Fusion Product Design Extension Tips and Tricks

VASEK PRCHLIK: Welcome to Autodesk Fusion Class. My name is Vasek. I'm leading one of the development teams in Autodesk. I will be talking about plastic part features from Fusion product design extension. So, again, I'm a UX designer, and I'll be demonstrating plastic part features in Fusion.

Designing plastic parts can take up a lot of time, and you can easily make errors. Practice and extension automates time consuming and repetitive tasks by using manufacturing eval features, such as Boss, Snap Fit, Rest, Geometric Pattern, Rip, Web, Thin Extrude, Shell, and Fillet. We will also show you how to use plastic part rules to gain additional productivity. Now, let's take a look through the model that we are going to use.

This is a simple case that's made to hold the Arduino board. And it's made by injection plastic production method. So it needs to be ready for this production type. While plastic partitions will help you to design a part that will fulfill all that needs, so we will take care about the thickness of the wall, draft angles, fillets, and so on. So, if you take a look to the case, on the bottom, you can see holes that are there for ventilation, too, that are going in and out.

And if you hide the top part, inside you will see the Arduino board. It's connected to the case by Snap Fit. That's one of the features we will be demonstrating. And if you hide the board, you can see the rest of the plastic part features.

So there is a thin shell that has the thickness that is driven by the material that we use for production. We will show you how to create both, including grips to make it stronger. That is a Snap Fit to hold a PCB board, Web that makes the case stronger and also serves as a support for the PCB board. And the bottom surface is flat because of we need to hold it on the wall, and it's created by the rest command.

So let's start with taking a look how we can use plastic part rules to modify, and drive into assembly. So part plastic rules capture know-how for easy creation, editing, and range of plastic part features. And Martin will start with showing how to edit entire model using rules, and then he will show you how to create rules. And we will talk about supported commands, and share a couple of tips and tricks.

So, now you have the plastic part that is decided to be produced by injection molding. So to be able to do that, well, you need to take care about a lot of things about thickness of wall draft, angles, and fillets, and doing that manually is a lot of work. So that's why we designed plastic part features to do it for you. And in addition, rules helps you to change that very easily when you change your material or setting. So in our model, you already have a plastic barrel for ABS material with a wall thickness of 0.1 inches.

And let's say that our design goal is to change that, and use a different type of ABS that will have a different wall thickness. Let's say 0.14 inches. Doing that by ULA, you will need to go through each single feature and modify it. But thanks to rules, it's just one-click operation. So you select the ABS with 0.14 wall thickness, and there are also different draft angles, and so on. And as soon as you click OK, it's going to modify entire model.

So it goes through the entire model and change all the thicknesses, draft angles, and fillets to create a new model. . Let's review the changes in more details. And here, you can see the before and after in one screen. And you can see that the shell thickness was 0.1, and now is 0.14. The Web is also bigger because the front material, the fillets are slightly bigger, and also both geometry changed a little based on the change of the material. So in one click, you modify the entire set of features to fulfill the need for the new material.

Now let's take a look to the list of features that are supporting plastic part rules. So we support following commands-- Boss, Snap Fit, Rest, Rib, Web, Thin Extrude, Shell, and Fillet. So let's take a look how to create a rule if-- you can go back to the Fusion and create a plastic part here. So what you see is a simple box that's like the beginning of our design of our plastic part. We need to add a shell there to make that hollow, and start adding features like Ribs, Boss, and so on.

To do it in a smart way, we are going to use rules. So let's start with assigning a rule. First step is to select the material, and that's like ABS 0.1. And as soon as we assign it to the model, now Fusion knows that this is a plastic part. So all other operations will behave in a smart way to fulfill the requirements of such a material. So let's start with a shell.

As soon as you click here, you can see that the Shell command is now behaving slightly differently because the thickness is all driven by the T-- the thickness from the ABS rule. So after clicking OK, we have thickness, and we can continue doing Web.

So we need to select the sketch points. And as soon as they are selected, you can see that the web is also taking the thickness, and draft angle from rules, and field radius is calculated as well. So if we click OK, now we created the basic of our case. If we take a look to the cross-section view, you can see that everything is automatically done using the rule from the material. So the raw thickness and thickness of the web is driven by the material thickness. We also use the draft angle and fillet.

