MENG 421 Assignment 9
Ansys in graphical mode: Stressed plate with hole
MENG 421 |
Class assignments |
Lecture notes --
this lesson, you use Ansys in graphics mode to
model a square plate with a hole.
You will use the 8-node Plane82 element that is similar
to the 4-node Plane42 element that you used for
You can use Plane82 in axisymmetric mode to create rods and pipes like you
did with Plane42 for Assignment 4.
Because there are eight nodes, the element sides are parabolas rather
than straight lines.
For previous labs, you ran Ansys with a batch file, only occasionally typing in commands.
By contrast, for today's assignment, you work entirely with the keyboard and mouse
rather than using a batch file.
You will define the Element Type, Real Constants, and Material Properties
as you have done previously in batch mode. But you will select these items from menus.
In the next lesson,
Assignment 10, you will
apply a load to this model and determine the deformation
and stresses. Because of symmetry, we will only model one quarter
of the plate. This will save computer time and show more detail.
Be careful however to properly support the lower and left edges of our quarter mode.
That is, we take the plate shown in left figure and cut out the upper-right
quarter for our model shown in the right figure. Then we will load the
quarter model on the right edge and constrain the model on the left and
lower edges where the model meet the remainder of the original plate.
The lower edge can move right but not down.
Similarly, the left edge can move up but not to the left.
You must be careful to chose one-dimensional (roller) supports not only
at the ends but also at
If the supports are incorrect, the edges
will not be straight.
First, you will let Ansys automatically create the mesh. Then you
will refine that mesh around the hole.
Finally, you will print a graphic of the meshed plate.
You will create the first figure
below in today's lesson and the others in the next lesson.
Click the figures to enlarge them.
If you find the lower part of a window off the screen, hold the Alt key
while pressing the Space Bar. Release both keys and press the M key.
Now you can move the window by pressing the cursor arrows.
For example, press the up arrow to raise the window.
Press Enter when the window is in the new position or
press the Esc key to cancel this action.
- Before starting Ansys be sure that your directory has at least
1.5 MB of free space. Otherwise, you will not be able to save your
work for next week.
- You learned how to change the screen resolution in
Check that the screen resolution is
1024x768x16 (High Color).
- Point a copy of Explorer to C:\WINDOWS\Temp and clear all files.
Today you will make frequent copies of the Ansys file named file.log
because this is where Ansys keeps a copy of all the keyboard commands you type.
Then you can easily rerun your work from the resulting batch file.
- Start Ansys
- Utility Menu: File | Change Jobname | Plate82 | OK
- Utility Menu: File | Change Title | (Put the usual here --
Plate 82 with hole, your name, and the date) | OK
Your file.log now
looks like this
- Notice that the Ansys Main Menu has the familiar items Preprocessor,
Solution, and General Postsproc. We will use these items to
define the element type, reals, material properties, nodes, elements,
etc, as we have done previously in batch mode.
- Main Menu: Preferences | Structural | OK
- Main Menu: Preprocessor | Element Type | Add/Edit/Delete
- Element Types: Add
- Structural Solid -- Quad 8Node 82
(notice that there is a 4Node 42) | OK
- Element Types: (Check that Element Type 1 is defined as Plane 82)
- Element behavior K3 -- click dropdown and select
Plane strs w/thk | OK
- Element Types: Close
- Preprocessor: Real Constants | Add/Edit/Delete | Add
- Check for Type 1 Plane 82 | OK
- Set Thickness THK to 0.25 | Apply
- To learn more about Element 82 click Help. You can see the
curving sides of the elements. File | Exit
- Real Constant Set: OK
- Real Constants: Close
- Preprocessor: Material Props |Material Models
to get the Define
Material Model Behavior
On left side check for Material Model Number 1.
- On right side, double-click structural to
expand it like this.
- Double-click Linear to expand it.
- Double-click Elastic to expand it.
- Double-click Isotropic to get
the dialog box.
- For EX (elastic modulus) enter the value 29e6.
- For PRXY (Poisson's ratio) enter the value 0.3.
