-
Inviscid Bump in a Channel
Inviscid Supersonic Wedge
Inviscid ONERA M6
Laminar Flat Plate
Laminar Cylinder
Turbulent Flat Plate
Transitional Flat Plate
Transitional Flat Plate for T3A and T3A-
Turbulent ONERA M6
Unsteady NACA0012
Epistemic Uncertainty Quantification of RANS predictions of NACA 0012 airfoil
Non-ideal compressible flow in a supersonic nozzle
-
Unconstrained shape design of a transonic inviscid airfoil at a cte. AoA
Constrained shape design of a transonic turbulent airfoil at a cte. CL
Constrained shape design of a transonic inviscid wing at a cte. CL
Shape Design With Multiple Objectives and Penalty Functions
Unsteady Shape Optimization NACA0012
Unconstrained shape design of a two way mixing channel
Turbulent CFD-RHT-CHT including Adjoint Sensitivities using multiple FFD-boxes
| Written by | for Version | Revised by | Revision date | Revised version |
|---|---|---|---|---|
| @rsanfer | 7.0.2 | @rsanfer | 2020-02-27 | 7.0.2 |
Solver: |
|
Uses: |
|
Prerequisites: |
|
| |
|
Complexity: |
Advanced |
Goals
This tutorial builds up on SU2’s Conjugate Heat Transfer and Radiative Heat Transfer capabilities, to solve a multizone, multiphysics problem involving incompressible turbulent flows, radiation, and conjugate heat transfer between a solid domain and a buoyancy-driven cavity. Upon the completion of this example, the user will be capable of
- Setting up a multiphysics simulation with Conjugate Heat Transfer interfaces between zones
- Solving a turbulent buoyancy-driven cavity with participating media and radiation
- Computing coupled adjoint solutions of problems involving incompressible flow and radiation
- Generating multiple FFD boxes to deform the system outer walls
- Projecting the surface sensitivities into the FFD parameters
In this tutorial, we define a problem similar to the Laminar Buoyancy-Driven Cavity, however using in this case the right wall is a solid wall rather than an isothermal boundary condition.
Where the inlet velocity is 3 m/s and its temperature is 450 K, while the outlet is a 0 pressure outlet.
Resources
For this tutorial, please download the contents of the folder multiphysics/turb_rht_cht of the Tutorials repository.
Background
CHT simulations become important when we cannot assume an isomthermal wall boundary or suitable temperature distribution estimate. In this tutorial, we assume that this is the case for the right boundary of our buoyancy-driven cavity, and the interface temperature distribution becomes part of the solution of the simulation, by balancing the energy in all physical domains.
Mesh Description
The flow domain is discretized using a structured mesh with a total of 4800 elements. The solid domain is discretized using 960 elements. The interface between the domains is matching.
FFD Box Generation
First, we define the two FFD boxes to parametrize the upper and lower boundaries of the fluid domain, using 14 design variables per boundary. This is shown next
In order to ensure that the solid domain remains fixed, the FFD boxes are defined so that they do not intersect the CHT boundary. This is shown in detail in the next image, where the red domain corresponds to the solid, and the blue to the FFD box
We define the FFD boxes using the FFD config file. In this case, we define 2 boxes using
DV_KIND = FFD_SETTING
DV_MARKER = (( upper ), (lower))
DV_PARAM = (( UPPER_BOX, 14, 1, 0.0, 1.0 ), ( LOWER_BOX, 14, 1, 0.0, 1.0 ))
where the parameters for each box (UPPER_BOX and LOWER_BOX) are set using
FFD_TOLERANCE = 1E-8
FFD_ITERATIONS = 500
FFD_DEFINITION = (UPPER_BOX, -0.02, 0.975, 0.0, 0.998, 0.975, 0.0, 0.998, 1.025, 0.0, -0.02, 1.025, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0); (LOWER_BOX, -0.02, -0.025, 0.0, 0.998, -0.025, 0.0, 0.998, 0.025, 0.0, -0.02, 0.025, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0)
FFD_DEGREE = ( 14, 1, 0); ( 14, 1, 0)
FFD_CONTINUITY = 2ND_DERIVATIVE
We run the following command
$ SU2_DEF config_ffd.cfg
which returns
--------------------- Surface grid deformation (ZONE 0) -----------------
Performing the deformation of the surface grid.
