Assigning bolt connectors in a Nastran analysis

00:08

In this exercise, we will be working with bolt connectors in an Inventor Nastran analysis.

00:15

So, before we begin adding in bolt connectors to an assembly in an Inventor Nastran analysis,

00:21

I wanted to discuss briefly what a bolt connector represents and what's happening in the background when you go to solve.

00:29

So, when you establish a bolt connector,

00:31

you are required to choose the edge that represents the head side of the bolt and an edge that represents the nut side of the bolt.

00:39

Once those have been chosen, Inventor Nastran automatically in the background,

00:43

creates a line element running through the middle of the hole from edge to edge.

00:50

The cross-sectional area of that line element will be equal to the cross-sectional area of your bolt that you define.

00:56

Coming off the end of your line element, attached to the edge of the hole that you select is a rigid body connector.

01:04

So, it creates what's called a wagon wheel or a spoke configuration,

01:08

where the rigid body connector represents the head on this side and the nut on this side.

01:14

And it establishes the stiffness that would be created by that bolt connection with much fewer elements.

01:21

So, when you go to create a bolt connector,

01:24

and you're asked to choose a edge for the bolt head and then one for the bolt nut,

01:32

this is actually what Nastran does in the background.

01:34

It creates these rigid body connections to the center point.

01:37

And then the bolt diameter that you specify here for your connector,

01:41

is directly correlated to the diameter of that line element that will span that distance.

01:47

You can then add in things like washers, materials and preload.

01:51

But this is the basic configuration that you are simplifying your three-dimensional body down to.

01:57

So, it's important to understand what's being created before you start adding these into an assembly.

02:02

So, now we'll move into an assembly and add these in for a Nastran analysis.

02:09

So, we're working with this fender assembly for this exercise.

02:13

And in this version, this is fender assembly number 1.

02:16

You'll notice there are bolts modeled into the Inventor assembly files.

02:21

You'll see there are M10 by 6 bolts being used to connect the flap here to the fender.

02:27

And if I rotate around, you can see this side out here is the head side and then the inside here is going to be your nut side.

02:35

And what we want to do is simplify this.

02:37

If I bring this directly into Inventor Nastran, I'll need to establish contacts between each of these individual bodies.

02:46

And I'm also going to need to mesh these small surfaces and these really small threads that are included on the bolt.

02:54

So, even if I do simplify these down as a three-dimensional body, I will still be adding hundreds of thousands of elements to my analysis.

03:02

When in reality, I may be more concerned about the structure as a whole rather than the individual bolts and the stress is seen local to those areas.

03:12

So, for the Nastran analysis, those bolts have been removed.

03:16

Everything else has remained the same.

03:17

But those 10-millimeter bolts will be simplified to a connector for purposes of FEA.

03:23

So, we'll start with this assembly here and I will go ahead and open up Inventor Nastran.

03:30

So, opening up Inventor Nastran, you'll notice that I have already meshed this assembly.

03:35

There's two idealizations.

03:36

There's a solid idealization for the alloy steel components and a second solid idealization for the aluminum component,

03:43

which is really just this flap down here.

03:47

So, we have those components modeled under the mesh settings.

03:51

I've chosen a element size of 10 millimeters, linear solid elements to speed up the analysis time a little bit and focus in on our key displacements.

04:03

So, we'll start with the bolt connectors.

04:05

So, if I activate the "Connectors" dialog box, I can change the type here to bolt.

04:11

Just like we've seen in prior connectors under materials, I can't determine or add a new material.

04:19

I can only choose from materials that have already been created.

04:22

So, keep that in mind, in this case, I'm going to use Alloy Steel as my material.

04:28

I can choose a surface or an edge for the bolt head and a surface or an edge for the bolt nut.

04:34

If you change the type up here from bolt to cap screw, you can choose a surface for a threaded region.

04:41

So, instead of having to choose an edge, you can actually choose a surface where the threads would be engaged.

04:47

It also gives you the ability to choose a useful length or how much of the thread length will be engaged in the part.

04:54

In this case, I am using bolts as we discussed before.

04:58

So, I'll need to first determine the edge where I want the bolt head, which was on the outside of this model.

05:04

So, zooming in, I can grab this edge right here.

05:08

For my nut side, I have to rotate the model around and on the other side, on this plate, I need to choose this edge right there.

05:16

What that will do is establish a bolt between those two components clamping together those parts.

05:25

Now, what you'll notice is for diameter, it automatically populated 12 millimeters.

05:31

However, keep in mind that the diameter that's chosen when you choose this edge is the diameter of that edge.

05:39

It may not be the diameter of the bolt.

05:42

In this case, we know that we're using 10-millimeter bolts.

05:46

So, I'll go ahead and change this to 10 and I can do that for all the bolts that I create in this set.

05:55

In this case, I'm not going to apply any washers.

05:58

However, the head washer height just increases the stack height.

06:01

The nut washer height does the same thing on the other side.

06:04

It does not disperse the load to a wider area.

06:09

It only increases how far, how long that internal line element is going to be.

06:15

Alloy steel is my material.

