Moving boundary problem based on calculated data

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

October 10, 2013, 06:09
#21
New Member

Aleksander Sandro Grm
Join Date: Feb 2010
Location: Slovenia, Kanal ob Soči
Posts: 9
Rep Power: 8
Yes it works. Results are identical as for single run. I added figures and log files. I run my Gentoo Linux in VM with 4 cores, so the scaling is not linear but is significant.

Cheers, Sandro
Attached Images
 result_parallel.jpg (17.0 KB, 124 views) result_single.jpg (16.6 KB, 110 views)
Attached Files
 myMoveMesh_results_log.tar.gz (1.0 KB, 39 views)

 September 10, 2014, 06:06 #22 Member   Join Date: Jul 2014 Posts: 37 Rep Power: 3 Thank you Aleksander Really helped me. I see this thread was last updated 2013, but I will try. 2 questions: 1. Is it possible to move the boundary in the direction of the boundary cells normal vectors? I want to have a cylinder which expands. 2. How can I specify the "expansion"? I want the boundary to expand according to a calculated variable. So far I figured out that each boundary will move with a fixed constant (specified in pointDisplacement) if the while-loop is placed just after the autoPtr in the solver and the endTime is increased, only the boundary (specified as patchName) will continue to move. This is fine, since I can allocate the outside of the cylinder as one boundary. Still figuring out how the constants alpha and Tmax work, since their constants from createField. thank you Vrede

 September 10, 2014, 06:27 #23 Senior Member   HECKMANN Frédéric Join Date: Jul 2010 Posts: 237 Rep Power: 8 Hi, 1. It is what my code on the first page does. There is one variable called pointnormal. This takes the normal vector at the node. But in your case I would suggest to use the radial direction instead of the normal. the normal vector theoretically matches the radial direction but from my experience I would not trust it. Simply give the location of the center of the cylinder (it can be hard coded) and after calculate the vector between the node and the center. This will be your expansion vector. 2)again look at the first page. I do an interpolation from the face center to the node. The face center is the "calculated variable" Tobi likes this.

September 15, 2014, 08:34
#24
Member

Join Date: Jul 2014
Posts: 37
Rep Power: 3
Hi Frédéric

Your method helped, thank you. So I experimented with moveMesh solver.

Below are 3 screenshots, the first is the original mesh, which consists of a block at the bottom and a block on top with a slight skew top boundary. The next screenshot shows the top and bottom boundaries move according to die pointDisplacement file in the 0 directory. Here is a snippet:

