fiber is, of course, in the middle of the height of the flat material that we use, but the imaginary neutral fiber is calculated so that the compression of the inside and the outside stretching results in the right values when we check our model dimensions.

A little side note here. It's some more information about bend and bend shortening and something like that. If you are new to that, this might be very interesting here on the right. And now, we are ready to create some flanges. Fusion 360 has a very optimized design in my environment for sheet metal. So we have here the flange.

Some of you may come from other systems and think, there is just this flange command, but where all the other features? So Fusion 360's developers decided to have a very specific flange command that is covering most of the standard procedures in the metal bending environment. So this means we start all-- we start with a sketch and create an extrusion, which is a first flange. Then we select an edge, and the edge gets extruded, so we have another flange.

So you can base your flange on a sketch, or on an edge, or even maybe-- or a complex sketch, which can also include blinds, for instance. So you have every capability that is possible, what you can come up in your design.

Further down the road, there are some more features and functions, like a flange join. You just have a sketch where you have a connection, or where you want to have the connection, and then you select the edge of the existing flange, and here we go. There is another flange.

Or what I find very interesting is a miter flange. Like, you have an existing one and you want to extract or create a flange and line along two edges, and then to ensure that we still can create a flat pattern of it, it gets metered so that there is no interference between these flanges. So how this all works, let us go to Fusion 360 and check it out.

So one thing I have to mention, when you start from scratch and create a sketch, maybe do something real quick here, like a rectangle sketch in the middle-- midpoint, something like this. Close this. And when we create here from the sheet metal section of the ribbon flange, then you will see that here, the flange will get created and we come to the details a little later, and you will have here a body.

So the important point is when you work with the sheet metal environment, you have to consider deciding how you want to use that. Because you can use it as a part, like it is now, but when you want to create an assembly from it in the same environment without inserting that one in another design, that's not-- that's essentially not possible because there are-- the limitations are kicking in from the sheet metal design environment. So when we would proceed as we usually do, let's say create here a component from the body, it will tell you that's not supported.

So it is important when you think about working with an assembly, you should apply rule number one. You may have heard about that, which is essentially creating a component first, then in that dialogue, you decide that you want to have a sheet metal component, and hit OK. So when you now start to sketch here, same procedure as done before, I select my center rectangle, click this here, extend this in the size that I want to see here, and then create my first flange.

So then we have already the right component. We can extrude or create this first flange, and it is creating a new body, and I hit OK. So this means everything is stored in the right component. So the component is the compartment, let's say, for the bodies and the sketches, and as rule number one tells you, this is the abo-- the way to go.

So here, the body is also included here and that is marked as a sheet metal body. So that's the first flange. Then when you want to create another flange along an edge, just pull this out and you can give it a height, you can adjust the angle. For this situation, I want to keep it at 90 degrees. And then we have our first edge along a flange-- a flange along an edge.

So next thing, the miter flange. Very easy to do. Select two edges and pull them out. And as you see, as I mentioned here, is a corner seam that is already included here and taken care of by Fusion 360, and also here, the gap is included. So very nice, easy to handle.

So when you want to create a profile flange-- this is a term that you may know when you use Inventor, or used Inventor in the past-- so I project here at first my edge, here up in the front, and say OK so I have a reference point here, and from there I start sketching. So with the line here, down here, let's say 30 mil, and then maybe adjust the angle 45 degrees, and then hit OK-- so with that done, I extend that sketch with an horizontal line of 20 mil and say OK.

And with that profile sketch, I'm also able to create another flange-- so a profile flange. At first, I select the sketch, select the edge, and you see the profile is created.

So with this in mind, you see you have a variety of features and functions included in the flange command. So play with it, and also when you want to have just sections, small elements-- for instance, when you want to have just-- let's do this real quick. Along this edge here, you extend this, and you might not want to use the full edge, you can adjust this. For instance, you can pull one side to here, something, and the other side from here, so that you have something where you may want to drill in a hole and then create-- have something to bolt this down.

