Author: Rajesh Bhaskaran & Yong Sheng Khoo, Cornell University

Problem Specification

1. Pre-Analysis & Start-Up

2. Geometry

3. Mesh

4. Setup (Physics)

5. Solution

6. Results

7. Verification & Validation

Under Construction

The following ANSYS tutorial is under construction.

#### Problem Specification

Consider the beam in the figure below. There are two point forces acting on the beam in the negative y direction as shown. Note the dimensions of the beam. The Young's modulus of the material is 73 GPa and the Poisson ratio is 0.3. We'll assume that plane stress conditions apply.

**Go to Step 1: Pre-Analysis & Start-Up**

Author: Rajesh Bhaskaran & Yong Sheng Khoo, Cornell University

Problem Specification

1. Pre-Analysis & Start-Up

2. Geometry

3. Mesh

4. Setup (Physics)

5. Solution

6. Results

7. Verification & Validation

## Step 1: Pre-Analysis & Start-Up

#### Start ANSYS Workbench

We start our simulation by first starting the ANSYS workbench.

**Start > All Programs > ANSYS 12.1 > Workbench**

Following figure shows the workbench window.

At the left hand side of the workbench window, you will see a toolbox full of various analysis systems. In the middle, you see an empty work space. This is the place where you will organize your project. At the bottom of the window, you see messages from ANSYS.

#### Select Analysis Systems

Since our problem involves static analysis, we will select the ** Static Structural (ANSYS)** component on the left panel.

Left click (and hold) on

**, and drag the icon to the empty space in the**

*Static Structural (ANSYS)***.**

*Project Schematic*Since we selected Static Structural (ANSYS), each cell of the system corresponds to a step in the process of performing the ANSYS Structural analysis. Right click on ** Static Structural ANSYS** and

**the project to**

*Rename***.**

*Beam*Now, we just need to work out each step from top down to get to the results for our solution.

- We start by preparing our geometry
- We use geometry to generate a mesh
- We setup the physics of the problem
- We run the problem in the solver to generate a solution
- Finally, we post process the solution to gain insight into the results

#### Specify Material Properties

We will first specify the material properties of the crank. The material has an Young's modulus E=2.8x10^{7} psi and Poisson's ratio ν=0.3.

In the Crank cell, double click on ** Engineering Data**. This will bring you to a new page. The default material given is

**. We will use this material and change the Young's modulus and Poisson's ratio.**

*Structural Steel*Left click on ** Structural Steel** once and you will see the details of Structural Steel material properties under

**. Expand**

*Properties of Outline Row 3: Structural Steel***, change**

*Isotropic Elasticity***and**

*Young's Modulus***to E=7.9e10 pa and ν=0.3. Remember to check that you use the correct unit.**

*Poisson's Ratio*Press the ** Return to Project** to return to Workbench

**window.**

*Project Schematic*Author: Rajesh Bhaskaran & Yong Sheng Khoo, Cornell University

Problem Specification

1. Pre-Analysis & Start-Up

2. Geometry

3. Mesh

4. Setup (Physics)

5. Solution

6. Results

7. Verification & Validation

## Step 2: Geometry

At Workbench, in the ** Beam** cell, right click on

**, and select**

*Geometry***. You will see the properties menu on the right of the Workbench window. Under**

*Properties***, select**

*Basic Geometry Options***. This is because we are going to create a line geometry.**

*Line Bodies*

In the ** Project Schematic**, double left click on

**to start preparing the geometry.**

*Geometry*At this point, a new window, ANSYS Design Modeler will be opened. You will be asked to select desired length unit. Use the default ** meter** unit and click

**.**

*OK*#### Creating a Sketch

Like any other common CAD modeling practice, we start by creating a sketch.

Start by creating a sketch on the ** XYPlane**. Under

**, select**

*Tree Outline***, then click on**

*XYPlane***next to**

*Sketching***tab. This will bring up the**

*Modeling***.**

*Sketching Toolboxes*Note: In sketching mode, there is ** Undo** features that you can use if you make any mistake.

On the right, there is a ** Graphic** window. At the lower right hand corner of the Graphic window, click on the

**axis to have a normal look of the**

*+Z***.**

*XY Plane*In the ** Sketching Toolboxes**, select

**. In the**

*Line***window, create three rough lines from starting from the origin in the positive XY direction (Make sure that you see a letter P at the origin and at each connection between the lines. The letter P the geometry is constrained at the point.)**

*Graphics*You should have something like this:

Note: You do not have to worry about dimension for now, we can dimension them properly in the later step.

#### Dimensions

Under ** Sketching Toolboxes**, select

**tab, use the default dimensioning tools. Dimension the geometry as shown:**

*Dimensions*

Under ** Details View** on the lower left corner, input the value for dimension appropriately.