2 Free Form Deformation boxes.
1 Free Form Deformation nested levels.
FFD box tag: UPPER_BOX. FFD box level: 0. Degrees: 14, 1.
FFD Blending using Bezier Curves.
Number of parent boxes: 0. Number of child boxes: 0.
FFD box tag: LOWER_BOX. FFD box level: 0. Degrees: 14, 1.
FFD Blending using Bezier Curves.
Number of parent boxes: 0. Number of child boxes: 0.
----------------- FFD technique (cartesian -> parametric) ---------------
Compute parametric coord | FFD box: UPPER_BOX. Max Diff: 2.28878e-16.
Compute parametric coord | FFD box: LOWER_BOX. Max Diff: 2.22045e-16.
Writing a Paraview file of the FFD boxes.
No surface deformation (setting FFD).
----------------------- Write deformed grid files -----------------------
|SU2 mesh |mesh_flow_ffd.su2 |
Adding any FFD information to the SU2 file.
In order to confirm that both FFD boxes information has been added to the mesh file, we open mesh_flow_ffd.su2 and check that the FFD information has been appended to the file
FFD_NBOX= 2
FFD_NLEVEL= 1
FFD_TAG= UPPER_BOX
FFD_LEVEL= 0
FFD_DEGREE_I= 14
FFD_DEGREE_J= 1
FFD_BLENDING= BEZIER
FFD_PARENTS= 0
FFD_CHILDREN= 0
FFD_CORNER_POINTS= 4
-0.02 0.975
0.998 0.975
0.998 1.025
-0.02 1.025
FFD_CONTROL_POINTS= 60
0 0 0 -0.02 0.975 -0.5
0 0 1 -0.02 0.975 0.5
0 1 0 -0.02 1.025 -0.5
0 1 1 -0.02 1.025 0.5
...
14 0 0 0.998 0.975 -0.5
14 0 1 0.998 0.975 0.5
14 1 0 0.998 1.025 -0.5
14 1 1 0.998 1.025 0.5
FFD_SURFACE_POINTS= 50
upper 103 2.368368087162328e-02 4.999999999999987e-01 5.000000000000000e-01
upper 5 1.964636542239686e-02 4.999999999999987e-01 5.000000000000000e-01
...
upper 150 9.932979180545798e-01 5.000000000000000e-01 5.000000000000000e-01
upper 151 9.979273210929932e-01 5.000000000000000e-01 5.000000000000000e-01
FFD_TAG= LOWER_BOX
FFD_LEVEL= 0
FFD_DEGREE_I= 14
FFD_DEGREE_J= 1
FFD_BLENDING= BEZIER
FFD_PARENTS= 0
FFD_CHILDREN= 0
FFD_CORNER_POINTS= 4
-2.000000000000000e-02 -2.500000000000000e-02
9.980000000000000e-01 -2.500000000000000e-02
9.980000000000000e-01 2.500000000000000e-02
-2.000000000000000e-02 2.500000000000000e-02
FFD_CONTROL_POINTS= 60
0 0 0 -2.000000000000000e-02 -2.500000000000000e-02 -5.000000000000000e-01
0 0 1 -2.000000000000000e-02 -2.500000000000000e-02 5.000000000000000e-01
0 1 0 -2.000000000000000e-02 2.500000000000000e-02 -5.000000000000000e-01
0 1 1 -2.000000000000000e-02 2.500000000000000e-02 5.000000000000000e-01
...
