Integrated ECAD, Modeling, and CAM in Fusion 360

EDWIN ROBLEDO: Well. My name is Edwin Robledo. I'm part of the EAGLE team. Been with Autodesk for approximately a year. We got purchased by Autodesk a year ago. But I have been working with EAGLE since 1991, which was actually started in 1988. So I've been part of the EAGLE support team for a very long time. And with us, Paul, which is our main speaker.

PAUL CLAUSS: My name's Paul Clauss-- I do support for Fusion 360 at Autodesk. I've been in that role for a little over a year now. And before that, I was actually in college and taught myself Fusion, because it's a great option if you're a student, anything like that. Then I started working for Autodesk. And yeah, Edwin and I are really excited today to walk you guys through the new EAGLE integration tools between EAGLE and Fusion.

EDWIN ROBLEDO: Absolutely. And today, the presentation-- we're going to be using some videos and a PowerPoint, but it will give you a really good idea exactly when it happens. I'll be hanging out on the answer bar almost all day, so if you actually want to come and have some specific questions, I'll go ahead and take care of those as well.

PAUL CLAUSS: Yep, and we should have some time for maybe if you guys want to see something live when we're through. And I'll also be at the Fusion answer bar all week. So I guess we should get started. So we're really excited today to show you the new Fusion 360 and EAGLE tools for integrated electrical and mechanical design. And what these tools are intended to do is give designers more efficient and collaborative workflows throughout the design process. So Edwin, do you want to start with a little-- what is EAGLE?

EDWIN ROBLEDO: What is EAGLE? Just for those that just in case don't know. It's actually a CAD package for designing electronic schematics, and it collaborates, works directly with the circuit board design software as well. So from this merger, we are going to be taking care of the electrical part of this integration. Paul?

PAUL CLAUSS: And Fusion is a mechanical product design platform-- we have multiple workspaces, we can model, render, perform simulations, set up Arcam and create 2D drawings. So in the past, the largest difficulty when working with these integrated electrical, mechanical designs was managing file conversions.

Every time we made a change to the PCB component, we'd need to export or create a new copy, bring that into our mechanical designs and work with that. And this could be really difficult to manage and introduces the potential for a lot of errors. So the integrated tools in Fusion and EAGLE seek to resolve this by allowing a PCB component in Fusion to be linked to an EAGLE board file.

And what this allows teams to do is work in a single Fusion design and a single EAGLE board file, which eliminates a lot of that file management-- the file management problems we used to see.

EDWIN ROBLEDO: Yeah, usually, there was a lot of errors when it came to conversion, so this eliminates that.

PAUL CLAUSS: So we're going to kind of walk through a bunch of different things with this in this presentation. We're going to start off slow. The PCB workspace and Fusion and the Fusion sync button are the tools that we use with this integration. We're then going to jump in and show the two main workflows-- we can either go EAGLE to Fusion or Fusion to EAGLE.

We're going to discuss when we should use those workflows based on our design intent in the situation we're in. And we're going to wrap up with some of the advantages of this integration and some of the things we like about it. So the PCB workspace in Fusion is how we can create PCBs in the Fusion design. And right now, the PCB workspace is relatively simple. We have only four tools.

We could access these tools in this workspace by using the Create PCB option. It's important to note that you're only going to see that option when you're working with the design history or in parametric mode in Fusion-- you won't see it in direct modeling. And using these tools, what our mechanical designers can do is, create a Fusion board shape and a board component with the PCB profile tool, we can copy the profile of a board brought in from EAGLE with the Copy EAGLE Profile, we can edit the layout of 3D components, the packages is from our EAGLE libraries that are applied to the board with the Move PCB Components. And we can use the PCB status tools to see if any changes have been made to the board in Fusion since the last push to EAGLE.

So looking at the-- and we'll be demoing these tools throughout the presentation. Looking at these, the first thing that you might notice is, we don't actually see anything to communicate with the EAGLE. And that's because all communications are actually done through the Fusion Sync button on the EAGLE side.

EDWIN ROBLEDO: So on the Fusion side, basically, you define the body. And then from EAGLE, you actually can see that body and pull it in. That's what happens. So all the magic is actually kind of being triggered by EAGLE. EAGLE is actually pushing the Fusion or pulling from Fusion. And we'll make this clear in a minute as well.

PAUL CLAUSS: Now, what happens is that--

EDWIN ROBLEDO: If you don't mind, I'll walk over here.

PAUL CLAUSS: Go for it.

