Enhancing Autodesk Inventor Nastran with Femap: Unleashing Advanced Meshing and Midsurfacing Capabilities

ANDREW JABOLA: All right. Thank you for attending our session today. Today we're going to be discussing how we are enhancing Autodesk Inventor Nastran with Femap. We're going to show some of the advanced meshing and mid-surfacing capabilities as well as other capabilities as well. Myself, Andrew Jabola, and during the live presentation, Dave Weinberg will be presenting at this session.

So first of all, here's the overall agenda. We'll discuss a little bit about ourselves, both about myself and our company and also, Dave Weinberg, who, again, is not able to make it today, but will be at the live presentation at Autodesk University. We'll discuss the objectives of what we're trying to show today for Femap and how we're able to improve workflows within Autodesk's Inventor Nastran.

We're going to show how Inventor Nastran and Femap have actually had a long history together. And then we'll discuss some of the requests that users have been looking for to add to Inventor Nastran. From this, we're going to show a lot of different capabilities of Femap, everything from meshing capabilities, specifically with the hex meshing and surfacing.

We're going to show some meshing of complex geometry and also, additional capabilities such as working with legacy data, post-processing, and other aspects. And then after that, we'll take any questions. And for those at the live event, we'll actually be having a raffle as well.

So let's discuss a little bit about the presenters or introduce ourselves. So my name is Andrew Jabola, and I am both a senior structural analyst and also, our director of business development at Structural Design and Analysis, Incorporated, also known as Structures.Arrow. And in parentheses, I actually mention our partner company, SDA Software, the one that would actually be reselling Femap to those that are interested.

You have a bit of my background. I provide a lot of metallic and composite structural analysis support for a variety of aerospace programs, ranging both from space to aircraft-type programs. On the space side, I've worked on programs such as the Nancy Grace Roman Space Telescope at NASA, or more recently, Blue Origin's New Glenn rocket. On the aircraft side, everything from drones to manned aircraft.

Here, I show Aerosonde from AAI Textron, and one of the most recent projects I worked on was being a lead structural analyst on the Electra eSTOL demonstrator hybrid electric aircraft shown here. In addition to this, I have provided software support for a lot of different products over the past 15 years as an application engineer role, supporting everything from Femap to Simcenter 3D and also Fibersim for a variety of customers. And finally, I do have a mechanical engineering degree from Walla Walla University.

Dave Weinberg, who will be at the live event and will be available to chat with, is one of the other presenters for this discussion. Currently, he's a consultant for SDA Software, and previously, he was a distinguished research scientist at Autodesk in the PDMS division, Nastran simulation, and generative design groups.

He's the former president and CEO and founder of NEi Software, the originator of Autodesk Nastran, and he owned that from '91 to 2014 until the acquisition of NEi by Autodesk in May of 2014. And he is the author, the primary developer of NEi Nastran and NEi inCAD and led the team at Autodesk on the Nastran side.

He has a aerospace engineering degree from Embry-Riddle, has been working in the industry for over 30 years as both a user and developer for large aerospace companies. In addition to that, he's actually a retired USAF aircraft commander and pilot, with over 28 years of military service.

Again, he's not with us during this virtual presentation, but if you attend the Autodesk University event, that's two weeks from this recording, he'll be, definitely, at that event, and we can definitely chat with him if you have questions.

Finally, a little bit about who SDA and SDA Software are. So Structural Design and Analysis, Incorporated is the services side of a company. We're an organization of 25 engineers that helps work with a variety of companies to help design lightweight and load-efficient structures.

We support a lot of aerospace companies all the way from conceptual design to detailed design, and we specialize in composites and lightweight structures, worked with a variety of companies that have made mainstream news, such as Boom Aerospace, Electra, as mentioned earlier, and also, many spacecraft as well.

