Introduction:
In this example
you will learn to model a 2D block subjected to varying boundary
conditions. Using ANSYS will allow you to output the temperature
distribution in an extremely simple and accurate way. By using
any combination of these boundary conditions one can model almost
any 2D heat transfer situation.
Problem Description:
·
We assume that our block is a rectangle made entirely of steel.
·
All units are S.I.
·
Boundary
Conditions:
1)
The top is insulated.
2) The right side has a constant temperature of
100K.
3) The left side has constant heat flux into
the block of 50 W/m^2.
4) The bottom side is exposed to a convective
boundary layer.
5)
Heat is uniformly generated in the bock at a rate of 20
W/m^2.
·
Material
Properties: (Steel)
h = 50
W/(m^2*K)
k =
20 W/m K
·
Objective:
To determine the nodal temperature distribution and create contour
plot.
·
Figure:
Basic Outline of the Problem:
Preprocessing:
1. Start ANSYS.
2. Create
areas.
3. Define the
material properties.
4. Define
element type. (Quad 8node 77 element, which is a 2-D element for
heat transfer analysis.)
5. Specify
meshing controls / Mesh the areas to create nodes and elements.
Solution:
6. Specify
boundary conditions.
7. Solve.
Postprocessing:
8. Plot the
temperature distribution.
Exit:
9. Exit the
ANSYS program, saving all data.
Starting ANSYS:
·
Click on
ANSYS 6.1
in the programs menu.
·
Select
Interactive.
·
The following menu comes up. Enter the working directory. All your
files will be stored in this directory. Also under
Use Default Memory Model
make sure the values
64
for Total Workspace, and
32
for Database are entered. To change these values unclick
Use Default Memory Model.
·
Click
RUN
Modeling the Structure:
·
Go to the ANSYS Utility Menu (the top bar)
·
Click
Workplane>WP Settings…
·
The following widow comes up:
·
Check the Cartesian and
Grid Only buttons
·
Enter the values shown in the figure above and then click OK.
·
Go to the ANSYS Main Menu (on the left hand side of the screen)
and click
Preprocessor>Modeling>Create>Areas>Rectangle>2 Corners.
·
The following window comes up:
·
Enter the values as shown and click OK.
·
Now you have created the rectangle. If at any time you cannot see
the complete Workplace then go to
Utility Menu>Plot Controls>Pan Zoom Rotate and zoom out
to see the entire Workplace. If you want to see the grid itself,
go to
Utility Menu>Workplane>Display Working
Plane
·
The model should look like this now: (note, you have a black
background)
Material Properties:
·
Now that we have built the model, material properties need to be
defined such that ANSYS understands how heat travels through this
steel solid.
·
Go to the ANSYS Main Menu
·
Click
Preprocessor>Material Props>Material Models.
·
The pop-up window will now look like this:
·
In the window that comes up choose
Thermal>Conductivity>Isotropic.
(Double click Isotropic). The following window comes up:
·
Fill in 20 for Thermal conductivity. Click
OK.
·
Now exit the “Define Material Model Behavior” Window
Element Properties:
·
Now that we’ve defined what material ANSYS will be
analyzing, we have to define how ANSYS should analyze our
block.
·
Click
Preprocessor>Element Type>Add/Edit/Delete...
In the 'Element Types' window that opens click on
Add... The following window opens:
·
Type 1 in the Element Type reference number.
·
Click on Thermal Mass Solid and select Quad 8node 77.
Click
OK.
Close the 'Element types' window.
·
Now we have selected Element Type 1 to be a Thermal
Solid 8node Element. This finishes the section defining how
the part is to be analyzed.
Meshing:
·
This section is responsible for telling ANSYS how to divide the
block such that it has enough nodes, or points, to analyze to make
an accurate enough analysis.
·
Go to
Preprocessor>Meshing>Size Controls>Manual Size>Lines>All Lines.
In the menu that comes up type 0.1 in the field
for ”Element edge length”.
·
Click on
OK.
Now when you mesh the figure ANSYS will automatically create
square meshes that have an edge length of 0. 1m along the
lines you selected.
·
Now go to
Preprocessor>Meshing>Mesh Attributes>Default Attributes.
The window is shown below:
·
This window appears such that the program knows you are sure that
you have selected the right material to mesh (selected by the
Element Type Number), and the right Material Number (1,
as defined in the Material Properties section). Once this
has been verified, Click OK and proceed to
Preprocessor>Meshing>Mesh>Areas>Free
·
A
popup window will appear on the left hand side of the screen.