14 0 0 9.980000000000000e-01 -2.500000000000000e-02 -5.000000000000000e-01
14 0 1 9.980000000000000e-01 -2.500000000000000e-02 5.000000000000000e-01
14 1 0 9.980000000000000e-01 2.500000000000000e-02 -5.000000000000000e-01
14 1 1 9.980000000000000e-01 2.500000000000000e-02 5.000000000000000e-01
FFD_SURFACE_POINTS= 50
lower 243 9.979273210929928e-01 5.000000000000000e-01 5.000000000000000e-01
lower 244 9.932979180545780e-01 5.000000000000000e-01 5.000000000000000e-01
...
lower 291 2.368368087164354e-02 5.000000000000000e-01 5.000000000000000e-01
lower 0 1.964636542239686e-02 5.000000000000000e-01 5.000000000000000e-01
Multiphysics Configuration File
We start the tutorial by definining the problem as a multiphysics case,
SOLVER = MULTIPHYSICS
We set the config files for each sub-problem using the command CONFIG_LIST, and state that each sub-problem will use a different mesh file:
MULTIZONE_MESH = NO
CONFIG_LIST = (config_flow_rht.cfg, config_solid_cht.cfg)
Now, we define the coupling conditions. In this case, the interface between the marker right in the flow domain, and leftSolid in the solid domain, is defined as
MARKER_ZONE_INTERFACE= (right, leftSolid)
We define the number of outer iterations for the multizone problem for a maximum of 30000 outer iterations
OUTER_ITER = 30000
Then, the convergence criteria is set to evaluate the averaged residual of the flow state vector (zone 0) (AVG_BGS_RES[0]) and the solid temperature (zone 1) (AVG_BGS_RES[1]) in two consecutive outer iterations, \(\mathbf{w}^{n+1}-\mathbf{w}^{n}\) and \(\mathrm{T}^{n+1}-\mathrm{T}^{n}\) respectively.
CONV_FIELD = AVG_BGS_RES[0], AVG_BGS_RES[1]
CONV_RESIDUAL_MINVAL = -8
The last step is defining our desired output. In this tutorial, we will use the following configuration for the history output
OUTPUT_WRT_FREQ = 1000
OUTPUT_FILES = (RESTART, PARAVIEW)
TABULAR_FORMAT= CSV
HISTORY_OUTPUT = (ITER, RMS_RES[0], HEAT[0], RMS_RES[1])
where the restart and paraview solution files are written every 1000 iterations, and the residuals of both zones and the heat properties of zone 1 are written to the history file, which has the same name as the config file but with extension .csv.
Applying simulation conditions to the individual domains: Flow domain
The flow domain is defined in config_flow_rht.cfg. An incompressible, Renolds-Averaged Navier Stokes simulation with an SST turbulence model is set
SOLVER = INC_RANS
KIND_TURB_MODEL = SST
We set the properties for the flow according to the problem definition
INC_DENSITY_MODEL = VARIABLE
INC_ENERGY_EQUATION = YES
INC_VELOCITY_INIT = ( 1.0, 0.0, 0.0 )
INC_DENSITY_INIT = 0.006
INC_TEMPERATURE_INIT = 450
INC_NONDIM = DIMENSIONAL
VISCOSITY_MODEL = CONSTANT_VISCOSITY
MU_CONSTANT = 1e-5
CONDUCTIVITY_MODEL = CONSTANT_CONDUCTIVITY
KT_CONSTANT = 0.01
FLUID_MODEL = INC_IDEAL_GAS
SPECIFIC_HEAT_CP = 1000
MOLECULAR_WEIGHT = 30
BODY_FORCE = YES
BODY_FORCE_VECTOR = ( 0.0, -9.81, 0.0 )
And the radiation model is defined as
RADIATION_MODEL = P1
MARKER_EMISSIVITY = ( upper, 0.0, lower, 0.0, left, 1.0, right, 1.0, inlet, 1.0, outlet, 1.0 )
ABSORPTION_COEFF = 1.0
CFL_NUMBER_RAD = 1E12
TIME_DISCRE_RADIATION = EULER_IMPLICIT
We incorporate a volumetric heat source in the form of an ellipse with principal axes \(a = 0.2\), \(b = 0.05\), centered at \((0.2,0.875,0)\), to mimic the effect of a flame in the domain
