CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Unable to run a case with OpenFOAM 1.6-ext that works with OpenFOAM 2.3.0

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 15, 2014, 04:17
Default Unable to run a case with OpenFOAM 1.6-ext that works with OpenFOAM 2.3.0
  #1
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
Hi,

I have of 2.3.0 and I installed 1.6ext version. However although I use command of16ext to switch openfoam version I cant make run cases which run under openfoam 2.3.0, such as simpleFoam.. Where is the mistake?
Jiricbeng is offline   Reply With Quote

Old   May 15, 2014, 04:27
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,419
Rep Power: 25
alexeym will become famous soon enoughalexeym will become famous soon enough
Hi,

what exactly did you mean by

Quote:
I cant make run cases
?

There can be lots of things: slightly different dictionary formats, wrong environment variables, etc.
alexeym is offline   Reply With Quote

Old   May 15, 2014, 04:32
Default
  #3
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
I mean - I have a simple case I created - a box with velocity inlet and pressure outlet (k - eps model) which worked fine in of 2.3.0. And when I write command to switch from 2.3.0. to 1.6ext and write "simpleFoam" to start calculation, it writes

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM Extend Project: Open source CFD |
| \\ / O peration | Version: 1.6-ext |
| \\ / A nd | Web: www.extend-project.de |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.6-ext-064a6e9f332e
Exec : simpleFoam
Date : May 15 2014
Time : 11:33:24
Host : 96GB
PID : 6070
Case : /home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading field p



--> FOAM FATAL IO ERROR:
Cannot open include file "/home/openfoam/OpenFOAM/OpenFOAM-1.6-ext/etc/caseDicts/setConstraintTypes" while reading dictionary "/home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps/0/p::boundaryField"

file: /home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps/0/p at line 24.

From function functionEntries::includeEntry::includeEntry(dictio nary& parentDict,Istream& is)
in file db/dictionary/functionEntries/includeEntry/includeEntry.C at line 105.

FOAM exiting

....
Have got any idea, what is wrong?
Jiricbeng is offline   Reply With Quote

Old   May 15, 2014, 04:44
Default
  #4
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,419
Rep Power: 25
alexeym will become famous soon enoughalexeym will become famous soon enough
Can you show your 0/p file? I guess the problem is in the line

Code:
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
There's no such file in 1.6-ext. As I don't know detail of your case, for the start I'd suggest you to comment out the line.
alexeym is offline   Reply With Quote

Old   May 15, 2014, 04:57
Default
  #5
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
I uploaded the case here http://leteckaposta.cz/843824944. You can have a look at the files. I will be really glad for help.
Jiricbeng is offline   Reply With Quote

Old   May 15, 2014, 05:22
Default
  #6
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,419
Rep Power: 25
alexeym will become famous soon enoughalexeym will become famous soon enough
Well, you need to remove (or comment out) line:

Code:
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
in 0/U and 0/p files. As in fact you don't need this line even if you're running the case with 2.3.0.
alexeym is offline   Reply With Quote

Old   May 15, 2014, 06:32
Default
  #7
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
Thank you,

however I still have the message:

--> FOAM FATAL IO ERROR:
keyword div((nuEff*dev(grad(U).T()))) is undefined in dictionary "/home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps/system/fvSchemes::divSchemes"

file: /home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps/system/fvSchemes::divSchemes

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 396.

FOAM exiting

Although I commented out the div((nuEff*dev(grad(U).T()))) in /fvSchemes (I also tried to comment out other lines in fvSchemes) it still writes the message above (I tried to close and open terminal as well)
Jiricbeng is offline   Reply With Quote

Old   May 15, 2014, 08:06
Default
  #8
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,419
Rep Power: 25
alexeym will become famous soon enoughalexeym will become famous soon enough
Well, you can't solve everything by just commenting it out

If you go to 1.6 tutorials, you'll find, this line

Code:
div((nuEff*dev(T(grad(U))))) Gauss linear;
should be

Code:
div((nuEff*dev(grad(U).T()))) Gauss linear;
The reason for it is the implementation of turbulence->divDevReff(U) method. If you look at UEqn.H:

Code:
    tmp<fvVectorMatrix> UEqn
    (
        fvm::div(phi, U)
      + turbulence->divDevReff(U)
    );
and then look at kEpsilon.C, in 2.3 divDevReff is:

Code:
tmp<fvVectorMatrix> kEpsilon::divDevReff(volVectorField& U) const
{
    return
    (
      - fvm::laplacian(nuEff(), U)
      - fvc::div(nuEff()*dev(T(fvc::grad(U))))
    );
}
while in 1.6 it is

Code:
tmp<fvVectorMatrix> kEpsilon::divDevReff(volVectorField& U) const
{
    return
    (
      - fvm::laplacian(nuEff(), U)
      - fvc::div(nuEff()*dev(fvc::grad(U)().T()))
    );
}
That's why you need different lines in your fvSchemes for different versions of OpenFOAM.
alexeym is offline   Reply With Quote

Old   May 15, 2014, 08:52
Default
  #9
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
that is true, commenting out is a dull kind of solutin.

