[PavanPal01]

When I try to run SU2 I faced with this error.
I have selected all my boundary conditions as markers.
Any guidance would be greatly appreciated.

[TKatt]

Hi,


in case you use a .su2 mesh please attach it here if possible. Having 0 elements and volume points is also not really perfect


In case you didn't do it yet please check with https://su2code.github.io/docs_v7/Mesh-File/ whether your mesh looks correctly build.


Maybe that already helps a bit, Tobi

[PavanPal01]

Thank you very much for your reply,

I am now facing another error Mismatch between NPOIN and number of points listed in mesh file. Do you have any advice for this?
I have seen other forum posts which say unselecting "save all elements" when exporting the mesh to a .su2 file solves this but it never worked for me.
I couldn't attach my .su2 file as it was too large of a file. I have attached the new error I am facing.

Once again any guidance will be appreciated.

[bigfootedrockmidget]

the NPOIN mismatch typically happens when exporting from gmsh. gmsh has created points that are not part of the final mesh. To prevent gmsh from saving points that are not part of the final mesh, you should deselect 'save all elements'. You should also make sure that the remaining points are in fact part of the mesh by defining (in gmsh) a surface or volume that contain the mesh points and elements.



Are you using gmsh?

[PavanPal01]

Hi,
Yes I'm using gmsh. I deselected "save all elements" when exporting as a .su2 and I'm certain that the remaining points are part of the mesh but I still have the NPOIN mismatch error.

// Gmsh project created on Wed Nov 10 21:01:41 2021
SetFactory("OpenCASCADE");
//+
Point(1) = {0, 0, 0, 1.0};
//+
Point(2) = {2, 0, 0, 1.0};
//+
Point(3) = {2, 0.5, 0, 1.0};
//+
Point(4) = {1, 0.5, 0, 1.0};
//+
Line(1) = {1, 2};
//+
Line(2) = {2, 3};
//+
Line(3) = {3, 4};
//+
Point(5) = {0.5, 0.5, 0, 1.0};
//+
BSpline(4) = {4, 5, 1};
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
Curve{4}; Curve{3}; Curve{2};
}
//+
Point(8) = {2, 5, 0, 1.0};
//+
Point(9) = {2, 0, 5, 1.0};
//+
Line(11) = {2, 8};
//+
Line(12) = {2, 9};
//+
Circle(13) = {9, 2, 8};
//+
Extrude {-7, 0, 0} {
Curve{12}; Curve{13}; Curve{11};
}

//+
Delete {
Surface{3};
}

//+
Delete {
Surface{4};
}
//+
Delete {
Surface{6};
}
//+
Delete {
Surface{5};
}
//+
Line(20) = {9, 7};
//+
Delete {
Curve{10};
}
//+
Delete {
Curve{12};
}
//+
Line(21) = {1, 10};
//+
Delete {
Curve{1};
}
//+
Delete {
Curve{14};
}
//+
Line(22) = {3, 8};
//+
Delete {
Curve{2};
}
//+
Delete {
Curve{11};
}
//+
Curve Loop(7) = {19, -18, -16};
//+
Plane Surface(3) = {7};
//+
Curve Loop(8) = {21, 16, -15, 20, 9, 7};
//+
Plane Surface(4) = {8};
//+
Curve Loop(9) = {22, -13, 20, -8};
//+
Plane Surface(5) = {9};
//+
Curve Loop(10) = {13, 17, -18, -15};
//+
Plane Surface(6) = {10};
//+
Curve Loop(11) = {22, 17, -19, -21, -4, -3};
//+
Plane Surface(7) = {11};
//+
Physical Surface("INLET_FAR_FIELD", 25) = {3};
//+
Physical Surface("SIDE_FAR_FIELD", 26) = {7};
//+
Physical Surface("OUTLET_FAR_FIELD", 27) = {5};
//+
Physical Surface("TOP_FAR_FIELD", 28) = {6};
//+
Physical Surface("BOTTOM_FAR_FIELD", 29) = {4};
//+
Surface Loop(1) = {7, 5, 6, 3, 4, 2, 1};
//+
Volume(1) = {1};
//+
Physical Volume("FAR_FIELD", 30) = {1};
//+
Transfinite Curve {4, 7, 5, 9, 8, 3} = 100 Using Progression 1;
//+
Transfinite Curve {21} = 100 Using Progression 1.1;
//+
Transfinite Curve {20} = 100 Using Progression 0.9;
//+
Transfinite Curve {22} = 100 Using Progression 1.1;
//+
Physical Surface("OGIVE", 31) = {1};
//+
Physical Surface("CYLINDER", 32) = {2};
//+
Recursive Delete {
Point{2};
}
//+
Recursive Delete {
Point{5};
}

