Combining Solid, Shell, and Line Elements with Inventor Nastran

ED GILLMAN: All right, welcome to Autodesk 2021. Thanks for joining my presentation. My name is Ed Gillman. I'm a manufacturing applications expert at IMAGINiT Technologies. And I'm going to be covering how to combine solid, shell, and line elements with Inventor Nastran.

So to kick things off, a little bit about myself. I am a mechanical engineer. I have worked in the industry for a number of years. I've bounced around through several different industries, including aerospace, medical, consumer product development, advanced manufacturing, a little bit of everything.

I've built up an Autodesk skill set that ranges from simulation, running analyses with Nastran, as well as fluid dynamics with CFD. I provide consulting services for clients of IMAGINiT Technologies. I also provide custom trainings. I also help with CAM programming and implementation, so CNC programming, advanced manufacturing, and I also do some generative design training as well.

I'm based in Denver, Colorado, which means if I'm not in the office, you're going to find me hiking and biking. I also do a lot of skiing and rock climbing, and recently, I joined a curling league. So any curlers out there, make sure to connect. This is my first time presenting at Autodesk University so I'd love to come back and do this again next year. So if you do have any topics that you'd like to see or any questions that come up regularly, please feel free to reach out.

Let's get things started. Some of the learning objectives that you're going to hopefully pick up on today is going to be, first off, what are the differences between solid, shell, and line elements? How do they differ? And what degrees of freedom do they have? So that when we connect to these, you know what techniques to use to make sure that it's connected accurately but also in a manner that doesn't cause errors or issues with our analysis.

While we go through connecting things, we'll also talk about continuous meshing. So if you are working with shell elements, continuous meshing is a great way to connect those. It eliminates contacts, which is obviously something that can add to your analysis time and cause issues. So continuous meshing is a great way to work with those shell elements.

And lastly, I'll be showing several different ways to simplify your geometry into those Nastran idealizations. So if you're creating solid elements, you don't need much simplification, but if you're creating shell elements or line elements, there is a process you have to go through to create these models ahead of time. And it's important to know what options you have that are out there, what tools you can use to build these models.

So starting with our element types, just some review on what type of elements we're working with and what their limitations are. First is your solid element. This is a pretty standard element for any FEA solver. If you've used Inventor Pro Simulation, SolidWorks simulation, anything that's out there, you've probably used a solid element.

Nastran uses tetrahedrons, so a linear tetrahedron with four nodes, a parabolic tetrahedron with 10 nodes. These have three degrees of freedom so each node can translate in the X, Y, and Z direction. The model doesn't require really any preparation so you can take your CAD assembly or your part file and bring it right into Inventor Nastran.

You don't need to do a whole lot of simplification, and you can work with the production level model if you'd like to. So that's one of the advantages as well as you have a lot of detail. So all of the faces and edges are available for selection. You haven't taken any of the detail out of the model.

The issue with solid elements that you'll run into when working with large structures and large components is the processing time really starts to increase rapidly. So it's going to take a long time to generate results, post process results, all of that starts to add up. And they can also be a little bit stiff when it comes to working with thin bodies.

So if you have a thin-walled component, think of sheet metal, think about structural components like box tube and channel, those components typically are fairly thin when compared with their length, and that's where you need several elements through the thickness to capture bending appropriately, and solid elements make it difficult to do that because of the processing time required.

That's where shell elements really start to perform well. These shell elements are a two-dimensional surface that you can simplify your CAD geometry into. So you need a surface model. These elements, the nodes have five degrees of freedom. So X, Y, and Z translation but also rotation about the X and Y-axis.

So these are going to allow you to accurately capture bending and buckling, especially when you have a thin-walled component. This will also mean fast processing times, and you can eliminate contacts using continuous meshing as well. So really great when you're working with a large welded structure, shell elements are definitely going to be your friend.

The downside of these is it does require some more CAD simplification. Hopefully, you're efficient with CAD and you're comfortable building a surface model. I'm going to show you some great ways to do that today. But if you do build a surface model, it does take some time. But again, remember, you're going to be saving time on the solve and on the post-processing so that time spent simplifying you usually get back.