Now let's talk about tips and tricks. First we'll be using the custom thickness, and save it as a preset. So let's edit the Web command. And let's say that in our design we need to have the thickness not having the same thickness as the outside wall, but we need just half of that. So we can adjust that here in expression.

So if we multiply it by 0.5, it's going to make it thinner. And if this is a knowledge we want to capture, we can save it as a preset. So now if we can click through the plus sign, it's going to add a preset here. We can rename it like My Preset, and that's a way how to capture know-how about using the same design practices. As soon as we create a preset, that we can also say that it will be the default one for future use. So there is ability to say that the current preset will be default for any future operations.

So let's click OK, and create it. Now, if we create a new web-- let's try to do another web inside of the body-- you can see that automatically the web is using the same rule. So if it is industry practice in your company, you can save it as preset, and capture the know-how, how to do the right design of plastic parts. So we can create that, this new web.

And the last interesting information is that, if you want to use the plastic part rules outside of the plastic part environment, you can still do that by using parameters. So if you display a Fusion parameters table, you can see that there is a new Plastic Rules section. And the parameters from the rules like Thickness are there so they can be used, for example, in your sketch. And then when we refine the rule, your sketch will change as well.

Now let me go through all the plastic part features, and we will start with Boss. Boss is used to create both the connections in plastic parts. It adds material to thin design, and it can also serve as a support. So Martin will show how to create a simple main geometry of Boss, how to add Screws, and how to add Ribs.

So here we are back with our case for Arduino board, and you can see that there is a bottom and top part, but they are not connected anyhow. So our goal is to connect these two parts together. To be able to do that, we will use Boss with board. As a first step, we need to create a sketch that will be on the splitting line between the top and bottom part. And this sketch points will be used as a definition for location for Boss. So now when I start a Boss command, first thing is to select these points. So we are going to select four of them.

And you can see a preview of the Boss. The preview includes both as well. Well, interesting point is that our Boss command doesn't create just a single Boss. It creates an entire Boss connection. So in the blue column, you can see the Boss in the bottom part of the case. Yellow color displays the upper part, and that is also a board. So entire connection by Boss is done by one powerful command.

Because we assign a rule to this the ABS plastic part, the both side one, the top one, and side two are using the ABS as a material. So dimensions of that are driven by selected material. So let's have a dialogue about what we can do here. First is the flip. Flips have to make a decision if the bolt is going from bottom up, or vise versa. We can also change the offset so the splitting line of Boss will be different from splitting line of the case. So we can move it to change the ratio between these two Bosses. But we will keep it as zero, and stay on the same surface.

Entire Boss is driven by bolt. So if you change bolt, it's going to change the Boss. And for bolt definition, there are a lot of different options. So you can select the head type. So if you'll go through it, you can see different type of head bolt. The head of the bolt actually defines also a hole in the Boss and dimensions of the Boss. So now you can see that the hole has a different shape, and everything is slightly bigger to be able to work with this bolt. Similar as the head, we can change also the drive type. So there are multiple options that will help you to configure the bolt that you need for your application.

Well, now let's try to change the diameter. And as soon as we change the diameter of the bolt, you can see that entire Boss was changed. So everything is driven by bolt. Instead of manually filling all the different parameters of Boss, you can simply change the bolt, and everything will follow the bolt and the requirement that this bolt breaks through to be able to connect upper and bottom side.

You can also adjust the length of the bolt using Rib. And there are multiple types of holes that we support. So if we take a quick look we support a simple hole here, the counterbore hole, and countersink bore hole. And for the depth of the hole, we have three options, being measured from the bottom, from the top, and making the hole that's going through. OK, so we are done with configuring the Boss. So let's say-- let's click to OK, and create a modal.

If you review results of that operation in the section view, you can see that there is one bolt that was attached to the bottom part, one bolt was added to the upper part of the case, and there are four bolts inside it. So let's hide the top part of the case, take a look inside. And you can see four bolts being positioned there as well.

So if you take it to the Boss, it may need to support-- to be a little stronger. To do that both command supports also creation of Ribs. So if we added the Boss, we can go to the Rib tab and start adding Ribs. We are going to add it to the size 2. Size 2, that means the bottom part. And you can use simple shapes, or you can actually extend it to the [INAUDIBLE].

Let's use that option. And now you can see the additional options in UI to click on and indicate what part of the Rib should we extend it to the wall. So we want all of them to be extended. So Martin is going to indicate that by clicking the appropriate boxes. And when the Ribs are down, we can also modify the size and parameters of the Boss. So let's change the length to make it a little shorter.

