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.
Utility Menu > File > Change Title ...
- Give example a Title
/title, Effects of Self Weight for a Cantilever Beam
ANSYS Main Menu > Preprocessor
- Open preprocessor menu
Preprocessor > Modeling > Create > Keypoints > In Active CS...
- Define Keypoints
We are going to define 2 keypoints for this beam as given in the following table:
Preprocessor > Modeling > Create > Lines > Lines > In Active Coord
- Create Lines
Create a line joining Keypoints 1 and 2
Preprocessor > Element Type > Add/Edit/Delete...
- Define the Type of Element
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).
Preprocessor > Real Constants... > Add...
- Define Real Constants
In the 'Real Constants for BEAM3' window, enter the following geometric properties:
- Cross-sectional area AREA: 500
- Area moment of inertia IZZ: 4166.67
- Total beam height: 10
This defines a beam with a height of 10 mm and a width of 50 mm.
Preprocessor > Material Props > Material Models > Structural > Linear > Elastic > Isotropic
- Define Element Material Properties
In the window that appears, enter the following geometric properties for steel:
- Young's modulus EX: 200000
- Poisson's Ratio PRXY: 0.3
Preprocessor > Material Props > Material Models > Structural > Linear > Density
- Define Element Density
In the window that appears, enter the following density for steel:
- Density DENS: 7.86e-6
Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All Lines...
- Define Mesh Size
For this example we will use an element edge length of 100mm.
Preprocessor > Meshing > Mesh > Lines > click 'Pick All'
- Mesh the frame
Solution > Analysis Type > New Analysis > Static
- Define Analysis Type
Solution > Define Loads > Apply > Structural > Displacement > On Keypoints
- Apply Constraints
Fix keypoint 1 (ie all DOF constrained)
- Define Gravity
It is necessary to define the direction and magnitude of gravity for this problem.
- Select Solution > Define Loads > Apply > Structural > Inertia > Gravity...
- The following window will appear. Fill it in as shown to define an acceleration of 9.81m/s2 in the y direction.
Note: Acceleration is defined in terms of meters (not 'mm' as used throughout the problem).
This is because the units of acceleration and mass must be consistent to give the product of force units (Newtons in this case).
Also note that a positive acceleration in the y direction stimulates gravity in the negative Y direction.
There should now be a red arrow pointing in the positive y direction.
This indicates that an acceleration has been defined in the y direction.
The applied loads and constraints should now appear as shown in the figure below.
Solve the System
Solution > Solve > Current LS
- Hand Calculations
Hand calculations were performed to verify the solution found using ANSYS:
The maximum deflection was shown to be 5.777mm
General Postproc > Plot Results > Deformed Shape ... > Def + undef edge
- Show the deformation of the beam
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