06:17

And then for preload for newtons, we're just going to go ahead and just do a 50 Newton preload on these.

06:23

It's good to do some level of preload which will pre stiffen the structure and that connection before completing the load application in your FEA.

06:32

So, it's good to add at least an axial or a torque preload to all of these bolts.

06:37

I'm going to rename my connector 10 millimeter bolts.

06:42

And then if I'd like to continue in this set and add them all together,

06:47

I will click "Next" under connector element and bolt two will be created,

06:52

and I can then repeat the process for these other bolt locations.

06:56

So, I'll go through the next one here before I jump ahead.

06:59

So, I'll grab the edge on the outside of that green part, the edge on the inside.

07:04

And then once again, the bolt diameter I will make 10, the preload stays populated,

07:10

material stays populated and I can continue from there clicking next and adding all five bolts.

07:18

So, now that I have my bolt connectors added into the analysis.

07:22

I can then add my constraints, loads and contacts.

07:26

We're working in an assembly. So, we need to make sure all of our surfaces are accounted for.

07:31

So, I will select "Constraints" to start and I am going to add a fixed constraint onto the end of these, flan is sticking out.

07:39

So, I'm going to select both of those end faces right there.

07:42

I'll rename the constraint fixed and I'll leave all my degrees of freedom checked, activate the glasses to see where that's at and then click "Ok".

07:53

Now, I can add in my load which will be added to the end of the flap here.

07:56

So, I'll add a load.

07:59

This will be a simple force applied to the end face right here.

08:05

So, the bottom face of that flap, the load direction is going to be the negative X direction.

08:11

It will be negative 200 newtons.

08:16

So, if I increase the density there, you can see that arrow being applied to that face, holding that flap outwards horizontally in the X direction.

08:26

So, I will rename this 200 Newton X load and select "Ok".

08:34

So, now I have my constraints and loads and now I'm ready to add my contacts.

08:41

So, I will use automatic contact to generate my contact sets and everything will be welded or joined together rigidly.

08:48

The only area that I want to allow for separation and sliding is everything between these parts here that is going to be bolted.

08:59

So, what I can do is I can go ahead and run automatic contacts.

09:05

It's going to create this photo with these 18 contacts and then I can go through and clicking on the contacts.

09:12

It highlights the faces involved.

09:14

So, where I want to focus is that area around the bolted connection.

09:18

So, this face right here.

09:23

So, contact 6, contact 7, those are going to be areas that we want to adjust and allow to separate.

09:36

So, I can take contact 6 and edit that connection.

09:40

Instead of being bonded, I'll change it to separation and click "Ok".

09:44

I can do the same thing for contact 7, that other face there.

09:49

That is also going to be separation.

09:51

So, I'll change the contact type select "Ok".

09:53

Everything else can remain bonded as I am holding the rest of the structure together with welds.

09:59

And now we are ready to run the FEA.

10:02

Before I do, so, I am going to right click on "Analysis 1" and go to "Edit" and like before I will activate force for the output set.

10:11

This will allow me to extract the forces on the individual bolt connectors as well as the stresses and displacements like usual.

10:19

So, I will select "Ok", and I'll Save my analysis and then I will Solve and then I'll view the results.

10:28

So, let me click on "Run" and we'll let the solver go.

10:33

So, once the analysis finishes, it should take roughly five minutes, maybe a little longer depending on your computer.

10:41

Once it's done, the first thing that it will show is your solid Von Mises stress.

10:45

So, this will only show stress on the solid elements.

10:48

Notice those line elements for the connectors do not have any stress shown because it is a different type of element.

10:55

You can only display one element stress type at a time.

10:59

So, the stress on the solid looks pretty good.

11:01

What I'll then do is go ahead and switch to displacement, to make sure my displacement results look reasonable.

11:10

About 1.7 millimeters at the end of that flap, which looks about right based off of the way this load is being applied horizontally.

11:20

And then if I'd like to see the forces acting on the line elements or the bolt connectors,

11:26

I can change my type to beam diagram and the beam diagram will actually give me the ability to go through this list,

11:34

and look at the bar forces which are the forces on those connectors.

11:40

So, if I were to look at Bar Force End A-X, there's A-Y Plane 1, A-Z Plane 2, these are broken down in the article for this exercise.

11:49

So, you can go through and determine which direction, which value you are worried about.

11:54

And when you select one of these, it will then populate this legend.

11:58

It will also display that value for any one of these.

12:02

So, if I go to Bar Force End A-X, it'll display it on the actual 3D model as well.

12:08

So, if I zoom in on these connectors, you can see they've changed to a red color,

12:13

meaning we're probably around couple pounds, sorry, a couple newtons in this case, per bolts,

12:22

and you can then probe those results as well.

12:25

And you can even use a combination of these images to build a nice report.

12:31

So, that's how bolt connectors work.

12:33

again, they're great to use in an assembly when you'd like to simplify your 3D model a little bit more,

12:38

and remove some of the smaller hardware components.

12:41

But you'd still like to take into account the strength and stiffness provided by those bolts.