Seems like they changed the way it works. Try the -h option to see if there are options you like. Run without arguments and see what happens. I'm currently on vacation so it might be faster for you if you try some experiments yourself

Hi, gschaider!

It seems that you know much about #0 Foam::error::printStack error.
I have received this kind of error when running interFoam with Gambit mesh.
Would you please check the error for me. Thanks a lot.
http://www.cfd-online.com/Forums/ope...tml#post434749

I installed openfoam 2.2.0 on ubuntu 12.04.

Best regards.

printStack can be anything. See http://openfoamwiki.net/index.php/HowTo_debugging on how to interpret it. And I don't answer questions that do not belong in this thread

Error while running ..rhocentralfoam
 

helo ,
i converted my 2D axisymmetry fluent mesh into OF and then changed the 0 folder according to my values also i checked mesh with checkmesh command its ok but when i tried to run it run it is giving me following error , can anybody please help me how to overcome from this error ?

FOAM FATAL IO ERROR:
inconsistent patch and patchField types for
patch type symmetryPlane and patchField type empty

file: /home/yash/OpenFOAM/yash-2.2.0/run/tutorials/compressible/rhoCentralFoam/exsercisePrb/0/p.boundaryField.Axis from line 39 to line 39.

From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 165.

look at the error line, it says:
so you should make those types consistent :), if you choose symmetryPlane as patch type, then p, U or other variables should have the same patch type means symmetryPlane not empty ;)

helo
can you please look into the p file and tell me wts wrong in it which you had mentioned , thanks alot for your reply ,

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [1 -1 -2 0 0 0 0];

internalField uniform 101325;

boundaryField
{
fuel_inlet
{
type zeroGradient;
}

coflow_inlet
{
type zeroGradient;
}

Outlet
{
type zeroGradient;
}
Axis
{
type empty;
}
Upperwall
{
type zeroGradient;
}

frontAndBack
{
type empty;
}
}

// ************************************************** *********************** //

well, it should be
also i thing your frontAndBack should be wedge type :P, however you may face this problem next ;)

thanks alot nima. i will try this and then inform you ......thanks again for helping :)

hi, all foamers,

I came across problems when using makeAxisMesh in OF2.3.0. Here are steps I went through:
1. run blockMesh, where axis_plane has been set as planar type
2. run makeAxialMesh -axis axis_plane -wedge frontAndback

however, it says
I changed the "axis_plane" to be "symmetric", it still cannot work.

Then I changed the coordinates, such as switching X axis and Y axis, it works somehow with a new error:
I tired several times rotating the coordinator. But still, nothing improved. So I'm wondering if anyone can provide hints on this issue.

I also enclosed my blockMeshDict for your reference.

Thank you in advance.

What do you mean with "set as planar type"? The type of the patch is irrelevant. The faces have to be in a plane (that's what "planar" means). That's what the utility checks for. Otherwise the patch can't be used as an axis

Hi, Bernhard,

Thank you for the response. Originally, I tried the test case you provided here
http://openfoamwiki.net/index.php/Contrib/MakeAxialMesh

I tried
1. blockMesh
2. makeAxialMesh -axis movingWall -wedge frontAndBack

it generates an error, saying

I'm confused why it says the points on movingWall is not on a planar.

Then I thought it probably due to the wrong direction since you mentioned "the axis of symmetry is parallel to the XY-plane". So I split the fixedWalls into three surfaces and selected different fixedWalls1(0 4 7 3), fixedWalls2(2 6 5 1), fixedWalls3(1 5 4 0) as the axis. Only the fixedWalls2 (2 6 5 1) can work and it is actually parallel to Y-Z plane.

Based on the experience of the test, I developed my own code

However, when I run
makeAxialMesh -axis axis_plane -wedge frontAndback

it says

I don't know what's wrong with this error. Again, I rotated the coordinator directions, but nothing is improved.

By the way, I'm using OF2.3.0.

Thank you
Zhixuan

Seems like there is some problem when patches are specified on the command line. I get the same error. But when I run it just with "makeAxialMesh" the dictionary in system is used and it works.

I'd recommend using the dictionary anyway as this is more flexible

Im facing the same problem as zhixuan. The thing is, even if I use the dictionary by just running the command makeAxialMesh, the "movingWall" keeps it's patch as "wall". Any thoughts?


Thanks!

Hi
Have you solved this problem now?

I managed to solve this problem by using the dictonary rotationDict, and using the option for setting MakeAxialMesh in old version. Below there is a rotationDict with this option turned on:

I tried using collapseEdges, but I just couldnt get it to work. So I decided to use my mesh with symmetryPlane in the face that was supposed to be the axis (dont know how correct this is, but the results are looking correct when compared to some 3D simulations I ran).

The patch type I had to change manually in my blockMeshDict file.

I played around with MakeAxialMesh for a while and I really think it has some compatibility error with OpenFOAM 2.3, because the errors occur even in really simple meshes.

Hi
I also tried rotateMesh ,but I don't know the usage .Can you help me ?

rotateMesh is not to create axial meshes, if you want to create an axial mesh use makeAxialMesh. Just create the rotationDict as I posted and put it on your system folder. Then run the command makeAxialMesh. This will create a mesh in a folder such as 0.005, or something like that. Use checkMesh command to see if the mesh is correct, then replace your orignal polymesh folder with the one in the 0.005 folder.

