##
Introduction

This tutorial is the second of three basic tutorials created to illustrate commom features in ANSYS. The plane stress bracket tutorial builds upon techniques covered in the first tutorial (3D Bicycle Space Frame), it is therefore essential that you have completed that tutorial prior to beginning this one.

The 2D Plane Stress Bracket will introduce boolean operations, plane stress, and uniform pressure loading.

###
Problem Description

The problem to be modeled in this example is a simple bracket shown in the following figure. This bracket is to be built from a 20 mm thick steel plate. A figure of the plate is shown below.

This plate will be fixed at the two small holes on the left and have a load applied to the larger hole on the right.

The first step is to simplify the problem. Whenever you are trying out a new analysis type, you need something (ie analytical solution or experimental data) to compare the results to. This way you can be sure that you've gotten the correct analysis type, units, scale factors, etc.

The simplified version that will be used for this problem is that of a flat rectangular plate with a hole shown in the following figure:

**Give the Simplified Version a Title****Utility Menu > File > Change Title**
**Form Geometry**Boolean operations provide a means to create complicated solid models. These procedures make it easy to combine simple geometric entities to create more complex bodies. Subtraction will used to create this model, however, many other Boolean operations can be used in ANSYS.

- Create the main rectangular shape
Instead of creating the geometry using keypoints, we will create an **area** (using GUI)

**Preprocessor > Modeling > Create > Areas > Rectangle > By 2 Corners**

- Fill in the window as shown above. This will create a rectangle where the bottom left corner has the coordinates 0,0,0 and the top right corner has the coordinates 200,100,0.(Alternatively, the command line code for the above command is
`BLC4,0,0,200,100`)

- Create the circle
**Preprocessor > Modeling > Create > Areas > Circle > Solid Circle**

- Fill in the window as shown above. This will create a circle where the center has the coordinates 100,50,0 (the center of the rectangle) and the radius of the circle is 20 mm.(Alternatively, the command line code for the above command is
`CYL4,100,50,20 `)

- Subtraction
Now we want to subtract the circle from the rectangle. Prior to this operation, your image should resemble the following:

- To perform the Boolean operation, from the Preprocessor menu select:
**Modeling > Operate > Booleans > Subtract > Areas**
- At this point a 'Subtract Areas' window will pop up and the ANSYS Input window will display the following message:
`[ASBA] Pick or enter base areas from which to subtract` (as shown below)

- Therefore, select the base area (the rectangle) by clicking on it. Note: The selected area will turn pink once it is selected.
- The following window may appear because there are 2 areas at the location you clicked.

- Ensure that the entire rectangular area is selected (otherwise click 'Next') and then click 'OK'.
- Click 'OK' on the 'Subtract Areas' window.
- Now you will be prompted to select the areas to be subtracted, select the circle by clicking on it and then click 'OK'.You should now have the following model:

(Alternatively, the command line code for the above step is `ASBA,1,2`)

**Define the Type of Element**
It is now necessary to define the type of element to use for our problem:

**Preprocessor Menu > Element Type > Add/Edit/Delete**

- Add the following type of element:
**Solid** (under the Structural heading) and the **Quad 82** element, as shown in the above figure.

PLANE82 is a higher order version of the two-dimensional, four-node element (PLANE42). PLANE82 is an eight noded quadrilateral element which is better suited to model curved boundaries.

For this example, we need a plane stress element with thickness, therefore
- Click on the 'Options...' button. Click and hold the K3 button, and select 'Plane strs w/thk', as shown below.

(Alternatively, the command line code for the above step is `ET,1,PLANE82` followed by `KEYOPT,1,3,3`)

**Define Geometric Properties**

- As in previous examples
**Preprocessor menu > Real Constants > Add/Edit/Delete**
- Enter a thickness of 20 as shown in the figure below. This defines a plate thickness of 20mm)

(Alternatively, the command line code for the above step is `R,1,20`)

**Element Material Properties**
- As shown in previous examples, select
**Preprocessor > Material Props > Material models > Structural > Linear > Elastic > Isotropic**We are going to give the properties of Steel. Enter the following when prompted:

(Alternatively, the command line code for the above step is `MP,EX,1,200000` followed by `MP,PRXY,1,0.3`)

**Mesh Size**
To tell ANSYS how big the elements should be, **Preprocessor > Meshing > Size Cntrls > Manual Size > Areas > All Areas**

- Select an element edge length of 25. We will return later to determine if this was adequate for the problem.(Alternatively, the command line code for the above step is
`AESIZE,ALL,25,`)

**Mesh**
Now the frame can be meshed.

- In the 'Preprocessor' menu select
**Meshing > Mesh > Areas > Free** and select the area when prompted(Alternatively, the command line code for the above step is `AMESH,ALL`)

You should now have the following:

**Saving Your Job**

**Utility Menu > File > Save as...**

You have now defined your model. It is now time to apply the load(s) and constraint(s) and solve the the resulting system of equations.

