[losiola]

hello,
good morning



i am trying to make this Mesh for an airfoil in 2D using Construct2D but i keep getting this error when i enter the file that contains the profile coordinates

Input > naca.dat
At line 142 of file src/util.f90 (unit = 13, file = 'naca.dat')
Fortran runtime error: End of file

Does anyone Have any IDea about what may the problem be?


Thanks in Advance.

[Flowkersma]

Hi,

Construct2D comes with sample airfoils which have the right format. Compare those files with your .dat file. For more information about Construct2D and OpenFOAM, have a look at this thread

Best, Mikko

[losiola]

Originally Posted by Flowkersma

Hi,

Construct2D comes with sample airfoils which have the right format. Compare those files with your .dat file. For more information about Construct2D and OpenFOAM, have a look at this thread

Best, Mikko

Hi Mikko ,
thank you for the replay



regarding the documentation i ve alredy seen it and it mentions that construct2D uses the XFOIL labled format which am respecting but yet still get the same error .


with the sample airfoils avalable i ve tried them and it works perfectly but for some reason it doesnt work for mine . I ve also tried to load airfoil data from the naca database and yet i still get the same error which is so disapointing (http://airfoiltools.com/airfoil/deta...l=naca64209-il).


still get this error

Input > naca.dat
At line 142 of file src/util.f90 (unit = 13, file = 'naca.dat')
Fortran runtime error: End of file

Really hope that someOne Can help me solve this issue



Thank yo for the Effort .
Regards

[Flowkersma]

Hi,

I just tried to copy paste the NACA 64-209 coordinates to a file (test.dat). Then I run construct2d with command 'construct2d test.dat' and it outputs 'Successfully loaded airfoil file test.dat'. After that I just write the commands 'grid' and 'smth' and construct writes the grid to a file (test.p3d). So it works without any problems. Can you elaborate a bit more what you are doing and share your airfoil data file?

Best, Mikko

[losiola]

Originally Posted by Flowkersma

Hi,

I just tried to copy paste the NACA 64-209 coordinates to a file (test.dat). Then I run construct2d with command 'construct2d test.dat' and it outputs 'Successfully loaded airfoil file test.dat'. After that I just write the commands 'grid' and 'smth' and construct writes the grid to a file (test.p3d). So it works without any problems. Can you elaborate a bit more what you are doing and share your airfoil data file?

Best, Mikko

That seems strange is it possible that i have some problem ?!!
Here are the coordinated for my airfoil in the file, please note that i had to make it a TXT because the forum refuses .dat format


Thanks

[Flowkersma]

You have an additional newline at the end of your file. Remove it and you are good to go.

[losiola]

Originally Posted by Flowkersma

You have an additional newline at the end of your file. Remove it and you are good to go.

That Actually Worked and i had no idea That a blanc line would do me such problems , Thank you very Much Mikko for your help You saved me , you are my hero .


Many Thanks

[losiola]

Originally Posted by losiola

That Actually Worked and i had no idea That a blanc line would do me such problems , Thank you very Much Mikko for your help You saved me , you are my hero .


Many Thanks

Hello Again,


i am still facing some issue in importing the Mesh to OpenFoam , and i really hope you can help me throught it .


so i ve created a mesh O-grid mesh with elliptic topology (even though my TE is sharp i went for it because its what i am looking for ) so once i Copy the file to my openFoam case i use this command :

 plot3dToFoam naca.p3d -2D 1 -singleBlock -noBlank

i get this result with a warning :

Reading 2D case by extruding points by 1 in z direction.

Create time

Reading 1 blocks
block 0 nx:200 ny:100 nz:2
Reading block points
block 0:
Reading 20000 x coordinates...
Reading 20000 y coordinates...
Extruding 20000 points in z direction...
Looking at cell 0 0 0 to determine orientation.
Left-handed block.

Merged points within 2.220446049e-16 distance. Merged from 40000 down to 39800 points.
Creating cells
Creating boundary patches
--> FOAM Warning : 
    From function Foam::polyMesh::polyMesh(const Foam::IOobject&, const Foam::Xfer<Foam::Field<Foam::Vector<double> > >&, const cellShapeList&, const faceListList&, const wordList&, const wordList&, const Foam::word&, const Foam::word&, const wordList&, bool)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 595
    Found 39800 undefined faces in mesh; adding to default patch.
Writing polyMesh
End

then i use this command to get patches :

autoPatch 80 -overwrite

i get the faces i need but once i reun checkMesh i get lots of errors about the mesh

Create time

--> FOAM Warning : 
    From function static Foam::instantList Foam::timeSelector::select0(Foam::Time&, const Foam::argList&)
    in file db/Time/timeSelector.C at line 274
    No time specified or available, selecting 'constant'
Create polyMesh for time = constant

Time = constant

Mesh stats
    points:           39800
    internal points:  0
    faces:            79003
    internal faces:   39203
    cells:            19701
    faces per cell:   6
    boundary patches: 5
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     19701
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    defaultFaces        0        0        ok (empty)                        
    auto0               199      398      ok (non-closed singly connected)  
    auto1               19701    19900    ok (non-closed singly connected)  
    auto2               19701    19900    ok (non-closed singly connected)  
    auto3               199      398      ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-2.49962617 -2.99990654 0) (3.5 2.99990654 1)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (0 -1.43760457e-17 -1.03426383e-15) OK.
 ***High aspect ratio cells found, Max aspect ratio: 3.914098022e+101, number of cells 19701
  <<Writing 19701 cells with high aspect ratio to set highAspectRatioCells
    Minimum face area = 7.004534805e-07. Maximum face area = 0.1461856339.  Face area magnitudes OK.
 ***Zero or negative cell volume detected.  Minimum negative volume: -0.01361617764, Number of negative volume cells: 19701
  <<Writing 19701 zero volume cells to set zeroVolumeCells
    Mesh non-orthogonality Max: 180 average: 168.9684194
 ***Number of non-orthogonality errors: 39203.
  <<Writing 39203 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 118206 faces are incorrectly oriented.
  <<Writing 79003 faces with incorrect orientation to set wrongOrientedFaces
    Max skewness = 1.450482967 OK.
    Coupled point location match (average 0) OK.

Failed 4 mesh checks.

End

Do you have any idea about why i get such bad quality mesh and how can i fix That?


Many Thanks

[Flowkersma]

Hi,

Have you visualized the mesh and where the bad cells are located? If you want a mesh with o-grid topology, you should not have a sharp trailing edge. Cut part of the trailing edge. You can do this by removing a couple of points from your .dat file (first and last).

In your checkMesh log:

Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)

You should define your front and back plane as empty so that checkMesh does not take the z-direction into account when calculating the aspect ratio.

Best, Mikko