- Click OK
- Close Define Material ... by clicking Material, Exit.
- Close Material Properties window.
- First, save a batch file of your commands so far
- Go to your Explorer that shows C:\WINDOWS\Temp and find the file named file.log
- Right-click it and drag to a blank area, relase the button and pick Copy
- Rename the copy Plate31.a to indicate the it reproduces
the lesson to line number 31.
- Ansys Toolbar: SAVE_DB to save a binaray copy your work so far.
There is now a 1-MB file named Plate82.db at C:\WINDOWS\Temp (or where ever set
you Ansys workspace). You can quit now and continue later
with this file.
- Now that you have defined the element type, real, and
material properties, you can define the nodes and elements.
- Preprocessor: Modeling -- Create
- -Areas- Rectangle
- By Dimensions
- Note: for Create Rectangle, put only one number in each of
the four boxes, pairs of XY are vertical
- Put 0 for X1 in first box and press Tab or click right box.
- Put 6 for X2 in next box to right.
- Put 0 and 6 in the other boxes to define (0,0) and (6,6)
A rectangle appears in the graphics window.
- Close the Rectangle and Create menus.
- Utility Menu: PlotCtrls | Pan, Zoom, Rotate |
(click small dot to zoom out)
- Utility Menu: PlotCtrls | Numbering |
Area numbers ON (click white box next to Off) | OK
- Utility Menu: Plot | Lines (Figure shows lines)
- Preprocessor: -Modeling- Create
- Now we have to subtract the circle from the square --
- Preprocessor: -Modeling- Operate
- Booleans -- Subtract
- In the Subtract Areas menu, check that the count changes
from 0 to 1 and that the Area No. becomes 1, while you pick the square.
Be careful not to pick near the circle.)
- Now pick the circle and check that the Count is 1 and the Area No. becomes 2
circle is subtracted from the square like this.
- Close the Subtract and Operate menus.
- Make another copy of file.log and name it Plate40.a
- Ansys Toolbar: SAVE_DB to save your work in binary
- Preprocessor: MeshTool
- MeshTool: Size controls: Global Set
- Global Element Sizes: SIZE 1.5 | OK
- MeshTool: (4th section down) Mesh: Areas | Mesh
- Mesh Area menu: Pick All
meshed plate should look like this.
As you know, the stresses are greatest around the hole, so there
should be smaller elements there. But, as you can see, the elements
are all about the same size. Therefore,
let us refine the mesh.
- MeshTool: Refine -- at Nodes | Refine
- Watch Refine mesh menu while you pick the three nodes around the hole |
check for Count = 3 | OK |
- Refine Mesh at Node: Choose refinement level 2 | OK
Your meshed plate should look
like the second one.
Notice how the elements are now smaller around the hole.
- MeshTool: Close
- Make the background black by typing the Ansys command
Then click the Plot menu and pick Replot.
- Make copy of file.log that has all your typed commands,
name it Plate52.a, and print it.
- Save your work in binary for next time. It will take about 900 KB of space.
Utility Menu: File | Save as | Plate82.db |
Be sure to save your file on the Ansys directory of Drive U. Otherwise, your
work is saved on the local PC you are currently working on
- Capture and print your meshed plate.
- Capture the figure and edit as usual
- Reverse colors with Effects, Negative
- Change to Gray Scale
- Click the Image menu and pick Balance. If necessary, adjust the
brightness to the right to show more detail.
- You went through a lot of material today.
Therefore, you might want to clear Ansys and redo the above lesson.
Utility Menu: File | Clear & Start New
- When you are finished, Toolbar: Quit | Quit - no save | OK
Create a cover sheet describing what you did and discuss stress concentration.
Include a graphic of your meshed plate and your list of commands from the log file.
Compare this lab with the previous ones where you used a batch file
and typed lines of keyboard input.
Do not combine with Lesson 10.
Turn in the package as specified at the lab.
MENG 421 |
Class assignments |
Revised: March 31, 2004
-- Copyright © 1997-2004