CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   SU2 (https://www.cfd-online.com/Forums/su2/)
-   -   3D Windturbine simulation in SU2 (https://www.cfd-online.com/Forums/su2/172463-3d-windturbine-simulation-su2.html)

 k.vimalakanthan May 31, 2016 15:34

3D Windturbine simulation in SU2

3 Attachment(s)
Dear All,

I'm trying to simulate a single blade 120deg axi-symmetric model of the CX100 turbine using the incompressible RANS solver in SU2. The 3D grid was made in Pointwise using this webinar - https://www.youtube.com/watch?v=_o0KOJ7RJXc. The SU2 configuration file is also attached.

https://we.tl/Nz7L2hjxrv
The attached images shows the boundary patches.

With the current set-up I'm not able to even reach one iteration. I've tried using the SU2_MSH processor and running the simulation with 'CX100_pre.su2' grid, which also fails. Could anyone please have a look at this case and suggest improvements that can actually enable me to run this problem.

The .cfg file:
Code:

```% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------% % % Physical governing equations (EULER, NAVIER_STOKES, %                              WAVE_EQUATION, HEAT_EQUATION, LINEAR_ELASTICITY, %                              POISSON_EQUATION) PHYSICAL_PROBLEM= NAVIER_STOKES % % Specify turbulent model (NONE, SA, SA_NEG, SST) KIND_TURB_MODEL= SST % % Mathematical problem (DIRECT, CONTINUOUS_ADJOINT) MATH_PROBLEM= DIRECT % % Regime type (COMPRESSIBLE, INCOMPRESSIBLE, FREESURFACE) REGIME_TYPE= INCOMPRESSIBLE % % Restart solution (NO, YES) RESTART_SOL= NO % -------------------- INCOMPRESSIBLE FREE-STREAM DEFINITION ------------------% % % Free-stream density (1.2886 Kg/m^3 (air), 998.2 Kg/m^3 (water)) FREESTREAM_DENSITY= 1.2886 % % Free-stream velocity (m/s) FREESTREAM_VELOCITY= ( 0.000, 0.000 , 4.000) % % Free-stream viscosity (1.853E-5 Ns/m^2 (air), 0.798E-3 Ns/m^2 (water)) FREESTREAM_VISCOSITY= 1.853e-05 % ---------------------- REFERENCE VALUE DEFINITION ---------------------------% % % Reference origin for moment computation REF_ORIGIN_MOMENT_X = 0.00 REF_ORIGIN_MOMENT_Y = 0.00 REF_ORIGIN_MOMENT_Z = 0.00 % % Reference length for pitching, rolling, and yawing non-dimensional moment REF_LENGTH_MOMENT= 1 % % Reference area for force coefficients (0 implies automatic calculation) REF_AREA= 0 % -------------------- BOUNDARY CONDITION DEFINITION --------------------------% % % Navier-Stokes wall boundary marker(s) (NONE = no marker) MARKER_HEATFLUX= ( Blade, 0.0, Spinner, 0.0) % % Farfield boundary marker(s) (NONE = no marker) MARKER_FAR= ( Inlet, Outlet, TopWall ) % % Periodic boundary marker(s) (NONE = no marker) % Format: ( periodic marker, donor marker, rot_cen_x, rot_cen_y, rot_cen_z, rot_angle_x-axis, rot_angle_y-axis, rot_angle_z-axis, translation_x, translation_y, translation_z) MARKER_PERIODIC= ( Per1, Per2, 0.0, 0.0, 0.0, 0.0, 0.0, 120, 0.0, 0.0, 0.0) % % Marker(s) of the surface to be plotted or designed MARKER_PLOTTING= ( Blade ) % % Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated MARKER_MONITORING= ( Blade ) % ------------------------- GRID ADAPTATION STRATEGY --------------------------% % % Kind of grid adaptation (NONE, PERIODIC) KIND_ADAPT= PERIODIC % % ----------------------- DYNAMIC MESH DEFINITION -----------------------------% % % Dynamic mesh simulation (NO, YES) GRID_MOVEMENT= YES % % Type of dynamic mesh (NONE, ROTATING_FRAME) GRID_MOVEMENT_KIND= ROTATING_FRAME % % Motion mach number (non-dimensional). Used for intitializing a viscous flow % with the Reynolds number and for computing force coeffs. with dynamic meshes. % MACH_MOTION= 0.01 % % Coordinates of the motion origin MOTION_ORIGIN_X= 0.0 MOTION_ORIGIN_Y= 0.0 MOTION_ORIGIN_Z= 0.0 % % Angular velocity vector (rad/s) about the motion origi. Example 1250 RPM -> 130.89969389957471 rad/s ROTATION_RATE_X = 0.0 ROTATION_RATE_Y = 0.0 ROTATION_RATE_Z = 5.811 % % ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------% % % Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES) NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES % % Courant-Friedrichs-Lewy condition of the finest grid CFL_NUMBER= 1 % % Adaptive