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

Moving mesh

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

Like Tree4Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   November 24, 2010, 14:20
Default LaplaceFaceDecomposition
  #101
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,594
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi all

I am doing mesh motion using the laplaceFaceDecomposition method available in OF-1.5-dev. It is running without any problems in serial, however, when I decompose the case, the solver stalls on the very first encounter with mesh.update().

I have made the solver myself, so I used icoDyMFoam on the "movingConeMotion" tutorial, and the same behaviour is found for a decomposed case (2 processors).

My question is twofold: (i) Is it possible to use laplaceFaceDecomposition in parallel? (ii) If so, do I need to do something special to get the tet-solver to work?

Thank you very much for any help or suggestions

Niels
ngj is offline   Reply With Quote

Old   November 25, 2010, 06:27
Default
  #102
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
I think you have hit a long-standing bug that I have fixed in 1.6-ext, the fix is coming your way.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   November 25, 2010, 09:18
Default
  #103
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,594
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi Hrv

Thank you very much. Your help is most appreciated.

I do believe you already have my email address.

Best regards

Niels
ngj is offline   Reply With Quote

Old   November 27, 2010, 09:25
Default
  #104
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,594
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi Hrv

Congratulations on the release of 1.6-ext (also to the rest of the ext-team). I have a question regarding the bug for laplaceFaceDecomposition. I am a bit reluctant to change version a couple of month before I turn in my thesis, hence:

Is the bug localised to a corner of OF, so I will be able to lift that part of the code back to version 1.5-dev?

I am looking forward to have time to use all the additions in the new release.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   November 28, 2010, 15:47
Default
  #105
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Well, this was pretty major and I have been delaying it in 1.5-dev until the new release went out. You should have no problems with the new code and I would advise to upgrade.

Sorry for being imprecise,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   December 20, 2010, 11:51
Default
  #106
Member
 
Join Date: Nov 2010
Posts: 86
Rep Power: 6
abminternet is on a distinguished road
Hi guys,

now that you are talking about it, I am trying to set up a case using the laplaceFaceDecomposition motion solver, and I don't really understand what "distancePatches" does. Any ideas you could share? Thanks,

regards,
Fredrich Muller
abminternet is offline   Reply With Quote

Old   December 20, 2010, 12:03
Default
  #107
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,594
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi Fredrich

It is those patches based on which the diffusivity of the mesh movement is computed, as the diffusivity is a function of the distance to a given patch/set of patches. E.g. quadratic diffusivity is

1 / lambda^2

where lambda is the distance to the given set of patches.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   December 21, 2010, 07:05
Default
  #108
Member
 
Join Date: Nov 2010
Posts: 86
Rep Power: 6
abminternet is on a distinguished road
oooohhh great, thanx for the response. One more question though, I have an old tutorial and it uses the componentMixed boundary condition in the motionU file, with the laplaceTetDecomposition motion solver. I am using OpenFOAM-1.6-ext and that solver is no longer available, so I am using laplaceFaceDecomposition, which sounds quite similar i guess. My question is, is the componentMixed bc still available? and how does it work? there are two more fields when specifying this condition, refValue and valueFraction. Any ideas as to what they are? Thanks a lot.

best regards,
Fredrich
abminternet is offline   Reply With Quote

Old   December 27, 2010, 09:31
Default
  #109
New Member
 
Daniele Trimarchi
Join Date: Mar 2010
Location: Southampton, Uk
Posts: 11
Rep Power: 7
Daniele Trimarchi is on a distinguished road
Hi,
sorry to insist, but I'm still quite in trouble for the mesh point motion, as in the previous post linked below:

Quote:
Originally Posted by Daniele Trimarchi View Post
FSI in OF
The thing is, I'm actually using OF 1.7.x and I can't access the pointMotion boundaryField, in order to assign directly the point mesh displacements. I'm actually obliged to do a inelegant interpolation on the structural displacement, in order to define average face motions.

Please help..!! : )

Thanks a lot, Daniele
Daniele Trimarchi is offline   Reply With Quote

Old   February 4, 2011, 08:41
Default
  #110
Senior Member
 
Join Date: Oct 2009
Posts: 136
Rep Power: 7
Peter_600 is on a distinguished road
I am also interested in the componentMixed boundary condition.
How to set it up in in the motionU file ?

