CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Bugs

Wigley Hull with OpenFoam 2.0.0 problem

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 2 Post By Curro5150

Reply
 
LinkBack Thread Tools Display Modes
Old   July 1, 2011, 23:36
Unhappy Wigley Hull with OpenFoam 2.0.0 problem
  #1
New Member
 
Join Date: Jul 2011
Posts: 23
Rep Power: 6
Stephy is on a distinguished road
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
Stephy is offline   Reply With Quote

Old   July 20, 2011, 05:28
Default
  #2
New Member
 
Francisco Miguel
Join Date: Apr 2010
Posts: 13
Rep Power: 7
Curro5150 is on a distinguished road
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 and jovenitta like this.
Curro5150 is offline   Reply With Quote

Old   February 12, 2013, 10:36
Default same problem but not solved
  #3
New Member
 
atheel
Join Date: Dec 2012
Posts: 3
Rep Power: 4
jameel is on a distinguished road
Quote:
Originally Posted by Curro5150 View Post
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,
jameel is offline   Reply With Quote

Old   July 13, 2013, 17:45
Default
  #4
Member
 
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 7
jorkolino is on a distinguished road
Quote:
Originally Posted by jameel View Post
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
jorkolino is offline   Reply With Quote

Old   July 15, 2013, 04:17
Default
  #5
Member
 
sandy
Join Date: Mar 2013
Location: Cardiff, UK
Posts: 71
Rep Power: 4
sandy13 is on a distinguished road
Quote:
Originally Posted by jorkolino View Post
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,
sandy13 is offline   Reply With Quote

Old   April 11, 2014, 03:11
Default
  #6
New Member
 
Deniz
Join Date: Apr 2014
Posts: 2
Rep Power: 0
jovenitta is on a distinguished road
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 is offline   Reply With Quote

Old   April 16, 2014, 05:09
Default
  #7
New Member
 
Deniz
Join Date: Apr 2014
Posts: 2
Rep Power: 0
jovenitta is on a distinguished road
Somehow I couldn't solve wigleyHull turorial using OF 2.3. I installed OF 2.2.2 instead and now it works.
jovenitta is offline   Reply With Quote

Old   September 1, 2014, 00:54
Default
  #8
Member
 
Sachin
Join Date: Aug 2014
Location: India
Posts: 45
Rep Power: 3
Sachin m is on a distinguished road
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
Sachin m is offline   Reply With Quote

Old   October 4, 2014, 00:42
Default Problems with alpha1 all 0
  #9
New Member
 
Join Date: Sep 2014
Posts: 3
Rep Power: 2
kubashmuba is on a distinguished road
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
kubashmuba is offline   Reply With Quote

Old   October 7, 2014, 05:24
Default
  #10
Member
 
Sachin
Join Date: Aug 2014
Location: India
Posts: 45
Rep Power: 3
Sachin m is on a distinguished road
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.
Sachin m is offline   Reply With Quote

Old   October 11, 2014, 21:06
Default
  #11
New Member
 
Join Date: Sep 2014
Posts: 3
Rep Power: 2
kubashmuba is on a distinguished road
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?
kubashmuba is offline   Reply With Quote

Old   October 14, 2014, 05:25
Default
  #12
Member
 
Sachin
Join Date: Aug 2014
Location: India
Posts: 45
Rep Power: 3
Sachin m is on a distinguished road
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 is offline   Reply With Quote

Old   October 14, 2014, 05:27
Default
  #13
Member
 
Sachin
Join Date: Aug 2014
Location: India
Posts: 45
Rep Power: 3
Sachin m is on a distinguished road
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.
Sachin m is offline   Reply With Quote

Old   October 14, 2014, 23:11
Default
  #14
New Member
 
Join Date: Sep 2014
Posts: 3
Rep Power: 2
kubashmuba is on a distinguished road
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?
kubashmuba is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
problem with sampling Utility in openFOAM 1.6 carmir OpenFOAM Post-Processing 10 February 26, 2014 03:00
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM 6 April 12, 2011 11:24
a problem of valve simulation in openfoam xck1986 OpenFOAM 2 January 21, 2011 21:08
Negative Volumes in Wigley Hull ICEM CFD Carlos Andrés CFX 2 March 1, 2010 03:55
OpenFOAM 1.6 CreatePatch Problem TarifaPirata OpenFOAM Bugs 1 September 10, 2009 04:35


All times are GMT -4. The time now is 06:55.