Assigning spring connectors in a Nastran analysis

00:08

In this exercise, we will be assigning spring connectors to an Inventor Nastran analysis and using them to generate a result set.

00:18

So, before we jump into the Inventor Nastran environment to create this FEA,

00:22

first, we're going to review this free bio diagram of the problem we're looking to solve.

00:28

So, we have a simple horizontal beam.

00:31

It's 30 inches long, has a width of a half an inch and a height of three quarters of an inch.

00:36

And it's fixed on one end and supported by a spring (with a stiffness of 54 pound-force per inch) on the other end.

00:48

There is a distributed load being applied along the entire length of the beam of 5 pounds per inch.

00:56

So, we know all the inputs for the FEA and then the last remaining item is going to be our material properties for the beam,

01:03

which is going to be a modulus of elasticity or a Young's modulus of 30 times 10 to the sixth psi and then a Poisson's ratio of 0.3.

01:13

Those are the only material properties we need to represent the strength and stiffness of this equation.

01:21

So, using these inputs and performing hand calculations, we would expect that the deflection at point A.

01:28

So, at the end of the beam would be about half an inch.

01:32

So, we should see after we solve about a half an inch of displacement in the -y direction in this case,

01:40

and then the force transferred to the spring should be roughly 26.95 pound-force.

01:47

So, if our FEA is close to these numbers, we know that we have it set up appropriately and we can use it for design purposes.

01:55

So, we'll now move into the inventor environment and create this setup.

02:02

So, once again, we're going to start by creating a two-dimensional sketch for this problem.

02:07

However, keep in mind with spring connectors,

02:09

they can be added onto a vertex or a region of an existing CAD model within inventor Nastran to adjoin adjacent structures.

02:18

However, in this case, we're going to be using a line element to represent our beam.

02:25

So, we'll be applying a simple sketch and then cross-sectional properties to create that.

02:30

And then we'll be applying a spring connector between the end of the beam and then a point that will be fixed in space.

02:37

So, I'll need to define at least the basic dimension of this beam.

02:42

So, I'll create a sketch on the XY plane and I will create a simple line from the origin out horizontally 30 inches.

02:52

So, I can just type in 30, click "Enter".

02:54

So, I have a horizontal line there, hit the "Escape" key.

02:59

The only other thing that I need to define for this FEA problem is a point that represents the base of the spring that will be rigidly supported.

03:08

So, I'll create a point that is going to be directly below the end of that beam.

03:14

So, I can make sure that it is vertical to that point.

03:18

And then the dimension here is going to be 5 inches so that spring will be five inches below that 30-inch-long beam.

03:26

I do not need to define anything else,

03:29

since a simple line is all I need for a line element idealization and two points is all I need for a spring element.

03:37

So, I'm all set on the CAD modeling side.

03:40

So, I can click finish sketch and I'll go ahead and save this as Spring, click "Save".

03:50

And now I'm ready to open up inventor Nastran and solve this problem.

03:55

So, I'll open up in inventor Nastran and now we can set up our materials and our boundary conditions for this problem.

04:03

So, I will start by establishing the idealizations and the connectors that I need.

04:09

So, first for my line element, I will create a new idealization.

04:14

For the type here, we're going to change from solid to line elements.

04:19

And this allows me to put in either a cross section or directly the properties.

04:25

In this case, what we're going to do is define the cross section because we do know those values.

04:30

So, I'll activate cross section.

04:32

And then going to check the box here for associated geometry and choose that line.

04:38

Then if I go to cross section here, right next to it, there's this icon.

04:43

If you click on that icon, you can then put in those properties.

04:47

So, I'll click on that button which opens up this cross-section definition box.

04:53

So, the actual shape we'll be working with is not a rod.

04:56

But using the drop-down menu here, I can switch to any of these cross sections,

04:60

whether it's an I Beam, a Tube, a Channel or in this case, it's going to be just a simple Bar.

05:08

So, two dimensions, dimension one will be the width here,

05:12

dimension two is the height.

05:14

So, we know our width is going to be 0.75 and the height will be half of an inch, put those numbers in.

05:21

And then if you click "Draw End A" at the bottom left, it will show you what that cross section is going to look like.

05:28

So, you can verify the length and the width and it shows you your current coordinate system.

05:35

So, the Y and Z direction here shows me what I'm working with.

05:37

So, I know how this is going to relate back to the system that I have.

05:43

So, I'll select "Ok", I've already chosen that sketch segment, I can go and click "Ok".

05:50

And now beam 1 that idealization has been added to my subcase.

05:55

Once again, you'll notice generic material has been applied to that beam automatically.

05:60

That's Ok as long as I modify those material properties for poisson's ratio and of course, the Young's modulus.