Thx
Peter
Peter_600 is offline   Reply With Quote

Old   February 7, 2011, 12:22
Default
  #111
Member
 
Join Date: Nov 2010
Posts: 86
Rep Power: 6
abminternet is on a distinguished road
Hi Peter,

I found out how the mixed boundary condition works, it is just a mix between fixed value and fixed gradient. The refValue would be your fixed value, and valueFraction the proportion of fixedValue, and 1-valueFraction the proportion that corresponds to fixedGradient
abminternet is offline   Reply With Quote

Old   February 15, 2011, 09:15
Default
  #112
Senior Member
 
Andrea Pasquali
Join Date: Sep 2009
Location: Germany
Posts: 142
Rep Power: 7
andrea.pasquali is on a distinguished road
Hi,
I'm thinking to use RBF in OF 1.6-ext as morphing tool for optimization analysis.
I tried the tutorial movingBlockRBF. I can rotate and translate the block but I still haven't found how to morph the block surface with control points (for example increase the length or give a curvature).

Could anyone help me how to set the RBF for morphing or where I can find some examples?

Thanks in advance

Andrea
__________________
Andrea Pasquali
andrea.pasquali is offline   Reply With Quote

Old   March 7, 2011, 12:05
Default
  #113
New Member
 
Join Date: Jan 2010
Posts: 23
Rep Power: 7
jdiorio is on a distinguished road
Quote:
Originally Posted by Daniele Trimarchi View Post
The thing is, I'm actually using OF 1.7.x and I can't access the pointMotion boundaryField, in order to assign directly the point mesh displacements. I'm actually obliged to do a inelegant interpolation on the structural displacement, in order to define average face motions.
I'm having a similar problem to Daniele. Trying to use OF 1.6 to do an oscillating wing. Using dynamicMotionSolverFVMesh, getting mesh motion using oscillating wall or timeVaryingFixedValue no problem. But if you want to access the pointMotionU boundaryField directly (say to make the velocity non-uniform along the moving patch, e.g. to add a rotation or in Daniele's case some custom deformation) - is it possible? For simple things (like oscillation and rotation) is better to use solidBodyMotionFvMesh? Using that I get the ENTIRE mesh to move - but I want just a single patch.
jdiorio is offline   Reply With Quote

Old   March 8, 2011, 10:45
Default
  #114
New Member
 
Join Date: Jan 2010
Posts: 23
Rep Power: 7
jdiorio is on a distinguished road
To add on - tried changing the pointField read by solidBodyMotionFvMesh to just be the points on the patch I want to move, i.e.

Quote:
undisplacedPoints_
(
IOobject
(
"movingPatchPoints",
io.time().constant(),
meshSubDir,
*this,
IOobject::MUST_READ,
IOobject::NO_WRITE
)
)
where "movingPatchPoints" are the points only on the patch that I want to move. Motion starts but then chokes:

Quote:
solidBodyMotionFunctions::SDA::transformation(): Time = 0.01 transformation: ((0 -0.248858 0) (1 (0 0 0)))


Cannot move points: size of given point list smaller than the number of active points#0 Foam::error:rintStack(Foam::Ostream&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
coming from primitiveMesh::movePoints due to the size inconsistency between movingPatchPoints and active points (which I'm guessing is all the mesh points). Any ideas on how to make an individual patch move?
jdiorio is offline   Reply With Quote

Old   March 15, 2011, 13:57
Default
  #115
New Member
 
Join Date: Jan 2010
Posts: 23
Rep Power: 7
jdiorio is on a distinguished road
Aha, I'm an idiot. Found the derived pointPatchField classes in the fvMotionSolvers folder - maybe I should actually try looking more closely in the future. Can use that as a guide. Daniele, you should be able to access the point velocities/displacements directly there to do what you want to do.
jdiorio is offline   Reply With Quote

Old   March 23, 2011, 12:58
Default
  #116
New Member
 
Daniele Trimarchi
Join Date: Mar 2010
Location: Southampton, Uk
Posts: 11
Rep Power: 7
Daniele Trimarchi is on a distinguished road
Hi jdiorio, and thanks for your post. I'm looking at the derived class surfaceDisplacementPointPatchVectorField, as you suggested.

I should however admit to be quite confused. Could you please confirm if what I understand is true?

