Effect of Self Weight on a Cantilever Beam in Ansys

Introduction

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.

---

Preprocessing: Defining the Problem

1. Give example a TitleUtility Menu > File > Change Title ...
   /title, Effects of Self Weight for a Cantilever Beam
2. Open preprocessor menuANSYS Main Menu > Preprocessor
   /PREP7
3. Define KeypointsPreprocessor > Modeling > Create > Keypoints > In Active CS...
   K,#,x,y,zWe 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 LinesPreprocessor > Modeling > Create > Lines > Lines > In Active Coord
   L,1,2Create a line joining Keypoints 1 and 2
5. Define the Type of Element
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).

6. Define Real Constants
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.

7. Define Element Material PropertiesPreprocessor > Material Props > Material Models > Structural > Linear > Elastic > IsotropicIn the window that appears, enter the following geometric properties for steel:
   
   1. Young's modulus EX: 200000
   2. Poisson's Ratio PRXY: 0.3
8. Define Element DensityPreprocessor > Material Props > Material Models > Structural > Linear > DensityIn the window that appears, enter the following density for steel:
   
   1. Density DENS: 7.86e-6
9. Define Mesh SizePreprocessor > Meshing > Size Cntrls > ManualSize > Lines > All Lines...For this example we will use an element edge length of 100mm.
10. Mesh the framePreprocessor > Meshing > Mesh > Lines > click 'Pick All'

---

Solution Phase: Assigning Loads and Solving

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

2. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On KeypointsFix keypoint 1 (ie all DOF constrained)

3. 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.
  DK,1,ALL,0,
  ACEL,,9.8
The applied loads and constraints should now appear as shown in the figure below.



4. Solve the System
Solution > Solve > Current LS
SOLVE

---

Postprocessing: Viewing the Results

1. Hand CalculationsHand 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 beamGeneral 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.