[mechy]

when I compile the makeaxialmesh in openfoam 2 I enconter bellow problem please help me to compile makeAxialMesh


Making dependency list for source file makeAxialMesh.C
could not open file repatch.H for source file makeAxialMesh.C
SOURCE=makeAxialMesh.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/dynamicMesh/lnInclude -I/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/cfdTools/lnInclude -I/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/meshTools/lnInclude -IlnInclude -I. -I/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude -I/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/makeAxialMesh.o
makeAxialMesh.C: In function ‘void changeCoordinates(Foam:olyMesh&, Foam:lane, linie&, Foam::scalar, Foam::scalar, bool)’:
makeAxialMesh.C:198: error: ‘mathematicalConstant’ has not been declared
makeAxialMesh.C:199: error: ‘mathematicalConstant’ has not been declared
makeAxialMesh.C: In function ‘void splitWedge(Foam:olyMesh&, Foam::word, Foam:lane)’:
makeAxialMesh.C:255: error: invalid use of incomplete type ‘const struct Foam::SubField<Foam::Vector<double> >’
/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.H:62: error: declaration of ‘const struct Foam::SubField<Foam::Vector<double> >’
makeAxialMesh.C:257: error: invalid use of incomplete type ‘const struct Foam::SubField<Foam::Vector<double> >’
/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.H:62: error: declaration of ‘const struct Foam::SubField<Foam::Vector<double> >’
makeAxialMesh.C:258: error: invalid use of incomplete type ‘const struct Foam::SubField<Foam::Vector<double> >’
/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.H:62: error: declaration of ‘const struct Foam::SubField<Foam::Vector<double> >’
makeAxialMesh.C:261: error: invalid use of incomplete type ‘const struct Foam::SubField<Foam::Vector<double> >’
/home/yas/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.H:62: error: declaration of ‘const struct Foam::SubField<Foam::Vector<double> >’
makeAxialMesh.C:262: error: no match for ‘operator[]’ in ‘fcs[faceI]’
make: *** [Make/linux64GccDPOpt/makeAxialMesh.o] Error 1

[gschaider]

Originally Posted by mechy

when I compile the makeaxialmesh in openfoam 2 I enconter bellow problem please help me to compile makeAxialMesh

Hi!

I won't have time to look into this for the next month (actually I have time, but there is more interesting stuff to do during vacation).

For the time being I'd suggest that you use makeAxialMesh from one of your working 1.x-installations (the solver doesn't care where his mesh comes from, unless the mesh format changed).

If you want to be sure that I remember porting it please add a ticket at https://sourceforge.net/apps/mantisb..._view_page.php (Section "Breeder Stuff" - MAM doesn't have its own section). Of course: if somebody beats me with porting it ... I can live with that

Bernhard

[l_r_mcglashan]

makeAxialMesh.C: In function ‘void changeCoordinates(Foam:olyMesh&, Foam:lane, linie&, Foam::scalar, Foam::scalar, bool)’:
makeAxialMesh.C:198: error: ‘mathematicalConstant’ has not been declared
makeAxialMesh.C:199: error: ‘mathematicalConstant’ has not been declared

The above is because the mathematicalConstant namespace has been split into constant::mathematical. I updated my code using this (comes with a health warning):

grep -lre 'mathematicalConstant::' . | xargs -d'\n' sed -i 's/mathematicalConstant::/constant::mathematical::/g'

The rest of the errors are probably fixed by adding #include "SubField.H"

[mechy]

Hi McGlashan
thanks for your explanation
with your command the makeAxialMesh is compiled
I want to Run flow filed about a cone and I create a 2D mesh for this geometry can you help me to convert this mesh to a axisymmetric mesh (wedge mesh) ?
if It is possible Please give me your Email

best regards

[jordi.muela]

Originally Posted by l_r_mcglashan

The above is because the mathematicalConstant namespace has been split into constant::mathematical. I updated my code using this (comes with a health warning):

grep -lre 'mathematicalConstant::' . | xargs -d'\n' sed -i 's/mathematicalConstant::/constant::mathematical::/g'

The rest of the errors are probably fixed by adding #include "SubField.H"

Hi,

thanks! This worked for me! But now i'm having a problem with the function 'collapseEdges'.