From my understanding, the basic idea is that in constant there is a (deformable) trisurface; the correspondent surface in the fluid mesh (defined via the member fnct: surfaces() ) will follow this.

In the case of the 'NEAREST' option, the connectivity is found searching for the closest point of the the two surfaces.

If a point of the fluidMesh has been found on the trisurface (by the function hit() ), the point displacement to be assigned to the fluid mesh is calculated then as the difference between the initial point location and the current location.

More in detail:

displacement[i] = nearest[i].hitPoint() - points0[meshPoints[i]];

where:

displacement[i] is the displacement to be assigned to the fluid mesh point. It has the size meshPoints.size()

nearest[i] comes from surfaces().findNearest(...) . findNearest(...) is member of the class 'SearchableSurface', and it is applied to the local member function surfaces(), which restitutes the pointer to the trisurface. I suppose the meaning of this is to search for the connectivity of the points between the fluidMesh surface and the trisurface? If this is true, for every fluidMesh point i, nearest[i] stores the index of the correspiondent node of the trisurface and it is member of the class LIST<PointIndexHit>

hitPoint() is a function of the class PointIndexHit and applied to nearest[i] returns the actual coordinates of the trisurface point(?)

points0[meshPoints[i]] returns the mesh initial point coordinates.

If all of that is true, I imagine that your advice is to modify directly this class and assign the displacements externally calculated to displacement[i]?

Thanks,
Daniele

Last edited by Daniele Trimarchi; March 23, 2011 at 18:50.
Daniele Trimarchi is offline   Reply With Quote

Old   April 15, 2011, 14:13
Default
  #117
New Member
 
Join Date: Jan 2010
Posts: 23
Rep Power: 7
jdiorio is on a distinguished road
Sorry Daniele but I'm not familiar enough with the mesh motion code to address your problem. The fix that worked for me was finding examples of derived boundary conditions (e.g. "oscillatingDisplacement", "angularOscillatingDisplacement", etc.) that can be applied to the "pointMotionU" or "pointDisplacement" files when using the displacementLaplacian or velocityLaplacian solvers. From there it was easy to modify to do say, and oscillation with a rotation. You're problem sounds a little more unique.

For others - is there something special that needs to be done to handle mesh motion near symmetry planes? I have a 3D grid (imported from StarCCM+) of an airfoil with the root mounted on a symmetry plane.
Trying to make the airfoil rotate about its center - not doing any flow solving just moving the mesh. Using displacementLaplacian solver and the angularOscillatingDisplacment condition on the foil. Works fine up until a certain time when the residuals start to get funky and code eventually crashes (see pic) and some ugly error:

Quote:
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt in "/lib64/tls/libc.so.6"
#3 void Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::Field<Foam::Vector<double> >&, Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so"
#4 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so"
#5 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div<Foam::Vector<double> >(Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so"
#6 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div<Foam::Vector<double> >(Foam::tmp<Foam::GeometricField<Foam::Vector<doub le>, Foam::fvsPatchField, Foam::surfaceMesh> > const&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so"
#7 Foam::fv::gaussLaplacianScheme<Foam::Vector<double >, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so"
#8 Foam::tmp<Foam::fvMatrix<Foam::Vector<double> > > Foam::fvm::laplacian<Foam::Vector<double>, double>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&, Foam::word const&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfvMotionSolvers.so"
#9 Foam::tmp<Foam::fvMatrix<Foam::Vector<double> > > Foam::fvm::laplacian<Foam::Vector<double>, double>(Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&, Foam::word const&) in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfvMotionSolvers.so"
#10 Foam::displacementLaplacianFvMotionSolver::solve() in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfvMotionSolvers.so"
#11 Foam::motionSolver::newPoints() in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libdynamicMesh.so"
#12 Foam::dynamicMotionSolverFvMesh::update() in "/home/diorijd1/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libdynamicFvMesh.so"
#13 main in "/home/diorijd1/OpenFOAM/diorijd1-1.6/applications/bin/linux64GccDPOpt/pimpleDyMFoamMesh"
#14 __libc_start_main in "/lib64/tls/libc.so.6"
#15 __gxx_personality_v0 in "/home/diorijd1/OpenFOAM/diorijd1-1.6/applications/bin/linux64GccDPOpt/pimpleDyMFoamMesh"
Floating point exception
Looking at the grid on the symmetry (bottom) plane near the leading edge of the foil at t=0 and t=0.12, looks like the mesh starts to "buckle". Happens rather suddenly, and mesh doesn't appear to be having too much trouble up until that point. Is this a boundary condition issue? Is the mesh deformation too great? Any thoughts?
Attached Images
File Type: png residuals.png (18.9 KB, 42 views)
File Type: jpg t_0.jpg (40.8 KB, 88 views)
File Type: jpg t_0p12.jpg (45.5 KB, 117 views)
jdiorio is offline   Reply With Quote

