30+ Tips and Tricks with Inventor Nastran in 60 Minutes

JOHN HOLTZ: Hello, everyone. My name is John Holtz, Senior Technical Support Specialist with Autodesk. Today, I'm going to be talking about 30 or more tips and tricks with Inventor Nastran. And actually, I've managed to squeeze in 60 tips in our one-hour session here.

First, just a brief statement about the Safe Harbor, which basically says that I may be making some kind of statement regarding future development of the software. Those statements are not a guarantee of what will be in the future software, since plans always change during development work.

If you're watching this video but aren't sure what Inventor Nastran is, just a quick introduction-- Inventor Nastran is a general finite element analysis to perform a wide range of simulations such as stress, heat transfer, fatigue analysis. And, as implied by the name, it is a plug-in for the Autodesk Inventor software.

Here's what I hope we learn today-- just be more efficient with setting up the analysis, understanding the input for the analysis, find more ways to perform a given task, and most importantly, be more efficient when viewing the results. This is kind of a table of contents of the topics that I'm going to be covering. Generally, in the natural progression of building the model from the beginning to the end, there will be some overlap in the tips that I have, meaning that they might appear-- could appear in any of the sections. But if you're watching this video and want to jump to a particular topic, for example, this will give you an idea of how far to advance the video.

So with that, let's go ahead and begin with modeling in Inventor. It's always best if you plan your analysis before you create the model. Or at the very least, plan it a little bit before you go into the Nastran environment and actually start working on the analysis.

So tip number one-- Inventor has what's known as modeling states. So in the example here on the left, we see the model with all of the details, which are, of course, necessary for manufacturing, for creating the drawings. But you can create additional model states, in this case, called Simplified. And you can actually change the model. It's like having two models in the same file.

So here you can see we've suppressed some features that I feel are not important to the analysis. And that should be one of your goals, is to make the model as simple as needed for the analysis.

Tip number two is combining parts of an assembly. The advantages are that you minimize the contact and therefore, you get smoother results. A secondary benefit is it may be easier to mesh the model. Now, once you combine the parts, there are a few disadvantages. Obviously, you can't hide an individual part when you're viewing the results if it's been combined with other parts.

And if you do combine them, then they need to be the same material. So in the example here, let's look at the one where the parts are separate. Now there are two parts split right down the middle of the hole.

So you can see here how the stress on the left side is a little different than the stress on the right side. That's the effect of the contact that I mentioned. In comparison, if the parts are combined, the element-- the mesh-- is smooth across that boundary. So, therefore, the stress results are also smooth across the boundary.

Tip number three-- if you're going to be creating shell elements in your analysis, it's better to create a surface model in Inventor. The advantages are that you avoid using the command in Nastran called the Find Thin Bodies. That's this menu shown down here.

By avoiding that command, you're reduced the number of idealizations that are in the model, and that makes the model smaller, more efficient to work with. If you're creating a surface model, you have better control over the model, such as, you can create your shell so there's no gaps between the models. We'll see this here in the next two slides. The disadvantage is that you're generally starting from a solid model and converting that to a surface model, so it does take a little bit of time upfront. But hopefully, the-- getting the better results is worth the additional time.

So let's take a look at that to understand the differences. So here I've taken a wide flange beam that I made as a solid. I used the model state to create a surface model and imported that into Nastran. The two advantages are I have two idealizations because the flanges have a different thickness than the idealization for the web.

The other advantage, as you can see here, is that there's no gap between the web and the flange. And, in fact, the mesh matches between those, so I've avoided using contact. I'm going to get a smoother result.

In contrast, if you use the solid model from the master state to come into Nastran and you use the Define Thin Body command, you're only going to get one idealization, which means that all three of these faces have the same thickness. In this case, it's the average thickness. That's probably not what you want. Maybe in some models, it's fine.

The other disadvantage of using the Find Thin Bodies is that the flange-- the face that's created, excuse me, for the web-- is short of the mid-surface of the flange, so you have this gap. In order to account for that gap, you have to use contact. And contact is more of an approximation, so the results are going to be affected a little bit by that factor.

Topic number two-- there are some things you can set up in Inventor and Nastran to make the workflow more efficient. For example, tip number four-- if you're working with a surface model, Inventor generally shows those surfaces as translucent. So it actually makes it kind of hard to understand what the model looks like.