The only thing with shell elements that is also troublesome is that you can't mesh a complex part like a hub, a shaft, castings, complex extrusions, things like that. If the thickness varies or it's a complex shape, you cannot reference it and create a shell element for that. So keep that in mind.

Now if you want to work with a really large structure with really big structural shapes, line elements are extremely helpful for that. Really, any time you want to simplify things down and use just standard beam bending formulas, that's what line elements are intended for. The nodes themselves can translate in all directions as well as rotate so six degrees of freedom. The great thing about this is it uses a beam bending stress calculation to calculate stress. So you can easily verify your results with hand calculations that you can do most of the time on these shapes.

So the nodes along the length of these line elements, the strength and stiffness at each node is represented by the cross-sectional properties that you provide. So great for large structures. Your displacement numbers are going to be really accurate. You're going to have very good solve times. Again, you lose some complexity in your model. You lose that level of detail that you get with solids. So you can't model a complex connection like a bolt or a pin. Most of the time, these just need to be fully welded structures to work with line elements.

So those are three elements. Let's talk a little bit about when we could use a shell versus a solid. This is a good thing to keep in mind when you start looking at simplifying your assembly. Once you take the length of your component and you divide by the thickness, if that ratio is greater than 20, I would consider looking at using a shell element. This isn't the law so you're not required to do this, but it does become very helpful when you get into these larger lengths and thickness ratios.

So the example I gave on this slide is taking an 8 inch by 8 inch by 1/4 inch plate. If you take the length, so 8 inches, divided by the thickness, you get 32. That falls into the category I show here of using a shell element. So I would simplify this to a shell if you can because it's going to save you time on the analysis and really simplify your model into something that is easy to iterate with.

So this becomes really important when working with large frames. This is a frame that I'm going to demonstrate on today. Looking at this water tank frame, this thing is about 10 feet tall. You've got a large mass of water and the frame sitting on top of it. And working with solid elements, I took this into Nastran, and I generated a solid element mesh.

This is a fairly coarse mesh so I hadn't even really refined the mesh a significant amount, and I was already at 675,000 elements, 43 contact sets, which really adds into it, and the solve time alone was 10 minutes. Now, anyone that's worked up large models in Nastran knows that also the loads, constraints, opening the file, and viewing the results, all of that starts to slow down, too. So the time really starts to add up.

When I used a mixed element mesh, I was able to get the total number of elements down to 29,000. I simplified it into two total contact sets by using continuous meshing for my shell elements, and the total solve time is 30 seconds. So cut it down by a factor of 10. It's very fast. I can run multiple load cases quickly and start to generate meaningful results. So you're spending more time designing, and you're spending less time waiting for that Nastran Solver to finish.

So one thing before we get into connecting these elements is some other tips for analyzing large structures. The tools that I'm going to cover today fall into these four categories. So number one, applying a mixed element mesh to limit the number of nodes-- great way to cut out detail, cut out complexity, and just limit the total number of nodes in your model. That's going to save you solve time.

Number two, continuous meshing-- so if you're working with shell elements, continuous meshing removes those contacts, which also makes the analysis run a lot faster. Number three, symmetry-- so cut your model in half. If it's symmetric across the midplane, there's no reason not to cut it in half or cut it down into a quarter symmetry model. That's obviously going to limit the overall model size significantly.

And then last, if you have a non-structural mass-- so this would be things like a battery, a fuel tank, things like that that are not taking a direct load, they're not being constrained, they're just adding mass to your model-- most of the time, you can simplify those into a concentrated mass or a Force and a Moment.

If that's the case, you might as well do that. That way you're not wasting nodes and elements on something that is not structural and not important for your overall analysis. So these four things are great things to think about, and we're going to cover a couple of these in the demo.

So let's start with how we actually connect these elements together. So now we understand what these elements are. So first thing I'd like to talk about is shells to solids. This comes up quite often. The issue when you're connecting the edge of a shell to the face or the edge of a solid is that that additional degree of freedom that shells have-- so they have five degrees of freedom-- that shell is going to act like a hinge.

