Assigning rigid body connectors in a Nastran analysis

00:08

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

00:16

So, for this example, we'll be working with this large sheet metal plate.

00:21

This is a quarter of an inch thick.

00:23

And if you look at the shell element idealization that's already been created,

00:27

you will see that quarter inch thickness and alloy steel applied to that sheet.

00:33

What we would like to do for this example is apply a lumped mass that will sit on these four bolt hole locations.

00:42

So, it's going to be attached to the plate via those bolts.

00:45

And we want to represent the force that that mass would create in our FEA.

00:51

So, in order to do that, first, I need to create that concentrated mass at the control point.

00:59

So, if I look at my model, you will see there's a center of gravity work point that's been created, that's about a foot above this plate.

01:08

So, what I can do is under "Idealizations", I'll hit the drop-down menu and use concentrated mass this time.

01:16

And what this allows me to do is create a lumped mass at a given center of gravity.

01:20

So, if you're selected entities here you want to select a vertex.

01:24

This can be a sketch point or a work point.

01:27

In this case, I will choose the work point right there that I already created.

01:32

So, it creates this green and gray box.

01:34

This represents a lumped mass.

01:37

All you need to do here is enter in a mass value.

01:40

It will be converted into units of gravity.

01:44

So, it will be divided by gravity automatically.

01:47

You can just put in the value in pounds.

01:51

So, in this case, this is going to be a 200 pound mass.

01:55

So, you have to type in the units.

01:56

Otherwise, it won't be correct.

01:58

So, 200 pound and I'm going to go ahead and rename the mass "200 Pound Mass".

02:06

And then I can select "Ok".

02:08

And it will be added into the idealizations here as a concentrated mass.

02:13

If you double click on that mass to open it back up, you'll notice that it's been divided by gravity.

02:20

So, it's automatically been done for me.

02:23

And now in order for this mass to properly act on our system, we need to apply gravity load.

02:31

Otherwise, it doesn't know which way this mass is going to inflict a force.

02:37

So, if I create a new load, I can change that type to gravity and I'll rename it gravity as well just to be clear.

02:46

And then for my direction, it will be the negative Z direction in this case.

02:51

So, -386.4.

02:53

And if I turn on the little icon glasses here, it shows the arrow in the correct direction and the G icon in the bottom, right, I'll select "Ok".

03:01

So, now gravity has been applied and that will act on that mass.

03:05

Now, if I just solve the analysis now, there's nothing connecting this mass to my finite element mesh.

03:14

In order to connect a mass or a force to the mesh, that is not directly acting on a face, but it needs a intermediate member.

03:24

So, maybe there's a structure that I haven't modeled.

03:27

Maybe this is a battery or a fuel cell or something that I didn't model.

03:33

But I want to take into account its mass and its stiffness.

03:37

The best way to connect a mass or force to your mesh is using a rigid body connector.

03:44

So, if I select "Connectors" here it opens up my connector dialogue, I'm going to change to rigid body this time.

03:51

And this is where you have the option to choose dependent entities and an independent point.

03:55

Now there's two ways to do this rigid and interpolation,

03:58

rigid is going to require that whatever happens to the vertex point that is rigidly transferred to the dependent entities.

04:08

Whereas with interpolation, it averages that displacement.

04:11

So, it's more of a way to transfer a load.

04:14

But if you have a structure that's been bolted to this face,

04:18

that's going to be a very rigid connection and that's why I'm choosing a rigid or an RBE2 in this case.

04:24

For my dependent entities, I have to choose where this mass is connected to.

04:30

Which is going to be the edges of those four bolt holes.

04:34

So, I'll grab the edges of the shell at all four locations.

04:38

Make sure you select all four of these edges here.

04:41

So, there should be four selections edge 1, 2, 3 and 4, showing up independent entities.

04:49

The degrees of freedom here, you have Tx, Ty, Tz and Rx, Ry, Rz.

04:53

So, translation along each axis as well as rotation about the axis.

04:58

This is if you want the mass to be able to move or that rigid to be able to move independent from the dependent entities.

05:08

So, if you want the independent point to be able to move independent from the dependent ones.

05:13

In this case, I'm going to leave them all checked since this is going to be a rigid structure bolted to that plate.

05:19

For my independent vertex point, I can choose the point from which those edges are connected,

05:25

which will be the center point that I used for the mass already.

05:28

So, I'll click that point.

05:30

Work point number 1 shows up here and you can see it creates these rigid body connectors back to the nodes on those edges.

05:38

So, a rigid element is added from that point to all the nodes around the circumference of those edges attaching it to the mesh.

05:46

So, I can now click "Ok".

05:49

And now when I run this analysis, gravity will act on the mass,

05:52

which will transfer its force through the rigid elements to the nodes on those holes,

05:58

creating a stress and strain on the mesh.

06:01

So, I will go ahead and click "Save" and then I will go ahead and click "Run" to solve this study.

06:10

So, now the analysis completed successfully and you can see the effect of that mass sitting on the plate creating about 8000 psi of stress.

06:19

If I switch my result over to displacement, I can look at those results as well.

06:23

And you can see a few 1000th of an inch of displacement.

06:26

But it is as though I have a full structure sitting on the plate,

06:31

but it doesn't require me to mesh and add a bunch of nodes and elements to my analysis.

06:38

It really keeps things simple.

06:40

Allows me to take into account the strength and stiffness of those components without modeling them.

06:46

I can also get a better visual if I turn deformation off as well as the visibility of my constraints connectors and loads.

06:55

So, if I go to "Object Visibility", I'll deselect my Mass, Connector, Constraint and Load.

07:02

And now it's a little bit easier to see the displacement and it will also make it easier to see the stress on this model.

07:09

So, if you're looking to connect a constraint load or mass onto your part per assembly,

07:16

sometimes the best way to do that is using a rigid body connector, instead of actually creating the model and using contact.

07:23

So, keep that in mind next time you are setting up a more advanced assembly level analysis.