EDWIN ROBLEDO: I hate standing in one spot. It's too boring. OK, now, we've added into EAGLE a button, if you have EAGLE version 8 or larger. We have a new button no that says Fusion Sync. That's where all the magic actually will begin. Now, what happens is that we could use the Fusion Sync button to link EAGLE to a board, to a Fusion design-- either a new file or an existing PCB.

So when I click on the Fusion button, since you're using the same account in EAGLE that you have in Fusion, it actually will let you browse all the [? prior optics ?] that you have in Fusion, that way you could actually push that circuit board over to Fusion 360. Now, this keeps both teams-- so it could be my own account, or if you're already collaborating with another team, you could push to their account, to that collaborative. So I could push that circuit board. And we'll be demoing this in a few minutes as well.

Now, let's talk a little bit about the pull and push terminology that we're talking about. Now, the Fusion Sync button helps us know when the board needs to be push or pull. It gives us kind of a status of, where do we stand in our design collaborating with Fusion. And this is done by using a color code. When we see the Fusion Sync button and we click on it and we see these buttons-- and the Fusion Sync button will actually change colors. When it's red-- and you'll see it kind of in red-- you see that red there where it will say it's out of sync? The Fusion Sync will go red as well.

What does that mean? What does that define? What you're letting the electronic engineer know is that there's a new version-- there's been edits done to the Fusion design and I am out dated. So the mechanical engineer actually made modifications either to the board outline or to the components. So now I have that information that I actually should be pulling that new version. Are you with me? Understand what I mean? Status?

Now, if it goes green, what does that mean? It means that the Fusion design is out dated, OK? So now I need to push to Fusion to update. Either I've made some modifications to the board outline, I've added [? holes, ?] or I modify-- basically, it's board outlines, I've added holes, or I've moved my components and I need to push a new version to Fusion 360.

Now, this is important for communicating between teams, as a PCB status in Fusion only changes made in Fusion, not EAGLE changes since the last push. So that's what the status actually is all about. Now, when you're pushing and pulling, as you could see, you'll get that-- [INAUDIBLE]. This microphone and me don't agree today. Sorry about that guys.

OK, so the idea is, when you're doing your push and pull, it lets you see all of your projects, but it also lets you see any projects that you're collaborating with. Yeah, it's on-- any other product that you're collaborating with, that way you could push your body. Now, you have two options-- you either sync up with a project that already exists, or you actually push a brand new product as well, OK? That's it. This is basically the interface through EAGLE.

PAUL CLAUSS: And so because we can either push from EAGLE to Fusion or pull from Fusion to EAGLE, we've got two ways to get a PCB into a Fusion design. The first of which is, taking an EAGLE board and pushing it into a brand new Fusion file. And this will create a file that contains only the PCB board component and the applied 3D packages that we have mapped out in EAGLE. So we've got an example of this I think, let's just go right to that.

EDWIN ROBLEDO: So this is EAGLE right now that we're working on right now. Some of you are familiar with this workspace. So basically, I'm clicking on the Fusion Sync. In this example, we're actually pushing a brand new design into Fusion. Now, it lets me browse your account, lets you select-- basically, because you're using the same account between Fusion and EAGLE. So it lets you browse the different projects you have. And then, once you've found the project that you wish-- now remember, this is a brand new project. It lets you know that your 3D models have been mapped out-- that's what the green checkmark is.

I can make comments to my brand new push. And then, now I could go ahead and do the push. And now that will actually-- it takes a few minutes. So that's why we're using videos, because it may take a minute or two. This is all cloud based and it's using managed libraries. And now, once we push it, you'll get that toggle right there letting you know that it has been successfully pushed. Now, the mechanical engineer or yourself will actually see the render in 3D.

PAUL CLAUSS: So then, I can go into my hub, find the location that we pushed that board to. I can see version one, the comments that Edwin just left are shown in version one there-- initial push to Fusion. And then, I can open up the design. And we'll open up the design. And we can see we have our board component. And then, all our circuit components are at the top level of the browser. And this is something to be beware of, because there's some organizational things like that. Sometimes, we're going to want to create a sub-component to manage our browser a little better.

But for now, let's have a look at the PCB status tool. And what this will show is, that we only have an EAGLE board shape. We haven't used the PCB profile tool in Fusion to create a Fusion board shape. So let's say, maybe as an example, I just want to make this board slightly larger. What I'll actually do is roll back my design time line so I can create a sketch before the PCB. Create an empty sketch on the plane that the board lies on, which will default to the x/y plane.