Old   May 19, 2011, 13:00
Default Problem Solved!!
  #118
New Member
 
Daniele Trimarchi
Join Date: Mar 2010
Location: Southampton, Uk
Posts: 11
Rep Power: 7
Daniele Trimarchi is on a distinguished road
Hi Foamers,
I managed to sort out the problem of moving mesh points thanks to the precious help of Kassiotis. Here's the solution, I hope this will be useful.

1_Primarily some include are needed:

#include "pointMesh.H" //Perhaps not needed..?
#include "pointFields.H" //Perhaps not needed..?
#include "volPointInterpolation.H"

2_ Find the reference to the location of pointDisplacement field:

pointVectorField & PointDisplacement = const_cast<pointVectorField&>(mesh.objectRegistry: :lookupObject<pointVectorField>("pointDisplacement "));

3_ Find a reference to the moving interface:

word sail = coupling.lookup(Wing) //search in disctionary declared as 'coupling'
label fluidSideI = mesh.boundaryMesh().findPatchId(sail)
vectorField &pDisp=refCast<vectorField>(PointDisplacement.boun daryField()[fluidSideI]);

4_Find the relevant size of the vector and declare a vectorField. This will store the pointDisplacements values (in my case they come from the structural solver)

int Psize= pDisp.size();
vectorField dispVals(Psize);

5_ Once the values have been assigned to dispVals, assign them to cellDisplacement boundaryField

PointDisplacement.boundaryField()[ fluidSideI ] == dispVals;

6_ The mesh is updated via the motionSolver specified in dynamicMeshDict with

mesh.update();

7_ I observed a very triky thing, which gave me some headake in the last few days... I normally have in the time folder (let's say workdir/0) both files for pointDisplacements and cellDisplacements. When assiggning point movements THERE SHOULS BE NO cellDisplacement file. Otherwise the motionsolver does not affect, and the mesh displacement is not spread away (??!).

I normally apply those BC for the pointDisplacements:

> internalField uniform (0 0 0);
> boundaryField{
> Domain boundaries
> {
> type fixedValue;
> value uniform (0 0 0);
> }
> Moving Interface
> {
> type fixedValue;
> value nonuniform List<vector>
> 14 {(0 0 0)};
> }
> defaultFaces
> {
> type empty;
> }
> }


8_ This is not valid for cellDisplacements. In that case both cellDisplacements and pointDisplacements files are needed.
Daniele Trimarchi is offline   Reply With Quote

Old   January 26, 2012, 12:53
Default
  #119
Senior Member
 
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 7
Daniele111 is on a distinguished road
Hi all

I would coupling Openfoam with a my matlab code. With openfoam i resolved the flow around a terrain and it calculates tau on bottom surface, with it matlab code find the new bottom shape, Can I use move mesh openfoam capability to move mesh with matlab shape?
Daniele111 is offline   Reply With Quote

Old   February 21, 2012, 09:43
Default
  #120
New Member
 
Pal Schmitt
Join Date: Aug 2010
Location: Belfast
Posts: 19
Rep Power: 6
wavemaster is on a distinguished road
Hi Jdiorio,
I found the same problem in all OpenFOAM versions I am using....
Since it is a long time ago this question came up, did you find a solution?
Cheers,
Pal
wavemaster 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
Moving Reference frame - UDF - Moving mesh modisa FLUENT 0 April 18, 2008 13:31
Moving Mesh & Not Rotating Mesh AB CD-adapco 1 October 25, 2004 03:10
moving mesh Jim CD-adapco 2 August 27, 2002 07:39
moving mesh zqf CD-adapco 1 June 19, 2002 01:30
moving mesh khb Main CFD Forum 1 June 5, 2002 10:46


All times are GMT -4. The time now is 18:14.