Once the baseline model is prepared, you can define morph volumes, morph geometry, create design shapes and run DOE
studies. These tool work for both AcuSolve and ultraFluidX-based workflows.
ACU-T: 3201 Solar
Radiation and Thermal Shell Tutorial
This tutorial introduces you to setting up a CFD simulation involving solar radiation
and thermal shells using AcuSolve and HyperMesh CFD. Prior
to starting this tutorial, you should have already run through the introductory
tutorial, ACU-T: 1000 Basic Flow Set Up, and have a basic
understanding of HyperMesh CFD and AcuSolve. To run this simulation, you will need access to a
licensed version of HyperMesh CFD and AcuSolve.
Before you begin, copy the file(s) used in this tutorial to
your working directory.
The problem to be addressed is shown schematically in Figure 1. The model consists of an atrium with a couch and chairs in the center. Air flows
into the atrium through the inlet vent and exits through the outlet. The front
portion of the atrium consists of glass walls supported by an aluminum frame. This
aluminum frame will be modeled as a thermal shell; hence, this tutorial introduces
you to the process of setting up a transient solar radiation simulation and thermal
shells in HyperMesh CFD.
Solar Radiation Parameters
AcuSolve uses an ideal gray surface solar radiation model
to calculate the solar heat flux. The fluxes are computed using a ray trace
algorithm and five optical properties of the surface, specular transmissivity (), diffuse transmissivity (), specular reflectivity (), diffuse reflectivity () and absorptivity ().
A specular transmission occurs when a photon passes straight through a surface with
no change of direction. In a diffuse transmission the photon penetrates the surface,
but its outgoing energy is uniformly distributed in solid angle over the hemisphere,
weighted by projected surface area. For a specular reflection, the angle of
reflection is equal to the angle of incidence. Diffuse reflections are similar to
diffuse transmissions, except the hemisphere over which the outgoing energy is
distributed is on the same side of the surface as the incident photon. Finally, the
photon may be absorbed by the surface. These five interactions are associated with
five surface properties that together must obey the following
constraint:(1)
Where,
Specular transmissivity
Diffuse transmissivity
Specular reflectivity
Diffuse reflectivity
Absorptivity
Angle of incidence
For the solar radiative heat fluxes to be computed, a solar radiation surface needs
to be defined on that given surface.
In this tutorial, the solar flux loading is given in the form of a data file which
was generated using the acuSflux script available in AcuSolve. The script can be used to generate a data file with
a four-column array of solar flux vector data values. The piecewise linear type is
used in this tutorial to emulate the pattern of sunrise to sunset over the atrium.
For example, to generate the solar load data file for a location with known
geological coordinates, enter the following command in the AcuSolve Command Prompt: acuSflux -time "dec-3-2019
11:00:00" -tinc 1800 -nts 25 -lat 42.6064 -lon -83.1498 -ndir "1,0,0" -udir
"0,0,1"
Here,
time
The start time in GMT (ex: “dec-3-2019 21:00:00”)
tinc
The time increment in seconds
nts
Number of discrete time steps
lat
Latitude coordinates of the location in degrees North (ex: 45.112 or
-37.56 (equal to 37.56 S))
lon
Longitude coordinates of the location in degrees East (ex: 86.26 or
-54.84 (equal to 54.84 W))
ndir
The north direction unit vector in model coordinates (should be enclosed
in double quotes) (ex: “0,1,0”)
udir
The upward direction unit vector in model coordinates (should be
enclosed in double quotes) (ex: “0,1,0”)
Thermal Shell Modeling
The thermal shell in AcuSolve is a feature that creates
zero physical thickness volumetric shell elements from surface elements. This is
useful when the thickness of the component is too small to be modeled as a solid
medium. The thermal shell can have multiple layers, each with different thicknesses
and material models. A schematic of the thermal shell is shown below.
When defining a thermal shell on a surface, two sets of boundary conditions are
needed. One for the Primary Wall surface i.e. Shell Inner and one for the Shell
Outer Wall surface. In this tutorial, a solar radiation surface will be defined on
the outer shell surface so that it receives solar heat flux, whereas the inner shell
surface will be modeled as a default wall.
Start HyperMesh CFD and Create the HyperMesh Model Database
Start HyperMesh CFD from the Windows Start
menu by clicking Start > Altair <version> > HyperMesh CFD.
When HyperMesh CFD is loaded, the Geometry ribbon is open by
default.
Create a new .hm database in
one of the following ways:
From the menu bar, click File > Save.
From the Home tools, Files tool group, click the Save As tool.