So when you load it, even if you use a bonded contact, you're going to get an E5000 error. And anyone that's gotten an E5000 error knows that that can be really painful. Basically, it means that something in your model is not fully constrained and creating a large displacement. There's a chance it'll actually solve and give you results, but the displacement will be something ridiculous like 70,000 inches. If you see that, that's because you need to adjust the way you connect these two together.

So in this video here, you can see this is what's happening. That shell is hinging about the edge that it's connected to because it has an additional degree of freedom. So how do we handle this? There's three options for shells to solids. Number one is an Offset Bonded contact.

So the difference between a Bonded and an Offset Bonded is the Offset Bonded picks up rotational degrees of freedom and connects them. Bonded contacts only connect translational. So this is a great way to do this. It's probably the simplest way to solve this problem. And it's helpful if you have a lot of these connections in your analysis because it's very simple.

When you do this, the face will be the primary. The edge will be the secondary entity. And your activation distance needs to be 10% to 20% larger than the mesh. The reason that is is because the nodes don't always line up between the shell mesh and the solid mesh, especially if the element sizes are different.

This will help to pick up that gap and create a consistent welded contact between the two. The downside of this is sometimes you'll get stress singularities at the corner of the shell, and that's because the max activation distance, it makes it difficult to control the area that's welded. So there's some other methods you can use to control that with more detail.

Option number two is a great way to do that. You can model the weld as a shell element-- so basically, just a small shell element that wedges in and fills the space beneath the shell element to give it support and prevent it from hinging. It treats it just like a weld. You can also model in the solid weld.

But generally, representing the shape of that weld bead, the issue with that is usually these weld beads are so small compared to the size of the overall model that you have to use a really fine mesh on those beads to get anything meaningful. And generally, you're going to have a stress singularity at the corners. So it does do a pretty good job of holding together the assembly, but it does require some more prep time, and sometimes you get stress singularities on those solids. So when you do this, if you are going to try this, I do recommend using a shell instead of a solid.

Option three is a really great option as well. This involves actually creating a perpendicular surface to your shell. This is a T connection that then translates that into a face to face contact. So instead of it being a hinged edge, basically, what you're doing is you're adding an additional dimension to that shell element by capping the end of it.

So first, you create a shell idealization that is perpendicular to that component. You're going to make it equal to the thickness. So the height of it will be equal to the thickness of your shell. And then make the thickness of that idealization about 0.001 of an inch, maybe up to 0.005 of an inch. You're just giving it a small dimension in that additional orientation so that when that shell pulls down, it pushes into that welded contact, and you eliminate that additional degree of freedom.

So I'll show this in more detail in a moment so that makes more sense. Once you do this, you need an Offset Bonded contact between the T surface and the face of the solid. That will translate that stress from the shell into the solid. And if you split the solid around this T surface, you'll get the nodes to line up around the edge. So you can create a solid element node that lines up with the shell as long as you split the solid to match this T surface.

So when it comes down to it, you can kind of choose your weapon here. You can take your pick. When I ran this analysis using all four of the methods, it actually ended up yielding very similar results. Displacement was almost identical. The stress is varied slightly, but overall, these approaches are all very useful and can be used in combination if necessary as well.

The one that typically causes stress singularities is the Offset Bonded just because it's difficult to control that max activation distance and where you're picking up nodes along the face of the solid. So I do prefer option one and three which is using Offset Bonded if it's a larger structure with a lot of these or option three which is that T connection because it does do a really good job of translating that stress.

So other scenarios you'll run into if you're mixing your mesh-- lines to shells and solids. If your line element is coming in parallel like this situation here-- I have a box tube passing over the top of my shell and it's going to be welded together-- just use an edge to surface Bonded Contact. You don't need to think too far outside of the box here. Primary entity will be your face of the shell. Secondary will be the line element.

You're going to increase your max activation distance, though, to pick up that distance. If you don't increase the max activation distance, you might get an E5000 error. If that happens, increase the max activation distance so that you pick up every node along the shell face as well as the line element. You might need to split off the face to control that contact area better, but you can see here it does a good job of translating that box tube pressure onto that shell element without really too much additional work. So parallel, you can use contacts.

