[Shruti Arumbakkam]

Dear Sir/madam/anyone who might be able to help,

I recently started using SU2 to perform incompressible CFD analysis on a custom wing our research group made--the way I have the simulation set up right now is pretty much quite similar to the inviscid ONERA M6 example on the SU2 website, in terms of the placement of my wing in the geometry that's being meshed. If anyone could help answer my questions, I'd be very grateful:

1) When I tried to run the simulation, I got the following error:

Error in "void CPhysicalGeometry:istributeColoring(CConfig*, CGeometry*)":
-------------------------------------------------------------------------
Mismatch between NPOIN and number of points listed in mesh file.
Please check the mesh file for correctness.

On manually checking my mesh file, I did not find any discrepancy between the number of points stated in the file and the number of points there actually were (I just subtracted the line numbers between where the first line where the points started and where the last point was listed). What could be the problem? I couldn't really think of what was going wrong here

2) I'm trying to simulate the model with viscosity, and so I have the following markers:
Inlet (specified with temperature, and a velocity in the +ve x direction)
Outlet(specified with just atmospheric pressure)
Far-field (I used all the walls of my box expect the symmetry wall for this marker)
Symmetry (just the wall that is touched by the root of my wing)
Heatflux (my wing surface)
Plotting (wing surface)
Monitoring (wing surface)

Is that definition correct/ am I on the right track? Are those the correct things to specify/is there anything else I should add/remove?

Thank you so much to whomever can help me; I would be extremely grateful

[pcg]

Can you upload the mesh?

[trushant]

Hey Shruti -

Were you able to solve this problem ? I am having the same problem.

Pedro - I have attached my mesh file. Basically, I was trying to do a tutorial from one of the files online. It used .geo file with gmsh software for getting the .su2 mesh file. I modified the geometry file to include a spline from a number of lines in the nozzle contour. The original case works perfectly fine, but the modified one doesn't. I am also attaching my geometry file for gmsh. Can you please take a look and see if anything is wrong.

Thanks a lot,
Trushant Patel

[trushant]

Never mind. Found my mistake.

Upon close inspection, I saw that Gmsh was exporting the points used in construction of spline in the NPOINTS of SU2 mesh, but wasn't using those points in construction of NELEMENTS. So, I created a Physical space of the surface, and then exported it to SU2 format without checking the box of 'Save all'. And it did the trick for me.

Thanks anyways!!!

Sincerely,
Trushant Patel

[Shruti Arumbakkam]

Hi Trushant!

I am sorry for not getting back to you sooner, but I believe I fixed it in the same way! I fixed it a while ago and do not exactly remember how I did it, but what you described sounds right!

Thank you!

[AlphaSierra]

Hey Trushant,

I'm facing a similar problem. I have a face in my geometry created for the purpose of refining and structuring the mesh. So naturally, I don't want to associate any physical surface with it. Can you please tell me how you were able to fix the error? I tried assigning a physical surface to the face and exporting to SU2 format by unchecking save all elements but SU2 gives me an error saying I haven't defined this new marker. Thanks in advance.

[trushant]

Hey Anjay,

I am not very sure on what you are doing wrong. Make sure you don't miss any surfaces or edges when creating the mesh.

Mine was a 2D case. I meshed it with GMsh and used plane surface, and physical surface to define the domain. I also identified all the edges where I give my boundary conditions. The problem I had was GMsh was exporting extra points which were related to spline but weren't used in the cell connectivity.

One extra thing to check would be to open the su2 file and check the connectivity manually to see if everything is okay. If your mesh is too large, I would suggest making a smaller mesh to check.

Hope it helps.

Thanks,
Trushant Patel

[AlphaSierra]

Hey Trushant,

Thanks for the quick reply. I figured it out. There was a construction point used in the geometry that wasn't part of the mesh that was getting written to the mesh file. So SU2 was giving me an error. Thanks again.