So before creating the model, if you set up the File, Options, Part and check the box for Opaque Surfaces, or after you've created the model, if you don't have that turned on, you can use the View, Visual Style, Technical Illustration. When you do that, the model is not translucent, it's opaque. You can actually understand it a little bit better what you're looking at.

Nastran uses a number of parameters to change how the analysis behaves. And there's two parameters in particular that I recommend in tip number five. Those are-- the first one is Nprocessors, which is the number of processors that you use in the analysis. So if your computer has 20 processors, for example, you probably only want to designate somewhere between 8 to 12 processors. That's kind of an optimum number of processors to use.

The default is either two or four processors, depending on what version of Nastran you're using. And you can do a lot better than that by increasing it if you have them available.

The other parameter that you want to change is called FileSpec. This is where the temporary files are saved on the computer. So first thing you want to do is you want to point to a drive that has the most free space available. The second thing is you want to know where the FileSpec drive is because occasionally the temporary files will be left behind. You want to be able to go in there and delete those.

Next question-- the next tip is how do you change those parameters? If you want to change it only for the current model, you can do that in the Nastran environment. At the end of the model tree, you right-click on Parameters, Edit. That brings up this dialog. You can type in the parameter you want to find, and that will show all the hits. So here we're changing the number of processors.

Note that if you change it here, it's only changing it for the current model. But also important, it's changing it for all of the analyses that are in the current Inventor file.

In contrast, tip number seven-- if you want to change a parameter for every new model, you do that by editing the file called Nastran.ini. It's located wherever you installed the software, typically C, Program Files, Autodesk. Then, depending on what version you're using, it's some other folder, such as Inventor Nastran 2023, then Nastran.

When you edit the-- when you edit the Nastran.ini file, you get this text file. Excuse me, here-- you get this text file, and you can see you can change any of the parameters that you want.

Tip number eight-- sometimes when you go to run an analysis, you get this pop-up message. It says that there's some kind of problem with it. Of course, you can click the details to see what the problem is, but your only option is to close this dialog, which means you're not going to run the analysis.

Now sometimes, the warnings aren't that significant. It may just be warning you that a constraint is missing. Well, if you're running a transient analysis, it's perfectly fine to not have constraints in the model.

So in order to get by this, what you want to do is from the ribbon, go to the System panel, then Default Settings. That will bring up this dialog. Go to General and then Prompt for Solution with Warnings. When you click this checkbox and then you go to run the analysis, you get a similar pop-up. It still says that you have warnings or errors. It may not run.

But the difference is you have a button where you can say Yes, I accept the fact that there's some warnings. I know it's going to be OK. Please run the analysis. And when you click Yes, the analysis starts. You get results, and everything is good.

Tip number nine-- whenever you add loads or constraints to the model, by default, those are shown as a three-dimensional graphic. The arrowhead looks three-dimensional. When you have a lot of those symbols on the model, it can actually slow down the operation of the computer.

So tip number nine is go to the System, Default Settings. That brings up this dialog where you can go to Display options, and then check the box to Optimize Graphics for Faster Rendering. When you're using the faster rendering, the loads and constraints are shown as a two-dimensional object instead of a three-dimensional object. That just makes the analysis-- excuse me, not the analysis, it makes the operation, the graphics, perform faster.

Topic number three is regarding the idealizations, which relate to what element types you use for the model. And the tip here is to use the correct idealization for the type of geometry. For example, if you have a CAD solid part, it is correct to use solid elements on the idealization. Basically, a solid creates elements through the thickness of the part, so when you run the analysis, have your results, if you were to slice the model, you can see that you have results through the thickness. That is correct.

Likewise, we talked about creating surfaces to create shell elements. So in this case, the shell is just a surface. The thickness is not modeled. Essentially, the mesh is like a piece of paper.

In the Idealization, you choose Shell Elements, and the thickness is a number that you enter. When you look at the results, you slice the model. Actually, you don't technically need to slice the model in this case, but just to have a consistent set of images you can see that there's no elements due to thickness. With the shell elements, you'll get a different result on the top side versus the bottom side.

So this input here is correct. And what I wanted to point out is the incorrect usage of the idealization. In this situation, we have the CAD solid model, which we did not convert to surfaces. Under the Idealization, we said we want to create shell element so this is what the mesh looks like.

The question here is what thickness would you enter to represent the thickness of this actual part when these are shell elements? Because as you'll see when you get the results, if you slice the model, it's not just a single piece of paper that's representing the model. We actually have a double-wall vessel. This is an incorrect use of shell elements or a CAD solid model. And that's-- of course, you want to avoid that.