So OK, let's move on. I think it's pretty clear what the flange is capable of.

So the next one is the lofted flange. This is essentially just brought in with the July update 2022. So the very interesting feature because it addresses something that is long-term requested from the community, and you have the ability to create a lofted flange with a press break style or a die model style. You see here is the difference. The press break you need to have all these angles in here.

So let's do this real quick. In Fusion, I start with a new part, create a new sketch, something on xy, a circle right here-- so bring that in-- and then I need to have an offset plane from that one-- let's go with 75-- and then another sketch up here, and yeah. Obviously, let's do something with a rectangle. A little bit bigger, something like this.

So that's the foundation for our lofted flange. So therefore, since I'm not intending to create an assembly, I start right in that component, and now create a flange. And with that flange command up here on screen, you see there is a new button, which is the lofted flange. You select these two contours, and then you can decide how you want to have it-- as a press break form, which is a folding process as you know, and then the die form, where you bring it in that shape by pressing it in that form.

Very important here, it is all your first extrusion, or your first loft in this case. And since this is now the topic, you can adjust your sheet metal rule here, and mine is a steel [INAUDIBLE] desk, which I defined early on. So then, it is in here. And when it is done, you can change this, even now-- still now here to the press break version of it, and you can see this get folded section by section.

Important point here. You have to create a cut in here because when you want to flatten this out, you cannot have this as a closed loop, so you need to have a little gap somewhere here.

So let's do this real quick as a quick example. So I use an extrusion-- that one-- and here I select symmetrical pull distance, and that one year, the distance now can be adjusted-- let's say 2 mil-- and then as a cut. And now you're ready, good to go. Now you can unfold this.

So everything that you do in sheet metal is intended to be unfolded later on in the process. But let me hit that guy real quick so that you see what's going on here. I select a stationary phase, and boom, as you can see, it is possible to unfold this. And the unfold is very important for our later processes. Wow. So that's the lofted flange.

Bending is something that you also can do. For instance, when you have importance to the geometry that you want to fold on a specific point-- I'm not demoing that one because it's obviously how it works. You create a sketch on the created phase, and then this is your band line, and then you can use it for the angle of that created flange section here.

So one other thing that is very important, I think, is the unfolding an existing model and fold it back because in some cases, you just create a component, and later on someone says, oh yeah, we need to have here an opening. So you can just press through an extrusion here, but this is not the same like it is when it is made before bending. So the geometry in the end looks different.

So how we can do this, it's pretty easy. For instance, when we want to insert something here, [INAUDIBLE]-- so we have here in the sheet metal environment features the temporary unfold command. I select that phase and I'm activating here now, unfolding all the bends. So this means it flattens out the component completely. And here, I can add a sketch somewhere-- something like this, for instance, and then sketch a contour here on that phase-- for instance, something like this-- and then up here to there. And then I'll set one here, just as an example.

And when I extrude this through here-- so that is a cut in the other direction, then I'm good to go. Let's say through all, and then hit OK. So in our section here, that makes no big difference. But the process is the same, even when you do it on the section right here. So the opening is included and you fold it back. That's the important point here.

So OK, next one. Sheet metal components from other systems. That is-- I personally think that's a little bit more challenging than creating a new component in Fusion 360 as a sheet metal component, obviously.

So the situation with components that come from other systems, it's a little bit more difficult in case of what is coming in there. Maybe someone has provided you a sheet metal model and he says that it's a sheet metal model, but it isn't because there are closed gaps. You should be here, at that section, there should be a gap. So there is no gap. You cannot unfold it.

Or the other thing, someone made, in his attempts of modeling that component, he made a mistake, and when you unfold that later on in your process, they are overlapping. That's a total no-go in Fusion 360, or even with a vendor. So the geometry should not overlap, there showed no closed edges or something-- these are all important things.

But one, we don't want to be negative. Take it optimistic. So when we import something, this process will be applied. So we open the STEP file, check it real quick, if everything is OK, if it's possible to unfold this later on, and then activate the design history, and then convert it to sheet metal.