CFL number (NO, YES) CFL_ADAPT= NO % % Parameters of the adaptive CFL number (factor down, factor up, CFL min value, %                                        CFL max value ) CFL_ADAPT_PARAM= ( 2, 4, 500.0, 1000.0 ) % ----------------------- SLOPE LIMITER DEFINITION ----------------------------% % % Reference element length for computing the slope and sharp edges limiters. REF_ELEM_LENGTH= 0.1 % % Coefficient for the limiter LIMITER_COEFF= 0.1 % % Coefficient for the sharp edges limiter SHARP_EDGES_COEFF= 3.0 % % Reference coefficient (sensitivity) for detecting sharp edges. REF_SHARP_EDGES= 3.0 % % Remove sharp edges from the sensitivity evaluation (NO, YES) SENS_REMOVE_SHARP= NO % ------------------------ LINEAR SOLVER DEFINITION ---------------------------% % % Linear solver for implicit formulations (BCGSTAB, FGMRES) LINEAR_SOLVER= FGMRES % % Preconditioner of the Krylov linear solver (JACOBI, LINELET, LU_SGS) LINEAR_SOLVER_PREC= LU_SGS % % Minimum error of the linear solver for implicit formulations LINEAR_SOLVER_ERROR= 1E-4 % % Max number of iterations of the linear solver for the implicit formulation LINEAR_SOLVER_ITER= 10 % -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------% % % Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC, %                              TURKEL_PREC, MSW) CONV_NUM_METHOD_FLOW= ROE % % Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER) % SPATIAL_ORDER_FLOW= 2ND_ORDER_LIMITER % % Slope limiter (VENKATAKRISHNAN, MINMOD) SLOPE_LIMITER_FLOW= VENKATAKRISHNAN % % 1st, 2nd and 4th order artificial dissipation coefficients AD_COEFF_FLOW= ( 0.15, 0.5, 0.02 ) % % Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT) TIME_DISCRE_FLOW= EULER_IMPLICIT % -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------% % % Convective numerical method (SCALAR_UPWIND) CONV_NUM_METHOD_TURB= SCALAR_UPWIND % % Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER) % SPATIAL_ORDER_TURB= 1ST_ORDER % % Slope limiter (VENKATAKRISHNAN, MINMOD) SLOPE_LIMITER_TURB= VENKATAKRISHNAN % % Time discretization (EULER_IMPLICIT) TIME_DISCRE_TURB= EULER_IMPLICIT % --------------------------- CONVERGENCE PARAMETERS --------------------------% % % % Number of total iterations EXT_ITER= 4000 % % Convergence criteria (CAUCHY, RESIDUAL) % CONV_CRITERIA= RESIDUAL % % Residual reduction (order of magnitude with respect to the initial value) RESIDUAL_REDUCTION= 8 % % Min value of the residual (log10 of the residual) RESIDUAL_MINVAL= -9 % % Start convergence criteria at iteration number STARTCONV_ITER= 10 % % Number of elements to apply the criteria CAUCHY_ELEMS= 100 % % Epsilon to control the series convergence CAUCHY_EPS= 1E-4 % % Function to apply the criteria (LIFT, DRAG, NEARFIELD_PRESS, SENS_GEOMETRY, %                                            SENS_MACH, DELTA_LIFT, DELTA_DRAG) CAUCHY_FUNC_FLOW= LIFT % ------------------------- INPUT/OUTPUT INFORMATION --------------------------% % % Mesh input file MESH_FILENAME= CX100.su2 % % Mesh input file format (SU2, CGNS, NETCDF_ASCII) MESH_FORMAT= SU2 % % Mesh output file MESH_OUT_FILENAME= CX100_per.su2 % % Restart flow input file SOLUTION_FLOW_FILENAME= restart_flow.dat % % Output file format (PARAVIEW, TECPLOT, STL) OUTPUT_FORMAT= TECPLOT % % Output file convergence history (w/o extension) CONV_FILENAME= history % % Output file restart flow RESTART_FLOW_FILENAME= restart_flow.dat % % % Output file flow (w/o extension) variables VOLUME_FLOW_FILENAME= Results % % Output file surface flow coefficient (w/o extension) SURFACE_FLOW_FILENAME= surface_flow % % Writing solution file frequency WRT_SOL_FREQ= 500 % % Writing convergence history frequency WRT_CON_FREQ= 1```
I'm very new to SU2 and I hope this thread can help and learn from each other the best approach to simulating horizontal axis wind turbines in SU2.

Kind regards,
Kishore

 AbhinandanSingh May 31, 2016 15:53

hey,
Could you please elaborate what error you got.

 k.vimalakanthan June 1, 2016 05:27

Quote:
 Originally Posted by AbhinandanSingh (Post 602728) hey, Could you please elaborate what error you got.
This is the output when I run the case as it is:
Code:

```------------------------------------------------------------------------- |    ___ _  _ ___                                                      | |  / __| | | |_  )  Release 4.1.1  "Cardinal"                        | |  \__ \ |_| |/ /                                                      | |  |___/\___//___|  Suite (Computational Fluid Dynamics Code)        | |                                                                      | ------------------------------------------------------------------------- | SU2 Lead Dev.: Dr. Francisco Palacios, Francisco.D.Palacios@boeing.com| |                Dr. Thomas D. Economon, economon@stanford.edu          | ------------------------------------------------------------------------- | SU2 Developers:                                                      | | - Prof. Juan J. Alonso's group at Stanford University.                | | - Prof. Piero Colonna's group at Delft University of Technology.      | | - Prof. Nicolas R. Gauger's group at Kaiserslautern U. of Technology. | | - Prof. Alberto Guardone's group at Polytechnic University of Milan.  | | - Prof. Rafael Palacios' group at Imperial College London.            | ------------------------------------------------------------------------- | Copyright (C) 2012-2016 SU2, the open-source CFD code.                | |                                                                      | | SU2 is free software; you can redistribute it and/or                  | | modify it under the terms of the GNU Lesser General Public            | | License as published by the Free Software Foundation; either          | | version 2.1 of the License, or (at your option) any later version.    | |                                                                      | | SU2 is distributed in the hope that it will be useful,                | | but WITHOUT ANY WARRANTY; without even the implied warranty of        | | MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU      | | Lesser General Public License for more details.                      | |                                                                      | | You should have received a copy of the GNU Lesser General Public      | | License along with SU2. If not, see <http://www.gnu.org/licenses/>.  | ------------------------------------------------------------------------- ------------------------ Physical Case Definition ----------------------- Incompressible RANS equations. Turbulence model: Menter's SST Performing a dynamic mesh simulation: rotating reference frame. No restart solution, use the values at infinity (freestream). Dimensional simulation. The reference length/area will be computed using y(2D) or z(3D) projection. The reference length (moment computation) is 1. Reference origin (moment computation) is (0, 0, 0). Surface(s) where the force coefficients are evaluated: Blade. Surface(s) plotted in the output file: Blade. Surface(s) belonging to the Fluid-Structure Interaction problem: Input mesh file name: CX100.su2 ---------------------- Space Numerical Integration ---------------------- Roe (with entropy fix) solver for the flow inviscid terms. Second order integration with slope limiter. Venkatakrishnan slope-limiting method, with constant: 0.1. The reference element size is: 0.1. Scalar upwind solver (first order) for the turbulence model. First order integration. Average of gradients with correction (viscous flow terms). Average of gradients with correction (viscous turbulence terms). Gradient Computation using weighted Least-Squares method. Artificial compressibility factor: 1. ---------------------- Time Numerical Integration ----------------------- Local time stepping (steady state simulation). Euler implicit method for the flow equations. No CFL adaptation. Courant-Friedrichs-Lewy number:        1 Euler implicit time integration for the turbulence model. ------------------------- Convergence Criteria -------------------------- Maximum number of iterations: 4000. Reduce the density residual 8 orders of magnitude. The minimum bound for the density residual is 10^(-9). Start convergence criteria at iteration 10. -------------------------- Output Information --------------------------- Writing