We use quite a few different tools, everything from hand analysis to Femap to, obviously, NX Nastran, and STAR CCM for CFD and many other aspects of the engineering side. Our partner company that we work closely with effectively is one company, is SDA Software. SDAR Software is a value-added reseller and supports products such as Femap and Nastran and many other products as well. Again, these are two sister companies that effectively act as one company, and from this, we're able to provide both services and software to a variety of customers across many different industries.

So now, we're going to discuss a little bit of the history of-- or sorry, discuss the objectives of how we're going to show how Femap enhances Autodesk Inventor Nastran. So we're going to show today is how easy it is to integrate Nastran with the Femap environments. Really, just a quick preference, and you're able to run as if you were almost running a native environment.

We'll show how Femap has excellent hex meshing capabilities to really be able to model solid meshes very quickly and efficiently. We'll also show Femap's geometry idealization and simplification methods that really speed up the process and being able to generate complex structures, both on the solid side and also, on the plate mesh side as well.

Finally, we're going to show Femap's other capabilities, such as working with legacy Nastran data and post-processing and also, just other geometry types as well. So hopefully, from this, we'll be able to show the value Femap adds to the Autodesk Inventor Nastran environment.

So let's discuss a little bit of the history between Femap and Autodesk Nastran. So when NEi Software was formed by David Weinberg, he actually coupled Femap with then, NEi Nastran, now Autodesk Nastran, together, and it was known as NEi Nastran for Windows. NEi Software is actually a Femap value-added reseller and became one of the largest Femap resellers in the early 2000s.

And Femap has actually been a primary use of many of Autodesk Nastran's capabilities, and it supports many of the extensions natively, such as surface contact, tension-only shells, and a lot of other aspects. And then in 2014, Autodesk acquired NEi Nastran, and from there, many products that probably many people here are familiar with, the Autodesk Inventor Nastran was born. So again, Femap and Autodesk Nastran have been integrated, actually, for quite a few years.

From this, though, there's actually been a lot of user requests, and so we're going to show how Femap tackles some of these requests. So some of the top requests that have been found on the Autodesk Inventor Nastran forums are the following. Seeing a lot of things with hex or hex-dominant meshing, something that was added recently in Femap that has been a game changer as far as meshing capabilities for solids.

Continuous solid element meshing, having maybe multiple solids that are all connected together has actually been another area where we need to be able to have mesh nodes. Femap, again, simplifies this process, which we'll demonstrate here shortly. Mid-surfacing with tapered shells and offsets is another aspect, and also, better results processing and better xy charting are other areas.

So the next couple of slides just show some of the areas of people asking these questions, people asking for quad brick meshing, what's the status on that, continuous solid element meshing, and hex-dominant meshing, and even to the point even in some of the requests have actually come from other Autodesk employees.

So from this, we're going to show how Femap tackles these and gives you that ability today very easily within, giving your team a much more capable analysis environment with your current solver. So the first thing we're going to do today is we're actually going to demonstrate this live within the Femap environment using a very simple example here. This is just a little bathtub fitting, and we're going to show how we can create different meshes from tet to hex to plate and how we can easily define boundary conditions and also, reflect the geometry and also, take advantage of many of the mid-surfacing geometry idealization.

So with this, we're going to go straight into the Femap environment. And the first thing we need to do is link up Autodesk Nastran. And this is actually a very simple process. So let's say this is a brand new install. You've just installed Femap for the first time. We can go to Solvers, and in this case, I've already pointed to it, but you simply point to your Autodesk Nastran license.

At that point, you're pretty much up and running and ready to start working with Autodesk Nastran. We're going to actually solve a couple problems live while we're working with this.

Now, with Femap, Femap is geometry neutral, and it's actually solver neutral. Again, we're going to be working with Autodesk Nastran, but we actually can support quite a few other analysis packages. So in case maybe you've received files that were built in Ansys or NX Nastran or other aspects, we can import that in. So that is one of the powers of Femap is being very neutral.