HEAT_SOURCE = YES
HEAT_SOURCE_VAL = 50000
HEAT_SOURCE_ROTATION_Z = 0
HEAT_SOURCE_CENTER = (0.2,0.875,0)
HEAT_SOURCE_AXES = (0.2,0.05,0)
Next, the flow boundary conditions are applied
MARKER_ISOTHERMAL = ( left, 600.0 )
MARKER_HEATFLUX = ( upper, 0.0, lower, 0.0 )
MARKER_PLOTTING = ( right )
MARKER_MONITORING = ( right )
INC_INLET_TYPE = VELOCITY_INLET
MARKER_INLET = ( inlet, 450.0, 3.0, 1.0, 0.0, 0.0)
INC_OUTLET_TYPE = PRESSURE_OUTLET
MARKER_OUTLET = ( outlet, 0.0 )
and the right boundary is defined as a CHT interface
MARKER_CHT_INTERFACE = (right)
Applying simulation conditions to the individual domains: Solid domain
The solid domain is defined in config_solid_cht.cfg. Only the heat equation is considered by the solver
SOLVER = HEAT_EQUATION
The properties of the solid domain are defined next
SOLID_TEMPERATURE_INIT = 300.0
SOLID_DENSITY = 2000
SPECIFIC_HEAT_CP = 1000.0
SOLID_THERMAL_CONDUCTIVITY = 1.0
INC_NONDIM = DIMENSIONAL
And the boundary conditions are, for this case
MARKER_ISOTHERMAL = ( rightSolid, 300.0, upperSolid, 300.0, lowerSolid, 300.0)
MARKER_MONITORING = ( NONE )
while the coupling conditions are defined using
MARKER_CHT_INTERFACE = (leftSolid)
Running the primal simulation
We now run the simulation in parallel with 2 cores, using
$ mpirun -n 2 SU2_CFD turbulent_rht_cht.cfg
and we obtain
+--------------------------------------+
| Multizone Summary |
+--------------------------------------+
| Outer_Iter| avg[bgs][0]| avg[bgs][1]|
+--------------------------------------+
| 0| 0.376042| -0.201907|
| 1| 0.308690| -0.837103|
| 2| 0.130097| -1.039244|
| 3| -0.060423| -1.232387|
| 4| -0.194779| -1.419352|
| 5| -0.345477| -1.592573|
| 6| -0.447955| -1.744954|
| 7| -0.521272| -1.874409|
| 8| -0.540495| -1.980951|
| 9| -0.594882| -2.067258|
| 10| -0.651959| -2.138538|
...
| 14000| -7.822037| -5.978975|
| 14001| -7.822255| -5.979198|
| 14002| -7.822479| -5.979420|
| 14003| -7.822697| -5.979642|
| 14004| -7.822920| -5.979864|
| 14005| -7.823138| -5.980086|
| 14006| -7.823362| -5.980308|
| 14007| -7.823580| -5.980530|
| 14008| -7.823803| -5.980752|
| 14009| -7.824021| -5.980975|
| 14010| -7.824245| -5.981197|
...
| 23115| -9.831339| -7.997863|
| 23116| -9.831563| -7.998084|
| 23117| -9.831779| -7.998305|
| 23118| -9.832003| -7.998526|
| 23119| -9.832220| -7.998747|
| 23120| -9.832443| -7.998968|
| 23121| -9.832661| -7.999189|
| 23122| -9.832884| -7.999410|
| 23123| -9.833101| -7.999631|
| 23124| -9.833324| -7.999852|
| 23125| -9.833541| -8.000073|
We need to converge the problem thoroughly in order to obtain a converged heatflux at the CHT boundary, as this will be our objective function for adjoint purposes. From the history file, we can observe that, although the residuals have been reduced by 5 and 7 orders of magnitude respectively after 14000 iterations, the heaflux is not yet fully converged, and it takes almost another 10000 iterations to converge
"Time_Iter","Outer_Iter","Inner_Iter", "HF[0]" , "maxHF[0]"
0, 0, 0, 4781.631841, 8284.801073
0, 1, 0, 206.661296, 407.9247674
0, 2, 0, 157.8829329, 305.847306
0, 3, 0, 129.1211842, 247.3569023
0, 4, 0, 114.5644202, 217.9004096
0, 5, 0, 107.1377363, 202.2141012
0, 6, 0, 102.9648849, 193.3549536
0, 7, 0, 100.6066882, 188.5484424
0, 8, 0, 99.04567981, 185.4970227
0, 9, 0, 97.67690982, 182.8558711
0, 10, 0, 96.36114436, 180.2696727
...
