Static stress overview

00:06

In this video we talk about a Static Stress analyses,

00:09

specifically their purpose, workflow capabilities, and what results they produce.

00:15

Perform a Static Stress analysis to determine stress, strain, displacement and safety factor

00:20

in a part or assembly resulting from various applied loads.

00:24

You can also determine contact pressures between parts of an assembly.

00:28

In order for this type of study to be valid, the model must have the following characteristics.

00:34

For accurate results, stresses cannot exceed the yield strength of the materials.

00:39

The loading must cause only small deflections or rotations,

00:43

so deformation can't have a significant effect on the load direction, magnitude,

00:47

or the surface area to which loads are applied.

00:51

Also, the deformation can't alter where or in what manner the parts are constrained.

00:56

Finally, dynamic effects from the loading are not significant.

01:01

Static Stress analysis do not consider damping or inertial effects that is momentum.

01:07

This model is a three-part assembly consisting of a connecting rod and two round pins.

01:12

A 2000-pound tensile load is applied to the assembly.

01:16

Separation contact is defined between the parts,

01:19

meaning that the pins can freely slide along or separate from the connecting rod

01:23

but the parts can't penetrate through each other.

01:29

Let's take a look at the process of setting up and solving the analysis.

01:34

The first time you enter the Simulation workspace,

01:37

the New Study dialog launches automatically.

01:40

Choose the Static Stress analysis type.

01:44

Click this icon to access the Study Settings.

01:48

We'll define an absolute mesh size of 0.125 inch

01:51

which will produce two elements through the thickness

01:54

in the thinnest regions of the connecting rod.

01:59

If you want to make changes to the model for your simulation, use the Simplify command.

02:04

The tools in the Simplify workspace enable you to

02:08

remove unnecessary components or features.

02:11

Split faces to confine a loader constraint to only a portion of a larger face,

02:16

or to provide edges or vertices for locating loads and constraints.

02:20

Or modify the geometry in any way you want to achieve the desired results.

02:27

Any changes you make here affect only the simulation model.

02:31

The production geometry represented in the Model workspace (Design workspace)

02:35

remains unchanged.

02:37

Click Finish Simplify to return to the Simulation workspace.

02:42

The materials were previously defined in the Model workspace (Design workspace)

02:46

we'll confirm that the study materials match the model materials.

02:51

Let's apply the following constraints to make the model statically stable

02:55

without impeding its expected displacement under load.

02:59

Fully fix the ends of the small pin.

03:02

You can left-click and hold the mouse button down to see a menu of items to select,

03:07

including hidden ones.

03:10

Apply a Z constraint to the straight edges on the large pin.

03:14

This constraint prevents the pin from spinning in its hole

03:20

and prevents the connecting rod from rotating about the center line of the small pin.

03:31

Apply a Y constraint to the pin and connecting rod edges at the middle of the large hole.

03:39

This constraint prevents the connecting rod from sliding axially along the small pin,

03:44

and it prevents the large pin from sliding axially in the large hole.

04:01

Next, apply a total load of 2000 pounds in the minus X direction to the ends of the large pin.

04:17

Automatically detect all contact sets.

04:20

The default tolerance is fine because the parts are touching at each contact face.

04:26

Edit all contact sets to change the contact type from “Bonded” to “Separation”.

04:37

Now let's clone this study to make a new one, in which we'll use a different setup.

04:43

In the Settings dialog, enable the “Remove rigid body modes” option.

04:48

The solver will stabilize the model automatically

04:51

by adding a global acceleration load and soft spring constraints.

04:55

Delete the fixed constraint on the small pin.

04:59

There is now no X constraint anywhere on the model.

05:03

Also, we'll balance the applied load with an opposite force at the ends of the small pin.

05:09

This method will allow the small pin to rotate at its ends,

05:13

behaving like a simply supported beam.

05:15

In the first study, the pin behaves like a built-in beam due to the fixed constraint at the ends.

05:21

The studies are ready to solve.

05:39

When the solution finishes, the Study 2 safety factor results appear.

05:43

The orange and white exclamation point indicates that the design is marginal.

05:48

The result is greater than one, meaning that the yield strength has not been reached.

05:52

However, the safety factor is lower than typically recommended.

05:56

Since we're going to look at the results of two different model setups,

05:60

we'll go to the Compare workspace.

06:02

Here we can see the two studies side by side.

06:06

Ensure that Study 1 is on the left and Study 2 on the right.

06:10

By default, the model viewpoint and result type are synchronized for the compare windows.

06:16

The minimum safety factor is greater for Study1. We'll see why in a moment.

06:23

Let's compare the Von-Mises stress results.

06:26

In Study 1, the maximum stress occurs at the ends of the small pin where it's constrained.

06:36

In Study 2 the stress is greater and occurs at the middle of the pins length

06:41

which explains the difference in the safety factors.

06:47

Display the X displacement component.

06:53

Notice that in Study 1, all X displacements are zero or negative.

06:57

In Study 2, because of the opposing forces, both negative and positive X displacements occur.

07:04

The difference between the minimum and maximum displacement values is greater than the maximum displacement in Study 1.

07:11

The reason is that the small pin bends more freely without the fixed constraints at the ends.

07:17

Finally, the maximum contact pressure is greater in Study 2.

07:22

The increased bending deformation of the small pin causes more localized contact

07:27

between the pin and connecting rod.

07:29

So, this result is not surprising.

07:38

Thank you for watching.