Thank you very much indeed mate, I finally used the whole files fvSchemes and controlDict from the 1.6ext tutorial, cause there were other fvSchemes errors.

Anyway, I would like to ask crucial question that I yearn to sort out, that is how could I run MRFSimpleFoam tutorial? There is folder "Make" and files createFields.H and MRFSimpleFoam.C, I do not know how to make it run. Could you give me a clue ?
Jiricbeng is offline   Reply With Quote

Old   May 15, 2014, 09:07
Default
  #10
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,419
Rep Power: 25
alexeym will become famous soon enoughalexeym will become famous soon enough
If you're talking about tutorials/incompressible/MRFSimpleFoam/mixerVessel2D from 1.6 then there is Allrun script. In the folder tutorials/incompressible/MRFSimpleFoam/MRFSimpleFoam solver itself is located, it's not a case folder.
alexeym is offline   Reply With Quote

Old   May 15, 2014, 09:30
Default
  #11
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
Yes, I thought it is two separate folders ( mixerVessel2D and MRFSimpleFoam) I am just working with it (due to Allrun in mixerVessel2D).
Thanks a lot
Jiricbeng is offline   Reply With Quote

Old   May 16, 2014, 02:56
Default
  #12
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
I am just going through the mixeVessel2D files. I obviously do not understand, what is actually the logic of MRFSimpleFoam - in this case I cannot see any mixing plane and there is no segment rotating, it is full circle.

I assumed in polymesh/boundary there will be a definition of cyclicGGI or GGI.. but there are just walls for rotor and stator.

Where can I find a case with rotating segmend connected via mixing plane to another segment or to a draft tube?
Jiricbeng is offline   Reply With Quote

Old   May 16, 2014, 07:52
Default
  #13
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
Hello,
I uploaded my rotor stator case I wish to simulate by using 1.6ext.

http://leteckaposta.cz/897752382

I d be very happy if you had little time to have a look at the case.
Jiricbeng is offline   Reply With Quote

Old   May 18, 2014, 14:50
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,635
Blog Entries: 39
Rep Power: 99
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

@Jiri:
Quote:
Originally Posted by Jiricbeng View Post
Where can I find a case with rotating segmend connected via mixing plane to another segment or to a draft tube?
I was planning on answering here on this thread, but after looking into this topic, I found out that 1.6-ext has the mixing plane feature in another branch and not in the standard one. And that it's preferable to install foam-extend 3.0, as it already has this feature integrated.
For more information, please read my revised post #7 on this thread: Installing Mixing_plane in either OpenFOAM 2.3.0 or 1.6-ext

For future reference, looking for tutorials that have this mixing-plane feature, at least for now, can be done with this command:
Code:
find $FOAM_TUTORIALS -iname "*mixingPlane*"
Of course that this requires that you've installed a version of source code that has this feature

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   May 19, 2014, 07:11
Default
  #15
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
Thank you much for your information, I am just struggling with installation of extend -3.0. I am stuck on the step 11 which should last max 30 minutes, I waited nearly two hours and nothing.
Jiricbeng is offline   Reply With Quote

Old   May 21, 2014, 03:52
Default
  #16
Member
 
Jiri
Join Date: Mar 2014
Posts: 80
Rep Power: 4
Jiricbeng is on a distinguished road
Hi,
I successfully installed extended version 3.0.
I have meshes of stator.msh and rotor.msh which were created in commercial software. In OF 2.3.0 I used fluent3DMeshToFoam to convert meshes .msh to OF format. Then I used mergeMeshes and meshes were merged together.

However, I want to use mixing plane between rotor and stator, using OF3.0. I cant find where to set revolution of the rotor as I cant find it neither in tutorial mixingPlaneAxial nor in mixingPlaneDomADomB.

Moreover when typing simpleFoam a receive the error message:

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Initializing the mixingPlane interpolator between master/shadow patches: outflow/wall-4


--> FOAM FATAL ERROR:
Face zone name outflowZone for mixingPlane patch outflow not found. Please check mixingPlane interface definition.

From function label mixingPlanePolyPatch::zoneIndex() const
in file meshes/polyMesh/polyPatches/constraint/mixingPlane/mixingPlanePolyPatch.C at line 724.

Cause in polymesh/sets I have only folders:
highAspectRatioCells
nonOrthoFaces
region0
region1
wrongOrientedFaces

How shall I get there files with zones, as in tutorial mixingPlaneAxial
Jiricbeng 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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
Test directory missing in OpenFOAM 1.6 ext andrewryan OpenFOAM 2 March 20, 2011 16:41
Need help with the error cfdproject OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 0 April 14, 2009 15:45
64bitrhel5 OF installation instructions mirko OpenFOAM Installation 2 August 12, 2008 18:07
Help I canbt run FoamX report Unable to contact name server error cornerstone OpenFOAM Installation 0 May 3, 2006 01:14


All times are GMT -4. The time now is 13:09.