This tutorial was created using ANSYS 7.0
The purpose of this tutorial is to create and use 'paths' to provide extra detail during post processing.
For example, one may want to determine the effects of stress concentrators along a certain path.
Rather than plotting the entire contour plot, a plot of the stress along that path can be made.
In this tutorial, a steel plate measuring 100 mm X 200 mm X 10 mm will be used. Three holes are
drilled through the vertical centerline of the plate. The plate is constrained in the y-direction
at the bottom and a uniform, distributed load is pulling on the top of the plate.
- Give the example a Title
- Utility Menu > File > Change Title ...
/title, Use of Paths for Post Processing
Open preprocessor menu
- ANSYS Main Menu > Preprocessor
Define Rectangular Ares
- Preprocessor > Modeling > Create > Areas > Rectangle > By 2 Corners
- Create a rectangle where the bottom left corner has the coordinates 0,0 and the width and
height are 200 and 100 respectively.
- Preprocessor > Modeling > Create > Areas > Circle > Solid Circle
cyl4,WP X,WP Y,Radius
- Create three circles with parameters shown below.
|WP X||WP Y||Radius|
|1|| 50 || 50 || 10 |
|2|| 100 || 50 || 10 |
|3|| 150 || 50 || 10 |
Subtract the Circles
- Preprocessor > Modeling > Operate > Booleans > Subtract > Areas
- First, select the area to remain (ie. the rectangle) and click OK. Then, select the areas to be subtracted (ie. the circles) and click OK.
- The remaining area should look as shown below.
Define the Type of Element
- Preprocessor > Element Type > Add/Edit/Delete...
- For this problem we will use the PLANE2 (Solid Triangle 6node) element.
This element has 2 degrees of freedom (translation along the X and Y axes).
- In the 'Element Types' window, click 'Options...' and set 'Element behavior'
to Plane strs w/thk
Define Real Constants
- Preprocessor > Real Constants... > Add...
- In the 'Real Constants for PLANE2' window, enter a thickness of 10.
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:
- Young's modulus EX: 200000
- Poisson's Ratio PRXY: 0.3
Define Mesh Size
- Preprocessor > Meshing > Size Cntrls > ManualSize > Areas > All Areas...
- For this example we will use an element edge length of 5mm.
Mesh the Area
- Preprocessor > Meshing > Mesh > Areas > Free > click 'Pick All'
- Define Analysis Type
- Solution > Analysis Type > New Analysis > Static
- Solution > Define Loads > Apply > Structural > Displacement > On Lines
- Constrain the bottom of the area in the UY direction.
- Solution > Define Loads > Apply > Structural > Pressure > On Lines
- Apply a constant, uniform pressure of -200 on the top of the area.
The model should now look like the figure below.
Solve the System
- Solution > Solve > Current LS
To see the stress distribution on the plate, you could create a normal contour plot, which would
have the distribution over the entire plate. However, if the stress near the holes are of interest,
you could create a path through the center of the plate and plot the stress on that path. Both cases
will be plotted below on a split screen.
- Contour Plot
- Utility Menu > PlotCtrls > Window Controls > Window Layout
- Fill in the 'Window Layout' as seen below
- General Postproc > Plot Results > Contour Plot > Nodal Solu > Stress > von Mises
The display should now look like this.
To ensure the top plot is not erased when the second plot is created, you must make a couple of changes.
- Utility Menu > PlotCtrls > Window Controls > Window On or Off. Turn window 1 'off'.
- To keep window 1 visible during replots, select Utility Menu > PlotCtrls > Erase Option > Erase Between Plots
and ensure there is no check-mark, meaning this function off.
- To have the next graph plot in the bottom half of the screen, select Utility Menu > PlotCtrls > Window Controls > Window Layout
and select 'Window 2 > Bottom Half > Do not replot'.
Map the Stress onto the Path
Now the path is defined, you must choose what to map to the path, or in other words, what results
should be available to the path. For this example, equivalent stress is desired.
- General Postproc > Path Operations > Map onto Path
- Fill the next window in as shown below [Stress > von Mises] and click OK.
- The warning shown below will probably pop up. This is just saying that some of the 1000 points
you defined earlier are not on interpolation points (special points on the elements) therefore there is no data
to map. This is of little concern though, since there are plenty of points that do lie on interpolation
points to produce the necessary plot, so disregard the warning.
Plot the Path Data
- General Postproc > Path Operations > Plot Path Item > On Geometry
- Fill the window in as shown below
The display should look like the following. Note, there will be dots on the plot showing node locations.
Due to resolution restrictions, these dots are not shown here.
This plot makes it easy to see how the stress is concentrated around the holes.
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