I also have tried makeaxialMesh.
but ,
my movingWall's type is empty, I also tried symmetry and symmetryPlane, but all failed.

and another question: rotateDict is used accompany with rotateMesh.
I think makeaxialMesh don't need this dictionary.

The dictionary for makeAxilMesh is rotationDict not rotateDict. Can you post your blockMeshDict here so I can take a look?

oh,thanks!

oh
you mean the command rotateMesh don't need any dictionary?

Ok, so I figured out how to use makeAxialMesh properly thanks to this old thread: http://www.cfd-online.com/Forums/ope...mmetric-6.html

Forget what I said before about using the option makeAxialOldMode 1.

Just put the rotationDict and collapseDict in your system folders (you can use the ones attached, they work on your case). After that, run blockMesh to generate your mesh, then makeAxialMesh. Finally, run collapseEdges -latestTime . Your directory will look something like this (the numbers of the folders may change a bit):

0/ 0.0025/ 0.005/ constant/ system/

Copy the polymesh folder inside the 0.005 directory and replace it with your polymesh inside the constant/ folder (remember to back it up, so you dont lose your original blockMeshDict). And that's it.

P.S: rotateMesh is not for creating axial meshes, so you dont need to use it.

thanks for your kindness!
I will try it.

maybe I can operate in another way:blockMesh...makeAxialMesh -overwrite...collapseEdges -overwrite?

Try it. (as some time passed you probably did it and it worked)

Help
 

I have a problem to generate the axisymmetric mesh in my work, someone could help me, I am sending the files, would be grateful if anyone could help.


My openFoam 2.3

Thanks.


:D

Hi Santos,
 

Hi Santos,
1~~~At first,the makeAxialMesh tools should be compiled correctly.
2~~~In the file "blockMeshDict" , you should add a face named "center" which the mesh can rotate around it. Like this :

center
{
type symmetryPlane;
faces
(
(13 0 14 27)
);
}
3~~~And then,in the dictionary "system",two files "rotationDict" and "collapseDict" are needed. See the #183 floor.
4~~~At last,input these commands in order:
blockMesh
makeAxialMesh -overwrite
collapseEdges -overwrite
checkMesh
5~~~Good luck!
6~~~Forgive my poor English.

thanks
 

Thank zhangyan, I will try to perform these procedures. No problem, sorry my English.

Help
 

hello zhangyan,

I tried to take the steps you suggested, but the mesh was the same as the initial mesh. Execultar got the makeAxialMesh program, was generated the 0005 file, but nothing has changed.

Chosen as the center

(
(0 1 7 6) // Bot (0)
(1 12 14 7) // Bot (2)
);

Would have a question,

frontandback is the type empty?

If you could generate this mesh to me with the axis of symmetry equal to figure Site: https://openfoamwiki.net/index.php/C.../MakeAxialMesh

Conveerting a 2D mesh to axisymmetric using MAM in OF-2.3.1
 

Hi Foamers

I am encountering a strange problem creating axisymmetric meshes using MAM. The mesh looks pretty fine in paraview, before using collapseEdges. But when I use collapeEdges, it converts the axisymmetric mesh to the original 2D mesh.
I also tried using makeAxialMesh -overwrite. Thereafter, OF exits by (Floating point exception) error, when I use collapeEdges or checkMesh.
Does any body use MakeAxialMesh_2.x on OF-2.3.1? From what I have read in this thread, I guess it is a compatibility problem.

Thanks in advance


PS: please find attached the corresponding case.

You might want to try OF 2.4, they made some improvements to the makeAxialMesh.

Cheers

makeAxialMesh
 

Hi,

While running makeAxialMesh i am getting this warnig quite often.


--> FOAM Warning :
From function wedgePolyPatch::calcGeometry(PstreamBuffers&)
in file meshes/polyMesh/polyPatches/constraint/wedge/wedgePolyPatch.C at line 72
Wedge patch 'wedge_neg' is not planar.
At local face at (1.5137 0.0402188 -0.000877755) the normal (8.01877e-18 -0.0218097 -0.999762) differs from the average normal (-3.78148e-22 -0.0218097 -0.999762) by 1.72515e-15

is there something i should check or can i ignore this?

Thanks

round off
 

Looking at the digits of the normal vectors, it appears that this small discrepancy is a consequence of round-off. My guess is that you can safely ignore this warning.

checkMesh
 

Thanks schmidt,

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?

sorry for the previous post.

the error is

Try to use extrudeMesh after snappyHexMesh

extrudeMesh
 

Thanks Davibarreira,

extrudeMesh did not help. But i don't see the use of extrudeMesh. Do i have to make any changes in extrudeMeshDict or in collapseMeshDict??

Hallo Antony,

Have you defined frontAndBack_neg as wedge in your constant/polyMesh/boundary file?

Best regards
Hisham

@Hisham.
After running snappyHexMesh frontAndBack is patch.
After running makeAxialMesh frontAndBack is patch, frontAndBack_pos is wedge and frontAndBack_neg is wedge.