This window allows you to select the area to be meshed.
·
Click anywhere within the blue rectangle you created to select the
area and then click
OK
in the pop-up window.
·
The block should now look like this:
Boundary Conditions and Constraints:
·
Now that we have modeled the block and defined how ANSYS is to
analyze the block we will apply the appropriate Boundary
Conditions. ANSYS refers to all Thermal Boundary Conditions as
Loads, so be aware that Load and Boundary Condition mean the same
thing within the software…
·
Go to
Preprocessor>Loads>Define Loads>Apply>Thermal
(from here one can apply any of the loads, or Boundary Conditions,
offered by ANSYS.)
Apply Convection (Base)
·
First we’ll apply the Convection Boundary layer at the base
of the plate. For this click
Convection>On Lines within the Thermal Load category.
·
A
popup window will appear on the left hand side of the screen.
This window allows you to select the line you wish the load to be
applied.
·
Select the base of the plate and click
OK. The following window
will appear:
·
Fill in the h value in the Film Coefficient blank
and the Air temperature in the Bulk Temperature blank.
Click OK when finished.
Apply Constant Temperature (Right side)
·
Now we’ll apply the given temperature boundary condition on the
right side of the block.
·
This time, within the Thermal Load category select
Temperature>On Lines.
·
A
popup window will appear on the left hand side of the screen.
This window allows you to select the line you wish the load to be
applied.
·
Click the right side of the block and then
OK.
·
Enter 100 in the popup window as the set temperature for
the right side:
Apply Heat Flux (Left Side)
·
Now to apply the Heat Flux into the left side of the plate...
·
Within the Thermal Load category again, select
Heat Flux>On Lines and click
OK. Then enter 50
into the blank and Click OK.
Insulated Surface (Top)
Since the top
of the block is insulated we don’t need to define a specific
boundary condition for the top, so we add uniform heat generation
to the block as a whole and we’re done.
Apply Heat Generation
·
The next step is to add the constraint of heat generation.
·
Preprocessor>Loads>Define Loads>Apply>Thermal>Heat
Generat>On Areas.
(Heat Generat is just short for Heat
Generation). You select Areas this time because you have to apply
this condition uniformly across the block.
·
Click anywhere within the area to select it and then click
OK.
·
Enter 20 as the heat generation value in the pop-up window
that appears:
·
Now we have applied all the necessary boundary conditions so we
move on to the Solution.
Solution:
·
Go to ANSYS
Main Menu>Solution>Analysis Type>New Analysis.
·
Select
Steady
State
and click on
OK.
·
Go to
Solution>Solve>Current LS.
·
An error window may appear. Click
OK
on that window and ignore it.
·
Wait for ANSYS to solve the problem.
·
Click on
OK
and close the 'Information' window.
Post-Processing:
·
This section is designed so that one can list the results of their
analysis as a nodal solution
·
Go to the ANSYS Main Menu. Click
General Postprocessing>List Results>Nodal Solution.
The following window will come up:
·
Select
DOF solution
and
Temperature.
Click on
OK.
The nodal temperatures will be listed as follows:
·
Within this window one can numerically find the maximum and
minimum value of the temperature within the block.
Modification / Plotting the Results:
The last
section displayed the numerical results, but most analyses will
require a plot of the temperatures on the block in addition to the
numerical results. This is how you go about doing that…
First
go to
General Postprocessing>Plot
Results>Contour Plot>Nodal Solution.
The following window will come up:
·
Select
DOF
solution
and
Temperature
to be plotted and click
OK.
The output will be like this:
·
This is the Final Solution
Important Notes:
Changing
Boundary Conditions and Constraints
·
There are no easy ways to explain ways for actually changing
existing constraints. The easiest was to accomplish a “change” is
the following: To change any of the boundary conditions simply go
to Preprocessor>Loads>Define
Loads>Delete>Thermal then select the appropriate
condition (Temperature, Heat Flux,
Heat Generation, etc…
)
·
The window that pops up will allow you to select the appropriate
Line, Area or Volume that has the constraints applied. Once you
have selected the correct regions, click
OK. Once the condition has
been deleted you may re-apply the appropriate condition as
explained in the tutorial above. Just recreate them using your
desired parameters.
Saving
Projects
·
Simply go to Utility Menu>File>Save
As… and save the project using the desired filename. To
open the file later, run Interactive (the first thing explained in
this tutorial) as usual, and when that is done, go to
Utility Menu>File>Resume From…
and choose the saved job from the directory it is saved in.