a flow solution every 500 iterations. Writing the convergence history every 1 iterations. The output file format is Tecplot ASCII (.dat). Convergence history file name: history. Forces breakdown file name: forces_breakdown.dat. Surface flow coefficients file name: surface_flow. Flow variables file name: Results. Restart flow file name: restart_flow.dat. ------------------- Config File Boundary Information -------------------- Far-field boundary marker(s): Inlet, Outlet, TopWall. Periodic boundary marker(s): Per1, Per2. Constant heat flux wall boundary marker(s): Blade, Spinner. ---------------------- Read Grid File Information ----------------------- Three dimensional problem. 2759777 points. 7 surface markers. 34994 boundary elements in index 0 (Marker = Blade). 1318 boundary elements in index 1 (Marker = Inlet). 1322 boundary elements in index 2 (Marker = Outlet). 16969 boundary elements in index 3 (Marker = Per1). 16969 boundary elements in index 4 (Marker = Per2). 5388 boundary elements in index 5 (Marker = Spinner). 8056 boundary elements in index 6 (Marker = TopWall). 10565786 tetrahedra. 435120 hexahedra. 1035964 prisms. 63800 pyramids. ------------------------- Geometry Preprocessing ------------------------ Setting point connectivity. Renumbering points (Reverse Cuthill McKee Ordering). Recomputing point connectivity. Setting element connectivity. Checking the numerical grid orientation. Identifying edges and vertices. Computing centers of gravity. Setting the control volume structure. Volume of the computational grid: 2.01e+05. Searching for the closest normal neighbors to the surfaces. Compute the surface curvature. Max K: 1.23e+04. Mean K: 11.2. Standard deviation K: 195. Computing wall distances. Area projection in the z-plane = 4.97. ------------------------- Driver Preprocessing -------------------------- Instantiating a single zone driver for the problem. ------------------------ Iteration Preprocessing ------------------------ Zone 1: Euler/Navier-Stokes/RANS flow iteration. ------------------------- Solver Preprocessing -------------------------- Force coefficients computed using MACH_MOTION. Viscous and Inviscid flow: rho_ref, and vel_ref are based on the free-stream values, p_ref = rho_ref*vel_ref^2. The free-stream value of the pressure is 0. Mach number: 0.0120497, computed using the Bulk modulus. Angle of attack (deg): 90, computed using the the free-stream velocity. Side slip angle (deg): 0, computed using the the free-stream velocity. Reynolds number: 278165, computed using free-stream values. Only dimensional computation, the grid should be dimensional. -- Input conditions: Bulk modulus: 142000 Pa. Artificial compressibility factor: 1 Pa. Free-stream static pressure: 0 Pa. Free-stream total pressure: 0 Pa. Free-stream density: 1.2886 kg/m^3. Free-stream velocity: (0, 0, 4) m/s. Magnitude: 4 m/s. Free-stream viscosity: 1.853e-05 N.s/m^2. Free-stream turb. kinetic energy per unit mass: 0.06 m^2/s^2. Free-stream specific dissipation: 417.248 1/s. -- Reference values: Reference pressure: 20.6176 Pa. Reference density: 1.2886 kg/m^3. Reference velocity: 4 m/s. Reference length: 1 m. Reference viscosity: 5.1544 N.s/m^2. -- Resulting non-dimensional state: Mach number (non-dim): 0.0120497 Reynolds number (non-dim): 278165. Re length: 1 m. Free-stream pressure (non-dim): 0 Free-stream density (non-dim): 1 Free-stream velocity (non-dim): (0, 0, 1). Magnitude: 1 Free-stream viscosity (non-dim): 3.59499e-06 Free-stream turb. kinetic energy (non-dim): 0.00375 Free-stream specific dissipation (non-dim): 104.312 Initialize Jacobian structure (Navier-Stokes). MG level: 0. Initialize Jacobian structure (SST model). ----------------- Integration and Numerics Preprocessing ---------------- Integration Preprocessing. Numerics Preprocessing. Setting dynamic mesh structure. ------------------------------ Begin Solver -----------------------------  Setting rotating frame grid velocities for zone 0.  Rotational origin (x, y, z): ( 0, 0, 0 )  Angular velocity about x, y, z axes: ( 0, 0, 2.76552e+52 ) rad/s  Segmentation fault```
Any idea why the Angular velocity z axes is so high, when it should be 5.81rad/s as specified in .cfg file???