Well, we can customize the Rib. Can have it extend it to wall, we can have-- completely suppress it, or we can use the simple wall. So that there is this three state checkbox to indicate what type of Rib you want to use. So now let's look, and create these Ribs.

And you can see a lot of the complex geometry includes the draft angle, and fillets were created in the Boss command. Let's take a look to a couple of tips and tricks that will make you even more productive. First it's using variables for expression. So we are going to create a new Boss to demonstrate that.

We're going to see a preview of the Boss, and there is Advanced section in the UI. So let's click on it, and show all the details that we can influence. So the Advanced sections give you access to all the parameters of the Boss. So you can customize it to fill-- to fulfill the needs of your company or industry best practices. There is a cross-highlighting between the dimension and field, so you can easily navigate to whatever dimensions you want. Tooltips will guide you to give you information about what a variables means. So here you can see the name of the variable, description, also the current expression.

We talk about entire Boss being driven by the bolt. So if you describe-- if you show the tooltip on the bolt, you can see additional parameters that are used here-- variables like HD for head diameter, and so on. So tooltips is your guidance to understand the shortcuts for the variables. So let's do some modification. Let's make E-- that that's a number of-- that's a quantity of material under the head-- to be bigger. You can see the variable, or you can actually switch to the numerical value, if you are interested about what was the result of your expression. So we modified the boss. Let's click to OK, and take a look at it.

So this is our new boss. Now we want to add Ribs as well, but we will show a trick how to make the Ribs in a custom way. So we will change number of them, and also rotation. So let's edit this Rib. If you go to the right page, we can say that we will add Ribs to the bottom part of the Boss. And the quantity is four by default, but you can make it smaller. You can use only three, two, or even one Rib. In our case, let's leave it four. But let's not distribute it over the full circle, but limit it to just half of it.

So we can use the Grip to change the part of the circle, and we can also use Grip to rotate it to play the position that's needed in the design. So if we click OK, you can see that now you have customized Ribs. The last step is about modifying the outer shape, because Boss and all plastic part features are smart enough to react to changes on the shape of your model. So Martin is going to modify the outer shell a little. And as soon as he does that, the Boss is automatically recalculated. So if you go to cross-section, you can see that the Boss is now modified to work with this different shape.

Let's take a look to Snap Fit. Snap Fit helps to connect parts together. It is great for rapid assembly, and it decreases the cost of the design. There are multiple types of Snap Fits. First is parallel. Next picture on the slide shows you the perpendicular one, and we also support hook and loop. So let's take a look how we can create such a Snap Fit.

Well, we are back with our model of the case for the Arduino board. And now instead of connecting it with Bosses, we want to connect it with Snap Fit. So first thing is to have a sketch point that defines the position of Snap Fits, and you have it here on the split line. So let's start the Snap Fit command from plastic part toolbar. And you can see preview of the parallel Snap Fit.

As a first step, we need to rotate it to adjust it with our model. You can rotate all of them together, or there is an option to rotate that individual one-by-one. So now we align the geometry of Snap Fit with geometry of our case, and you can take a look to preview how the Snap Fit looks like, and that had two things that you probably want to modify. First is that the hole that Snap Fit is connected to, it's not coming through. So it will be difficult to disassemble it.

So we are going to modify it to go through. So by clicking through the dimension, it highlights the field, and we will edit the value to be the same as the thickness of the wall. And another issue we want to fix is that the root of the hook is not going to the bottom of the part, so we are going to extend it. Now let's create the-- let's create a model. And if you take a look here, there are four holes, four for the Snap Fits. So Snap Fit is there connecting the bottom and upper part.

If you hide the top part, you will see that there are actually all four of [INAUDIBLE] there. OK, so now let's continue by doing another Snap Fit. And it will be Snap Fit that will hold a PCB board. You can see that PCB board is positioned in the right position using Bosses. However, we need somehow hold it. And Snap Fit is great for that type of functionality.

So first, we need to define the position where the Snap Fit would be, the position of the hook. And we do that by specifying the points on the bottom surface of our case. So after creating these two points, we can call the Snap Fit command again. So as the first thing, we need to change the type of the Snap Fit to be perpendicular one. And now, again we need to rotate it to be aligned with our PCB board.