This is my gmsh code, I hope you can help me

[TKatt]

You also need to define a Physical Volume. See also here for a little more explanation https://stackoverflow.com/questions/...13327#69713327

[PavanPal01]

Hi,
I deleted the physical volume and then re-added it. I now have the yellow sphere in my far field indicating the volume.
However, I Still have a mismatch error.
Do you have anymore advice you could give me?

Thank you very much for what you have done already,
Pavan

[bigfootedrockmidget]

to pinpoint where the problem is, you can use a small piece of python code to find which points are not used.

Originally Posted by bigfootedrockmidget

This is usually because additional supporting points are saved that were used for e.g. defining circles.

The solution is to put the entire mesh surface (2D) or mesh volume (3D) into a physical group and then when saving you have to unselect the 'save all elements' option.

here is a piece of python code that you can use to check if you have unused points in your point list. You can copy-paste this into a jupyter labs session.

filename="bend.su2"
 def getnpoints():
    npoints=0
    with open(filename) as f:
        
        for line in f:
            l=line[0:4]
            if l=="NPOI":
                npoints=line.split()[1]
                print(npoints)
                break
    f.close()
    return (npoints)



# now loop over elements and check which points are used in the mesh
def getunusedpoints():
    numberarray=list(range(0,npoints))
    print("len=",len(numberarray))
    print(numberarray[1:4])
    nelems=0
    with open(filename) as f:
        line = f.readline()
        line = f.readline()
        if line[0:4]=="NELE":
            nelems=int(line.split()[1])
            print("number of elements=",nelems)
            
        counter=0
        for line in f:
            l = line.split()
            for i in range(1,len(l)-1):
                try:
                    numberarray[int(l[i])]=-1 
                except:
                    # do nothing
                    numberarray
                    
            if counter==nelems:
                break
            counter=counter+1
    
    unusedpointsarray=[]
    for i in numberarray:
        if i != -1:
            unusedpointsarray.append(i)            
    return(unusedpointsarray)


npoints = int(getnpoints())
print("number of points =",npoints)
 p = getunusedpoints()

[TKatt]

I overlooked that you already have a physical volume ... my bad


The MARKER_INTERNAL is suspicious. Can you please remove those and only have OGIVE and CYLINDER as MARKER_HEATFLUX

[TKatt]

If you like you can also attach your .cfg here so I can take a look

[PavanPal01]