Anjay

[nivi]

Hi Trushant, This is Vivek here.

i am also getting the same error like

Error in "void CPhysicalGeometry:istributeColoring(CConfig*, CGeometry*)":
-------------------------------------------------------------------------
Mismatch between NPOIN and number of points listed in mesh file.
Please check the mesh file for correctness.

I checked the geometry, I don't have any extra points. Points defined in mesh file is same as calculated by SU2.

can you please help me by explain exactly where and what to check?

Thank you.

[bigfootedrockmidget]

Hi,


This issue pops up when you have defined points that are not used to construct a mesh cell. For instance, if you want to simulate the 2d flow over a cylinder, you have to define a circle. In gmsh, you need to add the center of the circle as a point. This point is not used in the meshing but it is saved in the su2 file.



This could be considered either a bug in gmsh for writing these points, or an inflexibility in su2 for not ignoring these points.

[pedrovsc27]

Hi,

Do you know what could be the fix for this problem?

[bigfootedrockmidget]

Hi,

In gmsh, you have to create a physical surface in 2D or a physical volume in 3D. Then when you export to su2 format you do not choose "save all elements".

[pedrovsc27]

In the case of a wing, what should I do? because if I define a surface volume for it it will become part of the domain mesh and there will be no wing. I have the following surfaces defined.

Physical Surface("Wing") = {1,9,13,14};
Physical Surface("Farfield") = {ns1, ns2, ns3, ns4};
Physical Surface("LowerSide") = {lower_side};
Physical Volume("Domain") = {domain};

[omzo]

Hello everyone, I have made the mesh of a rocket but while making the simulation with SU2 I have this error.

Error in "void CPhysicalGeometry:istributeColoring(const CConfig*, CGeometry*)":
-------------------------------------------------------------------------
Mismatch between NPOIN and number of points listed in mesh file.
Please check the mesh file for correctness.

I have spent many hours looking for the problem but nothing if anyone can help me. Thank you very much for your help.



// Gmsh project created
SetFactory("OpenCASCADE");
//+


////////////////////////////////////////////////

// DEFINITION GEOMETRIE

// (paramètres en décimètre)

//dimensions peau

r = 0.52; // rayon extérieur de la fusee
l = 12.5; // longueur peau

//dimension ogive

h_o = 1.9; // hauteur ogive

//dimensions ailerons

e = 2.5; // emplanture des ailerons
h = 1.75; // hauteur des ailerons (envergure)
s = 1.8; // saumon des ailerons
f = (e-s)/2; // fleche des ailerons

//taille cube
t_c = 100;

//paramètre maillage


lc1= 0.1; // taille points maillage pour la peau
lc2= 0.05; // taille points maillage pour l'ogive
lc3= 0.01; // taille points maillage pour les bords d'attaque des ailerons
lc4= 4.0; // taille points maillage pour le farfield



////////////////////////////////////////////////


// PEAU

Point(1002) = {0, r, 0, lc1};
Point(1009) = {-l, r, 0, lc1};

Line(1039) = {1009, 1002};

Extrude {{1, 0, 0}, {0, 0, 0}, 2*Pi} {
Curve{1039};
}
// -> surface 1 : cylindre


Curve Loop(1023) = {1041};
Plane Surface(1019) = {1023};
// -> surface 1019 base cylindre


////////////////////////////////////////////////


// OGIVE

Point(3) = {-l, 0, r, lc2}; // point base ogive
Point(4) = {-(l+h_o), 0, 0, lc2}; // sommet ogive
Point(100) = {-(l+0.8), 0, 0.4, lc2}; // point pour former courbe ogive

Spline(4) = {4, 100, 3}; // courbe ogive

Extrude {{1,0,0}, {0,0,0},2*Pi} {Line{4}; } // ogive





////////////////////////////////////////////////


// AILERON 1

Point(5) = {0, 0, r, lc1};
Point(6) = {-f, 0, (r+h), lc1};
Point(7) = {-(f+s),0, (r+h), lc3};
Point(8) = {-e, 0, r, lc3};

Line(7) = {5, 6};
Line(8) = {6, 7};
Line(9) = {7, 8};
Line(10) = {8, 5};