If I use SU2_MSH to adapt the CX100.su2 grid file for periodic boundary conditions the output is:
Code:

```------------------------------------------------------------------------- |    ___ _  _ ___                                                      | |  / __| | | |_  )  Release 4.1.1  "Cardinal"                        | |  \__ \ |_| |/ /                                                      | |  |___/\___//___|  Suite (Mesh Adaptation Code)                      | |                                                                      | ------------------------------------------------------------------------- | SU2 Lead Dev.: Dr. Francisco Palacios, Francisco.D.Palacios@boeing.com| |                Dr. Thomas D. Economon, economon@stanford.edu          | ------------------------------------------------------------------------- | SU2 Developers:                                                      | | - Prof. Juan J. Alonso's group at Stanford University.                | | - Prof. Piero Colonna's group at Delft University of Technology.      | | - Prof. Nicolas R. Gauger's group at Kaiserslautern U. of Technology. | | - Prof. Alberto Guardone's group at Polytechnic University of Milan.  | | - Prof. Rafael Palacios' group at Imperial College London.            | ------------------------------------------------------------------------- | Copyright (C) 2012-2016 SU2, the open-source CFD code.                | |                                                                      | | SU2 is free software; you can redistribute it and/or                  | | modify it under the terms of the GNU Lesser General Public            | | License as published by the Free Software Foundation; either          | | version 2.1 of the License, or (at your option) any later version.    | |                                                                      | | SU2 is distributed in the hope that it will be useful,                | | but WITHOUT ANY WARRANTY; without even the implied warranty of        | | MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU      | | Lesser General Public License for more details.                      | |                                                                      | | You should have received a copy of the GNU Lesser General Public      | | License along with SU2. If not, see <http://www.gnu.org/licenses/>.  | ------------------------------------------------------------------------- ------------------------ Physical Case Definition ----------------------- Input mesh file name: CX100.su2 ----------------------- Grid adaptation strategy ------------------------ Grid modification to run periodic bc problems. -------------------------- Output Information --------------------------- Output mesh file name: CX100_per.su2. Output mesh file name: CX100_per.su2. Restart flow file name: restart_flow.dat. ------------------- Config File Boundary Information -------------------- Far-field boundary marker(s): Inlet, Outlet, TopWall. Periodic boundary marker(s): Per1, Per2. Constant heat flux wall boundary marker(s): Blade, Spinner. ---------------------- Read Grid File Information ----------------------- Three dimensional problem. 2759777 points. 7 surface markers. 34994 boundary elements in index 0 (Marker = Blade). 1318 boundary elements in index 1 (Marker = Inlet). 1322 boundary elements in index 2 (Marker = Outlet). 16969 boundary elements in index 3 (Marker = Per1). 16969 boundary elements in index 4 (Marker = Per2). 5388 boundary elements in index 5 (Marker = Spinner). 8056 boundary elements in index 6 (Marker = TopWall). 10565786 tetrahedra. 435120 hexahedra. 1035964 prisms. 63800 pyramids. ----------------------- Preprocessing computations ---------------------- Setting local point and element connectivity. Check numerical grid orientation. Identify faces, edges and vertices. Set control volume structure. Volume of the computational grid: 201013. -------------------- Setting the periodic boundaries -------------------- Setting the periodic boundary conditions. Checking Per1 boundary against periodic donor, Per2.   Bad match for point 1026073.        Nearest donor distance: 8.5443461700e-09.   Bad match for point 1038733.        Nearest donor distance: 8.5443461700e-09.   Bad match for point 1065889.        Nearest donor distance: 1.7181944039e-08.   Bad match for point 1037906.        Nearest donor distance: 1.7191530396e-08.   Bad match for point 1055474.        Nearest donor distance: 1.7364121476e-08.   .   .   .   Bad match for point 1189530.        Nearest donor distance: 8.3956174894e-09.   Bad match for point 1190592.        Nearest donor distance: 7.2492817214e-09.   Bad match for point 1189506.        Nearest donor distance: 1.3692191254e-08.   Bad match for point 1189453.        Nearest donor distance: 5.3120100478e-09.  !!! Warning !!! Bad matches found. Computation will continue, but be cautious. Number of new points: 11360. Number of new interior elements: 51634. Number of new boundary elements added to preexisting markers: 376. Completed in 165.0100000000 seconds on 1 core. ------------------------- Exit Success (SU2_MSH) ------------------------```
This outputs CX100_per.su2, so if I use this grid file with SU2_CFD I get the following output

Code:

```------------------------------------------------------------------------- |    ___ _  _ ___                                                      | |  / __| | | |_  )  Release 4.1.1  "Cardinal"                        | |  \__ \ |_| |/ /                                                      | |  |___/\___//___|  Suite (Computational Fluid Dynamics Code)        | |                                                                      | ------------------------------------------------------------------------- | SU2 Lead Dev.: Dr. Francisco Palacios, Francisco.D.Palacios@boeing.com| |                Dr. Thomas D. Economon, economon@stanford.edu          | ------------------------------------------------------------------------- | SU2 Developers:                                                      | | - Prof. Juan J. Alonso's group at Stanford University.                | | - Prof. Piero Colonna's group at Delft University of Technology.      | | - Prof. Nicolas R. Gauger's group at Kaiserslautern U. of Technology. | | - Prof. Alberto Guardone's group at Polytechnic University of Milan.  | | - Prof. Rafael Palacios' group at Imperial College London.            | ------------------------------------------------------------------------- | Copyright (C) 2012-2016 SU2, the open-source CFD code.                | |                                                                      | | SU2 is free software; you can redistribute it and/or                  | | modify it under the terms of the GNU Lesser General Public            | | License as published by the Free Software Foundation; either          | | version 2.1 of the License, or (at your option) any later version.    | |                                                                      | | SU2 is distributed in the hope that it will be useful,                | | but WITHOUT ANY WARRANTY; without even the implied warranty of        | | MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU      | | Lesser General Public License for more details.                      | |                                                                      | | You should have received a copy of the GNU Lesser General Public      | | License along with SU2. If not, see <http://www.gnu.org/licenses/>.  | ------------------------------------------------------------------------- ------------------------ Physical Case Definition ----------------------- Incompressible RANS equations. Turbulence model: Menter's SST Performing a dynamic mesh simulation: rotating reference frame. No restart solution, use the values at infinity (freestream). Dimensional simulation. The reference length/area will be computed using y(2D) or z(3D) projection. The reference length (moment computation) is 1. Reference origin (moment computation) is (0, 0, 0). Surface(s) where the force coefficients are evaluated: Blade. Surface(s) plotted in the output file: Blade. Surface(s) belonging to the Fluid-Structure Interaction problem: Input mesh file name: CX100_per.su2 ---------------------- Space Numerical Integration ---------------------- Roe (with entropy fix) solver for the flow inviscid terms. Second order integration with slope limiter. Venkatakrishnan slope-limiting method, with constant: 0.1. The reference element size is: 0.1. Scalar upwind solver (first order) for the turbulence model. First order integration. Average of gradients with correction (viscous flow terms). Average of gradients with correction (viscous turbulence terms). Gradient Computation using weighted Least-Squares method. Artificial compressibility factor: 1. ---------------------- Time Numerical Integration ----------------------- Local time stepping (steady state simulation). Euler implicit method for the flow equations. No CFL adaptation. Courant-Friedrichs-Lewy number:        1 Euler implicit time integration for the turbulence model. ------------------------- Convergence Criteria -------------------------- Maximum number of iterations: 4000. Reduce the density residual 8 orders of magnitude. The minimum bound for the density residual is 10^(-9). Start convergence criteria at iteration 10. -------------------------- Output Information --------------------------- Writing a flow solution every 500 iterations. Writing the convergence history every 1 iterations. The output file format is Tecplot ASCII (.dat). Convergence history file name: history. Forces breakdown file name: forces_breakdown.dat. Surface flow coefficients file name: surface_flow. Flow variables file name: Results. Restart flow file name: restart_flow.dat. ------------------- Config File Boundary Information -------------------- Far-field boundary marker(s): Inlet, Outlet, TopWall. Periodic boundary marker(s): Per1, Per2. Constant heat flux wall boundary marker(s): Blade, Spinner. ---------------------- Read Grid File Information ----------------------- Three dimensional problem. 2749827 points and 21310 ghost points. 9 surface markers. 34994 boundary elements in index 0 (Marker = Blade). 1364 boundary elements in index 1 (Marker = Inlet). 1368 boundary elements in index 2 (Marker = Outlet). 16969 boundary elements in index 3 (Marker = Per1). 16969 boundary elements in index 4 (Marker = Per2). 5539 boundary elements in index 5 (Marker = Spinner). 8189 boundary elements in index 6 (Marker = TopWall). 2 periodic transformations. 10611732 tetrahedra. 435120 hexahedra. 1041592 prisms. 63860 pyramids. ------------------------- Geometry Preprocessing ------------------------ Setting point connectivity. Renumbering points (Reverse Cuthill McKee Ordering). Recomputing point connectivity. Setting element connectivity. Checking the numerical grid orientation. The surface element (1, 1325) doesn't have an associated volume element.```
Has anyone experienced anything similar with SU2 in the past?