Code:
```dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
top
{
type            fixedValue;
value           uniform (0 0.1 0);
}

bottom
{
type            fixedValue;
value           uniform (0 -0.1 0);
}
outlet
{
type            fixedNormalSlip;
n               (0 0 0);
}

defaultFaces
{
type            empty;
}
}```
As I have said before, the movement defined in the pointDisplacement file will only occur once, therefore all values can be set to zero especially if the speed of the movement will be determined in the solver. The 3rd screenshot show the 4th iteration where only the top boundary move.

As seen, it is only the top "layer" of cells which expand. My question: Is it possible to enlarge all the cells in the top block as the boundary moves?

Thank you
Vrede
Attached Images
 test_org_0.png (14.4 KB, 47 views) test_org_1.png (15.6 KB, 41 views) test_org_4.png (15.8 KB, 44 views)

September 16, 2014, 14:43
#25
Member

Join Date: Jul 2014
Posts: 37
Rep Power: 3
My previous problem has become somewhat irrelevant since my mesh movement is very small and my solver takes the change in volume into consideration.

Not sure I need to start a new thread...

My next challenge/question is how to "fix" a mesh when two sides combine (see figures) after movement. Is there a way to remove the cells (or nodes) when they "enter" the mesh?

Kind regards
Vrede
Attached Images
 test00.png (7.5 KB, 30 views) test01.png (7.7 KB, 33 views) test02.png (8.0 KB, 35 views) test03.png (7.9 KB, 32 views)

 October 10, 2014, 06:31 #26 New Member   Simon Lindberg Join Date: Oct 2014 Location: Gothenburg Posts: 2 Rep Power: 0 Hey, Very nice work of you and Frédéric! Thanks a bunch! I'm just a bit wondering about a few things that I was wondering about. Why did you not use the mesh.update() function and instead do a timeloop? Is it better? And what is the use of the buf variable? The nondimensional alpha value? I know this is an old thread but I hope I can get a closer understanding for this piece of code ! Thanks /Simon

 October 10, 2014, 13:15 #27 Senior Member   HECKMANN Frédéric Join Date: Jul 2010 Posts: 237 Rep Power: 8 Hi, I don't really know who you are talking to and what you are referring to. You need to have one mesh.update at each time step because it is this command that actually move the mesh. Therefore the mesh.update has to be inside a time loop. I don't understand what is the buf variable you mentioned. Also I don't know where is your alpha. Usually alpha is a non dimensional number that is called the collection efficiency. This number tells you how much matter impact your boundary compared to the mass flux in the free stream. It is defined as the mass flux in the free stream (kg.m-2.s-1) divided by the mass flux at your boundary.

 October 10, 2014, 18:26 #28 New Member   Simon Lindberg Join Date: Oct 2014 Location: Gothenburg Posts: 2 Rep Power: 0 Thanks for the answer! Sorry for the confusion, first post here so didn't really understand how a "quick reply" would work. My questions was mainly for Aleksander regarding the changes he did in his version of the code compared to your code. Thnaks for the clarification though!

December 1, 2014, 11:28
#29
Member

Fei Fan
Join Date: Jun 2013
Location: NanJing, China
Posts: 49
Rep Power: 4
Quote:
 Originally Posted by fredo490 Here is my dynamicMeshDict file that is in Constant Code: ```dynamicFvMesh dynamicMotionSolverFvMesh; motionSolverLibs ("libfvMotionSolvers.so"); solver displacementLaplacian; displacementLaplacianCoeffs { diffusivity quadratic inversePointDistance (wall); }``` and an example of "pointDisplacement" file that is in 0: Code: ```FoamFile { version 2.0; format ascii; class pointVectorField; location "0"; object pointDisplacement; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 0 0 0 0 0]; internalField uniform (0 0 0); boundaryField { inlet { type fixedValue; value uniform (0 0 0); } sides { type empty; } wall { type fixedValue; value uniform (0 0 0); } }```
Hi HECKMANN Frédéric:
I use your method to move mesh on the boundary of my solver. however, there is a error as i test a case. could you give me a hinte, where should i to modify the code. Thanks.

best Regards
Fan fei
Attached Images
 movemesh_errot.jpg (64.5 KB, 38 views)

 December 1, 2014, 20:03 #30 Senior Member   HECKMANN Frédéric Join Date: Jul 2010 Posts: 237 Rep Power: 8 Hi, it seems that you used the extended version of openfoam. Unfortunately I am not familiar with this version... In your solver, did you include all the library that I used? Edit, see the post #10 of page 1

December 1, 2014, 21:19
#31
Member

Fei Fan
Join Date: Jun 2013
Location: NanJing, China
Posts: 49
Rep Power: 4
Quote:
 Originally Posted by fredo490 Hi, it seems that you used the extended version of openfoam. Unfortunately I am not familiar with this version... In your solver, did you include all the library that I used? Edit, see the post #10 of page 1