Curve Loop(6) = {7, 8, 9, 10};

Surface(6) = {6};


// AILERON 2

Point(9) = {0, 0, -r, lc1};
Point(10) = {-f, 0, -(r+h), lc1};
Point(11) = {-(f+s), 0, -(r+h), lc3};
Point(12) = {-e, 0, -r, lc3};

Line(11) = {9, 10};
Line(12) = {10, 11};
Line(13) = {11, 12};
Line(14) = {12, 9};

Curve Loop(8) = {11, 12, 13, 14};

Surface(8) = {8};


// AILERON 3

Point(13) = {0, -r, 0, lc1};
Point(14) = {-f, -(r+h), 0, lc1};
Point(15) = {-(f+s), -(r+h), 0, lc3};
Point(16) = {-e, -r, 0, lc3};

Line(15) = {13, 14};
Line(16) = {14, 15};
Line(17) = {15, 16};
Line(18) = {16, 13};

Curve Loop(10) = {15, 16, 17, 18};

Surface(10) = {10};


// AILERON 4

Point(17) = {0, r, 0, lc1};
Point(18) = {-f, (r+h), 0, lc1};
Point(19) = {-(f+s), (r+h), 0, lc3};
Point(20) = {-e, r, 0, lc3};

Line(19) = {17, 18};
Line(20) = {18, 19};
Line(21) = {19, 20};
Line(22) = {20, 17};

Curve Loop(12) = {19, 20, 21, 22};

Surface(11) = {12};



// FARFIELD


Point(1018) = {-(t_c+(l+h_o))/2, -t_c/2, -t_c/2, lc4};
Point(1019) = {-(t_c+(l+h_o))/2, -t_c/2, t_c/2, lc4};
Point(1020) = {-(-t_c+(l+h_o))/2, -t_c/2, -t_c/2, lc4};
Point(1021) = {-(-t_c+(l+h_o))/2, -t_c/2, t_c/2, lc4};
Point(1022) = {-(t_c+(l+h_o))/2, t_c/2, -t_c/2, lc4};
Point(1023) = {-(t_c+(l+h_o))/2, t_c/2, t_c/2, lc4};
Point(1024) = {-(-t_c+(l+h_o))/2, t_c/2, -t_c/2, lc4};
Point(1025) = {-(-t_c+(l+h_o))/2, t_c/2, t_c/2, lc4};

Line(1027) = {1018, 1019};
Line(1028) = {1018, 1020};
Line(1029) = {1019, 1021};
Line(1030) = {1020, 1021};
Line(1031) = {1018, 1022};
Line(1032) = {1019, 1023};
Line(1033) = {1020, 1024};
Line(1034) = {1021, 1025};
Line(1035) = {1022, 1023};
Line(1036) = {1022, 1024};
Line(1037) = {1023, 1025};
Line(1038) = {1024, 1025};

Curve Loop(1016) = {1032, 1037, -1034, -1029};
Plane Surface(1012) = {1016};
Curve Loop(1017) = {1034, -1038, -1033, 1030};
Plane Surface(1013) = {1017};
Curve Loop(1018) = {1033, -1036, -1031, 1028};
Plane Surface(1014) = {1018};
Curve Loop(1019) = {1031, 1035, -1032, -1027};
Plane Surface(1015) = {1019};
Curve Loop(1020) = {1028, 1030, -1029, -1027};
Plane Surface(1016) = {1020};
Curve Loop(1021) = {1038, -1037, -1035, 1036};
Plane Surface(1017) = {1021};

Surface Loop(101) = {1012, 1015, 1014, 1013, 1017, 1016}; //SURFACE BOX
Volume(1) = {101}; //VOLUME BOX



// WALL


Surface Loop(100) = {1020, 1, 1019, 8, 11, 10, 6}; //wall
Volume(2) = {100}; //VOLUME FUSEE
Physical Surface("wall") = {1020, 1, 1019, 8, 11, 10, 6}; //wall

