Assigning contacts in a Nastran analysis

00:08

In this exercise, we will be assigning contacts to a Inventor Nastran analysis.

00:16

For this exercise, we'll be working with this Yoke assembly.

00:20

It is actually five total components.

00:23

So, looking at the assembly in the model tree, you'll see the two components here and then the subassembly has three parts as well.

00:30

So, there are five separate solid bodies that we will need to connect using contacts to properly solve this FEA.

00:39

Another thing to note with this analysis is that this assembly has been cut into a quarter symmetry model,

00:46

which means it's been cut along two planes.

00:48

The first I have labeled here as the Z symmetry plane.

00:52

So, you can see this entire part has been cut down its middle along its length.

00:57

So, there will be a symmetry constraint applied on that back face there called Z symmetry.

01:03

The other cut plane here, I've labeled Y symmetry.

01:07

So, on the other side here, all of the components have been cut along the Y symmetry plane.

01:13

So, we will need a symmetry constraint on that surface as well.

01:17

And then we will be applying a fixed constraint to the areas where these parts will be bolted together.

01:24

So, for the boundary conditions, I'll work through this fairly quickly.

01:27

I'm going to start with my symmetry constraints.

01:30

So, along the plane called Z symmetry, I'll activate constraints, I'll select that face.

01:37

And then for the symmetry condition, I'll select "Symmetry Z" and I'll rename it Z symmetry as well.

01:44

So, I know what it is.

01:46

In the subcase, you can activate the glasses and update the density of the icons if you want to be able to see better.

01:53

But that's all I really need for that one.

01:54

So, I'll select "Ok", I'll also need symmetry along the Y plane here,

01:60

which is going to be all of the faces touching that Y symmetry plane, which is quite a few.

02:05

So, I work my way through selecting those as well and I'll rename the Constraint "Y Symmetry".

02:10

I'll select "y" underneath "Symmetry" in the dialogue box,

02:15

and then I'll just go through and start selecting all of those faces,

02:20

everything that is touching that plane.

02:23

So, take your time on this, make sure that you've selected all the faces you need to,

02:29

as you work your way along, you can always go back and double check,

02:32

but just be careful as you're making these selections not to select anything that is not touching that plane.

02:41

So, it looks pretty good. That should be all the faces of the parts and the subassembly that are touching that Y symmetry plane.

02:47

It looks pretty good.

02:48

So, I'll select "Ok".

02:50

And it's added into the subcase.

02:54

And then lastly, I'm going to go ahead and fix the faces that would be clamped down and not subjected to any rotation or sliding.

03:03

So, I'll go to constraints,

03:05

and I'll add a fixed constraint onto all of these flat faces here that will be clamped down with a bolt that we have not modeled.

03:12

So, that's going to create enough pressure to fix that face.

03:16

So, I'll select those four there.

03:17

And then same thing on the other side here of the assembly, all four of those faces as well.

03:24

So, eight total in this constraint, I'll rename to fix.

03:28

So, I know exactly what that is and then select "Ok".

03:32

And now I have my constraints here in my "Subcase 1".

03:37

So, now I'm ready to add my bearing load to the yoke component.

03:41

So, to do that, I'll go ahead and select loads and the type here is going to be a bearing load.

03:48

So, I'll change the type to Bearing.

03:50

I'm going to rename this "5000lbf Bearing".

03:56

And then for Selected Entities rotating this part around,

03:60

I'm going to select the kind of curved phase here of the yoke on this side,

04:05

and then the other side will receive that same selection as well.

04:10

But notice because I'm applying 5000 pound-force total, I need to check the box right here under load definition for total force.

04:18

Otherwise, it will be 5000 pound-force per entity, but I want it to be 5000 pound-force total.

04:24

So, I'll activate that check box and for direction, it will be the positive y direction 5000 pound-force and turning on the glasses.

04:32

You can then see that load applied to both of those faces, essentially 2500 pound-force each.

04:39

So, I'll select "Ok", once I'm ready to go and now my boundary conditions are complete.

04:46

bBefore I go any further, I am going to turn the visibility of the planes and the boundary conditions off.

04:51

So, it's a little bit cleaner and easier to see what I'm doing with contacts.

04:56

So, I'm going to go to "Object Visibility" and I'm going to deactivate Constraints, Loads.

05:01

That looks pretty good. And I'm just going to go ahead and right click on these planes and then turn their visibility off.

05:06

It's usually the easiest way to do it.

05:08

I can always bring them back in later if I need them, but that should be good to go and now I can go ahead and add in some contacts.

05:16

So, for this assembly, I'm going to use primarily automatic contacts,

05:20

but I will make some adjustments to the settings and the overall contact type specified.

05:26

To start, I always edit my Analysis.

05:28

So, I'll right click and go to edit.

05:32

I go to the Options tab and this is where you see Contact Data Bonded and a Tolerance of 0.1 millimeters or 0.0039 inches.

05:42

I'm going to update this to be 5/1000 of an inch,

05:46

which means any surfaces that are 5/1000 of an inch away from one another will automatically receive a bonded contact type.

05:54

I like to adjust the tolerance to make sure I know what that number is and it's not a guessing game.

05:60

So, I'll then select "Ok".

06:01

And now when I run automatic contacts, it should use that 5/1000 of an inch tolerance.

06:06

So, I'll click on auto contacts from the panel.

06:11

And now over in the analysis tree, you'll see "Surface Contacts" folder.