Hi, I copy all the library you used. And I found some library are different in extend version. so I'm trying to find where is wrong.

Best regards
Fan Fei

 December 1, 2014, 23:21 pointMotionU #32 Member   Tony Ladd Join Date: Aug 2013 Posts: 35 Rep Power: 4 My postdoc and I have been working on a moving mesh code for a while now, starting with Frederic Heckmann's post as a template. Let me just make a few general points: 1) pointMotionU is better than pointDisplacement. In long runs with large mesh motion a discrepancy builds up between the positions of the cell centers calculated by averaging the vertexes (how OF determines them) and the original position + pointDisplacement. In the end the code breaks in situations where it runs fine with pointMotionU. I think pointDisplacement is intended for solid motion (small displacements). pMU works in differential mode and there is no inconsistency. 2) faceToPointInterpolate is a method of the primitivePatch class. Thus it does not work properly across coupled patches such as cyclic or processor. Connected with this is that pointNormal is a vector field (with no information about boundaries, just a list of data). Thus you cannot get OF to apply coupled patch type boundary conditions and pointNormal is always wrong across cyclic or processor patches. 3) Combining these ideas, a better strategy is to calculate the MotionU field at the face centers using the faceNormals. Then interpolate to the points to get the pointMotionU field. Since pMU is a pointVectorField (with boundaries) we think you can use OF's methods for coupled patches. Right now we are doing this by hand but I think we will have a proper solution soon. 4) One last point. OF always seems to apply the correct boundary conditions to the points field. So if pointMotionU has a component across a cyclic patch (for example), the points are still OK (ie on the cyclic boundary). But since pMU is wrong the Laplace solver gets the wrong solution and the internal points go haywire. Hope this helps a few people Tony

December 2, 2014, 21:34
#33
Member

Fei Fan
Join Date: Jun 2013
Location: NanJing, China
Posts: 49
Rep Power: 4
Quote:
 Originally Posted by fredo490 Hi, it seems that you used the extended version of openfoam. Unfortunately I am not familiar with this version... In your solver, did you include all the library that I used? Edit, see the post #10 of page 1
Hi HECKMANN Frédéric:
I try all the ways i know. But the problem didn't solve. the header field as below:
Quote:
 #include "fvCFD.H" #include "meshTools.H" #include "dynamicFvMesh.H" #include "singlePhaseTransportModel.H" #include "turbulenceModel.H" #include "faCFD.H" #include "incompressible/singlePhaseTransportModel/singlePhaseTransportModel.H" #include "RASModel.H" #include "primitivePatchInterpolation.H" #include "pointFields.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { # include "setRootCase.H" # include "createTime.H" # include "createDynamicFvMesh.H" # include "readGravitationalAcceleration.H" # include "createFaMesh.H" # include "createFields.H" # include "initContinuityErrs.H"
and options are
Quote:
 EXE_INC = \ -I\$(LIB_SRC)/turbulenceModels/incompressible/turbulenceModel \ -I\$(LIB_SRC)/transportModels \ -I\$(LIB_SRC)/turbulenceModels \ -I\$(LIB_SRC)/turbulenceModels/incompressible/RAS/RASModel \ -I\$(LIB_SRC)/transportModels/incompressible/singlePhaseTransportModel \ -I\$(LIB_SRC)/finiteVolume/lnInclude\ -I\$(LIB_SRC)/finiteArea/lnInclude\ -I\$(LIB_SRC)/sampling/lnInclude\ -I\$(LIB_SRC)/dynamicMesh/dynamicFvMesh/lnInclude \ -I\$(LIB_SRC)/dynamicMesh/dynamicMesh/lnInclude \ -I\$(LIB_SRC)/dynamicMesh/meshMotion/lnInclude \ -I\$(LIB_SRC)/meshTools/lnInclude EXE_LIBS = \ -lincompressibleTransportModels \ -lincompressibleTurbulenceModel \ -lincompressibleRASModels \ -lincompressibleLESModels \ -lfiniteVolume \ -lfiniteArea \ -ldynamicMesh \ -lmeshTools \ -ldynamicFvMesh \ -lfvMotionSolver\ -ltopoChangerFvMesh \ -llduSolvers \ -L\$(MESQUITE_LIB_DIR) -lmesquite
I don't kown where is wrong. Could you help me.

Best regards
Fan Fei

December 3, 2014, 10:51
#34
Member

Fei Fan
Join Date: Jun 2013
Location: NanJing, China
Posts: 49
Rep Power: 4
Quote:
 Originally Posted by Fanfei Hi, I copy all the library you used. And I found some library are different in extend version. so I'm trying to find where is wrong. Best regards Fan Fei
Hi HECKMANN Frédéric:
I find the reason of this error, which is caused by the incompatiable of creatDynamicFvMesh.H and creatFamesh.H. The creatFamesh is used to create a areField to use FAM. As deleted #include "creatFamesh.H", it will be work. But the warnning is still there. As dynamicMesh I has a question. in our program pointdisplacement is used, that means the point of bounday patch will move, however, in fvSolition the cellDisplacement is used, is that mean the value will interpolated from point to cell(Vol), is that right? I so sorry to trouble you again, but i hope i can get some help. Thanks.