And then, I'll label this sketch-- I'll just call it Board Profiles For Organization. And then what I'll actually do is go back into the PCB workspace and use the Copy EAGLE Profile tool to copy in the sketch for reference. And the reason I'm doing this is because we need to have a sketch before the PCB profile to create the Fusion board profile from. That's how the design timeline works-- we need to have that future in the order beforehand.

So I'll copy EAGLE profile-- open by sketch. I'll just-- simple example here-- we'll just drag out a larger rectangle using that first one for reference. And now we could actually go back into the PCB workspace and define our Fusion board shape with the PCB profile tool. So I'll just grab those two sketched loops, it'll merge them together. I'll keep my origin in the same place as the EAGLE board. This is important, because Fusion actually uses two board shapes, but only one set of components that refer to the origin. So you can get them jumping around.

And now we'll see in the PCB profile that my Fusion board shape has changed since the last push, my EAGLE board shape is always going to refer to the EAGLE board used during the last push to Fusion. And we'll notice that I end this with the Fusion board shape activated. And that's because we'll want to pull those changes into EAGLE during our next pull. If we had the EAGLE board shape selected, there would be no changes to pull into EAGLE.

EDWIN ROBLEDO: So this was basically an example of a simple way of pushing from EAGLE. So now we'll just go into other scenarios as well.

PAUL CLAUSS: So our next scenario is, we might want to start in Fusion. And a lot of times, we're going to want to do this to use the drafting tools in Fusion to start our board. So we can start, create the PCB, create the sketch PCB profile and that will create the Fusion board shape, kind of like we showed in the second half of that last video. And the workflow that we're often getting use here is, create our PCB profile, pull it into EAGLE, apply our circuit components and then push it back to check.

So we've got an example of this here. This is a graphics card for a desktop computer. And we have all our other components in there. And I've already got the sketch for where we want to create this board. So first thing I'll do here is activate a sub-component in my design. I created my sketches for the board profile in there. This will allow us to manage the PCB board and all the components. And they'll all be included in that component, so our browser is not going everywhere.

I'll use the PCB profile tool. This will create my Fusion board shape. The origin I select here will be the origin used in EAGLE. And now I've got my board. We can see, I've got a Fusion board shape-- no EAGLE board shape yet. And I can save this design. And then, Edwin can actually pull it into Fusion, or into EAGLE.

EDWIN ROBLEDO: Yeah. So when you're defining a PCB, it actually gives you the option of thick it is. But we've used values in this. That way, it uses the most common type of prototype [INAUDIBLE]. So that doesn't need to be modified, but it can be if necessary.

PAUL CLAUSS: And one thing I didn't go into much detail there on is, we can redefine our axes for the board. So I'll leave some comments that Edwin will see in the Fusion Sync-- ready for pull to EAGLE. And then, we can go into EAGLE.

EDWIN ROBLEDO: Now we're going to go ahead into EAGLE. Could you pause that really quick?

PAUL CLAUSS: Yeah.

EDWIN ROBLEDO: Now I'm going to go into EAGLE. There it is. So now, what we're going to do is that we're going to launch EAGLE. And EAGLE doesn't know about that outline yet. OK, so now what we're going to do is that we're going to fire up EAGLE, hit the Fusion Sync button. That will let me navigate through the different folders and directories that I have. That way I could find that PCB body that Paul created in Fusion 360. And now, I'll go ahead and pull that in. And this is how the process goes. So I'm going to go ahead and navigate, find that body that he defined.

PAUL CLAUSS: And we'll see a lot of designs are grayed out there. Those are designs that don't include a PCB component. We need to have created a PCB component to link that design to EAGLE.

EDWIN ROBLEDO: So you see that automatically when I linked it-- the first time, it goes in red letting me know that, yes, it got synced up. So now it's in green, because now, it has it in EAGLE. Now it has not been pushed back to Fusion, so it goes green. Now, I'm going to go ahead and use a design block, which is a brand of feature of EAGLE, and add the electronics to this board outline that we have here. Basically, it's a graphics card-- it looks upside down. That's how I imported it. And then, I ahead and add my electronic components to this.

Now, EAGLE gives you all of the checks necessary for an electronic circuit board. Now, once I've placed my components and I'm satisfied with the circuit board-- now, I'm going to go ahead and I'm going, in a few minutes, I'm going to push it back to Fusion and he'll get the notification on Fusion that it has been pushed back to him as well.

