This tutorial was completed using ANSYS 7.0 The purpose of the tutorial is to show the required steps to account for the weight of an object in ANSYS.

Loads will not be applied to the beam shown below in order to observe the deflection caused by the weight of the beam itself. The beam is to be made of steel with a modulus of elasticity of 200 GPa.


  1. Give example a Title Utility Menu > File > Change Title ...
    /title, Effects of Self Weight for a Cantilever Beam

  2. Open preprocessor menu ANSYS Main Menu > Preprocessor
    /PREP7

  3. Define Keypoints Preprocessor > Modeling > Create > Keypoints > In Active CS...
    K,#,x,y,z

    We are going to define 2 keypoints for this beam as given in the following table:

    Keypoint Coordinates (x,y,z)
    1 (0,0)
    2 (1000,0)

  4. Create Lines Preprocessor > Modeling > Create > Lines > Lines > In Active Coord
    L,1,2

    Create a line joining Keypoints 1 and 2

  5. Define the Type of Element
  6. Preprocessor > Element Type > Add/Edit/Delete...

    For this problem we will use the BEAM3 (Beam 2D elastic) element. This element has 3 degrees of freedom (translation along the X and Y axes, and rotation about the Z axis).

  7. Define Real Constants
  8. Preprocessor > Real Constants... > Add...

    In the 'Real Constants for BEAM3' window, enter the following geometric properties:

    1. Cross-sectional area AREA: 500
    2. Area moment of inertia IZZ: 4166.67
    3. Total beam height: 10

    This defines a beam with a height of 10 mm and a width of 50 mm.

  9. Define Element Material Properties Preprocessor > Material Props > Material Models > Structural > Linear > Elastic > Isotropic

    In the window that appears, enter the following geometric properties for steel:

    1. Young's modulus EX: 200000
    2. Poisson's Ratio PRXY: 0.3

  10. Define Element Density Preprocessor > Material Props > Material Models > Structural > Linear > Density

    In the window that appears, enter the following density for steel:

    1. Density DENS: 7.86e-6

  11. Define Mesh Size Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All Lines...

    For this example we will use an element edge length of 100mm.

  12. Mesh the frame Preprocessor > Meshing > Mesh > Lines > click 'Pick All'

  1. Define Analysis Type
  2. Solution > Analysis Type > New Analysis > Static
    ANTYPE,0

  3. Apply Constraints
  4. Solution > Define Loads > Apply > Structural > Displacement > On Keypoints

    Fix keypoint 1 (ie all DOF constrained)

  5. Define Gravity
  6. It is necessary to define the direction and magnitude of gravity for this problem.

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

  7. Solve the System
  8. Solution > Solve > Current LS
    SOLVE

  1. Hand Calculations

    Hand calculations were performed to verify the solution found using ANSYS:

    The maximum deflection was shown to be 5.777mm

  2. Show the deformation of the beam General Postproc > Plot Results > Deformed Shape ... > Def + undef edge
    PLDISP,2

    As observed in the upper left hand corner, the maximum displacement was found to be 5.777mm. This is in agreement with the theortical value.


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.