0, 14000, 0, 113.1030141, 200.7535431
0, 14001, 0, 113.1030134, 200.7535423
0, 14002, 0, 113.1030127, 200.7535414
0, 14003, 0, 113.1030119, 200.7535406
0, 14004, 0, 113.1030112, 200.7535398
0, 14005, 0, 113.1030105, 200.7535389
0, 14006, 0, 113.1030098, 200.7535381
0, 14007, 0, 113.103009, 200.7535373
0, 14008, 0, 113.1030083, 200.7535364
0, 14009, 0, 113.1030076, 200.7535356
0, 14010, 0, 113.1030069, 200.7535348
...
0, 23116, 0, 113.1015985, 200.7519326
0, 23117, 0, 113.1015985, 200.7519326
0, 23118, 0, 113.1015985, 200.7519326
0, 23119, 0, 113.1015985, 200.7519326
0, 23120, 0, 113.1015985, 200.7519326
0, 23121, 0, 113.1015985, 200.7519325
0, 23122, 0, 113.1015985, 200.7519325
0, 23123, 0, 113.1015985, 200.7519325
0, 23124, 0, 113.1015985, 200.7519325
0, 23125, 0, 113.1015985, 200.7519325
The temperature and velocity fields for the primal settings are as follows
Running the adjoint simulation
Only the following minor changes are required to the multiphysics adjoint file, turbulent_rht_cht_adjoint.cfg, to compute the adjoint of the integrated heatflux through the CHT boundary:
MATH_PROBLEM = DISCRETE_ADJOINT
OBJECTIVE_FUNCTION = TOTAL_HEATFLUX
Then, the restart files need to be renamed as solution files, restart_flow_rht_0.dat → solution_flow_rht_0.dat and restart_solid_cht_1.dat → solution_solid_cht_1.dat. We run the adjoint in parallel using
$ mpirun -n 2 SU2_CFD_AD turbulent_rht_cht_adjoint.cfg
The simulation starts from the converged point
-------------------------------------------------------------------------
Storing computational graph wrt CONSERVATIVE VARIABLES.
Objective function : 113.102
Zone 0 (flow) - log10[U(0)] : -15.7308
Zone 0 (turbulence) - log10[Turb(0)] : -14.9704
Zone 0 (radiation) - log10[Rad(0)] : -7.60211
Zone 1 (heat) - log10[Heat(0)] : -11.9829
-------------------------------------------------------------------------
and the simulation converges quickly
+--------------------------------------+
| Multizone Summary |
+--------------------------------------+
| Outer_Iter| avg[bgs][0]| avg[bgs][1]|
+--------------------------------------+
| 0| 0.000000| 0.000000|
| 1| -2.963087| -2.536124|
| 2| -2.938999| -2.493938|
| 3| -3.079946| -2.573465|
| 4| -3.135020| -2.624314|
| 5| -3.213446| -2.669019|
| 6| -3.261026| -2.710054|
| 7| -3.293646| -2.746341|
| 8| -3.329728| -2.776762|
| 9| -3.364945| -2.801132|
| 10| -3.393157| -2.820130|
...