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/libc.so.6"
#3  Foam::polyMesh::calcDirections() const in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::polyMesh::polyMesh(Foam::IOobject const&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/collapseEdges"
#6  __libc_start_main in "/lib/libc.so.6"
#7  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/collapseEdges"

Anybody else is having the same problem with OF 2.0.x?

Best regards,

Jordi.

[l_r_mcglashan]

What are you trying to do? Did this work in previous versions? Can you post your mesh up here?

[gschaider]

Originally Posted by jordi.muela

Hi,

thanks! This worked for me! But now i'm having a problem with the function 'collapseEdges'.

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/libc.so.6"
#3  Foam::polyMesh::calcDirections() const in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::polyMesh::polyMesh(Foam::IOobject const&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/collapseEdges"
#6  __libc_start_main in "/lib/libc.so.6"
#7  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/collapseEdges"

Anybody else is having the same problem with OF 2.0.x?

Best regards,

Jordi.

I just pushed a version that is fixed for 2.0 to the SVN (see the wiki for the URL). Tried to reproduce your problem with the testcase (set the origin-vector to (0 0 0)) and "collapseEdges 1e-5 45" works fine for me

[jordi.muela]

Hi,

sorry for my late answer. First of all, thanks for the new version . I've tested it with the testcase, and it works perfectly, as you've said.

But i'm still having the same problem with my own case. The problem starts when i do the makeAxialMesh. Before using the utility makeAxialMesh, if i do a checkMesh i'm obtaining a "Mesh OK", but if i do the checkMesh after run makeAxialMesh then i'm getting the same message error (floating point exception) that i've posted in the previous post, thus it's a problem with my geometry and the utility makeAxialMesh...

I'm using makeAxialMesh utility after a snappyHexMesh and a extrudeMesh (great improvement of this tool in OF 2.0.x!), because i'm using a STL geometry but i want to solve the case in 2D axisymmetric. In OF 1.7.1 it works great...

I attach an image of the mesh after the makeAxialMesh with the patch names... it's seems ok, at first view..

Thanks a lot for your time, i keep investigating.

Jordi.

[gschaider]

Originally Posted by jordi.muela

Hi,

sorry for my late answer. First of all, thanks for the new version . I've tested it with the testcase, and it works perfectly, as you've said.

But i'm still having the same problem with my own case. The problem starts when i do the makeAxialMesh. Before using the utility makeAxialMesh, if i do a checkMesh i'm obtaining a "Mesh OK", but if i do the checkMesh after run makeAxialMesh then i'm getting the same message error (floating point exception) that i've posted in the previous post, thus it's a problem with my geometry and the utility makeAxialMesh...

I'm using makeAxialMesh utility after a snappyHexMesh and a extrudeMesh (great improvement of this tool in OF 2.0.x!), because i'm using a STL geometry but i want to solve the case in 2D axisymmetric. In OF 1.7.1 it works great...

I attach an image of the mesh after the makeAxialMesh with the patch names... it's seems ok, at first view..

Thanks a lot for your time, i keep investigating.

Jordi.

Does the FPE still occur in calcDirection of polyMesh? I'm afraid then the problem is there. What probably happens is that MAM produced faces with an area of 0 and it is difficult to calculate a normal vector on these in a numerically stable way.

What you could do to pinpoint this problem: use MAM 2.0 then do checkMesh and or collapseEdges with 1.7. If that works then something in 2.0 was reimplemented that makes this fail. In that case write a bug-report on the OpenCFD-Mantis

Bernhard

[Pallav]

Hi Bernhard,

I am using your makeAxialMesh utility with OF-2.0 but running into problems that I cannot resolve.

<code>

object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;

vertices
(
(5 505 -0.5)
(0 505 -0.5)
(5 500 -0.5)
(0 500 -0.5)
(5 0.5 -0.5)
(0 0.5 -0.5)
(15 500 -0.5)
(15 0.5 -0.5)
(5 505 0.5)
(0 505 0.5)
(5 500 0.5)
(0 500 0.5)
(5 0.5 0.5)
(0 0.5 0.5)
(15 500 0.5)
(15 0.5 0.5)
);
blocks
(
hex (3 2 0 1 11 10 8 9) (20 5 1) simpleGrading (1 1 1)
hex (5 4 2 3 13 12 10 11) (20 1000 1) simpleGrading (1 1 1)
hex (4 7 6 2 12 15 14 10) (30 1000 1) simpleGrading (1 1 1)
);
edges
(
);
patches
(
patch inlet
(
(0 1 9 8)
)
wall inletWall
(
(0 2 10 8)
)
patch atmosphere
(
(7 4 12 15)
(4 5 13 12)
(2 6 14 10)
(6 7 15 14)
)
empty frontAndBack
(
(1 0 2 3)
(2 6 7 4)
(3 2 4 5)
(9 8 10 11)
(10 14 15 12)
(11 10 12 13)
)
patch center
(
(1 3 11 9)
(3 5 13 11)
)
);
mergePatchPairs
(
);
// ************************************************** *********************** //

