CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Bugs (http://www.cfd-online.com/Forums/openfoam-bugs/)
-   -   Wigley Hull with OpenFoam 2.0.0 problem (http://www.cfd-online.com/Forums/openfoam-bugs/90150-wigley-hull-openfoam-2-0-0-problem.html)

Stephy July 1, 2011 23:36

Wigley Hull with OpenFoam 2.0.0 problem
 
Hello all,
I am trying to run the wigley hull tutorial on OpenFoam 2.0.0.
I have built the mesh using snappyHexMesh and I ran the LTSInterFoam computations. No error, eveything went well.
But then, when I run paraFoam, I can see the mesh, but when playing and displaying any vector like U or p, they would mysteriously disappear (I cannot select them instead of "Solid color"), and when clicking "apply" again, paraView closes automatically and I receive the following error message :
"
created temporary 'wigleyHull.OpenFOAM'
--> FOAM Warning :
From function polyMesh::readUpdateState polyMesh::readUpdate()
in file meshes/polyMesh/polyMeshIO.C at line 204
Number of patches has changed. This may have unexpected consequences. Proceed with care.


--> FOAM FATAL IO ERROR:
size 12000 is not equal to the given value of 182759

file: /home/alex/OpenFOAM/stephy-2.0.0/run/tutorials/multiphase/LTSInterFoam/wigleyHull/100/nut from line 18 to line 12043.

From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
in file lnInclude/Field.C at line 236.

FOAM exiting
"

I checked the files mentionned, but I couldn't find where this value of 182759 comes from, I couldn't find it in any file.

Could you please help me if you have any idea of what could solve the problem ?

Thank you very much,

Stephy

Curro5150 July 20, 2011 05:28

Try renaming the "0" folder to something like "0.org" and then renaming the "2" folder to "0". Otherwise openFoam (or maybe paraFoam) gets somehow confused with the original mesh before using snappyHexMesh. That solved the problem for me.

Regards,

Francisco

jameel February 12, 2013 10:36

same problem but not solved
 
Quote:

Originally Posted by Curro5150 (Post 316744)
Try renaming the "0" folder to something like "0.org" and then renaming the "2" folder to "0". Otherwise openFoam (or maybe paraFoam) gets somehow confused with the original mesh before using snappyHexMesh. That solved the problem for me.

Regards,

Francisco

Dear Francisco,
I have the same problem above, I tried to use your solution and I changed the zero file name to 0.org. but what do you mean by( the"2" folder ). please write to me
atheel,

jorkolino July 13, 2013 17:45

Quote:

Originally Posted by jameel (Post 407427)
Dear Francisco,
I have the same problem above, I tried to use your solution and I changed the zero file name to 0.org. but what do you mean by( the"2" folder ). please write to me
atheel,

Hi,

maybe I can help. When constructing the mesh, snappy does it in several steps (1st castellating the mesh, then 2. snapping the mesh, then 3. adding layers). Each stage is written into a numbered folder, starting from 1. (0 goes for the blockMesh I suppose). So your final mesh should be the latest number (it can be number 3 or 1 instead of 2, depending on which steps you employed in the meshing process). So follow the instructions above with your latest folder number instead of number 2. Regards

sandy13 July 15, 2013 04:17

Quote:

Originally Posted by jorkolino (Post 439590)
Hi,

maybe I can help. When constructing the mesh, snappy does it in several steps (1st castellating the mesh, then 2. snapping the mesh, then 3. adding layers). Each stage is written into a numbered folder, starting from 1. (0 goes for the blockMesh I suppose). So your final mesh should be the latest number (it can be number 3 or 1 instead of 2, depending on which steps you employed in the meshing process). So follow the instructions above with your latest folder number instead of number 2. Regards

Dear jorkolino,
Thank you so much for this explanation. It was very helpful,

jovenitta April 11, 2014 03:11

Hi all. I am a newbie and trying to run wigley hull in OpenFoam 2.3. I get the same error message. I did exactly what has been told but the end of the message doesn't change. When I try to apply the volume fields in paraview (4.1). It suddenly exits and I get the error message below:
--> FOAM FATAL IO ERROR:
size 12000 is not equal to the given value of 182759

file: /home/itu/OpenFOAM/itu-2.3.0/run/tutorials/multiphase/LTSInterFoam/wigleyHull/2000/nut from line 18 to line 12047.

From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/Field.C at line 292.