Topic number four, meshing. There's actually two ways to create the mesh. One is from the ribbon using the Mesh, Mesh Settings and that brings up this dialog, where you can enter the mesh size. Note that this mesh is the entire model using the same mesh size.

The alternative is from the ribbon, use the command Mesh, Table. That brings up this dialog, where it lists all the parts in the assembly, and you can then specify a different mesh size for the different parts. The other thing you can do is you have to indicate which parts you actually want to mesh. So if I only wanted to mesh pusher and the part named support, I just check those when I click the Generate button. That will mesh whatever I have checked. So that's very useful.

So that brings up the question and tip number 12. Maybe a coworker was working on the model beforehand and he's handed it off to you, and you want to know what-- did they use the mesh settings or did they use the mesh table? When I get a model in tech support, I have the same question. Ah, did he mesh this using settings or table?

The way you find out is you right-click on Mesh Model, go to Switch To, and the checkbox indicates here that the mesh table was used. So then you know which menu to open up and to make changes.

Section five is talking about connectors. Connectors are things such as bolts, springs, a rigid connector. They're used to simplify the analysis instead of making a solid model of a bolt, for example. The commands for connector is Prepare, Connectors on the ribbon.

Tip number 13 is that you can create multiple connectors on one dialog. So for example, I'm adding some bolts to a model. So I created the first bolts, selected the head, the surface for the nut, size of the bolt, and the preload.

Well, if I have another bolt that had the same 3/8ths inch and the same 200-pound preload, you want to click the Next button here, and that creates bolt number two. You specify the surface for the head nut. Create, Next. Now creating bolt number three. Specify the surface and the nut and click OK.

The advantage of doing this is that you only have one entry in the model tree. So if I want to make a change to these 3/8ths inch bolts-- for example, maybe the stress was too high in the bolts and I now want to change it to a half-inch bolt, you can right-click on the one entry to get this dialog that has all three bolts. You just change this entry here and click OK, and you've changed all of those bolts.

If you didn't use Next, then you'd have three entries in the model tree. You'd have to edit each one individually. And of course, that's not very efficient.

For the rigid connector, there's actually two types of connectors-- two types of rigid connectors that you can create. When you get to the dialog, you're going to choose Rigid Body for the type of connector you're creating. But the Type, you have an option for Rigid or for Interpolation.

In this example, we have a motor frame and a motor resting on it. We don't want to include the motor in the analysis. There's a lot of detail. It's not our job to design the motor. What we want is we want the weight or the mass of the motor located up here at the center of gravity.

So you'd use a rigid connector to connect that mass to the bolt holes, the four bolt holes. So the question is, should this connector be rigid, in which case you're saying the motor is much more rigid than the frame, and therefore, these four bolt holes are going to kind of move around together, or do you want to ignore the stiffness of the motor? In that case, you would set the type to be an interpolation connector, and therefore, the mass gets distributed to the four holes, depending on the position of the mass relative to the holes. It's interpolating the mass to the holes and it's not changing the stiffness of the model itself.

Another type of connector that's convenient is the spring connector. Now naturally, there are times when you have a real spring in the model, and you'd use the spring to represent it, such as this here. I'm supporting this beam with a spring. But other times, you want to use the spring to stabilize a part that is held by separation contact using a small stiffness so that there's only a small reaction force in the spring, but you're preventing the part from flying off into space.

The two tips here are number one, you want to click the Advanced Options button so that you see all of this input here. And then tip number two is, you want to click the Stiffness button and enter all six stiffness values-- K1, 2, 3 are the translational stiffness in X, Y, Z. 4, 5, 6 are the rotational stiffnesses about X, Y, and Z.

Topic six, for contact-- you use contact in an assembly because parts need to transfer load from one body to another, and that is done through the contact. As we'll see, there's three types of contacts that can be defined-- auto, manual, and solver.

Tip number 16 is to use solver contact when possible instead of manual. Here's the advantages. The solver contact's useful when all or most of the model has the same type of contact and parameters. For example, maybe 90% of the model is bonded together, so you can use the solver contact. It applies to the entire model, although optionally, you can select individual regions.

But the advantage is it does not overwrite any manual contacts you define. So instead of having 100 contact pairs that are all bonded, you just create one solver contact and set it up to be bonded.