So how does this look in real life? We start a new component and I insert-- and I insert, I'm opening a STEP file from my computer-- something like this. So OK.

So this is the STEP file. It's not a big challenge here, but it shows the process. So keep in mind, when you move-- when you come from the situation that when you import a STEP, the design history is turned off. So if you switch to a sheet metal component-- sheet metal type here, then you have a very limited access to the features and functions. And when you straight ahead go here on the convert to sheet metal, then it says the parametric modeling should be enabled, let's say, and this is done by enabling the design history.

So after that, we don't see any big differences or problems, no opens, things, no-- yeah. No irritations have been in that sheet metal component on the other system.

So after that, we can continue to the next step, which is converting sheet metal. And I have to select a stationary phase, which is this one here. I can decide what kind of sheet metal rule I want to apply. In this case, we use aluminum. So it recognized automatically the constant thickness of 4 millimeters, and then-- cool. We are ready. We can create a flat pattern, which is our main goal on that component. You save that one to your hard drive and you're good to go. Next topic.

Little side note. 2D to 3D, there is an-- we will cover this later-- there is an app that helps you with the import of 2D DXF files.

Documentation is an important point because most of you know you have your base view, you have your side views. But in some cases, it always turns up that someone is not able or doesn't know how to get the sheet metal flat parent on the drawing. That's very easy. You-- I have your drawing created, so I'm not covering how to create a drawing. I think you know quite well how to do this.

But the important point is when you have your views right here. Set it up correctly, everything is fine. And you want to have your sheet metal component visible up here and create the bending table. Therefore, you go to base view, and then in the dialogue, you have the option to change the representation. And this is only available when you have created the flat pattern. So with that, you're able to place that view, say OK, and then you can insert, based on that view, your bending table. Easy, but sometimes overlooked.

OK. Going back to the presentation. And we are now in the production area, which is our first-- or fourth point in that production is production planning, which means not directly producing the parts instantaneously, we have to nest the components. As you know, we work with flat material and we need to cut the shapes out of the stock material, and we want to optimize what is left here so that we have most beneficial outcome in our protection area so that we don't have not too much left.

And therefore, we use nesting, which means you have different components, and these components are positioned and aligned by an algorithm-- a nest algorithm-- nesting algorithm, so that brings those parts into one flat material layout.

So to do that, you have two options. There is on one side, the Arrange tool from Fusion Core technology, which means that it's included in every license from Fusion 360, and then we have the Nesting and Fabrication Extension, where all the advanced stuff is in there. So when you work with your hobby project, you're already able to do nesting. But the Arrange tool is just for the existing opening open design file. You cannot include other parts. So in the Nesting Fabrication Extension, which is-- which needs to be purchased, you have more capabilities as you can see here.

But at first, let's quickly check out what the Arrange command can do. So therefore, I take these little example here, and I open that one real quick, look. So this is a full design of that wooden chair here, and what you have to do, I have to prepare, of course, the chair, and then you have to draw or create something that represents the stock or, in range terms, the envelope, which is the flat material where you cut the individual wooden pieces from.

So in the first moment, you may go up here and check, is there something that I can use for that? In the modeling environment, solid modeling environment, there is nothing because the Arrange command lives in the manufacturing production model. So therefore, we have to switch to manufacturing.

And the first step that needs to be taken here is to create a manufacturing model, which means that we can-- with that, we can repair this chair. We don't want to disassemble it in any case. We just want to have the components copied and laid out here on the stock material. So we don't touch the model that is in the design environment.

So when we are in the editing mode of that manufacturing model, you see we have kind of similar features and functions here-- a little bit limited compared to the design version, but here you have the Array command, which is that what we are going for, and then, at first you have to select the components that you want to array, and then you define your envelope, which these are the common components that are laid out on this flat material.