Best regards
Fan Fei

 December 3, 2014, 20:08 #35 Senior Member   HECKMANN Frédéric Join Date: Jul 2010 Posts: 237 Rep Power: 8 In openfoam and most CFD software, you can only move the nodes. Indeed, the cell is built from the nodes coordinate. Usually we only move the nodes of a boundary and after we ask a "solver" to find the position of the nodes of the domain. The solver will move the nodes of the domain (not those of the boundaries) according to a law that you specify. The Laplace law is often used because it is robust (it consider the rotation) but you can also use a proportional displacement that will act as a spring that push the nodes with a force that decrease as you go away from the boundary. There are tens of morphing solver and each one has its advantages and drawbacks. You have to choose it depending of the motion you are expecting.

 February 7, 2015, 18:12 #36 New Member   Join Date: Apr 2009 Posts: 11 Rep Power: 9 Hi Frédéric, Thanks for your nice job. I could adapt your code to my application. The only problem is that the mesh is moving as what is defined but only at the first time step. while (runTime.loop()) { PointDisplacement.boundaryField()[patchID] == dispVals; Info<< "Time = " << runTime.timeName() << endl; //mesh.movePoints(motionPtr->newPoints()); mesh.moving(); mesh.update(); runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; }

 February 7, 2015, 22:45 #37 Senior Member   HECKMANN Frédéric Join Date: Jul 2010 Posts: 237 Rep Power: 8 Hi, I think that your solver is ok. The problem might be located in your "0" folder and in the "pointdisplacement" file. From my guess the "pointdisplacement" file is not updated/forwarded to next time step.

 February 23, 2015, 10:54 #38 Member   Join Date: Mar 2013 Posts: 92 Rep Power: 5 Hi to all, I'm doing simulations moving a wall boundary where the dispacement of the movement is chosen by a variable evaluated during the simulation. The first movement steps work very well but at certain iteration I encounter the same problem shown by Vrede in the post #25. I was thinking to use add/remove layers to solve it. Does anyone have some ideas to solve it? Vrede, did you solve the problem? Thanks to all Regards Giacomo

 February 23, 2015, 11:11 #39 Member   Join Date: Jul 2014 Posts: 37 Rep Power: 3 Hi Giacomo No, sorry, I have not solved this problem yet. I do not know if there is any existing utility to remove points when faces overlap. You could try to identify and remove these points and then define the corresponding faces with the new point, but this will be brute force. Sorry, I could not help more

 March 2, 2015, 09:32 #40 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,688 Rep Power: 27 Dear all, I find it interesting to have a thread, where these things are being discussed. I have noticed above that it was suggested to use the faceToPointInterpolation method, which is available in the PrimitivePatchInterpolation class. I have just finalised a paper where the mass conserving properties of this exact interpolation scheme was analysed (http://onlinelibrary.wiley.com/doi/1....4015/abstract). The conclusion was that the scheme does not conserve the volume of sand in the bed, when the bed level change is interpolated from the faces to the points. This lack of mass conservation is not uniquely related to sediment transport and morphodynamics. There are several issues related to error, but to mention a few: There is not made a projection of the distance weights onto the horizontal plane. This means that the interpolation weights change over time, as the boundary deforms. This even though the displacements are perpendicular to the horizontal plane. In 2D simulations, the width of the computational domain in the empty direction has an effect on the mass conservation error. This is solely related to the fact that the weights are from the faces to the points. For instance, on non-equidistant grids and very wide meshes in the empty direction, the interpolation becomes a simple average (identical weights for all points). This is obviously not correct, since the mesh is defined as non-equidistant. An alternative interpolation method is proposed in the same paper. I hope that these finding are valuable for some of you. Kind regards, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post volo87 CFX 5 June 14, 2013 17:44 happy CFX 14 September 6, 2012 01:54 Arnoldinho OpenFOAM Running, Solving & CFD 0 May 17, 2011 12:48 Pankaj CFX 9 November 23, 2009 05:05 liu OpenFOAM Running, Solving & CFD 6 December 30, 2005 18:27

All times are GMT -4. The time now is 21:06.

 Contact Us - CFD Online - Top