Hi there,
here is my .cfg file

 %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%                                                                              %
% SU2 configuration file                                                       %
% Case description: Ogive-Cylinder		    	      			   %
% Author: Pavan Pal  														   %
% Institution: Univesity of Strathclyde								   %
% Date: 02th Nov 2021                                                          %
% File Version                                                %
%                                                                              %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Solver type (EULER, NAVIER_STOKES, RANS,
%                               INC_EULER, INC_NAVIER_STOKES, INC_RANS,
%                                NEMO_EULER, NEMO_NAVIER_STOKES,
%                               FEM_EULER, FEM_NAVIER_STOKES, FEM_RANS, FEM_LES,
%                               HEAT_EQUATION_FVM, ELASTICITY)
SOLVER= RANS
%
% Specify turbulence model (NONE, SA, SA_NEG, SST, SA_E, SA_COMP, SA_E_COMP, SST_SUST)
KIND_TURB_MODEL= SA
%
% Mathematical problem (DIRECT, CONTINUOUS_ADJOINT, DISCRETE_ADJOINT)
MATH_PROBLEM= DIRECT
%
% Restart solution (NO, YES)
RESTART_SOL= NO
%
SYSTEM_MEASUREMENTS= SI
%
% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------%
%
% Mach number (non-dimensional, based on the free-stream values)
MACH_NUMBER= 0.086
%
% Angle of attack (degrees, only for compressible flows)
AOA= 0.00
%
% Free-stream option to choose between density and temperature (default) for
% initializing the solution (TEMPERATURE_FS, DENSITY_FS)
FREESTREAM_OPTION= TEMPERATURE_FS
%
% Free-stream pressure (101325.0 N/m^2, 2116.216 psf by default)
FREESTREAM_PRESSURE= 101742.9
%
% Free-stream temperature (288.15 K, 518.67 R by default)
FREESTREAM_TEMPERATURE= 301.4
%
% Free-stream density (1.2886 Kg/m^3, 0.0025 slug/ft^3 by default)
%FREESTREAM_DENSITY= 1.176
%
% Free-stream Turbulence Intensity
FREESTREAM_TURBULENCEINTENSITY = 0.5
%
% Reynolds number (non-dimensional, based on the free-stream values)
REYNOLDS_NUMBER= 171689.5566
%
% Reynolds length (1 m, 1 inch by default)
REYNOLDS_LENGTH= 1
%
% Init option to choose between Reynolds (default) or thermodynamics quantities
% for initializing the solution (REYNOLDS, TD_CONDITIONS)
INIT_OPTION= TD_CONDITIONS
%
% Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE,
%                              FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE)
REF_DIMENSIONALIZATION= DIMENSIONAL
%
% ---------------------- REFERENCE VALUE DEFINITION ---------------------------%
%
% Reference origin for moment computation (m or in)
REF_ORIGIN_MOMENT_X = 0.00
REF_ORIGIN_MOMENT_Y = 0.00
REF_ORIGIN_MOMENT_Z = 0.00
%
% Reference length for moment non-dimensional coefficients (m or in)
REF_LENGTH= 1
%
% Reference area for non-dimensional force coefficients (0 implies automatic
% calculation) (m^2 or in^2)
REF_AREA= 0
%
% ------------------------------ EQUATION OF STATE ----------------------------%
%
% Different gas model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS)
FLUID_MODEL= IDEAL_GAS
%
% Ratio of specific heats (1.4 default and the value is hardcoded
%                          for the model STANDARD_AIR)
GAMMA_VALUE= 1.4
%
% Specific gas constant (287.058 J/kg*K default and this value is hardcoded 
%                        for the model STANDARD_AIR)
GAS_CONSTANT= 287.06
%
% --------------------------- VISCOSITY MODEL ---------------------------------%
%
% Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY, POLYNOMIAL_VISCOSITY).
VISCOSITY_MODEL= SUTHERLAND
%
% Molecular Viscosity that would be constant (1.716E-5 by default)
MU_CONSTANT= 1.716E-5
%
% Sutherland Viscosity Ref (1.716E-5 default value for AIR SI)
MU_REF= 1.716E-5
%
% Sutherland Temperature Ref (273.15 K default value for AIR SI)
MU_T_REF= 273.15
%
% Sutherland constant (110.4 default value for AIR SI)
SUTHERLAND_CONSTANT= 110.4
%
% --------------------------- THERMAL CONDUCTIVITY MODEL ----------------------%
%
%
% ----------------------- DYNAMIC MESH DEFINITION -----------------------------%
%
% Type of dynamic mesh (NONE, RIGID_MOTION, ROTATING_FRAME,
%                       STEADY_TRANSLATION,
%                       ELASTICITY, GUST)
GRID_MOVEMENT= ROTATING_FRAME
%
% Motion mach number (non-dimensional). Used for initializing a viscous flow
% with the Reynolds number and for computing force coeffs. with dynamic meshes.
MACH_MOTION= 0.3456
%
% Coordinates of the motion origin
MOTION_ORIGIN= 0.0 0.0 0.0
%
% Angular velocity vector (rad/s) about the motion origin
ROTATION_RATE = -573.717 0.0 0.0
%
% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
%
% Navier-Stokes (no-slip), constant heat flux wall  marker(s) (NONE = no marker)
% Format: ( marker name, constant heat flux (J/m^2), ... )
MARKER_HEATFLUX= ( CYLINDER, 0.0, OGIVE, 0.0)
%
%
% Far-field boundary marker(s) (NONE = no marker)
MARKER_FAR= (TOP_FAR_FIELD, BOTTOM_FAR_FIELD, SIDE_FAR_FIELD )
%
% Internal boundary marker(s) e.g. no boundary condition (NONE = no marker)
MARKER_INTERNAL= (CYLINDER, OGIVE)
%
% Inlet boundary type (TOTAL_CONDITIONS, MASS_FLOW)
INLET_TYPE= TOTAL_CONDITIONS
%
% Inlet boundary marker(s) with the following formats (NONE = no marker)
% Total Conditions: (inlet marker, total temp, total pressure, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Mass Flow: (inlet marker, density, velocity magnitude, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Inc. Velocity: (inlet marker, temperature, velocity magnitude, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
% Inc. Pressure: (inlet marker, temperature, total pressure, flow_direction_x,
%           flow_direction_y, flow_direction_z, ... ) where flow_direction is
%           a unit vector.
MARKER_INLET= ( INLET_FAR_FIELD, 301.4, 102272.6278, 1.0, 0.0, 0.0)
%
% Outlet boundary marker(s) (NONE = no marker)
% Compressible: ( outlet marker, back pressure (static thermodynamic), ... )
% Inc. Pressure: ( outlet marker, back pressure (static gauge in Pa), ... )
% Inc. Mass Flow: ( outlet marker, mass flow target (kg/s), ... )
MARKER_OUTLET= ( OUTLET_FAR_FIELD, 101742.9)
%
% Periodic boundary marker(s) (NONE = no marker)
% Format: ( periodic marker, donor marker, rotation_center_x, rotation_center_y,
% rotation_center_z, rotation_angle_x-axis, rotation_angle_y-axis,
% rotation_angle_z-axis, translation_x, translation_y, translation_z, ... )
%MARKER_PERIODIC= ( PERIODIC_1, 0.0, 0.0, 0.0, 90.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0)
%
%
% ------------------------ SURFACES IDENTIFICATION ----------------------------%
%
% Marker(s) of the surface in the surface flow solution file
MARKER_PLOTTING= (CYLINDER, OGIVE)
%
% Marker of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= (CYLINDER, OGIVE)
%
% ------------------------- GRID ADAPTATION STRATEGY --------------------------%
%
% Kind of grid adaptation (NONE, PERIODIC, FULL, FULL_FLOW, GRAD_FLOW,
%                          FULL_ADJOINT, GRAD_ADJOINT, GRAD_FLOW_ADJ, ROBUST,
%                          FULL_LINEAR, COMPUTABLE, COMPUTABLE_ROBUST,
%                          REMAINING, WAKE, SMOOTHING, SUPERSONIC_SHOCK)
%
% Percentage of new elements (% of the original number of elements)