Kind regards,
Kishore

 talbring June 1, 2016 10:23

Hi Kishore,

as far as I know, the incompressible solver is currently not able to handle a rotating frame (at least the additional terms are not included in the flux computation).

You could try to use the compressible solver.

However, this will not solve your problem with the periodic boundaries.
What exactly is the difference between the first run and the third one ?

Tim

 k.vimalakanthan June 1, 2016 12:59

Quote:
 Originally Posted by talbring (Post 602853) Hi Kishore, as far as I know, the incompressible solver is currently not able to handle a rotating frame (at least the additional terms are not included in the flux computation). You could try to use the compressible solver. However, this will not solve your problem with the periodic boundaries. What exactly is the difference between the first run and the third one ? Tim
Hi Tim,

The differences are that the first run was performed with the grid directly from pointwise 'CX100.su2' without any pre-processing for SU2 periodic simulation (halo cells, renumbering etc.), while the second run was performed with the grid outputted from the SU2_MSH 'CX100_pre.su2' - grid adapted for periodic boundaries.

Have you or anyone successfully simulated a 3D periodic problem in SU2 using the grid from pointwise?

Kind regards,
Kishore

 Jiba June 1, 2016 13:38

Hi,

I tried to run your grid, but the file seems different, as there are only 5 markers and they are named:
MARKER_ELEMS= 34994
MARKER_TAG= Farfield
MARKER_ELEMS= 8944
MARKER_TAG= Per1
MARKER_ELEMS= 7393
MARKER_TAG= Per2
MARKER_ELEMS= 7393
MARKER_TAG= Spinner
MARKER_ELEMS= 5388

I modified cfg file accordingly and the output of SU2_MSH gave log similar to yours with the following ending lines:

Quote:
 Number of new points: 4878. Number of new interior elements: 23049. Number of new boundary elements added to preexisting markers: 329.
Running SU2_CFD computes as angular velocity ( nan, nan, inf)
I'm using release 4.1.2

 k.vimalakanthan June 1, 2016 14:15

Quote:
 Originally Posted by Jiba (Post 602879) Hi, I tried to run your grid, but the file seems different, as there are only 5 markers and they are named: MARKER_TAG= Blade MARKER_ELEMS= 34994 MARKER_TAG= Farfield MARKER_ELEMS= 8944 MARKER_TAG= Per1 MARKER_ELEMS= 7393 MARKER_TAG= Per2 MARKER_ELEMS= 7393 MARKER_TAG= Spinner MARKER_ELEMS= 5388 I modified cfg file accordingly and the output of SU2_MSH gave log similar to yours with the following ending lines: Running SU2_CFD computes as angular velocity ( nan, nan, inf) I'm using release 4.1.2
Hi Jiba,

I realised that I uploaded the wrong grid file and updated the link above this morning with the grid shown in the images, maybe you were using the old link. Regardless as you've already found out, they only vary in the boundary names.

Its interesting that your are getting up to the angular velocity output from SU2_CFD, so the SU2_MSH in v4.1.2 is better at adapting periodic boundaries for this grid than the v4.1.1. Because my run failed on "The surface element (1, 1325) doesn't have an associated volume element.". Did you get bad matches too from SU2_MSH?

I'm glad we got progress with handling the grid, maybe as Tim said we need to try the compressible solver to get the rotating frame and the periodic BCs to work?

My next step will be to get v4.1.2 and set-up a compressible case..maybe with very low mach numbers to skip any compressibility effects? - adjust the fluid models so it computes the same density for all pressure and temperatures perhaps. maybe I can do isothermal compressible simulation? where we change the fluid model to set same density for all pressures...I'm sure there is more to it than that...

Has anyone tried to compute a incompressible solution using the compressible SU2 solver?

Thanks a lot,
Kind regards,
Kishore

 ymc11 June 1, 2016 23:13

Quote:
Hi Kishore,

For the bad matches in SU2_MSH, since the nearest donor distance is about 1e-8 level, which is close to the truncation error of single precision, I think you could try to output the mesh with double-precision in Pointwise. Besides,you could also adjust the tolerance in function CPhysicalGeometry::SetPeriodicBoundary,which is currently 1e-10, and changing it to 1e-8 may be helpful in this case.

Muchen

 k.vimalakanthan June 2, 2016 12:59

Quote:
 Originally Posted by ymc11 (Post 602934) Hi Kishore, For the bad matches in SU2_MSH, since the nearest donor distance is about 1e-8 level, which is close to the truncation error of single precision, I think you could try to output the mesh with double-precision in Pointwise. Besides,you could also adjust the tolerance in function CPhysicalGeometry::SetPeriodicBoundary,which is currently 1e-10, and changing it to 1e-8 may be helpful in this case. Muchen
Hi Muchen,

Many thanks for your advice. The grids were generated with double double-precision, so maybe that is the maximum matches I could get from Pointwise?

So from what I understand if I have grids with 1e-8 or more bad match I can set CPhysicalGeometry::SetPeriodicBoundary to higher values to not allow CFD_MSH to modify the location of the grid elements but still renumber them for periodic BC?