FOAM exiting

Segmentation fault (core dumped)

This is quite an old thread but is there still anybody can help me with this issue? Thanks..

jovenitta April 16, 2014 05:09

Somehow I couldn't solve wigleyHull turorial using OF 2.3. I installed OF 2.2.2 instead and now it works.

Sachin m September 1, 2014 00:54

Hi Jovenitta,

Try the following steps and it will work.

1) first use the blockMesh command
2) snappyHexMesh -overwrite
3) renumberMesh -overwrite
4) foamToVTK
5) LTSInterFoam

kubashmuba October 4, 2014 00:42

Problems with alpha1 all 0
 
Hi,

I tried what Sachin m suggested, and it works once I have copied alpha1.org into alpha1. I have OpenFOAM 2.1.1 installed and took the wigleyHull tutorial from 2.0.0 I believe, since it doesn't seem to feature in versions after that. Running paraFoam and creating a contour plot for alpha1 at 0.5 to visualize the free surface gives nothing though, and the info in the contour plot for [min, max] of alpha1 says [0, 0]. So there seems to be a problem somewhere. I am new at openFOAM so I'm not even sure where to look for an error... What additional information could I provide to get help?

Thank you

Sachin m October 7, 2014 05:24

I am using 2.1.0

once you have completed the calculations, open parafoam. tick the tab on the left bottom corner which says alpha1. then on the active variable control tool bar , change the tab showing 'p' to alpha1.
Then on the common filters tab click on contour. You ll get the free surface.

kubashmuba October 11, 2014 21:06

Ah I see. I'm using OpenFOAM 2.1.1 because I'm on Ubuntu 14.04, and that was the closest version to 2.1.0, which can only be installed on Ubuntu 10 or 11.

I'm using a virtual box so I guess I can start from scratch again so I can install 2.1.0. First I'll try to compile 2.1.0 so I don't have to reinstal Ubuntu, maybe that will work, doesn't anybody know if it's possible to compile 2.1.0 for Ubuntu 14.04?

But I'm wondering why a minor version bump (2.1.0 -> 2.1.1) would break the wigley hull tutorial that badly, and why is it that I get [0,0] for alpha1. The computation didn't seem to go wrong or crash, just the result seems incorrect. Was there a change in format or to LTSInterFoam that could explain the difference in outcome between 2.1.0 and 2.1.1?

Sachin m October 14, 2014 05:25

Hi all,
there is a slight mistake in the steps that i mentioned. i forgot to mention the setField command.
So here is the steps :

1) first use the blockMesh command
2) snappyHexMesh -overwrite
3) renumberMesh -overwrite
4) foamToVTK
5) setFields
6) LTSInterFoam

Sachin m October 14, 2014 05:27

Hi kubashmuba,

the reason u dont get a free surface is because you did not type the command setFields. Which converts the domain into air and water.In your case you have only one value of alpha; that is zero.
Try the steps that i have mentioned just now.

kubashmuba October 14, 2014 23:11

Hi Sachi m,

I downloaded and compiled 2.1.0 instead, it took me a little while to recompile everything.

- I then copied alpha1.org into alpha1 in the 0 folder
- I also decompressed wigley.stl and wigley-scaled-oriented.stl from $FOAM_TUTORIALS/resources/geometry into wigleyHull/constant/triSurface

I then ran blockMesh with no visible problem
Then I ran snappyHexMesh -overwrite, no apparent problem
Running renumberMesh -overwrite however gave me this error:

-->FOAM FATAL IO ERROR:
keyword hull_wall is undefined in dictionary "/home/.../OpenFOAM/.../run/tutorials/multiphase/LTSInterFoam/wigleyHull/0/nut::boundaryField"

file /home/.../OpenFOAM/.../run/tutorials/multiphase/LTSInterFoam/wigleyHull/0/nut::boundaryField from line 26 to line 29

From function dictionary::subDict(const word& keyword) const
in file db/dictionary/dictionary.C at line 461.

FOAM exiting

So then I tried rerunning snappyHexMesh and I started getting jovenitta's errors:

size 12000 is not equal to the given value of 182759

So I ran ./Allclean and ran ./Allrun, which doesn't have some of the steps Sachi m listed, but I think this proves that you can get in a bad state and running ./Allclean can help you recover from that.

It did work in the end, so thanks a lot for your help Sachi m.

I see some artefacts when large cells can be seen in the alpha data, so I'm going to try again with your additional renumberMesh and foamToVTK commands. By the way, what do they do?


All times are GMT -4. The time now is 13:55.