You do use manual contact when you need a different contact for a different part of the model. Or if you're using Separation contact and there's large sliding motion, it's more efficient to use the manual contact. With the manual contact, you have to select the actual faces that are in contacts. That takes time to do. And also, if you have hundreds of contact pairs in the model tree, then it takes time to go through those and find and make changes if you have to.

Before I go to the next tip, let me just mention this auto contact, this command here. Really, what that does is that goes through the model and finds two faces that are in contact and it just creates a manual contact. So that's how you can have a model that ends up with hundreds of contact pairs in the model, whereas one Solver contact would be more efficient.

When you're using the manual contact, as I mentioned, you need to designate the faces that are in contact. So in this example, I have a flange with eight bolts in it, and I could use the auto as I mentioned, but that would give me eight contact pairs-- one bolt to the flange, second bolt to the flange, and so on. It's more efficient to do it manually.

It's easy to select the face for the primary, but now the question is, how do you select the underside of the bolt where the eight secondary faces? Well, essentially, what you need to do-- or can do-- is hide the flange so that you can select the backside of the bolt.

Now the trip here-- the tip here is that you can right-click on the part in the model tree and uncheck Visibility, so that technically, the CAD body is hidden, but the mesh is still shown. I'll elaborate on this in a moment. But even though the mesh is shown, you can't select the face on the mesh. You can only select the face on the CAD body, meaning you can select the eight faces of the bolt.

The maximum activation distance is important to set up in the contact. And I always suggest that you enter the maximum activation distance mainly because you're trying to reduce the number of contact elements that occur, and also you understand the model better and what activation distance would be appropriate compared to letting the Solver, which has very little understanding of the model, and it just has some simple rules. It may create more elements than required.

So what is the maximum activation distance? Essentially, it's a distance from a node on the secondary entity, the distance of the node on the matching primary element. So in this example, it's kind of the hypotenuse of the triangle. We have a distance of the gap and the size of the element. So the maximum activation distance, the length of that hypotenuse is the element size, h squared, plus the gap squared, the square root. And then you multiply that by 10% or 20%, meaning 1.1 to 1.2, and enter that distance for the maximum activation distance.

So as you can see here, even if the gap were zero or virtually zero, the maximum activation distance still needs to be larger than zero because it's based on the size of the mesh. Now, in the manual contact, if you have sliding, then you have to take into account the distance that the model moves in the maximum activation distance because the thing to keep in mind is that the contact elements are created at essentially at time 0, meaning the position of the mesh that you create.

The distance from the secondary node to the primary element, in this case, is equal to L plus the mesh size-- so that distance squared plus the gap squared. Take the square root of that, multiply it by 1.1 or 1.2, and that would be the maximum activation distance to enter.

In tip number 19, the definition of the maximum activation distance is different when using solver contact compared to the manual contact that we saw on the previous two slides. The solver contact, the activation distance needs to be greater than zero, needs to be slightly larger than the gap between the two phases. So in this case here, if I wanted to connect this edge of the web to the flange of my beam, I need to enter a maximum activation distance that is slightly larger than that gap.

But you don't want to make it arbitrarily too large. Ideally, you want it to be less than half of the element size. The reason is that these are parabolic elements and therefore, you have a mid-sized node. There's a node right here that you do not want to be connected to the opposite face. So I guess actually this here probably should be activation distance less than the gap plus half the element height.

As I mentioned, what you're trying to do is to reduce the number of contact elements because that way you'll get the fastest solution. And I don't know about you, but when I run a model, I generally have to run it two or three times because I make some kind of mistake or the results are indicating something that I hadn't considered. So that's why you want to reduce the runtime.

In the contact setup, there's this input called the penetration type. And the two options are unsymmetric or symmetric contact. So what happens in the unsymmetric contact is that the nodes on the secondary body contact the primary elements. That gives the fewest number of elements, and therefore, the fastest solution. But it's not a good selection if there's sharp edges coming into contact. The next slide will make this more clear.

With the symmetric contact, it essentially applies to unsymmetric, meaning that the nodes on the secondary surface contact the primary, and the nodes on the primary contact the secondary. So it's better contact detection, especially with sharp edges, but you're generating essentially twice as many elements so the runtime is going to be a little longer.

Here's a graphical representation showing the two. In this example, we're going to drop this block onto the wedge. So if we were to use unsymmetric contact, we have two options. The wedge could be the secondary and the block would be primary. When you're using unsymmetric, forget about the faces on the secondary. The only thing that counts are the nodes on the secondary.