<code>

makeAxialMesh writes the new mesh to 0.01; however, collapseEdges 1e-8 180 gives
Collapsing 0 small edges
Collapsing 0 in line edges

The same is for values from 1e-6 to 1e-8

Please advise me as to what I should do.

Thanks and regards.

[jordi.muela]

Hi Pallav,

Are you running OF 2.0.x? This code for the dictionary blockMeshDict that you've posted is wrote in OF 1.x.x syntax, it shouldn't work in OF 2.0.x.

Best regards,

Jordi.

[gschaider]

Originally Posted by Pallav

Hi Bernhard,

I am using your makeAxialMesh utility with OF-2.0 but running into problems that I cannot resolve.


makeAxialMesh writes the new mesh to 0.01; however, collapseEdges 1e-8 180 gives
Collapsing 0 small edges
Collapsing 0 in line edges

The same is for values from 1e-6 to 1e-8

Please advise me as to what I should do.

Thanks and regards.

Are you sure that the axified mesh is the one that CE wants to collapse? Check the output which mesh is read (make sure that startFrom in controlDict is set to latestTime)

If that is not the problem visually check the mesh in paraview

[Pallav]

Hello Bernhard,

Thanks for your reply.

Here are the steps that I took:

1. cd case_folder
2. blockMesh
3. cd ..
4. makeAxialMesh -axis center -wedge frontAndBack (This created a folder 0.01)
5. cd case_folder/system (to edit controlDict for changing startTime to latestTime)
6. cd ..
7. collapseEdges 1e-8 180

This gives the following output:

<code>
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0.01

Merging:
edges with length less than 1e-08 meters
edges split by a point with edges in line to within 179 degrees

Collapsing 1006 small edges
Morphing ...
Collapsing 0 small edges
Collapsing 0 in line edges
Max face area:6.54291e-07
Collapse area factor:1e-09
Collapse area:6.54291e-16
Collapsing 0 small high aspect ratio faces
Writing collapsed mesh to time 0.02
End
<code>

So, if I understand correctly, the final axisymmetric mesh is in the folder 0.02.

How do I check the mesh for this time step? I get an error if I try paraFoam or paraView.

Thanks a lot.

Regards,
Pallav

Originally Posted by jordi.muela

Hi Pallav,

Are you running OF 2.0.x? This code for the dictionary blockMeshDict that you've posted is wrote in OF 1.x.x syntax, it shouldn't work in OF 2.0.x.

Best regards,

Jordi.

Hello Jordi,

I am running OF-1.7-x on a supercomputer. I run OF-2.0.1 on my laptop.
I have run the corresponding svn codes to build makeAxialMesh at both places.

I transferred the case_folder from the supercomputer and ran it on my laptop. Hence, the difference in syntax in the blockMeshDict file. However, there is no problem when I run 'blockMesh'.

checkMesh gives 'OK'

However, I did get the same error as you when I did a checkMesh after makeAxialMesh.

So, I went back to the supercomputer and did everything from scratch in OF-1.7-x

Thanks and regards.

[gschaider]

Originally Posted by Pallav

Hello Bernhard,

Thanks for your reply.

Here are the steps that I took:

1. cd case_folder
2. blockMesh
3. cd ..
4. makeAxialMesh -axis center -wedge frontAndBack (This created a folder 0.01)
5. cd case_folder/system (to edit controlDict for changing startTime to latestTime)
6. cd ..
7. collapseEdges 1e-8 180

This gives the following output:

<code>
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0.01

Merging:
edges with length less than 1e-08 meters
edges split by a point with edges in line to within 179 degrees

Collapsing 1006 small edges
Morphing ...
Collapsing 0 small edges
Collapsing 0 in line edges
Max face area:6.54291e-07
Collapse area factor:1e-09
Collapse area:6.54291e-16
Collapsing 0 small high aspect ratio faces
Writing collapsed mesh to time 0.02
End
<code>

So, if I understand correctly, the final axisymmetric mesh is in the folder 0.02.