So for the geometry side, we're going to go ahead and pull in this bathtub fitting, bring this in. And so we brought in a parasolid file and actually just a mention here, again, we can support quite a few options, everything from parasolid to STL, to CATIA, so on and so forth, so quite a bit of power in that respect.

Now, typically, we need to assign boundary conditions at the start. So here, we can create constraint containers and load containers. Again, one of the beauties of Femap is the ability to be able to organize this. And many times, you'll have models with hundreds of different loading conditions. And so this can be easily organized using this environment.

In this case, we're just going to simply constrain the surfaces here. So we're going to fix the base here, and we're going to apply a 5,000-pounds load down onto this surface as well to be able to put a bending load into this bathtub fitting.

The next thing we need to do is, we need to go ahead and mesh the geometry. So if we do mesh geometry solids, first thing we need to do is define a material. Now, Femap can use a variety of libraries here. So for instance, here, we're going to use a 7050 material.

Now, these libraries can be edited so that in case maybe your company has a standard material library, instead of always having your analysts try and find that data, you can have them all point to a single file and use a uniform material data library, thus, reducing the error in your analysis. So here, we've loaded the data, specifically, Young's modulus, Poisson's mass density being the critical aspects.

Next, we're going to do updating, sizing. It usually gives a recommended size for the solid, and we have a lot of control on our meshing, so a lot of different options here. For the ease of this, we're just going to go with the defaults. And at this point, we're going to go ahead and mesh our geometry.

So here, we have a solid mesh with about 40,000 elements, and this is actually very quickly solved. So at this point, we can generate a new solution. Now, again, we have a variety of solution types we can write out to. So you could, again, import a model from a different solver or write to multiple solvers. In this case, though, we're going to use the Autodesk Nastran environment.

We have full control of everything from core counts to parameters and even being able to manually edit as well. So just to go through some of the options, a lot of this is easily editable inside the environment. And if you really need to add data, we can even preview the input and edit that preview right from the model.

Now, at this point, we're ready to go ahead and hit Run. So I'm going to go ahead and save this model into just a test folder, overwrite that one and go ahead and hit Run. And so at this point, this is actually running Autodesk Nastran. And so I'll pull this up as it's on the other window. And here, we're actually just directly running Autodesk Nastran. It automatically runs the file and imports and attaches the results as a neutral output file.

And we'll see here that now, we actually have our data. So we can activate this and go ahead and post-process the results. Deform it. We're going to use actual deformation, and let's go ahead and hide the geometry so we can actually see the model. And here, very quickly, we've actually started to look at the actual results.

Now, Femap has a lot of post-processing capabilities, and we're only going to touch the tip of the iceberg of these today. The post-processing toolbox is an excellent tool for being able to look at different vectors, so different stresses, for instance. In this case, I'm interested in just von Mises stress, but we can change this to however we need to look at the model.

So for instance, maybe I want to set a stress threshold. For instance, this being 7050, I want to keep a 60 ksi capability of the material. Many people want different color gradients. You can either generate your own. In this case, we're going to use the known magenta. Now, we can turn off Filled Edges and be able to look at this very quickly.

From this, as an engineer, you can quickly look at this and go, all right, we need to probably thicken up this part to be able to take the higher bending load. And we can see the overall critical stresses on the model. So again, the post-processing toolbox helps simplify a lot of these capabilities here and makes it very quick as an analyst to set up for the situations you need.

Now, we're going to go ahead and remesh this part. One thing to note here, this is a tetrahedral mesh. It had about 40,000 elements. We can actually do a lot quicker with a similar mesh resolution size and get quite a fewer elements in the model.

So we're going to delete the existing mesh. We're going to keep the property here, as shown. And let's go ahead and show my geometry again. Here, we're going to use the hex dominant meshing. So this is a capability added in Femap fairly recently that allows you to auto hex mesh this part.

In past, you would have to actually try and divide this thing up and do a bunch of different blocks that you could extrude to mesh. And that could take days, if not weeks, especially on complex geometry. But with the hex dominant mesher, it's almost just a single button click where this is replaced the tet mesher in the model here.