So what happens in this setup is the block falls. It makes contact with that secondary node. It tips over to one side-- oops, there's no node here because it's only the node on the secondary that's important. So the block falls through, and it falls through, and that's not the behavior you want.

Of course, with unsymmetric, you could have switched it. The block could have been the secondary, and the wedge could have been a primary. Again, it's only the nodes on the secondary that count. So the analysis really looks like this as far as the contact detection.

So the block falls down until the node makes contact with the wedge and it just sits there. So obviously, unsymmetric was not correct regardless of how you set it up in this situation.

In this situation, you wanted to be using the symmetric contact, in which case, the faces of the primary and the faces of the secondary are both used in the contact detection. In general, it doesn't matter which one is primary and which one is secondary. What happens is that it falls, makes contact, it slides down the faces because it's essentially face-to-face. Contact and the analysis behaves the way you wanted it to behave.

Tip number 21-- if you have friction in contact, you have to use specific settings. Friction is only applicable to separation contact. One of the things I often see is that there's a contact type called sliding, which you may think would use friction.

But to Nastran, sliding means that it is free to slide without friction. So you have to use separation contact. Friction is only applicable in a nonlinear analysis.

So those first two are very important and critical. The second two are suggested to get more accurate results. There's a parameter called SLINESLIDETYPE. If your parts are not sliding a great distance, then you can set SLINESLIDETYPE to STATIC. And because you're running a non-linear analysis, there's an input under the non-linear setup dialog which we'll see in a few moments. You want to set the number of increments to be 25 or larger to get more accurate results.

If you have contacts that you want to delete, you would think that you could just right-click on Contact in the model tree and choose Delete, but you'll notice there is no option. Instead, select the contact, press the Delete key on the keyboard, and note that the Backspace key does not delete it. So I need the Delete key.

Section seven-- let's talk about loads and constraints. First tip is if you want to apply a load to many faces that are connected together, you right-click in Selected Entities and choose Face Chain. Then when you click on the first face, all the other connected faces are selected.

This is-- you may not encounter this tip very often, but it is beneficial if you have a lot of elements that have a load applied to it. Instead of applying a force, it is more efficient to apply a pressure. And where you'll see the differences when you start to run the analysis and it says generating the Nastran file.

If you use a pressured load, the Nastran file can be generated very fast. If you use a force load, it can take longer to generate the Nastran file, and that's evident when you have many, many, many elements with a force load applied. So use the pressure if you can.

If you're applying a load or a constraint to multiple subcases, the proper way to do it is tip number 25. When you're defining the load, you can select which load cases they are assigned to. This is the proper method. You do not want to create a separate load or a constraint in an individual load subcase if it's, in fact, the same load that you want in multiple subcases.

There's two buttons on the dialog that you may have noticed down here at the bottom. First one is the New load case or constraint. What it does is, after you specify the setup and the selected entities, when you click New, it will apply this to the model. Sorry, I hit my mouse here.

It will apply this load or constraint, and it will keep the dialog open, still show the same load or constraint input, but it will clear the selection box. And that way, you can now select a different face edge. Tweak the constraint if you want and apply a new one instead of clicking OK to close the dialog and starting the dialog again.

The Duplicate is similar in that it applies the current constraint to the current selection. It keeps the dialog open, but it keeps all of this input. It keeps the same constraint. It keeps the same selected entities. To be honest, I'm not sure why you would want to keep both, but perhaps you have a good reason to do that. Maybe you're only making a minor change to one or the other.

Section eight-- we'll talk about some of the special tasks that you can do from the ribbon and the model tree. But first, let me just clarify so that we all have the same understanding. The model tree is the branch that typically is on the left side of the Inventor interface. The ribbon is the menus that go across the top of the interface.

Step number 28 is how to hide all of the CAD bodies in your model. You can do that from the Display menu, Object Visibility, and then uncheck CAD Bodies. This will hide the CAD bodies, but note that it doesn't hide the mesh. It does not hide the constraints.

So the question is, how do you hide the mesh? One way to do that is by using the Mesh Table. And you can just uncheck the visibility for certain parts in the assembly. That will hide the mesh. It does not hide the CAD body. It does not hide the loads or constraints.

The second way to hide things in the model is from using the model tree. When you expand the branch for the parts, you can right-click on a part and uncheck Visibility. That will hide the part.