//FARFIELD
Physical Surface("farfield", 1044) = {1016, 1014, 1017, 1012, 1013, 1015};

[dnaidu]

Hi Everyone,

I am trying to run the simulation on an aircraft, and I have generated a volume mesh by building a voxel block in Pointwise. Previously, I was able to execute the exported .su2 mesh file generated from pointwise. But now when I tried executing the newly created mesh files, I am getting NPOIN mismatch error as mentioned below:

-------------------- Output Preprocessing ( Zone 0 ) --------------------

WARNING: SURFACE_PRESSURE_DROP can only be computed for 2 surfaces (outlet, inlet)

Screen output fields: INNER_ITER, RMS_DENSITY, RMS_ENERGY, LIFT, DRAG
History output group(s): ITER, RMS_RES, CFL_NUMBER, AERO_COEFF, WALL_TIME
Convergence field(s): RMS_DENSITY
Warning: No (valid) fields chosen for time convergence monitoring. Time convergence monitoring inactive.
Volume output fields: COORDINATES, SOLUTION, PRIMITIVE

------------------- Geometry Preprocessing ( Zone 0 ) -------------------
Three dimensional problem.
7698100 grid points.
13647202 volume elements.
4 surface markers.
297 boundary elements in index 0 (Marker = farfield).
89274 boundary elements in index 1 (Marker = fuselage).
121477 boundary elements in index 2 (Marker = symm).
153430 boundary elements in index 3 (Marker = wing).


Error in "void CPhysicalGeometry:istributeColoring(const CConfig*, CGeometry*)":
-------------------------------------------------------------------------
Mismatch between NPOIN and number of points listed in mesh file.
Please check the mesh file for correctness.

I have recently started using SU2 and Pointwise. So, I don't know how to fix this error.
I am using SU2_CFD build for executing configuration file.
Attached the configuration file. I was not able to attach the mesh file as it is too large.

Could someone please help me how to fix this error.

Thanks for the help.

[bene_]

Hi to everyone,

I'm new with SU2, I have a similar problem, I created a mesh in ICEM of an actuator disk and now I want to do a calculation with SU2, but I have the same error of you, this is the message:



Reading the CGNS file: meshDoubleDisk.cgns.
CGNS file contains 1 database(s).
Database 1, BASE#1: cell dimension of 3, physical dimension of 3.
1 total zone(s).
Zone 1, Project: 1144151 total vertices, 1120680 total elements.
Loading CoordinateX values.
Loading CoordinateY values.
Loading CoordinateZ values.
Number of connectivity sections is 7.
Section FLUID contains 1120680 elements of type Hexahedron.
Section DISK_OUT contains 3600 elements of type Quadrilateral.
Section HUB contains 6060 elements of type Quadrilateral.
Section FAR contains 13560 elements of type Quadrilateral.
Section INLET contains 10260 elements of type Quadrilateral.
Section OUTLET contains 9360 elements of type Quadrilateral.
Section DISK_IN contains 3600 elements of type Quadrilateral.
Loading volume section FLUID from file.
Loading surface section DISK_OUT from file.
Loading surface section HUB from file.
Loading surface section FAR from file.
Loading surface section INLET from file.
Loading surface section OUTLET from file.
Loading surface section DISK_IN from file.
Three dimensional problem.
1144151 grid points.
1120680 volume elements.
6 surface markers.
3600 boundary elements in index 0 (Marker = DISK_OUT).
6060 boundary elements in index 1 (Marker = HUB).
13560 boundary elements in index 2 (Marker = FAR).
10260 boundary elements in index 3 (Marker = INLET).
9360 boundary elements in index 4 (Marker = OUTLET).
3600 boundary elements in index 5 (Marker = DISK_IN).




Error in "void CPhysicalGeometry:istributeColoring(const CConfig*, CGeometry*)":
-------------------------------------------------------------------------
Mismatch between NPOIN and number of points listed in mesh file.
Please check the mesh file for correctness.



Someone can help me?
Thanks in advance

[bigfootedrockmidget]

You should check in icem for unconnected vertices and remove them


unused points