So in this case, we have our mesh, our hex mesh. We have a very clean hex mesh here. We could clean it up even further through a little bit of refinement for simplicity. We're able to run with this simple model here. You can see the boundary conditions as such here. Still applied to the geometry. And the big thing is we dropped from 40,000 elements to only 6,000, so this should run a lot quicker.

Now, with this, we already have everything set up, so I'm just going to detach from the original result set and go ahead and run the new results and go ahead and start the model here. So once again, probably before I can even drag the file over, we've already run the model.

And you'll see this immediately loads in the Femap, and we get very similar results that we had earlier. And again, we get the same conclusion, same stress plots, everything. So again, the hex dominant measure, in all honesty, replaces the tet mesher giving you a much more efficient method of analyzing solid models.

Now, we can extend this even further. So for instance, maybe we want to model contact between these conditions here. So with this, we can go ahead and reflect this model very easily. So we'll go ahead and Mesh, Reflect, Element, select everything here.

Now, we can choose if we want to hold boundary conditions, coordinates, or other aspects of the model. In this case, we don't want to copy the load, but we do want to copy the constraints and everything else. And one of the things with Femap we can do is, we can actually take advantage of doing math arithmetic inside our selection box.

So for instance, I want to generate a plane that's about 0.5 offset from here. So we're going to actually just add that right into the model, and if we scroll to this way, we can see that we now have that offset plane that we're going to reflect around. So very easily able to do very quick calculations on the fly on your selections to generate data very quickly.

You'll also see that the mesh is copied and that our boundary conditions still exist, our loads are still attached. And then at this point, we just need to define the connections. So here, we'll go look for contact, and we'll let Femap do all the hard work in trying to find the contacts for us.

We'll hit OK, and what this generates is our regions. And you can see our two contact regions, how they're connected and a property. So from here, we're going to go ahead and edit this Autodesk Nastran property. I'm just going to give us a little bit of additional contact distance and change this to symmetric contact for the solution. But again, we can very quickly set up our contact in the model.

Now, it's going to take a couple seconds to run, so we're going to go ahead and run this and actually show in another instance of Femap another option here to tackle the continuous meshing. So while this is running, we're going to go ahead and pull up another instance, a Femap. So this will start up. And we're going to import the same geometry into the model here.

So we go back to our geometry, our bathtub fitting. And in this case, let's go ahead, and we're just going to reflect the geometry directly across the plane here so that these two faces are shared on the model here. So with this, you can see we have two faces here, two continuous pieces or two separate pieces, but we want to have a continuous mesh between them.

We can, for instance, assign different mesh attributes to this, so maybe mesh control. We're going to assign one property to here, so we'll just generate another material property. We'll just use the 7050 property we used earlier. We'll call this property 1, and let's generate property 2 that uses this. So we'll assign property 1 to this one and property 2 to the bottom.

So from this, we can then go ahead and again, use the same command earlier, hex mesh bodies, set the same size, and we're not going to need midside nodes. We're going to use a meshing attributes that exists in the model. And from here, we're actually generating a continuous part from two different bodies that are connected together. Again, this is tackling one of the requests that have come in from some of the different models here.

Now, we can see this if we change the colors here real quick and show property colors in the model. And see we have two different regions. And right now, they are disconnected, if we show the free edge here. But because we mesh this together as a single piece, we can actually go ahead and merge coincident nodes, and you'll see that Femap has already generated a clean connection between these two models here.

Thus, at this point, we merge the nodes, we show the free edge, and you'll see here now this is actually one piece from two different solids. So again, this tackles the question of doing solid continuum elements with the structure.

All right. We can go back to our contact problem and start taking a look at some of the results here. So this is solved. It actually solved pretty much when we had started the model here. Again, we can take a look at the results. We're going to set actual deformation. And you'll see here when the part is deformed, you can see how this part comes down, starts to touch, and it slips across this face. And even though we only applied the load to the top piece, it's starting to apply load to the bottom based off the stress contours.