| 8856| -5.662248| -4.997821|
| 8857| -5.662245| -4.998039|
| 8858| -5.662248| -4.998258|
| 8859| -5.662245| -4.998477|
| 8860| -5.662248| -4.998696|
| 8861| -5.662245| -4.998914|
| 8862| -5.662248| -4.999133|
| 8863| -5.662245| -4.999351|
| 8864| -5.662248| -4.999570|
| 8865| -5.662245| -4.999788|
| 8866| -5.662248| -5.000007|
Projecting the adjoint into the FFD box parameters
The same configuration file can be used with SU2_DOT_AD to project the sensitivities of the heatflux into the design parameters. We need to rename the adjoint solutions restart_adj_flow_rht_totheat_0.dat → solution_adj_flow_rht_totheat_0.dat and restart_adj_solid_cht_totheat_1.dat → solution_adj_solid_cht_totheat_1.dat
It is important to adequately define the projections settings config_flow_rht.cfg. Only the leftmost 12 points of each FFD boxes will be used, as the other 3 are kept still by SU2 to ensure continuity on the 2nd derivative.
DV_KIND= FFD_CONTROL_POINT_2D, FFD_CONTROL_POINT_2D, ..., FFD_CONTROL_POINT_2D, FFD_CONTROL_POINT_2D,
DV_MARKER = (( upper ), (lower))
DV_PARAM = ( UPPER_BOX, 0, 1, 0.0, 1.0 ); ( UPPER_BOX, 1, 1, 0.0, 1.0 ); ( UPPER_BOX, 10, 1, 0.0, 1.0 ); ( UPPER_BOX, 11, 1, 0.0, 1.0 ); ( LOWER_BOX, 0, 0, 0.0, 1.0 ); ( LOWER_BOX, 1, 0, 0.0, 1.0 ); ( LOWER_BOX, 10, 0, 0.0, 1.0 ); ( LOWER_BOX, 11, 0, 0.0, 1.0 )
DV_VALUE = 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0
We run the projection software
$ SU2_DOT_AD turbulent_rht_cht_adjoint.cfg
which yields the following projected gradients
Design variable (FFD_CONTROL_POINT_2D) number 0.
TOTAL_HEATFLUX gradient : 9.29141
-------------------------------------------------------------------------
Design variable (FFD_CONTROL_POINT_2D) number 1.
TOTAL_HEATFLUX gradient : 5.70395
-------------------------------------------------------------------------
...
Design variable (FFD_CONTROL_POINT_2D) number 22.
TOTAL_HEATFLUX gradient : -1.41853
-------------------------------------------------------------------------
Design variable (FFD_CONTROL_POINT_2D) number 23.
TOTAL_HEATFLUX gradient : -1.36538
-------------------------------------------------------------------------
The sensitivities for the FFD points are written to the file of_grad.dat.
Deforming the domain for design purposes
An example on how to deform the mesh is provided in sample_ffd_deform.cfg. We define the input mesh as mesh_flow_ffd.su2 and the output as mesh_flow_ffd_deform.su2.
MESH_FORMAT = SU2
MESH_FILENAME = mesh_flow_ffd.su2
MESH_OUT_FILENAME = mesh_flow_ffd_deform.su2
We define the design variables for this example as
DV_VALUE = 0.0, 0.05, 0.1, 0.14, 0.16, 0.17, 0.175, 0.17, 0.16, 0.14, 0.1, 0.05, 0.0, -0.05, -0.1, -0.14, -0.16, -0.17, -0.175, -0.17, -0.16, -0.14, -0.1, -0.05
and we run the SU2_DEF binary to deform the mesh
SU2_DEF sample_ffd_deform.cfg
By substituting the input mesh into the flow configuration file
MESH_FILENAME= mesh_flow_ffd_deform.su2
it is possible to run a deformed primal simulation. The temperature and velocity fields for this particular deformed configuration are as follows
Attribution
If you are using this content for your research, please kindly cite the following reference in your derived works:
Sanchez, R. et al. (2020), Adjoint-based sensitivity analysis in high-temperaturefluid flows with participating media, (Submitted to) Modeling, Simulation and Optimization in the Health- and Energy-Sector, SEMA SIMAI SPRINGER SERIES
-
This work is licensed under a Creative Commons Attribution 4.0 International License