06:15

If I expand it, you'll see there are six contacts created.

06:19

The first one here is between, looks like the lip of this first part and then the lip of the next.

06:27

Should be the same thing on the other side.

06:30

Got a couple of surface contacts between the face of the yoke and then the face of the next subassembly.

06:38

So that looks pretty good.

06:40

It's just mostly picking up those planes, those larger surfaces that are touching one another.

06:44

So, I'll leave that for now and I can always come back and fine tune this by adding additional contacts or editing these current contacts later.

06:52

But I like to solve the analysis first to make sure that there aren't any instabilities in my constraints,

06:59

or my basic contacts before I begin fine tuning it.

07:05

So, at this stage, I'll just select "Save" to save my changes and then now I can go ahead and run.

07:17

So, the analysis completes I will select "Ok".

07:19

And now it should show my Von Mises stresses and displacement.

07:23

What it's going to do by default is exaggerate the deformation.

07:27

So, I'm going to go to the top panel here and turn deformed shape off just so that I can see the stresses.

07:36

And this will make it a little bit more clear.

07:37

I don't have such a weird image that I'm looking at.

07:40

I can see the high stress is kind of here near the edge of that constraint at that sharp corner should be pretty symmetric.

07:48

So, I should see a similar result on the other side.

07:51

When you're working with a model, it's mostly symmetric. That's what you want to see.

07:55

If for some reason something looked off, I would go back and double check my constraints, but this all looks pretty good.

08:01

So, at this stage, I can then decide if I want to make any adjustments to my contacts before I do that,

08:08

I'll just double check displacement real quick.

08:12

And that looks reasonable, right? I'm not seeing like 10 inches of displacement.

08:16

I'm seeing less than 1/1000 of an inch, which is what I would expect from a linear static stable model like this.

08:23

So, I'm good for now, I'll go ahead and save my results as they are.

08:28

And then now I'm ready to fine tune the contacts.

08:32

So, to determine what changes I want to make to these contact sets.

08:36

One really useful tool from inventor Nastran 2024 is the ability to look at contact reaction forces.

08:44

So, for instance, Contact 1 here,

08:47

if I right click and I go to "Contact Reactions", it'll tell me some of the forces that this contact is seeing.

08:55

So, it's seeing about 126 pound-force in the negative Y.

08:59

So, as this lifts upwards, it's holding it down in the negative Y direction.

09:04

And then also quite a bit of force in the Z direction about 900 pound-force in the positive Z.

09:10

So, it's trying to move away in the Z and this is keeping it in that direction.

09:17

So, looking at that face, that contact, if I take a closer look at it, I'll right click and edit the contact.

09:25

It's between this face here and then this small lip face right there.

09:29

Now, those faces are touching, but they are not bonded together.

09:36

There's nothing that is welding those two faces together, they should be able to slide and separate.

09:42

Because I've applied a bonded contact it is actually creating a force between the two.

09:48

So, as this part is being lifted up by that bearing load,

09:53

those two parts are holding together with that bonded contact, creating artificial stiffness.

09:59

So, I need to edit both of those contacts, contact 1, and then the same thing here contact 2 on the other side,

10:06

I need to make those something besides bonded.

10:09

So, I'm going to go ahead and edit Contact 1.

10:12

So, right click and go to "Edit".

10:14

I can see the contact type is bonded.

10:17

If I hit the drop-down menu here, I can look at these other contact types.

10:21

Now, separation as we've gone through before, allows for sliding and separation bonded welds them together, sliding allows for sliding in plane,

10:32

but it would act like it's bonded in tension and compression.

10:35

I don't really want any bond between the two parts.

10:38

So, the best option here is going to be a separation contact that prevents the two parts from penetrating or overlapping one another,

10:46

but it will allow them to slide and rotate freely.

10:48

So, activate separation for that contact type and then I'll select "Ok".

10:55

I'm going to edit Contact 2.

10:59

Same thing here. I'm going to change it to separation and select "Ok".

11:03

So, now Contact 1 and 2, the icon has changed to a separation, contact.

11:08

The other four will remain bonded, which is what I want.

11:11

And this will give me a more accurate result when I go to solve because I'm going to allow for some more degrees of freedom to be available.

11:18

So, I'll go ahead and save this model with the contact updates,

11:22

and I'll solve it again and then I'll be able to compare the result for stress and displacement.

11:27

So, I'll select "Run".

11:32

So, after solving a second time I'll notice that the stresses and displacements look most of the same.

11:38

If I look at the area where I'm seeing the maximum stress, it has moved slightly.

11:44

It's now in between those two parts that are bonded together, but I still have similar hot spots around that area.

11:50

If I go to displacement, I should be seeing less than a thousandth of an inch and the displacement is very similar.

11:57

So, that's good. I haven't changed the model significantly.

11:59

But what I am allowing for is if I go to Contact 1 here,

12:04

and I look at the contact reactions once again, you'll notice now there's only a couple pound force of reaction force.

12:10

I'm not really seeing a significant amount of reaction in the Y or the Z where I was seeing about 100 and 60 in the Y and 900 in the Z before.

12:19

Now, there's not much of an interaction there that means that the load is being transferred to the correct components.

12:26

And I'm not artificially stiffening the model with an artificial bonded contact.

12:32

So, this is going to be a much more reliable and accurate contact set,

12:36

and I'm now ready to run a convergence study to analyze these results even further.