In the Save File As dialog, navigate to the directory
where you would like to save the database.
Enter Atrium_Solar as the name for
the database then click Save.
This will be your problem directory and all the files related to the
simulation will be stored in this location.
Import and Validate the Geometry
Import the Geometry
From the menu bar, click File > Import > Geometry Model.
In the Import File dialog, browse to your working
directory then select ACU-T3201_Atrium.x_t and
click Open.
In the Geometry Import Options dialog, leave all the
default options unchanged then click Import.
The model contains an atrium with glass panes supported by an aluminum frame
in the front. Air enters from the opening on the roof in the front and exits
through the outlet in the rear.
Validate the Geometry
From the Geometry ribbon, click the Validate tool.
The Validate tool scans through the entire
model, performs checks on the surfaces and solids, and flags any defects in the
geometry, such as free edges, closed shells, intersections, duplicates, and
slivers.
The current model does not have any of the issues mentioned above.
Alternatively, if any issues are found, they are indicated by the number in
the brackets adjacent to the tool name.
Observe that a blue check
mark appears on the top-left corner of the Validate icon. This indicates that the tool found no
issues with the geometry model.
Press Esc or right-click in the
modeling window and swipe the cursor over the green
check mark from right to left.
Save the database.
Set Up Flow
Set Up the Simulation Parameters and Solver Settings
From the Flow ribbon, click the Physics tool.
The Setup dialog opens.
Under the Physics models setting:
Set Time marching to Transient.
Set the Time step size to 1 and the Final time
to 30.
Set the Turbulence model to Laminar.
Activate the Heat transfer checkbox.
Click the Solver controls setting and set the Maximum
stagger iterations to 3.
Close the dialog and save the model.
Assign Material Properties
From the Flow ribbon, click the Material tool.
Verify that Air is assigned as the material for the fluid domain.
The legend in the top-left corner of the modeling window lists all the material models assigned to the current model.
Since this
model has a single volume, by default air is assigned as the material for
the fluid domain.
On the guide bar, click
to execute
the command and exit the tool.
Define Thin Solids
In this simulation, you will model the aluminum frames as a thin solid.
From the Flow ribbon, click the Thin tool.
In the modeling window, select the four surfaces
highlighted in the image below.
In the microdialog, set the Layer thickness to
0.025 and the Material to
Aluminum.
On the guide bar, verify that the number of Parent
Surfaces selected is 4 then click to execute the
command.
Once the command is executed, the legend should be updated accordingly
to reflect the changes.
Save the model.
Define Flow Boundary Conditions
From the Flow ribbon, click the Constant tool.
In the modeling window, click the inlet surface
highlighted in the figure below.
In the microdialog, enter the values shown below.
Click on the guide bar to execute
the changes.
Click the Outlet tool.
Select the surface highlighted in the figure below then click
on the guide bar.
Click the No Slip tool.
Select all three wall surfaces of the atrium, the roof, and the front glass
walls.
In total, 21 surfaces should be selected.
In the microdialog, enter the values shown in the
figure below.
Click . In the
new microdialog that appears, set the Nodal Output
frequency to 1.
On the guide bar, click
to execute the command and remain in the
tool.
On the guide bar, click the drop-down menu next to
Surfaces and change the selection entity to Thin
Solids.
The visibility of all the surfaces except the thin solids is made
transparent.
Select all the thin solid surfaces using the window selection method.
In the microdialog, enter the values shown in the
figure below.
Click . In the
new microdialog that appears, set the Nodal Output
frequency to 1.
On the guide bar, verify that the number of Thin Solids
selected is 4 and the Direction is set to Away from Parent
Surface, then click .
Change the selection entity on the guide bar back to
Surfaces.
From the Boundaries legend, right-click on Default Wall
and select Isolate.
Select all the surfaces except the aluminum frame, as highlighted in the figure
below.
In the microdialog, enter the values shown in the
figure below.
Click . In the
new microdialog that appears, set the Nodal Output
frequency to 1.
From the Boundaries legend, rename Wall 1 to Floor by
double-clicking on it.
Click on the guide bar.
The updated Boundaries legend should look similar to the one shown
below.
Turn on the visibility of all the surfaces by right-clicking in the modeling window and selecting Show All
or by simply pressing the A key.
Save the model.
Set Up Solar Radiation
Set Up the Solar Radiation Parameters
From the Radiation ribbon, Solar Radiation tools, click the Physics tool.
In the Solar Radiation Settings dialog, activate the
Solar radiation equation.
Click to load
the solar flux input from a file.