We actually have data as well of contact forces. So for instance, maybe I'm interested in contact pressures across the model here. So we'll go ahead and pull that data. Let's go ahead and hide the elements on one of these solids and change our environment.

And so we can see that our contact pressures, we have two high-point loads on the structure here and here, but we're seeing that contact on this surface and also, on the top surface as well of where we're touching across the structure. So again, we've shown how quickly we're able to generate solid meshes with hex meshing and generate contact and be able to post-process that within the Femap environment.

One other aspect is mid-surfacing, so we're going to take this same part and import this, use the same data here, and this time take advantage of mid-surfacing. And Femap has a lot of different tools for generating and modifying mid-surface geometry and being able to modify geometry, in general. A lot of this power comes in the meshing toolbox, which is an incredible tool that we're only going to touch the tip of the iceberg on its capabilities.

So first thing we need to do, as many times as analysts, we need to remove a lot of small features. For instance, these fillets are not useful to us. So we'll grab the blends, and Femap quickly identifies those blends, says, hey, which blends do you want to remove. We can actually quickly deselect ones that we don't need, and we can clean up the geometry here.

Next thing we can do is, we can go ahead and mid-surface. So from here, we're going to generate a plate mesh off this part. So what we do is we specify a target thickness. So we're specifying the max offset distance. It's going to look between surfaces. We're going to go ahead and combine. And from this, we have generated a mid-surface plate mesh that represents the mid planes of all these different points on the structure.

Now, Femap offers a lot of tools for cleaning up and also, maybe adding geometry. In this case, for instance, maybe we want to make sure we have mesh that captures this offset or this boss. So the geometry editing tool gives us a lot of those capabilities. Here, we can project the curves. So I'm going to say this surface, I'm going to grab these curves right here on the structure, hit OK, and you'll see here we have projected those curves from the existing geometry.

We can do things such as break curves on the fly. Maybe we want to do mid-curve breaks here. Split the geometry very quickly to prep for our meshing. So again, we're just quickly splitting our geometry overall across the structure.

But the beauty of this is, actually, this can be done both before and after the fact on meshing. So in this case, we're going to generate a new property once again, specify generic thickness, use the same material we used earlier, set the same mesh size, and set a mapped mesh condition, and apply a mesh to the model here.

Now, we can dynamically still do these geometry edits and have the mesh automatically update So for instance, maybe we want a cleaner mesh with a washer that transitions into the square regions on these holes. So here, we specify our factor. 0.75 is what worked best for this model. And you can see quickly, we are updating this to be a very clean, geometric, organized mesh.

Again, using the geometry editing tools, we can do very quickly modify our mesh to be split up into rectangular regions. So that's effectively what we're doing on the fly. And as we're doing this, you can see how we're getting that data very cleanly into the model here.

Now, from this, I'm going to go ahead and just apply another map to mesh. Just split this up. We've split this up into mesh rectangular regions. Re-specify the mesh, and you can see very quickly I have a very clean mesh in the model already that we can start working with.

We can dynamically size this. Maybe I want to have two elements around here, and I want a couple more elements around these. But all of this provides excellent tools for being able to very quickly and easily control your mesh to generate a very high-quality mesh in the model. Here's a quality indicator just showing that we have a clean mesh, overall.

One other aspect too, in addition to being able to do this, is to take an account of the thicknesses. Now, you'll notice here, when I turn on Thicknesses, these plate elements don't represent the actual thickness of the part. With Femap, we're able to modify these elements and account for that mid-surface directly in the model.

So I'm going to go ahead and select these surfaces to adjust the mid-surface mesh and you'll see just doing that one quick command, we have accounted for the tapered shells, so you can see the tapering as we go from the small to the large and also, offsets on the structure as well. So here, you can see how these elements are offset. We turn off thickness, you'll see that offset in the model here. So again, all of this allows you to very quickly and easily create plate meshes.