Scenario two would be when your line element is coming in in the axial direction or perpendicular to the face of your shell or the face of your solid. If that happens, you can't use a contact because you can't use a Bonded contact from a face to a point. You can only do it from a face to an edge. So you need to use a Rigid Body Connector or an RBE2 to connect the line to the shell face. So you need something on the shell face to connect to. So what I recommend doing is actually splitting off the shell to match the silhouette of your line element cross section.

So in this case, I was using a box tube so I created a split face on that shell surface that matches that silhouette. The Rigid Body Connector will connect from the shell face, which would be your dependent entity, to the end point of the line, which will be your independent vertex point.

There needs to be a small gap or else you might have issues with that Rigid Body Connector. So make sure the line doesn't go all the way into the shell surface, but this is an outstanding way to connect these together, and it'll translate the stress just as though you had welded that line element to that shell face directly.

Scenario three, so there's a lot of options in here, a lot of different things we'll run into, if you have a line element passing through or nearby a shell and you need to pick up that edge, so this would be an edge of the shell to the point along the line, again, contacts won't work. You can't do an edge to a point or an edge to an edge weld. So what you need to do is use a Rigid Body Connector like we did before. You'll select the edge of the shell element and then a point along the line.

Now, if you don't split that line, there's not going to be a point to select. You can't choose a single node. The only way to force a node to be there is by splitting your sketch line. So go into your sketch in Inventor, split the line at that junction. It'll create a node that you can then tie your Rigid Body Connector to. This is a great way to connect those as well.

Another really interesting one is when you have springs coming into shells and solids. This is going to require a Rigid Body Connector as well. It's generally the same approach as a line element to a shell or a solid. Split off the face of your solid or shell with the silhouette of the spring and then tie the Rigid Body Connector from the face to the endpoint of your spring.

This will transfer the spring stiffness over a larger surface area, which can't be done any other way. Typically, springs come into a single node. So if you don't do this, it won't pick up that full surface area. So this is a great way to tie those in. When you have a rubber isolator or a damper in your model that you need to include, this is a great way to do that.

So last thing here is looking at shells to shells. So shell to shell connections are actually easier than all the other ones because you can use what's called continuous meshing. So if you have a welded structure where you have a bunch of shell elements that are tied together with welds, there's no bolts or anything like that, what you can do is you have to have the edge of the shell co-planar with the face of the adjacent shell.

So as long as the edge is co-planar with the face that it's being welded to, the nodes in the elements will be tied together. So it picks up the nodes along that edge, and it ties the nodes together with the adjacent one, and so the loads will be transferred directly. So this requires no contacts. You can set up a shell model with no contacts at all, and it'll treat the whole thing like it's welded.

This is obviously going to speed up your analysis time and make things a lot simpler. There's less room for error when you have fewer contacts to manage. So this is a great way to connect shell elements together, and this is a method that I use regularly. It does not work for solids or lines. This only applies to shell to shell connections.

One thing to note with this is over the past few years, I feel like it's fair for me to give you a warning that some of the recent versions have had bugs with continuous meshing. Most of the issues stemmed from your boundary connections. So constraints and loads that were applied to shell edges would be applied to additional edges, or they would just go missing.

So what I would do is always open up your model in the Nastran Editor Utility. That will show the idealized version of your model that the Solver will be using. So you don't have to worry about Inventor and the graphics showing one thing versus something else going into the Solver. Always verify these connections in the Nastran Editor. Just make sure things look correct. And I will say the newest version, 2022, they did resolve this issue. So keep an eye on it if you're using an older version. Doesn't mean you can't use it, but just be very careful.

All right, last thing before we get into the demo, I'm going to be showing you some simplification tools. The reason that I use simplification and I create a surface model separate from my FEA production model here is because if you bring your assembly directly into Nastran, if you use the built-in surfacing tools like Midsurface and Offset Surface, a lot of times it struggles with complex structural shapes like channel and angle components because what happens is when it simplifies it to a Midsurface, you get these gaps.