So instantaneously, when I create-- select that flat material, Fusion starts calculating the layout of that specific nesting, or the Arrange. And then down here, you have your object spacing, you have the flip envelope thing, which means when you look from another angle you see we are perfectly aligned, but when we hit that guy here and everything is on the other side. So you sometimes need to check on which side's your arranged components are, and then you may have to flip that one.

So with that done, cool. Our components are laid out flat in that stock material, and you can start planning your cam operations.

So going back to the Powerpoint, and now we are hitting the road with nesting and fabrication extension. It needs to be purchased as it is available on a monthly fee so that you can order it when you need it, so or you can purchase for a whole year.

So the process overview is you prepare your design for nesting, then you assign materials and packaging, and then you define component sources, the Create and Edit nesting-- which is obviously something in direction to optimize where the components are adding production-related model changes and something like that-- then you can view, compare the nest information, and then you can create the nest report and can then, from there, continue with the production process.

So we will streamline that a little bit because we cannot dig in every single detail here, but the full process, we start here. So we have the-- I have prepared here a little audio stack now, which means this is an audio rack, let's say, that is for event management and something like that.

So this one is the DLL designed with Fusion completely. All the components are here. And now-- yeah, we need to start the nesting for our production planning.

So therefore in the design environment, we need to do the first step, which is preparation for nesting. Because as you know or you may see, internal components, there are screws and something-- everything is in there. And therefore, we go to the utilities, and here you find in the design environment the Nesting Preparation function.

So here you can define what you want to ignore, for instance. There are automatically existing sheet metal you may want to ignore. We don't want to do this. But you also can ignore sketches, you can ignore selected entities, something like that.

And as you can see here, it analyzes the situation here, and you can see which components are in that specific assembly here. And then this one is, for instance, the direct ear, so there's that one here, which is automatically recognized that it is there are two times. Then the inner case, which is a band round here. And then we have a couple of screws in there that needs to be ignored because these are not involved in the unfolding process. Then we have the lower and the upper, another set of screws-- and we have here the upper bended element here, and the rest are the rear casting.

So you can change the options here, but we don't need to do that when we have our full design here in Fusion 360 because as you can see, these are already sheet metal components and the others are ignored. So not a huge thing, not flashy, something-- it is just the preparation.

So next step is going to the manufacturing environment. In the manufacturing environment, there you have the fabrication tap on the ribbon. And here, when we concentrate on this one here, we-- the [? source ?] is actually clear because it's coming from our design. And then here we have directly our nesting command for creating the nesting study and generating the existing-- and existing nesting study, after a change, for instance.

So then you have cutting strategies here, simulation or something. And here, you have the process material where you can define what kind of material you are handling in your company. So that is in here.

In our situation, we concentrate on the nesting here, which is just that button here. So it starts calculating what is needed and brings up a dialog where we can define a command for nesting-- sorry-- here.

And the important thing is here, the job quantity. So this is now set here from an earlier session to 10, so I want to have the whole thing produced once. And that means we have these direct ears here, we have all our components here, so everything is listed.

And I can uncheck for instance, when I don't want to have the direct ears included, for instance. I can deselect that one, I can check the packaging because this automatically regenerated because we have the standard packaging that is in here, so that fits our needs. And-- [COUGHS], sorry.

So then we have global parameters where we weigh minimum compute time, maximum compute time, different settings that we have here. And important one here is the creating a manufacturing model. If you just want-- if you have a machinery that is capable of using DXF files directly, you don't need to generate a manufacturing model. So in some cases, it is interesting to have that one checked or unchecked.

So in my case, I can leave it checked because this doesn't limit my capabilities, so it may make the model a little bit bigger, and the result is right here on the screen. And you can see we have here the lower casing, the upper casing, so these are in here. And if I decide to check the other one here, there is, for instance, the inner cage that is in here.

So when I now decide I want to have the direct ears included in that, I have to edit the nesting-- sorry-- and bring them back in. And then I say, OK, and then use the right click and generate the nest again. And then we can see that here, the inner casing is here, the upper is here-- but I don't know why they are not in here. So, OK. OK. So it should be-- it should be maybe in the source files, but anyway, we will check this later on.

