// // Leave a Comment

Bracket Example in Ansys


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.

Preprocessing: Defining the Problem

  1. Give the Bracket example a TitleUtility Menu > File > Change Title
  2. Form GeometryAgain, Boolean operations will be used to create the basic geometry of the Bracket.

    1. Create the main rectangular shapeThe 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 sideThe 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:
      parametercircle 2circle 3
      XCENTER00
      YCENTER2080
      RADIUS2020
    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 - AdditionWe 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:
      parametercircle 1circle 2circle 3
      WP X8000
      WP Y502080
      radius301010

      • Now selectPreprocessor > 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

    • Preprocessor > Element Type > Add/Edit/Delete
    • Use the 'Options...' button to get a plane stress element with thickness(Alternatively, the command line code for the above step is ET,1,PLANE82 followed by KEYOPT,1,3,3)
    • Under the Extra Element Output K5 select nodal stress.

  5. Define Geometric Contants


    • Preprocessor > Real Constants > Add/Edit/Delete
    • Enter a thickness of 20mm.(Alternatively, the command line code for the above step is R,1,20)

  6. Element Material Properties

    • Preprocessor > Material Props > Material Library > Structural > Linear > Elastic > IsotropicWe are going to give the properties of Steel. Enter the following when prompted:
       EX 200000
      PRXY 0.3

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

  7. Mesh Size

    • Preprocessor > Meshing > Size Cntrls > Manual Size > Areas > All Areas
    • Select an element edge length of 5. Again, we will need to make sure the model has converged.(Alternatively, the command line code for the above step is AESIZE,ALL,5,)

  8. Mesh

    • Preprocessor > Meshing > Mesh > Areas > Free and select the area when prompted(Alternatively, the command line code for the above step is AMESH,ALL)

    Saving Your Job
    Utility Menu > File > Save as...

Solution Phase: Assigning Loads and Solving

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

    • 'Solution' > 'New Analysis' and select 'Static'.(Alternatively, the command line code for the above step is ANTYPE,0)

  2. Apply Constraints
  3. As illustrated, the plate is fixed at both of the smaller holes on the left hand side.
    • Solution > Define Loads > Apply > Structural > Displacement > On Nodes
    • Instead of selecting one node at a time, you have the option of creating a box, polygon, or circle of which all the nodes in that area will be selected. For this case, select 'circle' as shown in the window below. (You may want to zoom in to select the points Utilty Menu / PlotCtrls / Pan, Zoom, Rotate...) Click at the center of the bolt hole and drag the circle out so that it touches all of the nodes on the border of the hole.
    • Click on 'Apply' in the 'Apply U,ROT on Lines' window and constrain all DOF's in the 'Apply U,ROT on Nodes' window.
    • Repeat for the second bolt hole.

  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

Post-Processing: Viewing the Results

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
    • As shown previously, it is necessary to prove that the solution has converged. Reduce the mesh size until there is no longer a sizeable change in your convergence criteria.

  2. Deformation

    • General Postproc > Plot Results > Def + undeformed to view both the deformed and the undeformed object.The graphic should be similar to the following

    • Observe the locations of deflection. Ensure that the deflection at the bolt hole is indeed 0.

  3. Deflection

    • To plot the nodal deflections use General Postproc > Plot Results > Contour Plot > Nodal Solution then select DOF Solution - USUM in the window.Contour Nodal Solution Data
    • 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 bolt holes.

  4. Stresses
    • General Postproc > Plot Results > Nodal Solution... Then select von Mises Stress in the window.Stresses
    • You can list the von Mises stresses to verify the results at certain nodesGeneral Postproc > List Results. Select Stress, Principals SPRIN

0 comments:

Post a Comment