[idosil]

I would like to modify the movingCone tutorial to add/ remove mesh layers instead of changing mesh size. How do I do it? Is there an example, tutorial on setting dynamic mesh with topologic changes?
Where can I find info on using blockMesh to set sets and zones? I understand it is required in order to define topologic changes of the mesh.

Best regards, ido

[hjasak]

Try this:

movingConeTopo.tgz .

You may need some of my bug fixes etc as well, but that will give you an idea of what the case should look like.

Enjoy,

Hrv

[idosil]

Thanks Hrv,

It worked fine after a few small modifications. Now I have to work to understand the magic. Is there a demo with all the optional arguments to dynamicMeshDict file?

Best regards, Ido

[hjasak]

Actually, I am not too proud of that class and tutorial. There are much better and more flexible examples, either moving a user-defined box using the scaling or automatic mesh motion for more complex cases.

You should look at:

- dynamicBodyFvMesh
Automatic motion of the mesh around a moving body. A direction,
amplitude and frequency of translational motion and origin, axis,
amplitude and frequency of rotational motion must be specified.

- dynamicBoxFvMesh
Automatic simplified mesh motion for "box-in-mesh" cases. Here,
a direction of motion is defined, together with motion amplitude
and frequency. The domain is separated into three parts, where
the middle part moves accordign to the prescribed motion law.
Parts of the mesh before and after the obstacle are scaled.

- dynamicMotionSolverFvMesh
Dynamic FV mesh, where a motion solver is used to move the mesh.
The user specifies motion using the boundary condition on the
appropriate motion variable.

As for the parameters, the best things is to look at the constructor. I usually do not hide the parameters, but you never know

Enjoy,

Hrv

[idosil]

Boundary conditions for sliding interface

Dear Hrv,

I have been studying the various dynamic mesh solvers supplied with OpenFOAM. I am working now with movingValveLayersFvMesh and wrote a small test case for it (for icoDyMFoam solver). The model simulates a piston moving inside a cylinder, closing and outlet. The "insideSlider" patch boundary conditions should be wall (fixedValue (0 0 0)) where ever it is not attached to the "outsideSlider". Where they are attached it should be an internal boundary. When I set the boundary condition to fixedvalue it was so everywhere including where it is attached to the other patch. When I changed it to zeroGradient I get flow through the attaching zone but the velocity does not goes to zero on the "wall" zone. How can I get the required behavior?

Best regards, Ido

P.S. How does I attach a file to this post?

[idosil]

Boundary conditions for sliding interface (with attachment)

Dear Hrv,

I have been studying the various dynamic mesh solvers supplied with OpenFOAM. I am working now with movingValveLayersFvMesh and wrote a small test case for it (for icoDyMFoam solver, see attached file). The model simulates a piston moving inside a cylinder, closing and outlet. The "insideSlider" patch boundary conditions should be wall (fixedValue (0 0 0)) where ever it is not attached to the "outsideSlider". Where they are attached it should be an internal boundary. When I set the boundary condition to fixedvalue it was so everywhere including where it is attached to the other patch. When I changed it to zeroGradient I get flow through the attaching zone but the velocity does not goes to zero on the "wall" zone. How can I get the required behavior?

movingValve.rar

Best regards, Ido

[idosil]

Hi,

I tested the model again today with fixedValue boundary conditions on the sliding interfaces and it worked correctly.

Bye, Ido

[hjasak]

Sorry, don't get it - can you please confirm if this works OK or not. If there's trouble, I'll have a look (I've run it less than 2 weeks ago).

Hrv

[idosil]

Hi Hrv,

1) your model movingConeTopo works fine.

2) I have looked around and made a model to study the dynamic mesh solver movingValveLayersFvMesh. At first I had problem with boundary conditions on the sliding faces but later have been able to resolve it. The case is given in the attached file movingValve.tgz .

Bye, Ido

Hi, I have a question about the movingConeTopo tutorial. This tutorial adds/removes mesh layers instead of changing mesh size.

When the current cell layer thickness exteeds the maxThickness setted in the dynamicMeshDict, the new added cell layer thickness is fixed to the maxThickness?

Can I choose another thickness, for example, 0.8*maxThickness, to add the new cell layer? If can, how can I do it?

By the way, I am using the OF-1.4.1-dev.

Thanks.

ZHAO

[ngj]

Hi

Have you tried to play around with the minThickness/maxThickness in

~/OpenFOAM/mekngj-1.4.1-dev/run/tutorials/icoDyMFoam/movingConeTopo/constant/dyn amicMeshDict

I suppose that is where you want to go.

/ Niels

[hjasak]

You can use any thickness you like. Just make sure that your motion and time-step are appropriate, so that you do not move for eg. 2 layer thicknesses in a single time-step.

Enjoy,

Hrv

Hi, Niels.

Maybe you did not understand my question.

I know that the min/maxThickness parameters are setted in the movingConeTopo/constant/dyn amicMeshDict. But in the codes of OF-1.4.1-dev, where is the new added cell layer thickness fixed to this maxThickness of the dynamicMeshDict?

