| Verification Example | | Preprocessing | | Solution | | Postprocessing | | Command Line |
| Bracket Example | | Preprocessing | | Solution | | Postprocessing | | Command Line |

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.

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.

[Bracket Geometry]

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:

simple plate

  1. Give the Simplified Version a Title Utility Menu > File > Change Title

  2. 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.

    1. 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

        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)

    2. Create the circle
        Preprocessor > Modeling > Create > Areas > Circle > Solid Circle

        Solid Circular Area Creation Window

      • 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 )

    3. 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)

        ANSYS Input Window

      • 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)

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

  5. Define Geometric Properties
  6. Element Material Properties
  7. Mesh Size
  8. To tell ANSYS how big the elements should be, Preprocessor > Meshing > Size Cntrls > Manual Size > Areas > All Areas

  9. Mesh
  10. Now the frame can be meshed.

    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.

  1. Define Analysis Type
  2. Apply Constraints
  3. As shown previously, the left end of the plate is fixed.

  4. Apply Loads
  5. Solving the System
  6. Solution > Solve > Current LS

  1. Hand Calculations
  2. 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.

  3. Convergence using ANSYS
  4. 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.

    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.

  5. Deformation
  6. Deflection
  7. Stresses

The above example was solved using a mixture of the Graphical User Interface (or GUI) and the command language interface of ANSYS. This problem has also been solved using the ANSYS command language interface that you may want to browse. Open the .HTML version, copy and paste the code into Notepad or a similar text editor and save it to your computer. Now go to 'File > Read input from...' and select the file. A .PDF version is also available for printing.

Now we will return to the analysis of the bracket. A combination of GUI and the Command line will be used for this example.

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.

[Bracket Geometry]

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.


  1. Give the Bracket example a Title Utility Menu > File > Change Title

  2. Form Geometry

    Again, Boolean operations will be used to create the basic geometry of the Bracket.

    1. Create the main rectangular shape

      The main rectangular shape has a width of 80 mm, a height of 100mm and the bottom left corner is located at coordinates (0,0)

      • Ensure that the Preprocessor menu is open. (Alternatively type /PREP7 into the command line window)

      • Now instead of using the GUI window we are going to enter code into the 'command line'. Now I will explain the line required to create a rectangle:
        	BLC4, XCORNER, YCORNER, WIDTH, HEIGHT
        	BLC4, X coord (bottom left), Y coord (bottom left), width, height
        

      • Therefore, the command line for this rectangle is BLC4,0,0,80,100

    2. Create the circular end on the right hand side

      The center of the circle is located at (80,50) and has a radius of 50 mm

        The following code is used to create a circular area:

        	CYL4, XCENTER, YCENTER, RAD1
        	CYL4, X coord for the center, Y coord for the center, radius
        

      • Therefore, the command line for this circle is CYL4,80,50,50

    3. Now create a second and third circle for the left hand side using the following dimensions:

      parameter circle 2 circle 3
      XCENTER 0 0
      YCENTER 20 80
      RADIUS 20 20

    4. Create a rectangle on the left hand end to fill the gap between the two small circles.

      XCORNER-20
      YCORNER20
      WIDTH20
      HEIGHT60

      Your screen should now look like the following...

    5. Boolean Operations - Addition

      We now want to add these five discrete areas together to form one area.

      • To perform the Boolean operation, from the Preprocessor menu select: Modeling > Operate > Booleans > Add > Areas

      • In the 'Add Areas' window, click on 'Pick All'

        (Alternatively, the command line code for the above step is AADD,ALL)

      You should now have the following model:

    6. Create the Bolt Holes We now want to remove the bolt holes from this plate.

      • Create the three circles with the parameters given below:

      parameter circle 1 circle 2 circle 3
      WP X 80 0 0
      WP Y 50 20 80
      radius 30 10 10

      • Now select Preprocessor > Modeling > Operate > Booleans > Subtract > Areas

      • Select the base areas from which to subract (the large plate that was created)

      • Next select the three circles that we just created. Click on the three circles that you just created and click 'OK'.

        (Alternatively, the command line code for the above step is ASBA,6,ALL)

        Now you should have the following:

  3. Define the Type of Element
  4. As in the verification model, PLANE82 will be used for this example

  5. Define Geometric Contants
  6. Element Material Properties
  7. Mesh Size
  8. Mesh
  9. 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.

  1. Define Analysis Type
  2. Apply Constraints
  3. As illustrated, the plate is fixed at both of the smaller holes on the left hand side.

  4. Apply Loads
  5. As shown in the diagram, there is a single vertical load of 1000N, at the bottom of the large bolt hole. Apply this force to the respective keypoint ( Solution > Define Loads > Apply > Structural > Force/Moment > On Keypoints Select a force in the y direction of -1000)

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

  6. Solving the System
  7. Solution > Solve > Current LS


We are now ready to view the results. We will take a look at the deflected shape and the stress contours once we determine convergence has occured.

  1. Convergence using ANSYS
  2. Deformation
  3. Deflection
  4. Stresses

The above example was solved using a mixture of the Graphical User Interface (or GUI) and the command language interface of ANSYS. This problem has also been solved using the ANSYS command language interface that you may want to browse. Open the .HTML version, copy and paste the code into Notepad or a similar text editor and save it to your computer. Now go to 'File > Read input from...' and select the file. A .PDF version is also available for printing.

To quit ANSYS, click 'QUIT' on the ANSYS Toolbar or select Utility Menu > File > Exit... In the window that appears, select 'Save Everything' (assuming that you want to) and then click 'OK'.