%
% Scale factor for the dual volume
%
% Adapt the boundary elements (NO, YES)
% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------%
%
% Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES)
NUM_METHOD_GRAD= WEIGHTED_LEAST_SQUARES
%
% CFL number (initial value for the adaptive CFL number)
CFL_NUMBER= 1.0
%
% 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= ( 0.1, 1.2, 10.0, 100.0 )
%
% Runge-Kutta alpha coefficients
RK_ALPHA_COEFF= ( 0.66667, 0.66667, 1.000000 )
%
% ------------------------ LINEAR SOLVER DEFINITION ---------------------------%
%
% Linear solver or smoother for implicit formulations:
% BCGSTAB, FGMRES, RESTARTED_FGMRES, CONJUGATE_GRADIENT (self-adjoint problems only), SMOOTHER.
LINEAR_SOLVER= FGMRES
%
% Preconditioner of the Krylov linear solver or type of smoother (ILU, LU_SGS, LINELET, JACOBI)
LINEAR_SOLVER_PREC= ILU
%
% 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= 4.0
%
% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, JST_KE, JST_MAT, LAX-FRIEDRICH, CUSP, ROE, AUSM,
%                              AUSMPLUSUP, AUSMPLUSUP2, AUSMPWPLUS, HLLC, TURKEL_PREC,
%                              SW, MSW, FDS, SLAU, SLAU2, L2ROE, LMROE)
CONV_NUM_METHOD_FLOW= JST
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the flow equations.
%           Required for 2nd order upwind schemes (NO, YES)
MUSCL_FLOW= YES
%
% Slope limiter (VENKATAKRISHNAN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN
%
% Coefficient for the limiter
VENKAT_LIMITER_COEFF= 0.03
%
% 2nd and 4th order artificial dissipation coefficients
JST_SENSOR_COEFF= ( 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
%
% Monotonic Upwind Scheme for Conservation Laws (TVD) in the turbulence equations.
%           Required for 2nd order upwind schemes (NO, YES)
MUSCL_TURB= NO
%
% Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG,
%                BARTH_JESPERSEN, VAN_ALBADA_EDGE)
SLOPE_LIMITER_TURB= VENKATAKRISHNAN
%
% Time discretization (EULER_IMPLICIT)
TIME_DISCRE_TURB= EULER_IMPLICIT
%
% Reduction factor of the CFL coefficient in the turbulence problem
CFL_REDUCTION_TURB= 0.5
%
% --------------------- HEAT NUMERICAL METHOD DEFINITION ----------------------%
%
% ------------------------------- SOLVER CONTROL ------------------------------%
%
% Convergence criteria (CAUCHY, RESIDUAL)
CONV_CRITERIA= RESIDUAL
%
% Min value of the residual (log10 of the residual)
CONV_RESIDUAL_MINVAL= -9
%
% Start convergence criteria at iteration number
CONV_STARTITER= 10
%
% Number of elements to apply the criteria
%CONV_CAUCHY_ELEMS= 100
%
% Epsilon to control the series convergence
%CONV_CAUCHY_EPS= 1E-4
%
% Convergence field 
CONV_FIELD= RMS_DENSITY
%
% Number of total iterations
ITER= 500
%
%
% ----------- SLOPE LIMITER AND DISSIPATION SENSOR DEFINITION -----------------%
%
% -------------------------- MULTIGRID PARAMETERS -----------------------------%
%
% Multi-Grid Levels (0 = no multi-grid)
MGLEVEL= 0
%
% Multi-grid cycle (V_CYCLE, W_CYCLE, FULLMG_CYCLE)
MGCYCLE= W_CYCLE
%
% Multi-Grid PreSmoothing Level
MG_PRE_SMOOTH= ( 1, 2, 3, 3 )
%
% Multi-Grid PostSmoothing Level
MG_POST_SMOOTH= ( 0, 0, 0, 0 )
%
% Jacobi implicit smoothing of the correction
MG_CORRECTION_SMOOTH= ( 0, 0, 0, 0 )
%
% Damping factor for the residual restriction
MG_DAMP_RESTRICTION= 0.95
%
% Damping factor for the correction prolongation
MG_DAMP_PROLONGATION= 0.95