H1: 0.1 m

H2: 0.2 m

H3: 0.1 m

We are done with sketching.

#### Create Surface

Now that we have the sketch done, we can create a line body for this sketch.

**Concept > Lines From Sketches**

This will create a new line *Line*** 1**. Under

**, select**

*Details View***as**

*Sketch1***and click**

*Base Objects*

*A***. Finally click**

*pply***to generate the surface. This is what you should see under your**

*Generate***.**

*Tree Outline*

#### Create Cross Section

We will now add a cross section to the line body.

**Concept > Cross Section > Rectangular**

Under Details View, input value as follow:

B - 0.05m

H - 1m

Finally, under expand the Line Body

**Outline > 1 Part, 1 Body > Line Body**

And attach ** Rect1** to

**under**

*Cross Section***.**

*Details View*We are done with geometry. You can close the

**and go back to**

*Design Modeler***(Don't worry, it will auto save).**

*Workbench*Author: Rajesh Bhaskaran & Yong Sheng Khoo, Cornell University

1. Pre-Analysis & Start-Up

2. Geometry

3. Mesh

4. Setup (Physics)

5. Solution

6. Results

7. Verification & Validation

## Step 3: Mesh

Save your work in ** Workbench** window. In the

**window, right click on**

*Workbench***, and click**

*Mesh***. A new**

*Edit***window will open.**

*ANSYS Mesher*Use the default mesh. Under ** Outline**, right click on

**and click**

*Mesh***. This should be the mesh appear in the Graphics window.**

*Generate Mesh*

Author: Rajesh Bhaskaran & Yong Sheng Khoo, Cornell University

1. Pre-Analysis & Start-Up

2. Geometry

3. Mesh

4. Setup (Physics)

5. Solution

6. Results

7. Verification & Validation

## Step 4: Setup (Physics)

We need to specify point BC's at *A*, *B*, *C* and *D*.

Let's start with setting up boundary condition at A.

**Outline > Static Structural (A5) > Insert > Remote Displacement**

Select point A in the ** Graphics** window and click

**next to Geometry under**

*Apply***. Enter 0 for all UX, UY, UZ, ROTX and ROTY except for ROTZ. Let ROTZ to be free.**

*Details of "Remote Displacement"*

Let's move on to setting up boundary condition B.

**Outline > Static Structural (A5) > Insert > Remote Displacement**

Select point B in the ** Graphics** window and click

**next to Geometry under**

*Apply***. Enter 0 for all UY, UZ, ROTX and ROTY except for ROTZ. Let UX and ROTZ to be free.**

*Details of "Displacement 2"*We can move on to setting up point force at point C and D.

**Outline > Static Structural (A5) > Insert > Force**

Select point C in the ** Graphics** window and click

**next to Geometry under**

*Apply***. Next to**

*Details of "Force"***, change**

*Define By***to**

*Vector***. Enter -4000 for**

*Components***.**

*Y Component*Do the same for point D.

Check that you have for all the boundary conditions. Click on ** Static Structural (A5)** to view this in Graphics window.

Author: Rajesh Bhaskaran & Yong Sheng Khoo, Cornell University

1. Pre-Analysis & Start-Up

2. Geometry

3. Mesh

4. Setup (Physics)

5. Solution

6. Results

7. Verification & Validation

## Step 5: Solution

Now that we have set up the boundary conditions, we can actually solve for a solution. Before we do that, let's take a minute to think about what is the post-processing that we are interested in. We are interested in the deflection and bending stress on the beam. We would also like to look at the force and moment reaction at our support A and B. Let's set up those post-processing parameters before we click solve button.

Let's start with inserting Total Deformation.

**Outline > Solution (A6) > Insert > Total Deformation**

Next let's insert beam tool that will enable us to look at the stresses on the beam.

**Outline > Solution (A6) > Insert > Beam Tool > Beam Tool**

We would also like to look at the Force Reaction at point A and B.

**Outline > Solution (A6) > Insert > Probe > Force Reaction**

Select ** Remote Displacement** (which is point A) next to

**under**

*Boundary Condition***.**

*Details of "Force Reaction"*

Do the same step for Remote Displacement 2 (point B).

Next we will like to check and see that the moment at point A and B is zero.

**Outline > Solution (A6) > Insert > Probe > Moment Reaction**

Select ** Remote Displacement** (which is point A) next to

**under**

*Boundary Condition***.**

*Details of "Moment Reaction"*

Do the same step for Remote Displacement 2 (point B).

We are done setting up all the results. Click ** Solve** at the top menu to obtain a solution. Wait for a minute for the solution.