PAUL CLAUSS: And we'll see the Fusion Sync button turns green there letting Edwin know that he's made changes that aren't shown in the Fusion board.

EDWIN ROBLEDO: So as we go, we could make notations here-- lets me know which one-- what models actually have 3D models, has the board outlined. Now, I could go ahead and continue with my push over to Fusion. Now, please observe here that we're actually able to notate every time we push and pull, letting the engineer, either myself or whoever I'm collaborating, what changes, what modifications we did. And the beauty of Fusion 360-- it has version control, which is really nice. So every time you're pushing, it's actually creating a new version of it.

PAUL CLAUSS: Yeah, you can think of pushes as just saving a new version of the file. And you can do so either from Fusion or EAGLE. So now I see that Edwin has created that new version of the design. I can open it up. And when I open it up, we'll see that the 3D components from your EAGLE library are now shown on the board.

And maybe already I've decided to waffle on this design a little bit and make some changes. I'll fill in that corner that we're missing from the board. And maybe I actually want to pull those pins over there, because whatever we're interfacing with will be over there. So I'll add that loop into the PCB profile, keep the origin at the same place. Say, OK. And now, let's have a look at the PCB status tool.

So we'll see that in my Fusion board shape has changed and my EAGLE board shape-- still the same as the last push from EAGLE. So we'll keep our Fusion board shape active, because we want to work with it. And then I'll drag these pins. I'll use move PCB components and kind of just eye it out, put them down here and say, OK.

AUDIENCE: You're on the Fusion side right now?

PAUL CLAUSS: Yep.

EDWIN ROBLEDO: I'm just going to pause it really quick, Paul?

PAUL CLAUSS: Yeah, so we're on Fusion side right there.

EDWIN ROBLEDO: Yeah, we're on Fusion side. So we're able to change modify the board outline. And we're also able to move the parts. But those changes don't reflect with the circuitry on the circuit board. So when that gets modified, it has to be pulled back into EAGLE. That way, we can make the modifications to accommodate what the mechanical engineer has done. Is that understood?

AUDIENCE: Yeah. If I'm a mechanical engineer, I don't want to Have anything to do with electrical. But maybe I want to take a capacitor [INAUDIBLE]

EDWIN ROBLEDO: Exactly.

PAUL CLAUSS: Exactly.

EDWIN ROBLEDO: It might be hitting. There might be a violation. So this gives you the capability to move.

AUDIENCE: I can move it [INAUDIBLE]

EDWIN ROBLEDO: That's absolutely correct. You could move it-- you will get the notification that there is a movement. I'll pull that in. I'll see the traces kind of-- I'll crisscross. But now I could rip it up. That way I could do my trace and accommodate the component according to the-- with new placement. That way I could generate those paths, OK?

AUDIENCE: Will you go automatically [INAUDIBLE]?

EDWIN ROBLEDO: No. So in EAGLE, it's called rip up. You got to rip up those traces and turn them back with signals. And then invoke something manual routing or otter router. That way those traces can now be defined.

PAUL CLAUSS: Yep, and we can see that Fusion isn't updating the traces and the board routing from, we can see the footprint of that component still hanging out where it was. So something to note here is, when we go to the EAGLE board shape, we see that the PCB components have changed there. And they're kind of just floating out in space where we have the Fusion board. And Fusion keeps two boards, two board shapes, but only one copy of the PCB component's positions.

So if we were to push back to--

EDWIN ROBLEDO: To EAGLE.

PAUL CLAUSS: Yeah, if we were to pull back to EAGLE right now, with the EAGLE board shape active, we'd see that component in EAGLE would just be floating out in space. And then, Edwin could actually edit the profile in EAGLE. Because we've already done it, what we'll want to do is activate the Fusion board profile and then just pull that.

EDWIN ROBLEDO: Now, when I pull it, I'll see that cut-off taken away in EAGLE, because he saves it and stores it. Now, he can make the notations about using the connector that he wanted, as well as make the modifications to the board. And then, now I'll it in Fusion in red. And in EAGLE, I'll see the Sync button in red and I'll make those modifications there at that point. Any questions about this?

AUDIENCE: Yeah.

EDWIN ROBLEDO: Yeah, man?