So to continue solving this problem, we're going to do similar load cases, so same constraint conditions, we're going to do this time on curve instead of on Face. Grab these curves on the model. Fix that. We're going to go ahead and apply a load on surface. So for instance, here, we're going to add tangent surfaces and once again, apply a 5,000-pounds load to the model.

And then similar to what we did before, we're going to go ahead and reflect this once again. So we can do a mesh reflect, grab our elements. Again, we're going to grab the same options we had from before, and once again, use the same settings we have before. This time because we are accounting for the offset of the plate elements to include that thickness, we're also going to split the difference of adding half the thickness as a reflection plane, plus half that offset distance as well.

And from this, you'll see that, once again, we have effectively the same model with a constrained base here. Similar to what we did before, let's go ahead and define the contact. In this case, we need to increase our tolerance up a little bit. So this looked for all the contact conditions.

You'll see the same regions were identified. Here, Femap gives you the ability to really visualize to make sure, hey, are we grabbing the right faces to show the expanded contact positions as well. And then finally, we need to edit some properties here. So we need to account for the fact that there is a thickness offset. So we're going to change that, and also, change the distance so that we know what to look for and have the contacts see each other, even though the shell mid-surfaces are a little further out.

At this point, we can generate the analysis similar to what we did before. Let's take advantage of the fact that I have a multi-core capability. And right click and Analyze.

At this point, we're pulling up Autodesk Nastran again and just going ahead, it solves very quickly. So all of this is just showing how easy it is, while all this solves being able to generate solid elements, but also, mid-surface elements as well. We can create a lot of complex geometry.

And we've only, again, tackled some of the basics of the meshing toolbox. There's a lot of other capabilities, and we actually do have an appendix session that discusses some of those capabilities as well.

So as we wait for this to solve, you can see here it generates the neutral file and loads up the results, and we should get a very similar result set to what we had before. So we'll set this to actual deformation, set up the stresses. Let's take a look at the deformed shape, turn off geometry so we can see a little bit easier.

And you can see we have that same shape. And let's go ahead and set up the same properties we had earlier where we have a maximum threshold, [? 60 ksi ?] capability. We're getting those same hotspots that we had earlier. And also, once again, change your color profile. And so very quickly, we've been able to generate a similar result set for both a solid mesh, but also, this plate mesh as well.

So again, we've shown this excellent example of the bathtub fitting. And now, we're going to move on to some other examples of more advanced geometry and other aspects of software we can look at. So here's a couple of examples of some solid meshing geometry. We showed on a very simple piece of geometry, the hex meshing capability, and we're going to show an advanced piece of geometry that, yes, it took about 20 minutes to run, but it was only two button clicks to generate this advanced geometry.

So here, we're going to go ahead and open up an existing mesh. Here's our engine block assembly. And what this is is a very complex piece of geometry that would be very difficult, would take days, if not weeks, to try and hex mesh with block elements. And even with a tet mesh, would be a very expensive model to run.

So we're not actually going to run this command, but we'd go ahead and run the mesh bodies command. And using the defaults, we were able to get a very clean hex mesh of the model. So instead of running tets, you can see how we have the excellent definition of block elements, or hex elements, all throughout the model.

And we've captured a lot of the detail and higher curvature areas. And again, this is just only a couple of button clicks and about 20 minutes of wait time, but again, that's 20 minutes of computer time, not 20 minutes of or not two weeks of idealization time by an analyst. So again, very capable and a very useful tool for generating and hex meshing complex geometries.

Another aspect more recently is the use of 3D printing. And many of these files are usually generated in a format of STL files. So in this case, we're going to import geometry of an STL. And so if we go back to here in our geometry, here, we have a lattice geometry of the model.

And in this case, we want to take this 3D printed file and go ahead and mesh it and analyze it.