An alternate way to hide the mesh is from the idealization. Keep in mind that the idealization tells the solver what parts-- maybe a better way to say it is multiple parts can be assigned to an idealization. So when you right-click on the idealization, you can then hide that idealization. It hides the mesh on all of those parts.

Again, neither of those hides the loads or constraints. You can do that separately by right-clicking on the nodes and constraints.

Tip number 31 refers to how to display the cross-section when you're working with beam element. This is what a typical beam model looks like. Maybe we have three different cross-sections, an angle L, a tube or pipe, and a channel. I mean, when you're looking at this here, it's hard to know what the orientation is so that you can first orient your model properly or enter the cross-sectional information correctly.

So for tip 31, what you can do is right-click on Elements in the model tree and choose Display Cross Section. When you do that, it shows a little shaded view of each cross-section, and therefore, you can tell whether you need to rotate the channel, for example, or the angle to get the orientation that you want.

The second way to do that is right-click on Elements, Display Line Element, and you have two options. The Orientation shows an arrow pointed in the y-axis, and when you're entering the properties you see x-- er, excuse me-- you see y and z shown on the figure for the input about Iy and Iz. So Iy is about the y-axis, z would be perpendicular to the beam so that Iz is about that axis.

The second option is a direction that shows an arrow on the beam going from End A to Node B on the beam. And the reason that this is good to know is if you're entering an end release for the beam-- for example, maybe this beam is not fully welded. Maybe it's a pin connection here, so you want to release the rotation at End B on this beam element. You do that by displaying the direction and you know it's B and not A.

Next tip is that I suggest that you keep the model branch collapsed. The main reason is just it creates confusion. It's usually a lot longer than the analysis branch that you're working on, so it takes up a lot of space and as we'll see in a minute, there's things in the model branch that you typically do not want to enter or don't want to edit. So therefore, I suggest that you keep it closed.

Now, with that said, here are the reasons to use the model branch. Reason number one is if you want to add a concentrated mass to the model, you have to add the first one from the model branch. You expand it, expand Idealizations, right-click on Concentrated Mass and then say New. Once you add the first concentrated mass, you can collapse the model branch and add additional ones from the actual analysis.

Another reason to use the model branch is to copy loads and constraints from one analysis to another. You can have multiple analyses in the model. The way you do that is expand the model branch, expand the branch to find the load that you want to copy, you right-click and say Copy, and then you go up to the analysis where you want to copy it, right-click and say Paste.

Now the main reason-- the main things you do not want to change from the model branch are the following. For example, the material properties, the laminates if you're using composite shell elements, and any cables if, for example, you have a natural frequency-- not natural frequency-- if you have frequency response or a transient analysis you use tables to define the loads.

Now the reason-- I don't want to say you can't change them here because obviously you can change them. The potential problem with changing these items in the model branch is that these apply to every analysis in the model. So it's very easy to come in here and change Material 2. You may be thinking that that's going to change the material properties in model 5 because that's the one that you're working on currently.

That's not the case. If you change something down here in the model branch, it's changing every analysis that uses that item. So in this case here, because I only have one material, Material 2 is used in all 10 of my analyses. So if I change it down here, it's changing it in all 10 analyses.

Now maybe that's what you want to do, but often, that is not the case. So just be careful. Anything you change under the model branch is changing every analysis that item is used in. That's why I suggest keeping that branch collapsed.

Topic number nine, running an analysis. First tip is for a nonlinear static analysis, you should go to the Subcase, Nonlinear Setup and edit it. What you want to do is set the intermediate results to on. When they're turned on and you run the analysis, you're going to get results.

When step number one is done, you get results. When step number two is done, you get results. So you can be watching the results to make sure the analysis is performing as you want it to. The default is off, which means you don't see any results until the last time step is done, by which time you may have wasted time when you could have stopped the analysis and made a change.

The next tip is you can set the convergence criteria by clicking on the Nonlinear Setup, Advanced Settings. The reason you may want to do this is maybe the analysis is struggling to converge at the first iteration. Maybe it doesn't converge at all. And often, that's because the load is the hardest thing to converge on.

So if you come in here and turned off the load convergence criteria, then the analysis may run in converge, and you can at least see is the model behaving correctly? If it is, well, then let it run and maybe the results are accurate enough. But maybe it will converge and you'll see, oh, I missed a contact here, and that's why something isn't working properly.