AUDIENCE: In Fusion, they can [INAUDIBLE]

EDWIN ROBLEDO: So EAGLE, by default, has approximately 300 libraries of components that are categorized by manufacturers, or that are categorized by functionality. So you have your MOSFETs, you have your transistor's, you have your caps, you have the discrete components, your linear components. But we also have by different companies, like in Infineon and Samtec as well. So yeah, we have quite a bit. Now EAGLE does have a system by which in the background, we're constantly adding to the library. It's called managed library, so those libraries constantly get updated as well. Yes, we do. Yeah, man?

AUDIENCE: Can you communicate restriction areas to the [INAUDIBLE] for controlling the height [INAUDIBLE]

EDWIN ROBLEDO: In EAGLE, we don't see it yet. No, not really, not the height. So that would be something that they would need to collaborate when they're pushing and pulling and making the commentary. While they do the push and pull, they would have to let us know what commentary. That way we could actually use a right component according to the height.

Now, we use the 3D models. Usually, we used 3D models based from the manufacturer. So we're pretty-- we do our best to get as accurate height as possible. That way you could get enclosure violations if necessary. Absolutely.

AUDIENCE: Is this whole class of capabilities limited to Fusion Ultimate or Fusion [INAUDIBLE]?

PAUL CLAUSS: The EAGLE integration is available in both versions of Fusion-- the basic version and the ultimate.

EDWIN ROBLEDO: Yeah, and EAGLE-- we have a free version of EAGLE. You could start working with it today. This works already, even on the free version. Yes, it does.

PAUL CLAUSS: Any other questions? OK, cool.

EDWIN ROBLEDO: So now we're going to go do some workflows.

PAUL CLAUSS: So now that we've kind of seen pushing and pulling both ways, how should we apply this based on our different design scenarios? So we usually find ourselves in three main situations. We might have a standard board that goes into many different designs that we've modeled out in EAGLE, like this Arduino board. We may have situations in which the shape of the PCB and the form is dictated by the mechanical enclosure, like this electric gearbox here. And we have situations in which we have to assume that both the board and the enclosure design will still be being changed and we need to work flexibly.

So the first one of these that we'll go over is a standard board into many designs. And the big thing that we want to think about when we have this situation is, if we do update the board, we want to minimize the number of pushes and pulls between EAGLE and Fusion to update all our linked assembly designs. Another assumption that we can make is, usually if we're working with very standardized board, the mechanical designer is probably not that likely to be changing it. The preferred workflow would be to work around the existing board that's already been manufactured or any of that.

So what we want to do in this situation is take our EAGLE board, create a new Fusion design, and then we'll have our board only design. And then, we actually want to insert that Fusion design as an X Reference component into our assemblies. And what this allows us to do is keep the EAGLE, the Fusion link in a single design.

So if we make a change to the standard board, it will create a new version of the DC load AU board there. And then, in all the assemblies that that board has been inserted to, it will trigger the Get All Latest this command is, anyone that's familiar with working with XREFs knows. So instead of actually breaking the link repeatedly from EAGLE, pushing and pulling back and forth, we can do one push/pull and then the mechanical team can easily update all the mechanical assemblies.

We can even save different configurations of the board as file versions, because we have the Choose Version tool with XREFs and Fusion. In this little video down there, we have a version with and without a heat sink. And we may only know which one we want to work with later on in the design process. So we have the option to pull either easily into the design, visualize it, all of that.

One thing that's important to note here if you're not familiar with XREFs and Fusion is that, when we're using this technique, the mechanical assemblies and the board files do need to be saved in the same project at the highest level of the Fusion data panel hierarchy, because we can't maintain the link across projects at the highest level. Yep.

EDWIN ROBLEDO: Now here, basically what he's doing is that, we have a version of the circuit with the heat sync. And then we have a version of it without the heat sync. If you join my class tomorrow, we'll talk a little bit more about that heat sync and the thermal properties it actually causes on the circuit board. But that's the nice thing. And on the X References, you could have different teams working with the different versions-- one without the heat sync, one with the heat sync as well.

PAUL CLAUSS: Yeah, Edwin-- he has a whole class tomorrow with my colleague James [? Umats, ?] where they go through the thermal simulations. So if you're interested, have a look. The next situation we're going to have is when the mechanical design is complex and dictates the allowable form of the PCB. This is a complex sketch, it needs to fit into an oddly shaped area. And what we're going to want to do here is create the board in Fusion, pull it to EAGLE, apply our PCB components, and then check our 3D packages after a push back to Fusion, just like we showed in the graphics card demo actually.