% ------------------------- INPUT/OUTPUT FILE INFORMATION --------------------------%
%
% Mesh input file
MESH_FILENAME= cylinderbrandnew.su2
%
% Mesh input file format (SU2, CGNS)
MESH_FORMAT= SU2
%
% Mesh output file
MESH_OUT_FILENAME= mesh_out.su2
%
% Restart flow input file
SOLUTION_FILENAME= restart_flow.dat
%
% Restart adjoint input file
SOLUTION_ADJ_FILENAME= solution_adj.dat
%
% Output tabular file format (TECPLOT, CSV)
TABULAR_FORMAT= CSV
%
% Files to output 
% Possible formats : (TECPLOT, TECPLOT_BINARY, SURFACE_TECPLOT,
%  SURFACE_TECPLOT_BINARY, CSV, SURFACE_CSV, PARAVIEW, PARAVIEW_BINARY, SURFACE_PARAVIEW, 
%  SURFACE_PARAVIEW_BINARY, MESH, RESTART_BINARY, RESTART_ASCII, CGNS, STL)
% default : (RESTART, PARAVIEW, SURFACE_PARAVIEW)
OUTPUT_FILES= (RESTART, TECPLOT, SURFACE_TECPLOT, CSV, CGNS)
%
% Output file convergence history (w/o extension)
CONV_FILENAME= history
%
% Output file restart flow
RESTART_FILENAME= restart_flow.dat
%
% Output file restart adjoint
RESTART_ADJ_FILENAME= restart_adj.dat
%
% Output file flow (w/o extension) variables
VOLUME_FILENAME= flow
%
% Output file adjoint (w/o extension) variables
VOLUME_ADJ_FILENAME= adjoint
%
% Output Objective function
VALUE_OBJFUNC_FILENAME= of_eval.dat
%
% Output objective function gradient (using continuous adjoint)
GRAD_OBJFUNC_FILENAME= of_grad.dat
%
% Output file surface flow coefficient (w/o extension)
SURFACE_FILENAME= surface_flow
%
% Output file surface adjoint coefficient (w/o extension)
SURFACE_ADJ_FILENAME= surface_adjoint
%
% Writing solution file frequency
OUTPUT_WRT_FREQ= 20
%
% Writing convergence history frequency
%
%Writing the forces_breakdown.dat file for the coefficients
WRT_FORCES_BREAKDOWN = YES
%
% Read binary restart files (YES, NO)
READ_BINARY_RESTART= NO
%Screen Ouput
HISTORY_OUTPUT = (ITER, RMS_RES, AERO_COEFF)

