A basic example: Building and running - Nastran In-CAD Tutorial

- [Instructor] Now in this exercise, we're going to take an Inventor part and set it up ready for a normal modes analysis. So first thing we're going to do is open up the part, and if you navigate to the exercise folder, the begin state, you'll find this particular part. Now I've also saved this off as a parasolid part, so if you don't have Inventor 2019 or later, you can navigate here, find the parasolid part, and import that instead. We're going to carry on working with the inventor part, and if we open that up we can see it's a simple plate, and we're just going to explore that, so let's have a look at the sketch, it's rotated around. And we can see the units of the sketch or the dimensions of sketch, so you can rebuild this yourself if you like. It's just a simple six inch by three inch plate. Let's check the thickness. We go to the extrusion, just check, see what I did there. Edit the feature, and you can see it's .05 inches. So it's six by three by .05 inches. Again, please feel free to rebuild that if you need to. Let's go to the environment, let's just check the add ins, and what we're going to be using is the Autodesk Nastran In-CAD 2019 add-in. I click on the environment, this opens up the model tree window. So these are all the FE entities that we see running down here. We open up the solid, we can see at the moment, that we've got a solid model, we've got a solid part, and we want to change the analysis type, the default is linear static, we're going to change it. I'm going to change it to normal modes analysis, then you're going to change the title, this is just a label for the tree, and I'm going to call this basic plate, and then this title is what is actually written through to the Nastran input file. That's the difference between the name and the title. We just checked what units we've got, we're working US traditional units. In terms of output, I don't want to output reaction forces or stresses, they're meaningless in a normal modes analysis. The options include bonded contact, we'll see that a little bit later on. Now my material is just generic at the moment, so I want to change that, and again, on this course I'm going to be using consistently an inventor material, library material, which is going to be our carbon steel. Click okay, and what we're particular interested in is the density and it's a mass density, Young's modulus, and Poisson's ratio. There's nothing really else we need for this normal modes analysis. The yield and the limit, again, are not useful to us, we just check okay, and that's now setup that particular material to be used. They're ready to mesh, it's going to generate a default mesh, so a fairly simple mesh, obviously with solid entities, with solid elements. Now there are no loads applied. But I want to apply some constraints. So, I pick the face I want to apply the constraint to, which is this end face here, so I'll highlight that, we're using everything as fully fixed. Now in fact with solid elements, we only have the three translational degrees of freedom and we could just get away with that. But just for convenience we're just going to say fully fixed the three rotations are redundant. If we go to that home view, we can see the symbol for the constraints being applied there. Now we can setup the controls for the normal modes analysis. Again, I can give this a name so it'll be identifiable in the tree view, I'm just going to label this as 10 modes. Those are the 10 modes we want, everything else is going to be default. I'm under the model here, this is like a library of things we can add in to our particular analysis. So everything is echoed down in here. So the constraint for example is echoed down. I can rename that, I can call that edge, and then you'll see in the library it's also updated as edge. I can save this off, and we always want to save off before we run an analysis. So I'm going to save it into the end state, I can just call it plate end.