I think you can kind of see it in that image on the right there. Those gaps are created because it doesn't know how to mesh the radius on the inside. So you end up with it just picking up portions of those planes for the Midsurface. And there also will be the gap between components when you're using Midsurfacing so you can't create a continuous mesh.

The other downside is you can't split faces for connectors. If you need to tie a line element into your shell, you can't go and split that face because once you create that Midsurface in Nastran, you can't edit it. So I always create a surface model ahead of time because it gives you the most flexibility and control moving forward.

So some of the tools that I use-- the Inventor Simplification tools. In order to use Surfacing in Inventor, you need to derive your assembly into a part file. If it's not in a part file, you don't have access to those surfacing tools. You can also use Level of Detail and Model States to cut out things like hardware and unnecessary components like weld beads. But again, to use any of those trim and extend surface tools, you need to be in the part environment. So derive your assembly into a part, create the surface model, and then you can either bring it back and do an assembly or just work on it directly from the part.

My personal favorite for simplification is definitely Fusion 360. There's more simplification tools built in than Inventor. If you go into the Simulation Simplify environment, you'll notice there's a bunch of options for surfacing, removing features, splitting faces, and ultimately, it's a direct modeler so you don't have to worry about assembly connections getting screwed up when you remove a face. You can kind of just work on it directly and not have to worry about relationships. Once you modify this version of the model, just export it as a STEP file and then bring it into Inventor Nastran, and you're ready to go.

When you do import into Inventor, just be careful. If you represent your surfaces as composite, which is the default, you won't be able to apply separate idealizations to your shell. You can select that surface body as one single body, and that's it. So if you have multiple thicknesses-- so if you had a 1/4 inch box tube, and then you've got a 3/8 inch I-beam member, you need to specify that these surfaces are individual so that you can apply those idealizations separately to each face in the model.

So individual gives you the most flexibility for defining your Nastran idealizations so that's typically the preferred method. You can also use Inventor 3D sketch tools to create line elements from solids. I typically do that instead of using Fusion 360. It's just a lot faster for creating a center line in three-dimensional space. So I'll show you guys that method as well.

So enough with the PowerPoint, we'll go ahead and move into a demonstration here. I'm going to start in Inventor, and I wanted to clarify a couple of these connections that I had already mentioned. So the first is your shell to your solid connection. I will include this in the downloadable files so that you can spin through it yourself.

But what you'll notice is I've looked at all these different connection types, and if you look at the resulting results, all these same applied loads, constraints, and everything like that, the displacement on these is almost identical for every single one. We're within a matter of less than 0.001 of an inch difference between these four connections so very similar results.

Now, one of the ones that's a little bit more confusing is this T connection. You may not be super familiar with how to do this. What's going on here is this shell element is continuously meshed to this perpendicular surface. So you can see these nodes between the pink and the blue are shared. So what that means is the load will be directly transferred into the face, which is then bonded to the face of the solid. So this a way to pick up that additional degree of freedom.

To do this, what I recommend doing is actually in the solid part file, you'll notice I split off a section of that face with a sketch, and then I patched it with a surface, which means I can then tie my shell into the surface part and then bond the surface part to the solid. The advantage of doing it this way is because I split the surface, the boundary of the shell will share a node with the solid.

So what happens is you get a much better alignment between the nodes of the solid and the shell. Even though it's a different element type, it's a quadrilateral coming into a tetrahedron, the nodes along the edge of that solid where it was split will line up with the shell face, and we'll get a really nice transition of stress from one part to the next. So that's the method I recommend is actually creating the patch surface on the solid part and then continuously meshing it to your shell.

Another one to kind of glance at here is where you have a shell element coming into a line. So I have these two shells being pulled with a load, and the line element is constrained at the top and the bottom. So I can't use a Bonded contact between these two. This is where a Rigid Body Connector comes into play.