[PavanPal01]

I have also re-made my mesh the following way but still the mismatch error appears:

// Gmsh project created on Fri Nov 19 15:20:57 2021
SetFactory("OpenCASCADE");
//+
Point(1) = {0, 0, 0, 1.0};
//+
Point(2) = {5, 0, 0, 1.0};
//+
Point(3) = {6, 0.5, 0, 1.0};
//+
Point(4) = {7, 0.5, 0, 1.0};
//+
Point(5) = {7, 5, 0, 1.0};
//+
Point(6) = {0, 5, 0, 1.0};
//+
Point(7) = {5.5, 0.5, 0, 1.0};
//+
Line(1) = {6, 1};
//+
Line(2) = {1, 2};
//+
Line(3) = {4, 5};
//+
Line(4) = {5, 6};
//+
Line(5) = {3, 4};
//+
BSpline(6) = {3, 7, 2};
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Curve{1}; Curve{4}; Curve{2}; Curve{6}; Curve{3}; Curve{5}; 
}
//+
Physical Surface("OUTLET_FAR_FIELD", 17) = {4};
//+
Physical Surface("INLET_FAR_FIELD", 18) = {1};
//+
Physical Surface("TOP_FAR_FIELD", 19) = {2};
//+
Physical Surface("OGIVE", 20) = {3};
//+
Physical Surface("CYLINDER", 21) = {5};
//+
Curve Loop(6) = {3, 4, 1, 2, -6, 5};
//+
Plane Surface(6) = {6};
//+
Curve Loop(7) = {2, -13, 16, 15, 10, 8};
//+
Plane Surface(7) = {7};
//+
Physical Surface("SIDE_FAR_FIELD", 22) = {6};
//+
Physical Surface("BOTTOM_FAR_FIELD", 23) = {7};
//+
Surface Loop(1) = {4, 5, 3, 6, 2, 7, 1};
//+
Volume(1) = {1};
//+
Physical Volume("FLUID", 24) = {1};
//+
Transfinite Curve {13, 6, 11, 5, 16, 14} = 100 Using Progression 1;
//+
Transfinite Curve {2} = 100 Using Progression 0.9;
//+
Transfinite Curve {3} = 71 Using Progression 1.1;
//+
Transfinite Curve {15} = 71 Using Progression 1.1;

[PavanPal01]

Hi, I was wondering if you had any other advice you could give me.
I am still getting the mismatch error but I do not understand why.
I have 26489 volume elements and on my .SU2 file the volume elements go from 0-26488 meaning there are 26489 elements in total.
There are also 74509 points and on the .SU2 file the points go from 0-74508.
Are there any other ways I can check where this error is coming from?

[TKatt]

For the NPOIN mismatch maybe try adding 'Coherence;' and/or 'Coherence Mesh;' to the script .. removing duplicate (mesh) points.
So the normal Coherence before the meshing and Coherence Mesh after it.


So you might wanna add

Coherence;
Mesh 1; Mesh 2;
Coherence Mesh;

to the end of your gmsh script to do that and the meshing when calling the script





Just search the words here https://gmsh.info/doc/texinfo/gmsh.html for more info