Assigning rod connectors in a Nastran analysis

00:08

In this exercise, we will be assigning Rod connectors to an Inventor Nastran analysis.

00:15

So, for this exercise, we're going to be using a simple truss system.

00:20

And rather than create a full-blown CAD model and a three-dimensional or even a two-dimensional mesh,

00:26

we're going to create this problem using Rod connectors.

00:30

So, in order to create a Rod connector in Inventor Nastran, all you need is work points.

00:36

So, you can create this full FEA from just a very simple sketch.

00:41

So, taking a look at the inputs that we have, we know that we're going to be applying a force at the base of this truss of 10,000 pound-force.

00:49

We know the length of this overall system is about 120 inches.

00:55

The cross-sectional area of each member is a one by two-inch rectangle.

01:01

So, an area of two square inches.

01:03

We know our young's modulus 30 times 10 to the sixth psi.

01:08

We know that input.

01:10

So, we know exactly what the stress and strain relationship of the material will be.

01:14

Even if we don't fully define the material properties.

01:17

That is the only thing that will have an effect on the displacement.

01:22

We know the angle between each of these lines is 45 degrees,

01:26

and that is enough to give us a rough calculation of what the displacements and forces in each of these lines is going to be.

01:37

So, we'll start this exercise in the inventor 3D modeling environment.

01:41

I'm going to start by just creating a simple 2D sketch that lays out the coordinates of the points of each truss member.

01:48

Then when I enter inventor Nastran, I can assign the Rod connectors between each given point.

01:55

So, I'll create a new 2D sketch and I'm going to use the XY plane for this.

01:59

So, I'll go ahead and lay out my points.

02:01

So, I'm going to throw a point right at the origin, make sure it turns green.

02:04

So, you know, you're right on the center,

02:07

and then I'll go ahead and place my first point,

02:08

which I am going to assign a dimension between the origin and this point as 120 inches.

02:15

And you want to make sure with a vertical constraint that these are vertical from one another.

02:21

That way it doesn't end up being slightly off of that vertical axis or the Y axis, in this case.

02:28

I can do the same thing for my X axis point.

02:30

I'll place it, give it a dimension and give it a constraint.

02:33

So, 120 inches and then I'll add a horizontal constraint between the two to lock that in.

02:40

And then lastly, I just need a point that is out here in line with both of those just like that.

02:47

And you want to double check again.

02:49

You have constraints or else it can move around and it may not be the correct dimension.

02:53

So, your problem will not be correct.

02:55

So, it didn't add a horizontal constraint between the top,

02:59

and that side point and then a vertical constraint between that point and the lower point,

03:04

locking in its position without the need for any additional dimensions.

03:08

So, now I have the four data points, 1, 2, 3 and 4 that can be used to create my Rod connector.

03:15

So, now I'll go ahead and save this sketch as a part file.

03:21

This will just be saved as truss.

03:25

Click "Save". So, I know exactly what I have and now I'm ready to open up inventor Nastran.

03:30

So, I'll go to environments inventor Nastran.

03:34

You don't need a full 3D model.

03:36

You can work with a sketch in this case.

03:39

And what I'll start by doing is going to connectors.

03:44

And Rod connector is actually the first type of connector in the list.

03:48

But if you did need to switch, you can use this drop-down menu here to look at cable, spring, rigid body, or bolt.

03:55

Since we're using Rod, we'll leave it as is.

03:57

You can also rename it here if necessary.

04:00

That's really helpful when you have multiple connectors in one analysis to keep track of what is which.

04:05

Now, you will notice down below here, I have the end point of a connector and the end point of a connector.

04:12

These can be these sketch points that we've created.

04:15

Now, because I have multiple connectors, there'll be Element 1, Element 2 and Element 3 in this list, when I'm finished.

04:24

For each one, you want to make sure that the area that you've defined,

04:27

which is your cross-sectional area and your material right here is correct.

04:31

Notice you cannot create a new material from the connector dialogue box,

04:36

new materials need to be created in the analysis tree prior to opening up connectors.

04:43

You cannot create anything from here.

04:45

You can only select materials from here.

04:50

So, I'll start by populating the area up here as 2.

04:54

And if you're not sure of the units, if you hover over the box,

04:57

it will show you the units that have been assigned to that field, which is in inches squared.

05:02

So, 2 inches squared is correct here.

05:04

And now End point of connector. If I click in the box, it activates that field,

05:09

I'll select the origin, the end point for my first Rod will be at the very top here.

05:15

So, the vertical y axis Rod and it will create that blue connector to show you where you've placed it.

05:24

Now, if you would like to add another connector to this set,

05:27

you can do so, but not until you click the next icon here underneath "Connector Element".

05:33

Otherwise, it will continue to change the selections of your first connector.

05:38

So, I will go ahead and select "Next".

05:41

So, now Element 2 has been created.

05:42

Element 1 has already been locked in and I can repeat the process for the next two.

05:47

So, endpoint will be the origin, the other end point will be point number three out here.

05:56

I'll select "Next".

05:58

And now for my third Rod connector, my endpoint once again will be the origin point number four out here will be the other end point.

06:07

And now I have three elements that have been created.

06:10

So, three Rods that have been created in the same connector set.

06:15

So, connector one contains these three elements.

06:18

So, now I'm ready to confirm this and then add my loads and my constraints.