So with a Rigid Body Connector, my dependent entity can be the edge of the shell. My selected vertex point will be the point along the line that I split. So this sketch has been split into two separate segments leaving a node at the center that I can pick up with this Rigid Body Connector. So we can tie it in there. I can do the same thing on the lower section, click OK. Now those are rigidly tied together as though I had bonded my tube into those plates.

So looking at it in 3D, it looks something like that with a weld bead going around that tube member. And if I click Run, you'll notice this is a pretty big part, but you can run it in a matter of seconds because these elements are so lightweight computationally. There's not a whole lot going on here, really quick and easy to get results.

Right away, I've got my displacement results, and then I can look at stress on the line element as well as the shelf. This is showing my beam stress. I can then switch my result type to SHELL VON MISES, and I can observe the stress on those shells as well. And you can see that load's being transferred directly into the shell. So a couple of things to cover there. And you'll see that in the larger model.

So the large model I wanted to look at end up looking a lot like this. So this is that water tank frame I showed earlier. I've simplified the primary structural members into shell elements. So if I zoom in here, you can see the junction between these channel components is continuously meshed, which means these nodes along the edge are shared between the component coming in horizontally to this lengthwise member, and that will treat it as though that entire interface is welded. So this is a great way to eliminate contacts. Rather than have a contact at every single one of those locations, the entire shell frame is fully welded together at this point.

Another thing you'll see is where my line elements here-- so I simplified these bars into line elements. The reason I did that is looking at the 3D model here, these are only 3/4 of an inch in diameter. I can't represent them as shell elements because they have no internal wall. It's just a solid body.

So in order to fit a bunch of solid elements in there, I'd need 100,000 of elements to just fit along the length of that line. So I simplify it into a line element, but when I do that, it requires a Rigid Body Connector between the endpoint of the line and the face that I've split off along the shell.

So this is what we're going for. And now to get here, I recommend, again, considering using Fusion 360. So if I open up Fusion, I have that same model that I uploaded from Inventor. This is the original solid model. So the first step you have to take with a model like this is if you want to use continuous meshing, you'll need to first convert your solids into surfaces.

So anyway, I'm going to do that. I'll go ahead and use the Offset Surface tool. I'm going to select, let's say, this box tube. I'm going to offset it by the thickness. So I'm going to actually make it half the thickness to create a Midsurface, so negative 0.1875 inwards. And then I can take that body and simply remove it from my simplified model. So now I have a shell element surface ready to go.

So I've converted my solid into a shell. I can do the same thing with these channel components. So these are different thickness so I'm going to select the three surfaces that make up the channel. I can do that on both of these. These are going to be offset by 0.4 so half of that would be negative 0.2. I can then remove those bodies. So now I have surfaces where those were. I can grab this one as well. So these surfaces have been created.

If I were to bring this in Nastran now, the problem is a continuous mesh will not be added. The reason is by Midsurfacing, I've created a gap here between the edge of my shell and the adjacent face. That's an easy fix, though. With Nastran, you'd be stuck with it, but because I'm in Fusion still, I can extend using the Surface Extend tool. I can grab onto all three of these edges, and I can extend them to match that face. Click OK, and now those are co-planar.

So when we get into Nastran if I go back, that will create a continuous mesh between the edge of that channel and the face of that box tube. So by spending a little bit of time in Fusion 360 extending and trimming those surfaces, I'll have a continuous mesh that requires no contacts, and it's really low maintenance in Nastran to work with.

The other prep work that I will do is going to be for these solid bodies that represent my 3/4 inch bar. Where these are welded into the box tube, if I create a line element, there's no way for me to connect it to the face unless I split that silhouette along that face. So again, I'm going to go to Split Face this time.

I'm going to select the face that I want to split, which is going to be the face of the box tube. My splitting tool will be this bar, and with Fusion 360, you can check this box to extend the splitting tool, and it extends it into infinity creates an intersection. So when I click OK, it creates a silhouette split along that surface that I can then tie my Rigid Body Connector into.

So in Fusion 360, I'm going to create my surface part. I'm going to trim and extend the surfaces to create a continuous surface. And then anywhere I have line elements coming into my solids or my surfaces, I'm going to create a split that represents the silhouette of that part.