When the current cell layer thickness exteeds the maxThickness of dynamicMeshDict, can I fix the new cell layer thickness to be any multiples of maxThickness by modifing the codes?

Thanks.

ZHAO

Hi, Hrvoje. Thanks for your reply.

When the old master cell layer thickness exceeds the maxThickness, the new points are added. If the new points are added at the maxThickness away from the master zone points, a old slave cell layer whose thickness is equal to the maxThickness, and a new cell layer whose thickness is equal to (the old master layer thickness - maxThickness) will be created. If the old master cell layer thickness exceeds the maxThickness very slightly, the newly created layer may be very thin. The very thin cell layer is not good for the convergence.

However, if I fix the old slave cell layer thickness to be less than 0.8*maxThickness, the newly created layer thickness will be greater than 0.2*maxThickness, and will be not very thin. So, how can I introduce this 0.8 or any other value to the codes, so that a thin cell layer can be avoided neatly?

Thanks.

ZHAO

[gmc_salta]

Dear Prof Jasak
We was starting to work with dynamic mesh. We began with icoDyMFoam of tutorial and work fine, but we need refined mesh in some place our domain (transient problem) and not in moving mesh.
We look some discussion on forum. One of them indicate that exits improved version of icoDyMFoam.

We download of this site http://openfoam-extend.svn.sourceforge.net/viewvc/openfoam-extend/trunk/Core/Ope nFOAM-1.4.1-dev/applications/solvers/incompressible/
all files of solver icoDyMFoam (by HJasak). Then we tried to compiled them, with version OF1.4.1, and it give this message:

Making dependency list for source file icoDyMFoam.C
could not open file initTotalVolume.H for source file icoDyMFoam.C
could not open file checkTotalVolume.H for source file icoDyMFoam.C
SOURCE=icoDyMFoam.C ; g++ -m64 -Dlinux64 -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-40 -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/dynamicFvMesh/lnInclude -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/dynamicMesh/lnInclude -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/meshTools/lnInclude -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude -IlnInclude -I. -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/icoDyMFoam.o
icoDyMFoam.C:45:32: error: initTotalVolume.H: No existe el fichero o el directorio
icoDyMFoam.C:56:37: error: checkTotalVolume.H: No existe el fichero o el directorio
make: *** [Make/linux64GccDPOpt/icoDyMFoam.o] Error 1

We search files initTotalVolume.H and checkTotalVolume.H, in home/usr/OpenFOAM/OpenFOAM-1.4.1 but no found them.
We copied checkTotalVolume.H of another solver (icoMeshMotionFoam) but we not sure that it's correct. Please, could you send us the correct files or indicated how to take them?
Thanks very much
Sonia and Ana

[deepsterblue]

Ensure that you have the $(FOAM_SRC)/OpenFOAM/lnInclude directory added to your Make/options file. The files you're looking for exist there.

[gmc_salta]

Hi, Sandeep
Thank you for your quick answer, our version OF-1.4.1, was updated at sep/07.
We look for the files and find them but we have another error,
>> cannot find -llduSolvers
Again search this file in

http://openfoam-extend.svn.sourceforge.net/viewvc/openfoam-extend/trunk/Core/Ope nFOAM-1.4.1-dev/src/

and we find all files that needed, we are compiled them now.

Regard and thank for your suggestion
Sonia y Ana

Hi,
I start using openFoam less than a month ago, version 1.5 and I'm not very familiarized with it.

I try to run movingValve and movingConeTopo but it didn't work.
I wanted to know if I have to install something previously to running the case or what do I do wrong

I'm the only one with this problem?
Thanks, René

[deepsterblue]

You have to be specific. Can you post some output?

Ok, here are the outputs.

Starting time loop

Courant Number mean: 0 max: 0
deltaT = 0.111111
Time = 0.111111

time:0.111111 curMotionVel_1.77987e-05 0 0) curLeft:-0.007 curRight:-0.0035
No topology change

Executing mesh motion

Attempt to return dictionary entry as a primitive

file: /home/wops/OpenFOAM/wops-1.5/run/movingConeTopo/system/fvSolution::U::preconditi oner from line 70 to line 70.

From function ITstream& primitiveEntry::stream() const
in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 83.

FOAM aborting

#0 Foam::error::printStack(Foam:stream&) in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::IOerror::abort() in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::dictionaryEntry::stream() const in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#3 Foam::dictionary::lookup(Foam::word const&, bool) const in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 Foam::fvMatrix<foam::vector<double> >::solve(Foam::Istream&) in "/home/wops/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/icoDyMFoam"
#6 Foam::lduMatrix::solverPerformance Foam::solve<foam::vector<double> >(Foam::tmp<foam::fvmatrix<foam::vector<double> > > const&) in "/home/wops/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/icoDyMFoam"
#7 main in "/home/wops/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/icoDyMFoam"
#8 __libc_start_main in "/lib/i686/cmov/libc.so.6"
#9 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/wops/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/icoDyMFoam"

thanks,