You can actually run multiple analyses sequentially, but you cannot do that from the Inventor interface. You can do it from an interface known as the Nastran Editor. So what you do is generate the Nastran file for each of the analyses. You note what the name of that Nastran file is, then you start the Nastran Editor Utility, this window here.

You do File, Open and open each of the Nastran files. And you'll notice that those get loaded into the queue window. When you right-click, you can say Start Queue, and it will run each analysis sequentially.

You can also run the analyses sequentially using a batch file. It's very similar that you need to generate the Nastran files. Get the name of those, and then you have to create a batch file from the command prompt. And essentially, you just specify that you want to run Nastran.exe from the appropriate folder.

In this case, I just substituted the S: drive for where the software is actually installed. And then you indicate which model you want to run. In this case, model from batch/nas.

The second model is called model2. Those are located in the M: drive, which I substituted for this actual long path here. One of the advantages of using a batch file is that you can close the Inventor interface so you're not using any RAM to be displaying the model Inventor. You're essentially freeing all the RAM for the analysis.

After you run the analysis, you should always review the warnings and error messages. Those are located in the log file, and as shown here, there were three warnings that occurred this number of times. And the way to get to the-- excuse me-- the way to get to the log file is right-click on Results, and choose Show in Folder, and that will open File Explorer. Highlight the analysis file name, and you can then open the log file or you can manually browse to the folder with the model then go modelname, InCAD, FEA.

So the next series of slides, I'll talk about the errors and warnings that you definitely want to pay attention to. E5000, 5001, 5004-- that will stop the analysis, so you'll know that there's a problem. Basically, it indicates the model is statically unstable. So, of course, the solution is to make it stable. You either missed constraints or you missed a contact.

Another possible reason is the material properties are wrong. For example, you forgot to change from the generic material that has a modulus of elasticity of essentially 0 to the real material. Or you're using the rubber from the material library, which has a Poisson's ratio of 0.5, which is technically correct, but that's not acceptable mathematically. So you want to change that to 0.48, for example.

Another cause for these errors is that the mesh is distorted. You just have to improve the mesh quality.

This Warning message is critical. And the reason it's critical is it doesn't stop the analysis, but it may indicate that the results are inaccurate. The 5118 Warning is this technical jargon which basically means the reaction forces do not match the applied loads. So you're going to want to check are they just a little bit inaccurate or are they wildly inaccurate?

So what you do is you open the output file, which is a text file in the same location, just like opening the log file. You do a search for the E5118. And then the load resultant this is the sum of the applied loads to the model and XYZ translations and then moments XYZ rotation or moments. And the single point resultant-- this is the sum of the reaction forces.

So as you can see here, everything matches pretty well. This is off only slightly a tenth of a unit out of 7,000. That's insignificant because the forces are slightly different, the moment loads and reaction forces are slightly different but I don't think this is insignificant this is caused just by this moment arm if these differences were large then there's a problem in the analysis. In that case, I suggest using a non-linear static and hopefully, this message will not occur again.

Another common warning is the G3051. It's modifying a node on the secondary contact face. The reason this occurs is shown here, that we're approximating the surfaces with a mesh. So the shaft in yellow, the nodes are on the theoretical surface, of course. And the hole that the shaft fits in, those nodes are also on the theoretical surfaces.

But note because the mesh is random, the node on the shaft is interfering or penetrating the face of the hole. And that's what this G3051 message is about. It's moving this node, the secondary node, to eliminate that interference.

The question is the interference insignificant and therefore, the distortion that's caused by moving this is insignificant, or is the interference large, which means there's probably a problem with the setup of the contact and most likely a problem that when it moved the node, it's creating a distorted mesh.

So what you want to do is edit the log file and search for this term here or "surface penetration" until you find where it says "initial maximum contact surface penetration." In this case, the largest penetration or the largest interference is 11.5 units, whether that's 11 and 1/2 inches or millimeters it doesn't matter. That is too large and would be unexpected. You should correct how you have the contact defined.

That brings up the question. It identifies a node number, 36,841. How do you find that node in the model? Tip number 45, you can use the Inventor user coordinate system to locate a specific node.

The way you do that is you view the Nastran file to get the coordinates. So here's the node number. I just happened to be-- this is a different node number, of course. But I've highlighted the coordinate for x-coordinate, y-coordinate, z-coordinate in scientific notation. You go to the 3D Model menu, Work Features, UCS.