**Define Analysis Type**

- Ensure that a Static Analysis will be performed (
**Solution > Analysis Type > New Analysis**).(Alternatively, the command line code for the above step is `ANTYPE,0`)

**Apply Constraints**
As shown previously, the left end of the plate is fixed.

- In the
**Solution > Define Loads > Apply > Structural > Displacement > On Lines**
- Select the left end of the plate and click on 'Apply' in the 'Apply U,ROT on Lines' window.
- Fill in the window as shown below.

- This location is fixed which means that all DOF's are constrained. Therefore, select 'All DOF' by clicking on it and enter '0' in the Value field as shown above.You will see some blue triangles in the graphics window indicating the displacement contraints.

(Alternatively, the command line code for the above step is `DL,4,,ALL,0`)

**Apply Loads**

- As shown in the diagram, there is a load of 20N/mm distributed on the right hand side of the plate. To apply this load:
**Solution > Define Loads > Apply > Structural > Pressure > On Lines**
- When the window appears, select the line along the right hand edge of the plate and click 'OK'
- Calculate the pressure on the plate end by dividing the distributed load by the thickness of the plate (1 MPa).
- Fill in the "Apply PRES on lines" window as shown below. NOTE:
- The pressure is uniform along the surface of the plate, therefore the last field is left blank.
- The pressure is acting away from the surface of the plate, and is therefore defined as a
**negative** pressure.

The applied loads and constraints should now appear as shown below.

**Solving the System**
**Solution > Solve > Current LS**

**Hand Calculations**
Now, since the purpose of this exercise was to verify the results - we need to calculate what we should find.

*Deflection*: The maximum deflection occurs on the right hand side of the plate and was calculated to be 0.001 mm - neglecting the effects of the hole in the plate (ie - just a flat plate). The actual deflection of the plate is therefore expected to be greater but in the same range of magnitude.

*Stress*: The maximum stress occurs at the top and bottom of the hole in the plate and was found to be 3.9 MPa.

**Convergence using ANSYS**
At this point we need to find whether or not the final result has converged. We will do this by looking at the deflection and stress at particular nodes while changing the size of the meshing element.

Since we have an analytical solution for the maximum stress point, we will check the stress at this point. First we need to find the node corresponding to the top of the hole in the plate. First plot and number the nodes

**Utility Menu > Plot > Nodes**

Utility Menu > PlotCtrls > Numbering...

- The plot should look similar to the one shown below. Make a note of the node closest to the top of the circle (ie. #49)

- List the stresses (
**General Postproc > List Results > Nodal Solution > Stress, Principals SPRIN**) and check the SEQV (Equivalent Stress / von Mises Stress) for the node in question. (as shown below in red)

The equivalent stress was found to be `2.9141 MPa` at this point. We will use smaller elements to try to get a more accurate solution.

- Resize Elements

- To change the element size, we need to go back to the Preprocessor Menu
**Preprocessor > Meshing > Size Cntrls > Manual Size > Areas > All Areas**now decrease the element edge length (ie 20)
- Now remesh the model (
**Preprocessor > Meshing > Mesh > Areas > Free**). Once you have selected the area and clicked 'OK' the following window will appear:

- Click 'OK'. This will remesh the model using the new element edge length.
- Solve the system again (note that the constraints need not be reapplied). (
** Solution Menu > Current LS **)

- Repeat steps 'a' through 'd' until the model has converged. (note - the number of the node at the top of the hole has most likely changed. It is essential that you plot the nodes again to select the appropriate node). Plot the stress/deflection at varying mesh sizes as shown below to confirm that convergence has occured.

Note the shapes of both the deflection and stress curves. As the number of elements in the mesh increases (ie - the element edge length decreases), the values converge towards a final solution.

The von Mises stress at the top of the hole in the plate was found to be approximatly 3.8 MPa. This is a mere 2.5% difference between the analytical solution and the solution found using ANSYS.

The approximate maximum displacement was found to be 0.0012 mm, this is 20% greater than the analytical solution. However, the analytical solution does not account for the large hole in the center of the plate which was expected to significantly increase the deflection at the end of the plate.

Therefore, the results using ANSYS were determined to be appropriate for the verification model.

**Deformation**

**General Postproc > Plot Results > Deformed Shape > Def + undeformd** to view both the deformed and the undeformed object.

- Observe the locations of deflection.

**Deflection**
**General Postproc > Plot Results > Nodal Solution...** Then select DOF solution, USUM in the window.

- Alternatively, obtain these results as a list. (
**General Postproc > List Results > Nodal Solution...**)
- Are these results what you expected? Note that all translational degrees of freedom were constrained to zero at the left end of the plate.

**Stresses**
**General Postproc > Plot Results > Nodal Solution...** Then select Stress, von Mises in the window.

- You can list the von Mises stresses to verify the results at certain nodes
**General Postproc > List Results**. Select **Stress, Principals SPRIN**