Now, at this point, the mesh is very not great. This would not be a good model for us to work with as far as being able to actually work with the analysis capabilities. But one of the commands that we can do is we can actually do mesh-on-mesh command.

With this, we select all the elements we're going to mesh, specify our parameters here. In the case here, I would hit OK. It takes about 2 minutes, so we're going to show the result. And about 2 minutes later, we would end up with this right here. And so with this, it creates a very nice-looking remesh of that geometry. All surface mesh to capture enough resolution that we could actually use it for analysis.

Now, in this case, this is only surface meshed right at the moment, but Femap can then turn this into solids. So here, we have about 160,000 plate elements. So here, we'll go ahead and mesh geometry solids from elements. And again, having no existing CAD, no existing geometry, we're able to generate a very clean, solid mesh here in the model.

So here, this generates tets You're going to see this generates about 420,000 tetrahedral elements. And if we go ahead and hide the elements here, you can see, once again, how this data is now a solid mesh that we can actually start working with and apply boundary conditions.

With this data, we can go ahead and start generating new elements. So for instance, I might want to put some load application points, so I'm going to generate a rigid element. And again, no existing geometry using the mesh only, we can search for tangent faces. So for instance, here, I might want to apply a mesh to these elements here.

So about 10 degrees tangency is what we need, so we want to grab those elements, highlight that to make sure, create a new node at the center. And again, once again, we're able to generate a very quick model of new geometry and integrate from geometry sources that may not be typical, such as STL files.

To save time, I've actually already set up this model. The only additions after this point was adding the boundary conditions and solving the model here. So here, we have a 100-pound load, and it's constrained at the other end. And from this, we can then generate advanced stresses of the model and be able to look very quickly to see where our hotspots might be on some very unique geometry in the system model here.

So once again, we've shown some of the complex geometry that we can mesh in the second demo here, everything from hex meshing extremely complex parts and then also taking advantage of geometries we typically don't work with, such as STL files, as shown here.

This final session is going to show a couple other capabilities of Femap as well, specifically working with legacy data and also, post-processing. So many times. You might have models that were generated-- close all these parts-- that were generated in earlier versions of Nastran or from other vendors, and all you have is a .nas file.

So in this case, we have an aircraft that we were working with a while back, and now, we're coming back and you're either another company that has to do an STC and modify the existing mesh or you need to go back and reuse this model.

So in this case, for instance, let's say that on this aircraft model, we need to punch a hole here and take an account of a cutout that was added for maybe a new sensor or a new window or something like that in the structure. Now, we could try and regenerate all this, but you already have legacy data that is going to be easier to work with.

Femap makes this very easy to do, where we can take this and create geometry from a mesh. So in this case, we're going to take this geometry and we're going to create a cutout right in this region of the structure. So I'm using that Pick by Faces command again to easily grab our block of elements. And we're going to go ahead and delete the mesh. And let's go ahead and apply a circle.

Now, at this point, if you were doing this for real, we could, for instance, import other geometry that maybe represents the actual cutout or new interface that we're going to work with. In this case, for simplicity, we're just generating a circle that happens to be in between here that's about 5 inches. And again, using the meshing tool box, we can go ahead and project this curve onto the geometry and then go ahead and even toss a mesh on here.

So we're just going to go ahead and set a default mesh size just from what we know. It's about a default of 2 inches. And here, we could specify a new property. And because this was created from the original mesh, you'll see that-- I'll do that-- when we mesh this and turn this off, it will keep the interface nodes matched up with the original geometry.

Now, again, we have all the capabilities of the meshing toolbox. So for instance, maybe we want to add a 1 inch washer around this piece and go ahead and mesh this. Maybe there's a different property we want to apply to this region, and let's use a mapped mesh to create a nice, cleaner mesh in that model.

And finally, we can go ahead and use a lot of the capabilities that the toolbox to increase our element count, be able to add elements and maybe add some other details into the structure here. And then finally, we've made this change. We can actually quickly integrate this into the model.