And now it's already in the right way. And we are going to modify it to better fit this situation. So first, we probably want to decrease the thickness. So let's find the thickness on the picture here, click through dimension, and we will make the thickness a little smaller. Now let's increase the size of the hook, because it needs to go up to the top of the PCB board desk. So we can modify that as well. And to make the connection stronger, we probably want to make it wider. So if we click through the width of the hook, we can modify that as well.

So now the parameters are set, and we can take a look also to the vital part of the dialogue, where we show the hole. Because it creates not only the hook, but it plays the hole collection by creating both hole and a hook. So when you click OK, it creates the hook, and hole that holds the PCB board.

Let's take a look through the cross-section, and you can see that it was created as we wanted. However if you take a closer look, you will see that it would be hard to produce such type of a hook, because it will be difficult to remove it from the mold. So that's one of the type of tricks we want to share with you. If you edit it again, you can actually create the hook undercut.

In the dialogue, there is a checkbox for Hook Undercut. And as soon as you select it, you will see a preview of your undercut, and you can modify dimensions of it. So in our case, we will see the thickness of the hook, and we will not use any radiuses here. Well, another tip is to use a fillet on the root of the hook to make it stronger. That's a great practice to do that, so let's put a fillet there.

So when we modify it, we can click OK and review the results. And now it looks as expected. So you have the undercut to be able to remove it from the mold, there is a fillet that makes the hook stronger. You can see clearance for assembly purposes, and also a little chamfer that helps with assembling. So we created the second type of the hook.

Well, next feature in the set of plastic part features in Fusion is Rest. Rest is used when you need to create a planar sort of surface. Typically plastic parts uses nice, rounded shapes that are great visually and functionally, but not practical for mounting. So let's create a Rest feature here.

To be able to create a Rest feature, you need a thin pad body. So if you take a look through the design that we have here, it's surrounded. There is no planar surface. So it will be difficult to mount this to the wall. So our goal is to create a planar surface there, and that's exactly why we have the Rest feature here. But before using the Rest feature, let's use a little trick, and go back in the timeline. So we will remove all the features that are in the-- connected to the bottom surface, and let us do the sketch and use it for the Rest command.

After initiating this command, you can see that it automatically took the parameters on the rule. So the thickness, and draft angle are now driven by our material. And the preview shows you how it will look like. So let's say OK, and then create the Rest. Now if you will take a look through the cross-section, you can see that there is a planar surface, and it's fully compatible with the rules for material. So the thickness is the same as the thickness of the outer wall, and also there are draft angles to be able to remove it from the mold.

Well, we did the Rest, and now we can replay all the features that were connected to the original surface, and it will automatically adopt to a new surface. So if we move the marker in the timeline, now you can see that a Web is now connected not only the original surface, but the new one as well, and the Boss has done the same thing. So that's a great productivity gain. You can go back, and when you go forward, plastic part features will, in a smart way, attach to new surfaces.

So now let's take a look to Rib and Web. This is a little more complex example of a Rib, where we want to show that you can add and remove material at the same time.

MARTIN ZATECKA: It's actually-- yeah, I think it's still Rest.

VASEK PRCHLIK: Oh, I'm sorry.

[LAUGHING]

Right, right. So we are going to show how the Rest command is going add or remove the material. So let's call the last command. And you can see that now we are both adding and removing materials. If you take a grip, you can go down, and it's only removing material, or it's only adding a material. Let's put it back to the zero position.

And if you view this by a cross-section, you can see additional manipulators, where you can change the angles to have it more functional, or nicer from a visual perspective. OK, so let's create the Rest. And now we can take [INAUDIBLE] to the interesting functionality.

Rest can actually do a planar surface that is going outside of the body. So if we take a sketch that is defining the Rest and make it bigger than the body-- we'll click to OK-- it's going to be a smart way to add the material. So if we take a look to the other side, you can see that all the rules are fulfilled, the thickness of the wall is the same. But now there was material at-- to be able to support this Rest surface.

So now let's go to our Rib and Web, and take a look what we can do there. So we improve the Rib command that's already in Fusion by supporting plastic part functionality. So if we create a Rib here, you can see that now you need to select also the draft [INAUDIBLE] direction to define the direction how it will be removed from the mold, and how the angle will be applied. And it also takes variables from the expressions for both thickness and draft angle. So we can also define if we measure the thickness on the top or on the bottom.