So when you look at these, the nesting is ready, and we can analyze this year, for instance, the compare. So with the-- in our case now, I select it just once. Sorry. When I want to compare these two, for instance, then I can launch the Compare command, and you can see there is a full overview of this sheet with the aluminum stuff-- hold on. Oops. Again.

So here, when we create a nesting report, that one is here, for instance, so then you see what has been nested, where the components are nested, and then you can save this and provide this to someone that produces these components for you, and you also have the ability to compare these two, I think.

So compare, and you see here that I just selected the wrong entries. So you see these are the two nests, and you see which you can compare what kind of material is used for those components and so on.

So this means the nest is kind of ready. So when we-- the thing is-- very important is here that the nesting doesn't break any associativity. Nesting reacts on the complete process with all the entries.

So let's say, in my case here, I don't know why the direct ears are not included, so I'm going back, delete that one here, and insert the nest again. All shapes are now in here. So maybe I assumed I did something wrong, and now I use the correct ones. And as you can see-- yeah-- the ears, here are the ears. You see the two ears that are needed for producing the entire rack assembly are nested. OK. So if there is a change-- if there is a chance in the design, that will reflect here in the model.

So, OK. Let's move on. A very interesting point to many people that I met over during the rack-- during the day, is the import working with DXF files. And yeah, the process is-- I think the process is clear. You have to open the sketch and then you insert the DXF, but that's a lot of work just for importing the components.

This is why Autodesk decided to create an import utility. So the import utility provides you with the ability to move spacing and something like that. So an important process here is when you start a new design, and then you have to install that utility-- so here in your add-ins. And when you have installed it and started-- and you select that, it starts when Fusion is launched, then you will see the button right here.

So with that button, you can go to a folder on your system, select several DXF files-- so something like this. I take this two here. Maybe let's take three here. So that one. OK.

And then this brings up the bulk import dialogue. You have seen in the screenshot-- yours is in the screenshot, it's an inch in here, I am using millimeters. And the command on the-- comment on the-- or feedback on that is that it is only four inches. It is for both. It depends on what type of extension you bring in here. So you can use it in both environments.

And then you bring this one in here, you have rows-- you define the row, how many components are there, resetting the sketch. Extrude the profile is something interesting too. You can do this right here, and then the material is selected, and then hit OK.

This transfers and closes sketches, as you can see here, while that import is running. This one-- sometimes DXF files don't have close loops or something, and this is something that is processed here. And as you can see, those three components are imported and aligned here, and I can start using them in my nesting approaches here without any problem. They are available and some kind of already nested.

That import utility is free. You don't have to buy it. So I recommend taking advantage of it.

So next one is the other way around. As I said, you have, maybe in a nesting situation, and your machine that is available on your shop floor is capable of using directly DXF files and does the rest of the planning in the control. This is something that you can do with your nests that you have created.

So here, for instance, this is the same rec, what I used before in my presentation, but as you can see here, the manufacturing model is generated for one nesting study. So these side covers and one doesn't have the manufacturing model representation.

So how do we handle this? It's actually pretty easy. When you go up here to, for instance, this one where we generated all the manufacturing models, and you-- we just click on that entry, and then there is-- there should be-- [CHUCKLE]-- let's do-- go up here-- and there should be an export command.

So that one is here. So there is-- oh, OK. There's no export command. So let's stay up here. So there should be-- there is the export command.

You select that one, and then you define where you want to store your DXF files-- that is the first step here-- and then the export configuration editor comes up, and here is the standard configuration-- I define my own ones so that I have the ability to have the individual layers for the nesting, for the stock, in a name that I can work with. So but you can define your own.

And then you can preview the outcome of that, and then you just hit OK. And then these export as created a file.