In the Open file dialog, set the filter to Dat
file (.dat) and select the SolarLoad.dat
file provided with the input file for this tutorial.
Click Open.
The plot in the dialog should look like the one shown in the figure
below.
Close the dialog and save the model.
Define the Solar Radiation Models
From the Radiation ribbon, Solar Radiation tools, click the Model tool.
In the Solar radiation model library, click to add a new
solar radiation model.
In the Name column, enter BB out and set the Side to
Outward.
Similarly, create the other models and enter the values as shown in the figure
below.
Close the dialog and save the model.
Assign the Solar Radiation Models
From the Radiation ribbon, click the
Surface tool.
Select the three wall surfaces, the inlet, and the roof surface, as highlighted
in the figures below.
In the microdialog, set the Solar radiation model to
BB out then click
on the guide bar.
Select all the glass surfaces shown in the figure below, assign the
Glass model to them, then click
on the guide bar.
Rotate the model and select the floor surface. In the microdialog, assign the BB in model
then click on the guide bar.
From the Solar Radiation Model legend, right-click on
Unassigned and select
Isolate.
Select the surfaces of the couch, table, and chairs, assign the BB
def model to them, then click
on the guide bar.
On the guide bar, change the selection entity to
Thin Solids.
Using the window selection method, select the four thin solid surfaces and
assign the BB out model to them.
On the guide bar, verify that the Direction is set to
Away from Parent Surface then click to execute
the changes.
Turn on the display of all the surfaces and save the model.
Generate the Mesh
In this step, you will define the mesh controls and then generate the mesh.
Define the Surface Mesh Controls
From the Mesh ribbon, click the Surface tool.
Using the window selection method, select all the surfaces in the model.
In the microdialog, set the Average element size to
0.15 and the Mesh growth rate to
1.0.
On the guide bar, click
to execute
the command and exit the tool.
Save the model.
Generate the Mesh
From the Mesh ribbon, click the
Volume tool.
In the Meshing Operations dialog, set the Mesh growth rate
to 1.1 then click Mesh to start
the meshing process.
The Run Status dialog opens and the status of the
meshing process is shown.
Once the mesh is generated, close the Run Status dialog
and save the model.
Note: Considering the run time of the simulation, a very coarse mesh with no
boundary layers is used for this tutorial. Otherwise, a relatively fine mesh
with boundary layers to adequately resolve the gradients in the flow and
temperature fields should be used.
Compute the Solution
Define the Nodal Output Frequency
From the Solution ribbon, click the Field tool.
In the Field Output dialog, activate the check box for
Write initial conditions.
Set the Time step interval to 1.
Define the Nodal Initial Conditions and Compute the Solution
From the Solution ribbon, click the Run tool.
In the Launch AcuSolve dialog, set the Parallel processing
option to Intel MPI.
Optional: Set the number of processors to 4 or
8 based on availability.
Deactivate the Automatically define pressure
reference option.
Expand the Default initial conditions menu.
Deactivate the Pre-compute flow option.
Set the Temperature to 288.15.
Verify that all the values are set as shown in the figure below.
Click Run.
Once the solution process is started, the Run
Status dialog appears.
In the dialog, right-click on the AcuSolve run and
select View log file.
Once the run is complete, a summary of the solution process is shown in
the log file.
Post-Process the Results with HM-CFD Post
Create Surface Groups
Once the solution is completed, navigate to the Post
ribbon.
From the menu bar, click File > Open > Results.
Select the AcuSolve log file in your problem
directory to load the results for post-processing.
The solid and all the surfaces are loaded in the Post Browser.
Click the Boundary Groups tool.
Click on the guide bar to open
Advanced Selection.
Set the drop-down to By Boundaries then select
Thin Solid Wall and
Floor.
Exit the dialog then click on the guide bar.
The two boundaries are grouped together under the User Defined surface
group in the Post Browser.
Isolate the new surface group and rename it to
ThinSolid_Floor.
Plot the Temperature Contour
In the Post Browser, right-click on the
ThinSolid_Floor surface group and select
Edit.
In the display properties microdialog, set the display
to temperature and activate the
Legend toggle.
Set the legend bounds to 287 and
292.
Click and set the Colormap Name to Rainbow
Uniform.
Click on the guide bar.
Drag the animation slider at the bottom of the modeling window to the 31st
frame.
Summary
In this tutorial, you learned how to set up and solve a CFD analysis involving solar
radiation. You started by importing a geometry model into HyperMesh CFD and setting up the simulation parameters and boundary
conditions. Once you computed the solution, you post-processed the results using the
Post ribbon.