06:09

So, my Young's modulus is going to be 30 e to the sixth.

06:13

My poisson's ratio will be 0.3.

06:18

I can then select "Ok", which will update those material properties for the beam.

06:23

And then when I'm ready, I can just click "Generate Mesh" to create the mesh of that line element.

06:29

And now I'm ready to add in my spring connector.

06:32

So, for my spring connector, I will select "Connectors" from the ribbon along the top.

06:39

From the dialog box, I can then change my type from rod to spring and then I need an end point to represent the two ends of the spring.

06:48

So, for my first end point, I'll just choose the point underneath the beam.

06:52

Second point, I will select the end of the beam or the line connector here.

06:57

So, then I now have that spring.

06:60

It should show in 3D once you've established those two points.

07:04

Now, I can apply a stiffness or a damping coefficient.

07:07

So, you'll notice damping coefficient is your first option.

07:10

You can also apply a spring stiffness between the points.

07:15

Now, when you're applying this, you have to check the box for stiffness and then you'll notice this field is in pound force per inch.

07:22

However, it says K1, that value represents the stiffness in the X direction.

07:29

Which looking at my model, the spring is actually going to apply stiffness in the Y direction.

07:36

So, applying a value here would be incorrect.

07:39

So, in order to access the other degrees of freedom, I can click on "Advanced Options",

07:45

and you'll see K1 through K6, K1 is going to be your stiffness in the X, K2 is stiffness in the Y, K3 is stiffness in the Z,

07:56

K4 is the stiffness of rotation about the X axis, K5 is stiffness and rotation about Y and K6 is stiffness in rotation about Z.

08:07

So, in this case, I'm going to choose K2 or stiffness in the Y and type in 54 pound-force per inch as we reviewed in our free body diagram.

08:16

This means that there's no stiffness in any of the other directions.

08:20

But I'm not concerned about that since the load will be applied in the Y axis here.

08:25

So, I'll leave those blank.

08:28

I've created my spring connector. I can now click "Ok".

08:31

And I'm ready to add in my boundary conditions.

08:34

So, I'll start by adding in my constraints, I'll need a fixed constraint at one end of the beam.

08:39

And then I also need a fixed constraint on one end of the spring to support it rigidly from the ground or whatever else it's connected to.

08:47

So, I'll select "Constraints" and I will rename this fixed.

08:51

So, I know what it represents.

08:53

And then I will go ahead and choose the end point of the spring, point number 1.

08:58

And then the other end of the beam, which is point number 3.

09:02

And if I check the glasses here, you'll see those two icons.

09:05

Those are the fixed locations in this free body diagram.

09:10

So, I will select "Ok".

09:12

And now I'm ready to add in my distributed load.

09:16

So, I will select "Loads" and I will change the type here from force to distributed load.

09:24

And for select identities, I can then choose that line element.

09:30

And for my magnitude, it will be in the Y direction but -Y, so -5lbf/in in the Y axis.

09:39

And then if I increase the density here, I'll see more of those arrows and they should run all the way along the length.

09:45

So, I should have it evenly distributed across that 30 inch.

09:50

And then for name, I'm going to rename this 5lbf per inch.

09:59

So, I know exactly what it is.

10:02

I can then select "Ok".

10:04

And now I have my fixed constraints, my distributed load and my spring.

10:08

So, I'm ready to solve this and generate some results.

10:12

So, before I solve, I will go ahead and save my analysis and then I am going to right click on "Analysis 1" and edit my options.

10:21

What I want is the output set to include force.

10:25

That way I can easily extract the force that's being transferred to the spring to make sure it corresponds with my hand calculations.

10:33

So, I'll activate that check box select "Ok" and then now I'm ready to click on "Run".

10:39

Once the solver finishes, I can then start to extract my displacements, my forces and everything else that I need.

10:46

So, I'll select "Ok".

10:50

So, first thing it shows is my Von Mises stress in the bar element that I created.

10:55

I can then change this to displacement and verify that.

11:00

I was expecting roughly a half an inch or a little bit less of displacement at the end of that beam.

11:08

So, if I go back and look at my expected results,

11:12

once again, we are expecting about -0.499 for displacement,

11:18

and then -26.9 for my pound-force in the spring.

11:24

So, displacement looks good, which means the spring force should be correct.

11:28

To verify that, I can go to my type here and go to "Other".

11:33

Underneath "Other", the subtype that I want is "Bush Force-Y".

11:41

And right here, you can see the amount of force that is being transferred into that connector.

11:47

And you can see the max is -26.989 which is what I would expect.

11:54

And that matches my theoretical calculations as well.

11:58

So, at this point, I'm all set the spring is behaving as I would expect and I'm ready to move on.