So this gives us the ability to reference existing model geometry in the Fusion design while we're creating a board, which makes the sketch much easier to create. I can project a couple lines, do a couple offsets to define that sketch up there. Whereas, Edwin, do you want to walk through?

EDWIN ROBLEDO: Yeah, so some of our EAGLE users here, you'll understand that the complexity to create this type of board outline in EAGLE is actually no easy feat. Absolutely not. EAGLE is not really a drafting program. EAGLE is basically a circuit board designing program. So our drafting tools are extremely limited. So to be able to do that, it would take the engineering maybe half a day.

Now, he could also use maybe [? de-accept. ?] Now, that causes a lot of your prone to error for scaling in unit systems. Now with this new system, he's able to project that complex outline. And I'm able to pull it into EAGLE and actually populate it. And then, as soon as I populate it, he gets the information and is able to now see if the board actually will work for him and see if the heights will work for him as well.

PAUL CLAUSS: Yep, and if we needed to move anything around on the board after we see the PCB components, we could easily do that and then pull back to EAGLE.

EDWIN ROBLEDO: Now this is going to be a very common workflow, because usually, the board outline will lead this dance. Usually, the mechanical engineer, the board outline-- he's going to actually be working with some sort of enclosure. So this is a very, very common workflow. Yes, sir. Please?

AUDIENCE: Yes, I'm just wondering if the PCB sketch, does that follow the same rule [INAUDIBLE] sketch so that, for example, you've got [INAUDIBLE] those need to be changed. [INAUDIBLE]

PAUL CLAUSS: Absolutely. The important thing to note there is, only the Fusion board shape is linked in that way. Because we don't-- if we copy the EAGLE sketch, like we showed in the first example, that EAGLE Sketch won't update if we changed the board profile in EAGLE and then push in a new version. We'll still see the old shape there. So we need to do it again.

AUDIENCE: Can EAGLE handle [INAUDIBLE] profiles in our supply chain?

EDWIN ROBLEDO: Not yet. I don't think it can. Not yet.

PAUL CLAUSS: Sporadically. I wouldn't trust it at this point.

EDWIN ROBLEDO: Yeah, not yet.

PAUL CLAUSS: Yeah, so you want to kind of stick to [? arcs. ?] Yeah.

EDWIN ROBLEDO: But we're working on it.

PAUL CLAUSS: Absolutely. So the last situation is when both the board and enclosure are still being designed, we may have large changes made to the board. And in this situation, we want to approach the whole design in a way that allows both the board and assembly to be easily updated from either side. And this is actually easiest if we start with the Fusion board shape and then use it throughout the design process to drive the PCB.

The reason we want to do this is because we have the two board profiles present-- we have EAGLE and Fusion board. And starting with the Fusion board shape and then continuing to use it, presents the least risk of making changes to the board that may cause lost references or bad geometry that doesn't work out in the assembly design. And this is because the sketch defining the Fusion board shape, like I was just saying, is native to the Fusion design. We can parameterize it. We can refer to it more easily. And we can trust that the references aren't going to be lost, because we can use that one sketch throughout the whole design process.

The other advantage here is, changes to the Fusion board shape will be shown immediately in the Fusion assembly. We can easily visualize different configurations and changes to the board. We could set up an EAGLE board parametrically using joints and other techniques than the sketch to update correctly. But every time we wanted to visualize the new design, we'd need to push from EAGLE to Fusion.

So it's a little easier to view the configurations like we've got up here. We moved all the knobs and the switch around, all of that.

EDWIN ROBLEDO: Actually, when we were working with this, those knobs moved all over that board, to be honest with you. The knobs, the on/off switch, as well as the LED display. So we were constantly going back and forth, because now we had to take into consideration the thermal from the heat sync was going to damage our LED. So all sorts of changes that were needing to be done on the circuit board, and then pushing back and forth [INAUDIBLE].

PAUL CLAUSS: And when we used the Fusion board shape, we can see down in the corner.

AUDIENCE: There used to be an exporter from EAGLE to export your [INAUDIBLE] simple prototypes, you could actually cheat on [INAUDIBLE]

EDWIN ROBLEDO: Well, yeah. We still have that you ULP-- the export g-codes-- it's not really elaborate though.

AUDIENCE: Is there any plans to integrate that functionality into Fusion so that you could actually machine out some of the [INAUDIBLE].

EDWIN ROBLEDO: If I'm not mistaken, absolutely. Absolutely. Sure thing. Yep.