06:24

Now, before I do set up those boundary conditions,

06:26

I want to make sure that the material that I've selected, this generic material has the appropriate properties.

06:32

Otherwise, I'll need to change that material for something that's more representative.

06:37

So, I'll select "Ok" to create this connector.

06:40

But then what I can do is I can just double click on this generic material from the analysis tree to open up the materials dialog box.

06:48

And here with a Rod connector, the only thing that really matters is going to be your Young's modulus,

06:54

that will be used to calculate the forces and displacements that are seen in each element.

06:59

So, this needs to be updated to the appropriate value, which was 30e6 as we mentioned in the beginning of this exercise.

07:10

So, I'll go ahead and type that in select "Ok".

07:13

So, the material will be updated automatically for that connector since it was already assigned.

07:17

And now if I open that material back up, I should see 30 or 3 to the 730 to the sixth added in as that structural Young's modulus.

07:28

So, now for my boundary conditions, I know that I have a fixed constraint at the end of each of these Rods.

07:34

So, I'll select "Constraints".

07:35

I'll leave all of my degrees of freedom fixed, in this case.

07:40

I'll rename the constraint to "Fixed".

07:43

And then for Selected Entities, I am going to select each of these end points.

07:50

So, everything except for the origin point and then I can turn the glasses on so I can see those and this should be just those three.

07:59

I'll select "Ok". And that should be added into subcase 1.

08:03

And now I can add in my 10,000 pound-force load which is in the negative Y direction.

08:09

So, I'll select "Loads".

08:11

This will be a force applied to the origin point.

08:15

So, I rename it 10,000lbf.

08:19

Selected Entities.

08:21

I will select that point at the origin and then for magnitude in the y direction, it will be negative 10,000lbf.

08:31

And then if I click the glasses, I can visualize that arrow that looks like it's in the correct direction.

08:36

You can always go back and review your free body diagram if you're not sure, but that looks correct.

08:41

So, I will select "Ok", that will be added into subcase 1.

08:45

And then now we are ready to solve and start to extract displacements forces and all the other results we need.

08:54

So, I will now go ahead and select "Run" which will solve this analysis.

08:58

I don't need to generate the mesh because it's just using that connector element.

09:02

So, there's not a separate mesh setting that needs to be input.

09:06

I can just select "Ok" once it's complete and what it's going to display first is typically going to be your displacement,

09:13

when you're working with just a simplified line element model or connector model like this.

09:19

So, it shows you my displacement as 0.016 inches.

09:24

And if I'd like to, I can break this down into X, Y and Z directions as well.

09:28

Since this is the max displacement, it's not clear which axis that is along.

09:33

The visual here in 3D, gives me some indication.

09:37

But if I'd like to, I can switch from total right here to along the X axis.

09:44

So, about 4000 or so along the X, not a lot which I wouldn't expect since the load is in the Y direction.

09:53

If I switch to along the Y I can see about negative 0.016.

09:59

So, it shows me that in that specific direction, it's a negative 0.016 inch displacement along the y axis, which sounds correct.

10:09

And then for Z axis, I can double check that should be zero, right?

10:13

So, since there's no force acting in the Z direction, I shouldn't see any displacement in that direction.

10:19

So, it appears that my constraints and loads are acting as I expected.

10:24

I can then go look at Stress.

10:28

And this is neat because it gives me my Rod axial stress as well as my equivalent stress for those elements.

10:36

So, it's a very simplified problem, but these results should line up with the theoretical results,

10:40

since we're taking the error of 3D or even 2D elements out of the equation and we're working with simple one-dimensional elements.

10:49

So, typically, these types of problems in FEA should align very closely with your hand calculations.

10:56

The last thing I can do here is I can look at my reaction force and this is going to give me my actual force total.

11:06

And where that location is, I can also break this down by constraint.

11:11

If I right click on my "Fixed" constraint and go to "Reactions",

11:15

what I can then do is I can choose either all three points,

11:17

or I can select them one by one and extract the reaction forces at each point.

11:23

So, at point 3 out here about 2900 pound-force total.

11:28

I can clear this list and choose point 4.

11:31

It shows me that in the negative X.

11:34

And then lastly, this first point up here is where I have my maximum force.

11:38

So, this is what I would expect.

11:42

So, Rod connectors are a great way to evaluate forces on a very simple system such as this when the cross-sectional properties,

11:50

and the shapes that you're using are not terribly complex and therefore, do not require a three-dimensional model.

11:56

The other thing you can do with Rod connectors,

11:58

and you can use these as intermediate elements between either solid elements, shell elements,

12:04

or even other line elements if necessary.

12:07

So, they can be used to connect adjacent geometry as well as simply look at forces in a simple system.

12:16

The last thing you may end up doing with these is if you are adding these to a larger structure,

12:21

you likely want to take into account the mass that these would generate,

12:25

especially when they are 10 ft long like they are here, that amount of mass will add up in the total assembly.

12:34

So, to do that, if you edit your connector, you will see there is an NSM value.

12:40

This is your nonstructural mass per unit length.

12:43

This allows you to add in mass to the overall FEA and the mesh without actually adding any additional stiffness to the Rod.

12:53

So, it's really helpful when you're doing total mass calculations or you have gravity applied.

12:58

And you'd like to evaluate the additional force created by that mass.

13:04

So, I'll select "Ok", we're good with this for now.

13:06

So, I'll select "Save" and then now we can continue on with additional analysis.