Let's do this again because I didn't recognize where I stored them. Oh, OK. In my 2D resources file folder. So my 2D resources folder, here is that sheet, and I can open that one with the DWG Design View. If you don't have that one, and if you have to work with DXF files and need to check them, I recommend downloading that sole piece of software so that you can check what the outcome is. Even better when you have an AutoCAD. At least an AutoCAD [INAUDIBLE] for such approaches.

And then when I hit the double click, now it extends to the entire layout. And when you check the Layer Management, for those of you that are a little bit familiar with AutoCAD, you can switch off visibility, for instance, of the nest, and you can identify where these are.

So with that, we continue our journey, going back to the PowerPoint. So where it is? Here it is. That's the wrong one. That's the one.

And then we are now ready to produce parts. When your nest is defined, you can create setups directly from that existing nest, which automatically aligns the WCS, and the setup definition can be adjusted. You can do this for plasma, water, and laser. And then you create a tool path in your way do you need them.

It is not-- by the way, it's not only limited to plasma, waterjets, or something. You can use the milling machine there too. It depends what type of material you're working with.

So how we can do this-- so go back to the Fusion environment. So we have now here our nesting study, and we can create-- it depends where we go, by the way.

Now, if we go up here and say Create Setups from Manufacturing Model, it creates instantaneously two setups. So one for each of the nesting stories I selected here-- or the sheet of the nesting studies, I should say better.

So with that said, I can edit the setup. And as you can see here, there is this parameter notification. It's not an error, it's just an information. So because there is no nesting list selected stock, we can do our adjustments, but it comes from the nesting study so we can keep them as it is, and I hit OK.

And then a warning comes up, no model is selected. All models will be used. And I want to say yes, that's the way I want to do it, and you see that warning disappears and I have all that set up here.

Next thing, pretty easy. Using the cutting tool on defining the 2D profile here. So I select the tool that I want to-- so based on that, I have a cutting tool here, and here are the cutting tools in inch, and the cutting tools are in metric from the few tricks, the library-- I have already one in here. And I select that laser pad and define the profile. So select the contour, which means at first setting this little checker, and then I select all of these components down here, and I'm good to go, and the process is calculated.

So pretty easy, straightforward, and improved. You don't have to define what kind of standard procedure you wanted to have here because already defined here that we are planning cutting procedure. So that's a good advantage of this. And we're ready to move on and define the NC program.

So this has been changed over time, as you may noticed. In the past, we have been selecting the setup and straightaway post out the NC code. These days, we handle this a little bit different. We create an NC program. This gives us the advantage to define which processes are included in that export, and then you are good to go, yeah?

So you can define several operations here. For instance, when you want to have [INAUDIBLE] or something on one component, you can include that here, something. And then you may want-- the other day, you don't want this, you can deselect this. So you have an in-depth setting-- the ability to adjust the settings here.

So the next one here is-- or the first one already, is the setting. Here, I selected the post for the Trumpf laser, though, and this one is part of the Fusion library, but you have to select-- in the first place, you look for cutting, but it is jet.

So in the jet environment, there you will find, for instance, the Trumph and a couple of others that-- for instance, Tarmac is here, or plasma kind-- you can select them from here. I have already defined that setting, I have my program number, the source where the output folder where [INAUDIBLE], later on the NC program, and then I hit OK.

NC program defined. Has a green checkmark, no problems. Right click, Post Process. And then, of course it says OK, there was something, because I've done that earlier, and that kind of review my NC program.

Fusion creates thousands of lines within seconds, and-- oops, that is not needed-- but you can see here the NC code can be now-- or it's now ready for transformation. Transform-- transfer into the NC machine.

With that, we are at the end of that session here, and thank you for your time. And when you want to ask-- later on, if you-- later on want to ask questions, send me-- drop in email at Helge.Brettschneider@autodesk.com.

Or the other way around, use the little black A or the white A on black ground, this is the Fusion chat where you instantaneously have direct support from us. There is a good chance, when you are early in the morning coming to the shop, want to ask a question, hit that button, to get me on the line. So let me know when you have questions. Until then, have a great day. Bye, bye.