PAUL CLAUSS: Yeah, my understanding is that will be down the road, but it will be something that--

[INTERPOSING VOICES]

EDWIN ROBLEDO: --and sketch your own boards. Absolutely. Sure.

PAUL CLAUSS: And going into the manufacturing side of things, we can see the sheet metal down here. If we use the Fusion board shape, we can easily update all our manufacturing to prototype immediately. Yeah, so same thing there. So we actually have a quick example of that.

So this is a DC load circuit that measures DC loading.

EDWIN ROBLEDO: Yeah, basically, what it does is that, you put a load on it, use the knobs, the C of the load that you're using will give you the current that you want. That's basically what this--

PAUL CLAUSS: And we'll just show-- this will all be on the Fusion side, but how some quick changes are updated. So its design is almost done, but as the manufacturing engineer, there's a couple changes I want to make. First, we'll show that all the cams completed here-- I'll show it with the sheet metal. So yeah, we have our water jet and we're all ready to actually make this part.

But let's say, maybe some of these holes I want to move around a little bit, and let's say, since we've been doing it for so long, I want to just move the knobs one last time just because. So first thing-- these holes, I don't like how they're on the sheet metal bend. And that's all driven. Those holes are for mounting of the board. So they're actually started their life in this design in the Fusion board shaped sketch here. So I can move them over. And we'll see that the model updates, as we would expect it to to do that. We have a little more space there. Things are looking a little better.

And we can see the board updates, those holes have moved, all my mounting hardware and the other components updates. That change is complete. So then, let's say I want to just move these switches and potentiometer knobs around just a little bit. Again, I could use Move PCB Components, get things just where I want them. And I'm not moving any of these components drastically here. What we're trying to illustrate here is, this example shows how the integrated tools make this a simple change.

We don't have to create a new version of the board and then export it out, bring it into Fusion, check it-- all of that. We can just do it, see that everything works. And then we'll see now, if I go to my metal component there, we can see that my flat pattern is out of date. So I'll go to Cam. Everything still looks like it's where it should be, but we know that flat pattern is out of date, so our manufacturing engineer already has a red flag there. So we'll update the flat pattern. And go back to our Cam workspace.

And now we can see this appears a little off. All I need to do to get our tool paths set up again, instead of exporting sheet metal to a new program, opening up a new Cam set up there-- all I need to do is regenerate the tool paths and we are good to go. We can continue our design process on this part and actually start prototyping it.

And if Edwin needed these changes to the board, all he would need to do is open up the board file in EAGLE, see that the board-- that the Fusion sync button is turned to red.

EDWIN ROBLEDO: So whatever components you move, then of course, we would make the modifications appropriately into EAGLE as well, then the traces, then the components as well. Because they need to be updated of course, because you move parts. As soon as you move part, no matter what you do, you got to go edit it back in EAGLE as components.

So we could go back into EAGLE, rip it up, retrace, run the outer router, whatever tool you want to use. And then, go ahead and push it back to Fusion-- that way they sync up.

PAUL CLAUSS: Yep. So when we approach designs using these different workflows and use them properly, they present a few advantages over our previous methods. The biggest advantage that I see here is that the mechanical and electrical teams can work through design iterations in a single Fusion design in a single EAGLE board. And this is great, because it eliminates the issues with file conversions and introducing the potential for errors there. And it's also much easier to track changes to the board.

We already talked about the Fusion sync button and the PCB status tool. We have the comments on all of our versioning. We can see in the Cam workspace out-of-date tool paths and the need to update flat patterns for sheet metal. And we can even go into A 360 where folks on both teams--

EDWIN ROBLEDO: Yeah, this is the best part. You could actually push this to A 360. And they can make comments. Anybody that is collaborating on this team, they could do markups as well, let us know if there's any other modification. So the entire team is exposed to this as well. And we can just keep track of that as well.

PAUL CLAUSS: And that actually shows an example with the Z height there was, from looking at the board and our sheet metal cap, I realized that this circuit components sits a little higher than we need it to. How can we work around?

EDWIN ROBLEDO: Yeah, exactly. So you'll get the violation from the height. So he either has to fix the enclosure to accommodate this. So what I want to mention is, it's always about using less mouse clicks. But this is a whole different world now. See, throughout the time, there's always been a demand for a 3D viewer for EAGLE. There's always been a demand for interaction with MCAD.

So out of this, as they line up with the future of making things-- has now taken both products that existed and actually make them collaborate. So now, there should be no error now between file conversions between the mechanical engineer as well as the electronic engineer. Those no longer exists in that gap. So for all that matter, we've closed that gap. That gap no longer exists and we're going to continue improving on it as time goes by, OK?