How do I check the mesh for this time step? I get an error if I try paraFoam or paraView.

"checkMesh -time 0.02" should tell you whether the mesh is OK

Of course the error would be helpful. Try the following: deselect all fields before changing the time-step.

Alternatively rerun all mesh-manipulation with -overwrite. That would make sure that the final mesh is in constant/polyMesh

[Pallav]

Thank you Bernhard.
I was able to visually check the mesh and everything looks great. (OF-1.7)

I adapted the new patches to the p_rgh, U, etc. files as per your comment about adapting fields at http://www.cfd-online.com/Forums/ope...tric-flow.html

However, I run into a few errors. I guess this is not the correct thread to discuss about the same. I will post them in some other thread.

Thanks once again for your help.

Regards,
Pallav

[Antony_Bosco]

Hi Guys,

I would like to compile makeAxialMesh . I have downoaded from openfoamwiki. But i dont know how to compile it.

Please help me.

Thanks&Regards,
Antony

[wyldckat]

Quick answer: I've added a chapter in the wiki page that explains how to install: http://openfoamwiki.net/index.php/Co...h#Installation

[Antony_Bosco]

Thanks wyldckat,

I have yet another problem. I am doing a external flow study on a axis symmetric body.

I am using blockMesh -> snappyHexMesh -> makeAxialMesh -> collapseEdges.

when i view the mesh it is all fine . but when i check the mesh with 'checkMesh' i am getting 7 errors.

I have attached the log file i received for checkMesh.

Is there anything that i have to do with rotationDict or collapseDict?

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
                   inlet      100      202  ok (non-closed singly connected)
                  outlet      100      202  ok (non-closed singly connected)
               upperWall     1200     2402  ok (non-closed singly connected)
            frontAndBack        0        0                        ok (empty)
               lowerWall     1532     2677  ok (non-closed singly connected)
                     ua1    31770    32535  ok (non-closed singly connected)
        frontAndBack_pos   142483   145823  ok (non-closed singly connected)
        frontAndBack_neg   142375   145713  ok (non-closed singly connected)

Checking geometry...
    Overall domain bounding box (-1.1 0 -0.0141658) (4.6 0.325 0.0141868)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 1)
    Wedge frontAndBack_pos with angle 2.49754 degrees
 ***Cannot find opposite wedge for wedge frontAndBack_pos
    Boundary openness (-9.02861e-19 1.54122e-14 1.31133e-12) OK.
 ***Open cells found, max cell openness: 0.0218662, number of open cells 152521
  <<Writing 152521 non closed cells to set nonClosedCells
  <<Writing 228809 cells with high aspect ratio to set highAspectRatioCells
 ***Zero or negative face area detected.  Minimum area: 0
  <<Writing 130 zero area faces to set zeroAreaFaces
 ***Zero or negative cell volume detected.  Minimum negative volume: -7.9226e-17, Number of negative volume cells: 120358
  <<Writing 120358 zero volume cells to set zeroVolumeCells
    Mesh non-orthogonality Max: 175.974 average: 70.2632
   *Number of severely non-orthogonal (> 70 degrees) faces: 330991.
 ***Number of non-orthogonality errors: 306103.
  <<Writing 637094 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 1338 faces are incorrectly oriented.
  <<Writing 1338 faces with incorrect orientation to set wrongOrientedFaces
 ***Max skewness = 1.58762e+06, 118079 highly skew faces detected which may impair the quality of the results
  <<Writing 118079 skew faces to set skewFaces
    Coupled point location match (average 0) OK.

Failed 7 mesh checks.

End

[wyldckat]

Quick answer: I very rarely need to use wedges, so I don't remember how it works exactly.
I need at least an example case based on the one you have to work with, so that I can inspect and do a bit of trial and error myself.

[Antony_Bosco]

@wyldckat. Thanks. I have also searched for examples online but was unlucky.
I am doing this work as a 'Studien Arbeit' at my university.