So let's create such a simple Rib, and let's take a look to the Web. So we will start with creation of a Web command, as we already did, and we will take a deeper look what's inside the dialog, and what are all the options. Well, when we started, you can see that now the web is going to the opposite direction we want. So there is a Flip button to select what part of the design would be used to create a Web.

Thanks to presets, all parameters are already set. So we did my preset in the beginning of the presentation, and you can see it's still there. So all the Webs are now just half of thickness of outer wall. We can measure the thickness in the start-- in the top or bottom. So let's take a look through the cross-section, how it changes when we measure the thickness from either top or bottom. So let's create a Web.

And let's move to the last feature, and that Geometric Pattern. Plastic part designers often use complex patterns for both design and functional purposes. This example on the screen shows a nice holder with grips that was created using the Geometrical Pattern. And on the slide, you can see key features that are differentiating Geometric Pattern from regular Fusion Pattern-- its ability to scale, supporting multiple distribution types, clear perimeter, perpendicular to face, and supporting operations. Let's go one-by-one through these in Fusion.

So we are back with our model of the case for Arduino. And you can see that there are no holes for air to go in and out. So we want to create holes for that, but we also want this to be nice looking. So we will be using a Geometric Pattern to do a little more complex pattern than just a simple one. So let's start with a Geometric Pattern command. And the first thing is to select a surface we want to apply pattern on.

So it will be the top surface, in our case. And we have multiple objects type here. We can do sphere, or cylinder, or box. But the most interesting and most powerful is a custom one, and we are going to use it. So when selecting that object that we did, like with a hexagonal object-- four, four, four-- to define shape of the hole, you can now see preview of the pattern. And, well, the object is too big, so we need to scale it. So let's start scaling it, and we can set both the maximum size using grip, or we can go to the dialog and set up the minimum size.

So after defining the size, you can see that now it goes from the small one under-- on the edge of the surface, and a big one in the middle. Now it's perpendicular to surface. So it can be a nice design feature. But in our case, because it's produced by injection molding, we need this to be parallel with the direction of this assemble of the mold. So we can go to Orientation, and change it from face direction to parallel one. And now we need to select the direction of the object.

So now it's parallel, and we can take [INAUDIBLE] to the different types of distributions. So distribution is defining how the object will be distributed around the face. First one is the rectangular one, but we can use a triangle. It makes it nice looking hexagon, circle, and also the radial one. But, in our case, the rectangular one is the one that looks great, so let's use it. Well, now if we Zoom to the edge of the face we selected, you can see that some of the objects are crossing the boundary, and that's something that doesn't look nice.

So that is a very powerful option named Clear Parameter. If you check that, it will remove all the objects that are crossing the boundary. But still, you can see, there are a couple of small objects close to the border, so we can even set an offset parameter. So let's do that, and it's going to remove all the cases that are too close to the border. And now we have a nice-looking pattern.

The last thing you need to do in Geometric Pattern is to specify the operations we are going to do. And it could be Create a New Body, Cut, Intersect, or Join. So in our case, we are going with Cut, because we want to create holes. So we're clicking OK. It's going to create all these holes.

So in one command, we created pretty complex geometry in Fusion. Let me share with you one trick, and that's how to influence the distribution-- the scaling of the elements. So if we take a look here, right now it's going from the small one to big one in the linear way. But Spread is there to change that. So if we can take a look to the slide it shows that. If Spread is zero, it's changing from small one to big one in another way. But you can make it a little more progressive if you go from minus one to plus one.

OK, so let's summarize what we talked about in this class. We did a design of that case for Arduino board, and it's going to be produced by injection molding. That's why everything is driven by that manufacturing process. So we have a nice pattern, nice design pattern that creates the holes on the top. And if we hide the top part of the design, you can see that a PCB board is now hold by the Snap Fit. And if you hide the board, you can see that the thickness of the wall of the case is driven by the rule. And all the features, all the complex features, that are created by the new command.

So we created Boss to hold the cases together. We created Ribs to make it stronger. That is a Snap Fit for keeping the PCB board on the place. There's Web to make the case stronger, and to support the PCB board, and also the flat surface on the bottom that was created by the Rest command.

And all of that is driven by plastic part rules. So changing that is way too easy, because by changing the material it's going to change entire model. So thanks for watching this video, and we will appreciate any feedback about improvements in plastic part features.