This tutorial was completed using ANSYS 7.0.
The purpose of this tutorial is to explain how to apply distributed loads and use element tables to extract data.
Please note that this material was also covered in the 'Bicycle Space Frame' tutorial under 'Basic Tutorials'.
A distributed load of 1000 N/m (1 N/mm) will be applied to a solid steel beam with a rectangular cross section as shown in the figure below.
The cross-section of the beam is 10mm x 10mm while the modulus of elasticity of the steel is 200GPa.
- Open preprocessor menu
Utility Menu > File > Change Title ...
- Give example a Title
/title, Distributed Loading
Preprocessor > Modeling > Create > Keypoints > In Active CS
- Create Keypoints
We are going to define 2 keypoints (the beam vertices) for this structure as given in the following table:
Preprocessor > Modeling > Create > Lines > Lines > Straight Line
- Define Lines
Create a line between Keypoint 1 and Keypoint 2.
Preprocessor > Element Type > Add/Edit/Delete...
- Define Element Types
For this problem we will use the BEAM3 element.
This element has 3 degrees of freedom (translation along the X and Y axis's, and rotation about the Z axis).
With only 3 degrees of freedom, the BEAM3 element can only be used in 2D analysis.
Preprocessor > Real Constants... > Add...
- Define Real Constants
In the 'Real Constants for BEAM3' window, enter the following geometric properties:
- Cross-sectional area AREA: 100
- Area Moment of Inertia IZZ: 833.333
- Total beam height HEIGHT: 10
This defines an element with a solid rectangular cross section 10mm x 10mm.
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 > Meshing > Size Cntrls > ManualSize > Lines > All Lines...
- Define Mesh Size
For this example we will use an element length of 100mm.
Preprocessor > Meshing > Mesh > Lines > click 'Pick All'
- Mesh the frame
Utility Menu > Plot > Elements
- Plot Elements
You may also wish to turn on element numbering and turn off keypoint numbering
Utility Menu > PlotCtrls > Numbering ...
Solution > Analysis Type > New Analysis > Static
- Define Analysis Type
Solution > Define Loads > Apply > Structural > Displacement > On Keypoints
- Apply Constraints
Pin Keypoint 1 (ie UX and UY constrained) and fix Keypoint 2 in the y direction (UY constrained).
- Apply Loads
We will apply a distributed load, of 1000 N/m or 1 N/mm, over the entire length of the beam.
- Select Solution > Define Loads > Apply > Structural > Pressure > On Beams
- Click 'Pick All' in the 'Apply F/M' window.
- As shown in the following figure, enter a value of 1 in the field 'VALI Pressure value at node I' then click 'OK'.
The applied loads and constraints should now appear as shown in the figure below.
To have the constraints and loads appear each time you select 'Replot' you must change some settings.
Select Utility Menu > PlotCtrls > Symbols....
In the window that appears, select 'Pressures' in the pull down menu of the 'Surface Load Symbols' section.
Solve the System
Solution > Solve > Current LS
General Postproc > Plot Results > Deformed Shape
- Plot Deformed Shape
- Plot Principle stress distribution
As shown previously, we need to use element tables to obtain principle stresses for line elements.
- Select General Postproc > Element Table > Define Table
- Click 'Add...'
- In the window that appears
- enter 'SMAXI' in the 'User Label for Item' section
- In the first window in the 'Results Data Item' section scroll down and select 'By sequence num'
- In the second window of the same section, select 'NMISC, '
- In the third window enter '1' anywhere after the comma
- click 'Apply'
- Repeat steps 2 to 4 but change 'SMAXI' to 'SMAXJ' in step 3a and change '1' to '3' in step 3d.
- Click 'OK'. The 'Element Table Data' window should now have two variables in it.
- Click 'Close' in the 'Element Table Data' window.
- Select: General Postproc > Plot Results > Line Elem Res...
- Select 'SMAXI' from the 'LabI' pull down menu and 'SMAXJ' from the 'LabJ' pull down menu
- ANSYS can only calculate the stress at a single location on the element.
For this example, we decided to extract the stresses from the I and J nodes of each element.
These are the nodes that are at the ends of each element.
- For this problem, we wanted the principal stresses for the elements.
For the BEAM3 element this is categorized as NMISC, 1 for the 'I' nodes and NMISC, 3 for the 'J' nodes.
A list of available codes for each element can be found in the ANSYS help files.
(ie. type help BEAM3 in the ANSYS Input window).
As shown in the plot below, the maximum stress occurs in the middle of the beam with a value of 750 MPa.
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