So here, we'll grab this data, merge the model right in, and you'll see very quickly we now have a clean update to our structure that was not included in the previous design. So that shows the ability of working with legacy data and being able to reuse existing models that were developed in previous iterations.

The next thing we're going to show is we're actually going to go ahead and show some post-processing capabilities in Femap as well. One of the areas of interest has been beam post-processing. So here, we have a beam model. This particular run here just simply had A1G load that was applied, in this case, down. And you might be interested to see the contours of the beams on the model.

Now, here's our thicknesses on the model. In this case, it's just a simple truss structure, but you would be able to see all the details of the actual thicknesses of the part. Now here, we can go ahead and show these contours, such as the bar moments on one side or the other. So you can see how the different nodes change as we go throughout and look at those contours. Maybe we're interested in the axial stresses or von Mises stresses on the part as well.

Now, one of the unique things that we can do on the beam post-processing side is actually show shear moment diagrams on the part. So for instance, here, I want to show a moment. Right now, we can see the peak moment. But Femap will actually draw these beam diagrams on the part.

So if we turn off Thicknesses, and let's go ahead and scale this down just a little bit so it's easier to see what's going on, you can see how we're capturing high peak moments that reverse directions as we go throughout. We can take a look at the other directions of the model and very quickly identify, hey, maybe there's some peak bending moments here on these beam elements and so on and so forth.

For instance, we might be interested in a shear diagram as well. So we can look here and see the overall shear on the part model. So again, this is a great tool for quickly identifying critical areas on your structure very dynamically and visually, again, using this post-processing toolbox.

One of the final things we're going to show here is the use of xy charting and also, the data table. So here, we have a model. We've already solved it, and we've sold it for two different conditions. The first case we looked at was an analysis case of we have a sign vibration type running, where we're applying a load in the z direction here. And we're interested in the results at different locations so that if let's say, hey, we had a 0.5 g side load occurring at 80 hertz and we mounted some structure on here, what's the acceleration going to be at these points on the structure?

So from here, one of the things we can do is, we can quickly evaluate this using the xy charting tool. So here, we have the charting tool. I'll go ahead and pull this over so we're able to see the mesh. We've already run a frequency response that pulled xyz accelerations across the structure, displacements, and other aspects across a bunch of different frequencies from 0 to 500.

At this point, we're going to go ahead and do a vector versus set. And we are going to use the results from our dynamic frequency response. And let's go ahead and look at the T3 acceleration. Now, here, we're going to pull all the data from those output nodes that we had earlier shown here, so again, all these different locations.

And we'll hit OK. And you see this will populate a chart that has all this data already. So we can already see that there's stuff happening around 70 hertz and around 475 hertz. Very quickly, we can change the style of this. So we can add points. We can change this to logarithmic, so we can easily see the data little bit easier. And very quickly, we can identify what's happening in our system model.

So for instance, we know that there's something happening here. One of the beauties of this tool is that we can still interact with the model directly using the Show Tool Tips command. So where is this location? We're interested to see where that node is, and we can see that it's about-- if we have a 1 g input, it ends up being magnified about 22 times at that point.

So let's say if we put a 0.5 g load at the base, the location here, you can see it highlighted is going to see about 10 g's. At the top, we also see that the other peak location is about where we would expect. And then some of our other peak locations across the structure are more in the central axis of the satellite dish.

But again, this just gives you a very quick tool to quickly look at the results and both visually see the data on a chart form, as well as on the model at the same time. The other thing I'm plotting here is actually the input point. One thing I want to make sure is that we have a 1 g input across our entire location, so this is just a confirmation of that.

Now, all this data could be sent out to Excel very quickly. So we can copy the chart and send it to Excel. And from here, you can see we've generated this data, the data points concerning it, and the plot of this information that you can use for reporting. Now, again, this gives you a lot of other capabilities as well, such as adding titles, justifications, so many options, again, a very powerful tool for post-processing inside the Femap environment.