Being able to export DXF, import DXF, get me a bit map, get me a [INAUDIBLE]. No, that's all gone. You just push and pull from Fusion from within EAGLE and that's been totally solved as well.

PAUL CLAUSS: And this really allows the design team, on both sides-- electrical and mechanical-- to just be more adaptive throughout the design process. It's easier to react changes from the other teams. And this allows for us to create better quality products in shorter time frames.

EDWIN ROBLEDO: Yeah, and these workflows are just some basic ones. We just want to give some examples of one. But the amount of workflows that can be embedded into this are [INAUDIBLE].

PAUL CLAUSS: Yeah.

AUDIENCE: So most of the components that exist are in EAGLE as a database [INAUDIBLE]

EDWIN ROBLEDO: OK, so let's talk a little about that.

AUDIENCE: [INAUDIBLE] a lot of these that are coming out where positional accuracy is really important. Is there a workflow for taking a model if you have to design a new model [INAUDIBLE] imported into EAGLE to use on the board itself?

EDWIN ROBLEDO: No, not really. No. No, not yet. So when it comes to the libraries-- so we have a system now called Manage libraries. And the managed library, we're giving the manufacturers of those components-- we're giving them an account. Now they have an account and I could see those accounts from within EAGLE. Before, you would have to download libraries. You would have to navigate to the manufacturer and hope they had it in EAGLE format. And then, you would download the library and hopefully you could convert it. If not, you would just have to recreate it.

So what we've done is that we've introduced something called Manage Libraries and we've given accounts of the different manufacturers. So when you're within the EAGLE environment, you go to add and you actually can see what they've contributed and bring in those parts now-- is what we're doing. So you don't have to go navigate for libraries.

I mean, you still might. This is all brand new, so we're trying our best to add as much and we're trying to update. Also, the 3D models-- not all of our libraries yet have all the 3D models mapped out. But we have a team only doing that by itself. And then, they're clearly labeled in EAGLE which ones are actually mapped out with 3D models. So when you push the Fusion, you'll get that realistic measurement-- the realistic component as well.

PAUL CLAUSS: And to tack onto that a little bit-- while you can't directly link a Fusion design to an EAGLE library right now, that is something that's coming in the future. Right now, you can model whatever you want in Fusion and put it in an EAGLE library. You just need to export it as a [? step ?] file and then import it to the library online at ecad.io.

EDWIN ROBLEDO: Yeah, so with your managed library, you could assign which component, which [INAUDIBLE] model it's going to have. And EAGLE actually links that modeling with the cloud. And that way when you push the Fusion-- that's how this whole magic works.

AUDIENCE: [INAUDIBLE]

EDWIN ROBLEDO: Yes, on EAGLE-- absolutely. Right now, we don't have it for rigid and flex boards. We do have certain technology, like tear dropping. So we have certainly some technology that will actually be able to help for that, but we're working on that. So right now, when Autodesk acquired the company, what we're doing is, we're actually adding-- what they've added in the last eight months would be-- I would dare to say, we haven't added that many features in EAGLE maybe in the last 20 years.

So soon we'll have push and shove. We've done some great-- when it comes to manual routing. So the use of EAGLE is actually getting a lot, lot better. And then, we'll start adding some more technology as well. Absolutely. Sure thing. Any other questions? Fusion or EAGLE? Well tomorrow, I'll be doing a presentation of a DC load board. But tomorrow, I think it's at 8 o'clock in the morning, it's going to be more about the simulation side of it.

EAGLE now has the capability of doing something called spice simulation. That was just added like two weeks ago. So I'm even kind of new to this for EAGLE. Now that allows me, gives me the capability to create a circuit and actually do a virtual test on it and see how it reacts to it. Like, taking a board and putting a couple oscilloscope probes and see what signals I get. But basically you could do that virtually.

Now tomorrow, we're going to do a thermal analysis on what happens on a MOSFET when you actually do simulation in EAGLE and what happens with the thermal reaction that happens in using the simulation capabilities of Fusion 360 as well. So we'll be doing that tomorrow, OK? Any other questions or anything? Well, thank you for joining us. We greatly appreciate it. Hopefully it was informative. This is all brand new to all of us, so if you have any questions, I have business cards, or you could visit us at the answer bar, OK? Thank you for joining us. Appreciate it.

PAUL CLAUSS: Thanks everyone.