So looking at my final tank frame in Fusion, you'll notice I've extended all of these surfaces to be co-planar with where they're going to be welded so I have one continuous surface part. And then, where I have line elements coming in, I've split off the silhouette so that I can use a Rigid Body Connector. So all this prep work was done ahead of time. Once you get efficient with it, it doesn't take long. And the advantage is now when I get into Inventor, it's going to be really quick and easy for me to set this up.

So when I import, one thing I want to look out for upon import of these is, number one, your surfaces, you'll want to make sure you represent those as individual. If you use composite, again, you'll just have one continuous surface part that you can't apply separate idealizations to.

So when I import the STEP file, it brings in my surface model from Fusion 360. Everything is set up and ready to go. The only thing I need to do is convert these solids into lines. I could have done it in Fusion, but STEP files don't maintain those sketches. So what I typically do is I create all my line elements in Inventor after I've built my surface model.

This sounds more complex than it really is. All I need to do is open up these solid parts, so this bar. The same process here works with I-beams, box tubes, anything like that. Open up the single solid part, especially if there's a pattern of those, and what I'm going to do is use the Inventor 3D Sketch. I'm going to create a line. And the Inventor 3D Sketch tool snaps to center points. So especially with cylindrical bodies, if I grab the edge of the cylinder, it snaps to the center point, and I can snap to the center point on the opposite side like this.

I'm going to create my 3D sketch, and then I don't need to delete anything. I can just go to my solid body folder, turn the visibility off, and now I have a sketch line. I can then just apply my line idealization to this line without having to do any other post-processing. If I go back to my frame, you'll notice it replaced that body with a line, and I can then do a component repair replace on the remaining ones with this first one and quickly create those line elements.

So now that I have the line element in there, I've already split off the face so when I go into Nastran, this is done and ready to connect. I don't need to worry about rebuilding the model. I'm going to create a line idealization for that, a shell for that, and then the connector will go between the two-- so Rigid Body Connector from a split face to the end of the line. It's a little bit large, but what you can see there is that it's connecting that point to that face, and it'll treat it as though I've welded that bar into the box tube member.

So a little bit of preprocessing on the front end in Fusion 360 to create this surface part, and then a little bit of 3D Sketching in Inventor, but the result, again, is a frame that looks like this where I have a continuous mesh between the shells, connections between lines and shells, and then my solids up here, I just bonded to the face of my shell element like you would to create any other contact in Nastran. You'll also see I have a concentrated mass here that I've tied into the face of those solids.

So instead of having a solid element frame that looks like this where I've got a lot of components going on, I've simplified it way down. And the great thing about this is it runs extremely fast. To prove it to you, I'll run it right now. So it's going to quickly generate this file. You'll notice if you've worked with this size of a frame in Nastran before, it can take several minutes just to kick the analysis off.

You'll notice using this lightweight model, it's extremely fast and efficient. It's already generated basically the entire stiffness matrix. It's going to start going through generating contacts. I only have a few contacts in the model between the solid and the shell so that should go pretty quick.

And so a large model like this-- this thing's 10 feet tall. It's 6 feet wide. It's a big model. I can run the analysis in a matter of 30 seconds to a minute, and it allows me to quickly iterate because I can go change some variables, run the analysis again, and I'm not waiting hours and hours for this to run. It can be done inside of a minute.

So I'll click OK. It's already finished the analysis and loaded the results. And then I can start digging through these and determine what the next steps are going to be. So it loads the shell element stresses first. You can see the stress along the length of that tube, and then you can see where there's no contact between these bodies. That's a continuous mesh. No Bonded Contacts required, and I'm getting a stress distribution from one to the next really quickly and efficiently.

So I will include these models in the data set so you can look through them. But again, simplify your models. Think about what could be a shell or a line, and then combine those using some of these techniques I showed today, and you're going to have a really great model to work with moving forward.

So I appreciate you attending today. Hopefully, these tips and tricks will help you with your next big Nastran analysis. If you have any questions, please submit them now, and I will be around to answer those moving forward. Thank you.