Kind regards,
Kishore

 ymc11 June 3, 2016 03:20

Quote:
 Originally Posted by k.vimalakanthan (Post 603143) Hi Muchen, Many thanks for your advice. The grids were generated with double double-precision, so maybe that is the maximum matches I could get from Pointwise? So from what I understand if I have grids with 1e-8 or more bad match I can set CPhysicalGeometry::SetPeriodicBoundary to higher values to not allow CFD_MSH to modify the location of the grid elements but still renumber them for periodic BC? Kind regards, Kishore
Hi Kishore,

Actually, no matter what the tolerance is, for each point on the periodic boundaries, the SU2_MSH command would still find its nearest point after the transformation defined in the config file and set it as the donor point . Since this is a point-to-point approach, it is best to create identical meshes on the two periodic boundaries, which means that these two meshes could completely overlap with each other after certain translation or rotation.
Besides, you could always check the "periodic_halo.dat" to see if the halo cells are created successfully.

Muchen

 k.vimalakanthan June 16, 2016 08:52

Quote:
 Originally Posted by ymc11 (Post 603238) Hi Kishore, Actually, no matter what the tolerance is, for each point on the periodic boundaries, the SU2_MSH command would still find its nearest point after the transformation defined in the config file and set it as the donor point . Since this is a point-to-point approach, it is best to create identical meshes on the two periodic boundaries, which means that these two meshes could completely overlap with each other after certain translation or rotation. Besides, you could always check the "periodic_halo.dat" to see if the halo cells are created successfully. Muchen
Hi Muchen,

In Pointwise, I did make surface mesh for both periodic boundaries to be identical (1:1) - the surface mesh from one side was rotated and the volumes were generated between them to make it easy for SU2_MSH. Maybe there is some tolerance issue with the copy/rotation in pointwise...

Still haven't tried the compressible solver with this grid, hopefully with the newer version V4.2 everything run smoothly....

Kind regards,
Kishore

 jywang June 16, 2016 09:41

Hi Kishore,

I am also working on the 3d Periodic BCs for rotor simulation using SU2. the link to download your grid isn't available anymore, could you please update it again? And I want try your run to see what happen.

Thanks!

 k.vimalakanthan June 17, 2016 04:45

Quote:
 Originally Posted by jywang (Post 605201) Hi Kishore, I am also working on the 3d Periodic BCs for rotor simulation using SU2. the link to download your grid isn't available anymore, could you please update it again? And I want try your run to see what happen. Thanks!
Hi jywang,

Can you please post your configuration file that we already have for a 3D periodic rotor cases? and any improvements you suggest for this case.

Any help is greatly appreciated,
Kind regards,
Kishore

 jywang June 20, 2016 05:27

Hi Kishore,

Now I am trying to run the Caradonna&Tung case using 3D rotating periodic BC, the procedures are:

1. Output the su2 mesh from pointwise.

2. Set up the configuration file, the periodic boundary and grid adaption parts are:

% Periodic boundary marker(s) (NONE = no marker)
% Format: ( periodic marker, donor marker, rot_cen_x, rot_cen_y, rot_cen_z, rot_angle_x-axis, rot_angle_y-axis, rot_angle_z-axis, translation_x, translation_y, translation_z)
MARKER_PERIODIC= ( per1, per2, 0.0, 0.0, 0.0, 0.0, 0.0, 180.0, 0.0, 0.0, 0.0)
% ------------------------- GRID ADAPTATION STRATEGY --------------------------%
%
% Kind of grid adaptation (NONE, PERIODIC)

3. Execute the SU2_MSH to output su2 grid with periodic halo element

4. Running the SU2_CFD using new su2 grid from step 3.

However, there are two types of error are occurred at the last step.

The first one is new halo element boundary surface cannot find associated element, the error information is
"Checking the numerical grid orientation.
The surface element (1, 10691) doesn't have an associated volume element. "
This surface (1,10691) is a new boundary surface created in step 3.

I have tested several grids for this case, and some grids could pass the step where the first error was occurred, but still cannot be start running. I think the second error is about MPI sending/receiving, the error information is segmentation fault when I executed the SU2_CFD in parallel. And the code can run several steps in serial execution, but the segmentation error will be occurred when the master node merge coordinates at solution writing out step.

These are the errors and information I got using 3d rotation periodic BC, and maybe we can discuss about it.

Thanks!

 k.vimalakanthan February 8, 2019 14:43

Final report on modelling Wind turbine using SU2 and OpenFOAM

Hi All,

I've managed to put together the steps and settings for wind turbine simulation using SU2 and OpenFOAM. It also includes some validation for the mexico rotor.

http://publications.tno.nl/publicati...018-R11648.pdf