
[Sponsors] 
[solids4Foam] Master point addressing is not correct! 

LinkBack  Thread Tools  Search this Thread  Display Modes 
September 5, 2019, 16:59 
[solids4Foam] Master point addressing is not correct!

#1 
Senior Member
Ali Shayegh
Join Date: Oct 2015
Posts: 126
Rep Power: 9 
Hi,
I am on a simulation of deformation of a solid body due to fluid flow using solids4Foam. Since I faced with the divergence of the simulation, I tried more stiff solid, then gradually loosen it every 5s of physical time of the problem. The last time that I loosen it (say at t=20s) and started solids4Foam, I got the following error: Code:
> FOAM FATAL ERROR: Master point addressing is not correct Code:
startFrom latestTime; 

September 6, 2019, 08:31 

#2 
Senior Member
Ali Shayegh
Join Date: Oct 2015
Posts: 126
Rep Power: 9 
As I understood, in the latest time step, there are some intersection points between solid and fluid interface zones. In the attached figure, red zones are fluid zone and white zones are solid zone. Does this intersection cause the problem of:
Code:
Extended GGI, master point distance, max: 1e+15, avg: 4.16667e+13, min: 0.0181481 > FOAM FATAL ERROR: Master point addressing is not correct I think using conforming mesh is helpful, because it may cause avoiding the problem of intersection of zones, may it? 

September 6, 2019, 08:49 

#3 
Senior Member
Ali Shayegh
Join Date: Oct 2015
Posts: 126
Rep Power: 9 
Another workaround for this problem is to use time varying stiffness rather than stopping the simulation and restarting it by a different stiffness (Young's modulus). But does anyone (specifically bigphil) know how to implement it in constant/solid/mechanicalProperties ?
(I think it would be better to post this as a new thread in order to make it more easy to be searched.) 

September 7, 2019, 05:39 

#4  
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 19 
Quote:
That error is due to the intersection of the boundaries at the interface which means the implicit fsi coupling loop could not achieve proper convergence within the specified max number of iteration. I guess you didn't receive this error before stopping the simulation for another restart due to the fact that you have not set the interpolator to get updated during the simulation! If you did so, you would have received the exact same error! For the time varying Young modulus and If you are using a linear elastic material model for the solid part, just create a new material model based on the following class: Code:
src/solids4FoamModels/materialModels/mechanicalModel/mechanicalLaws/linearGeometryLaws/linearElastic From the physical point of view and I'm not an expert in solid mechanics (@bigphil can help us here), do you expect a final steadystate result? Let me explain myself better, consider these two scenarios: 1 Set Young modulus to the real value from the beginning of the simulation and run the case for 30 seconds. 2 Define Young modulus using time dependent formulation and run the case for 30 seconds. Do you expect an identical final deformation for both cases? Regards, D. Khazaei 

September 8, 2019, 03:32 

#5  
Senior Member
Ali Shayegh
Join Date: Oct 2015
Posts: 126
Rep Power: 9 
Hi Daniel,
Quote:
Quote:
Code:
// 0 means the interpolator is update every timestep, whereas 10 would be // every 10 timesteps // Defaults to 0 // interpolatorUpdateFrequency 0; Quote:
Code:
E(t) = (EDesired  EStart) * (t)/(tDesired) + EStart In order to do so, I tried to modify neoHookeanElastic. The modified version, however, is not compiled successfully till now. The major modifications in *.C are: Code:
//** Constructors **// . . . EDesired_(dict.lookup("EDesired")), EStart_(dict.lookup("EStart")), tDesired_(dict.lookup("tDesired")), E_ ( IOobject ( "E", mesh.time().timeName(), mesh, IOobject::READ_IF_PRESENT, IOobject::AUTO_WRITE ), mesh, dimensionedScalar("zero", dimPressure, 0.0) calcE() ) //** Private Member Functions **// . . . Foam::tmp<Foam::volScalarField> Foam::neoHookeanElasticTimeVaryingE::calcE() const { scalar current_time((mesh.time()).value()); if (current_time < tDesired_.value()) { return ( (EDesired_  EStart_)/tDesired*(current_time ) + EStart ); } else { return ( EDesired_ ); } } Code:
public mechanicalLaw { // Private data . . . // Young's modulus volScalarField E_; . . . // Member Functions // Return the time varying E const volScalarField& E() const { return E_; } // Correct E void correct() { E_ = calcE(); } Quote:


September 8, 2019, 10:20 

#6  
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 19 
Quote:
Although it is written that "0 means the interpolator is updated every timestep", this piece of code in fluidSolidInterface.C which is responsible of updating interpolator is doing things differently! It doesn't update interpolator every timestep when interpolatorUpdateFrequency is set to 0: (take a look at the red line) Code:
void Foam::fluidSolidInterface::updateInterpolatorAndGlobalPatches() { if (!ggiInterpolatorPtr_) { ggiInterpolator(); } else if (interpolatorUpdateFrequency_ != 0) { if (((runTime().timeIndex()  1) % interpolatorUpdateFrequency_) == 0) { deleteDemandDrivenData(ggiInterpolatorPtr_); fluid().clearGlobalPatch(); solid().clearGlobalPatch(); fluid().makeGlobalPatch ( fluidMesh().boundaryMesh()[fluidPatchIndex_].name() ); solid().makeGlobalPatch ( solidMesh().boundaryMesh()[solidPatchIndex_].name() ); ggiInterpolator(); } } } Quote:
Regards, D. Khazaei 

September 8, 2019, 12:02 

#7 
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 19 
find the modified version of both linearElastic and neoHookeanElastic below
successfully compiled on foamextend4.0 but didn't have time to run a case... 

September 11, 2019, 08:24 

#8 
Senior Member
Ali Shayegh
Join Date: Oct 2015
Posts: 126
Rep Power: 9 
Dear Daniel,
I ran a case with timeVaryingNeoHookean model, without any problem. Sincerely, Ali 

September 27, 2021, 09:59 

#9 
New Member
Philipp Conen
Join Date: Jul 2021
Location: Germany, NRW
Posts: 22
Rep Power: 3 
Dear Foamers,
regarding my thesis, I am working on an FSI for an aircraft wing. I run the "microBeamInCrossFlow" tutorial case and it works. I wanted to have the exact setup, but with the geometry of my wing model. So I exported the existing case from ANSYS and imported it with Code:
fluentMeshToFoam writeZones When I now run solids4Foam I get the message: "Master point addressing is not correct..". Since I read this thread and tried to play around with the parameters I have no idea what I am looking for to fix this error. Could it be, that the mesh is broken? Do you have any other ideas? Here I like to present my case: https://github.com/PhilippConen/Ope...aftWing2WFSI And pictures are attached. Here you can see the log: Code:
solids4Foam /**\  =========    \\ / F ield  foamextend: Open Source CFD   \\ / O peration  Version: 4.1   \\ / A nd  Web: http://www.foamextend.org   \\/ M anipulation  For copyright notice see file Copyright  \**/ Build : 4.170b064d0f326 Exec : solids4Foam Date : Sep 27 2021 Time : 14:53:09 Host : "philippMS7A38" PID : 27236 CtrlDict : "/home/philipp/foam/philipp4.1/run/OF/2021_09_27/crossFlow_Own/system/controlDict" Case : /home/philipp/foam/philipp4.1/run/OF/2021_09_27/crossFlow_Own nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). allowSystemOperations : Disallowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time /**\  For further information on the solids4Foam toolbox implementations,   please see the following publications:     P. Cardiff, A Karac, P. De Jaeger, H. Jasak, J. Nagy, A. Ivankovic,   Z. Tukovic: An opensource finite volume toolbox for solid mechanics and   fluidsolid interaction simulations. arXiv:1808.10736v2, 2018, available   at https://arxiv.org/abs/1808.10736.     Z. Tukovic, A. Karac, P. Cardiff, H. Jasak, A. Ivankovic: OpenFOAM   finite volume solver for fluidsolid interaction. Transactions of   Famena, 42 (3), pp. 131, 2018, 10.21278/TOF.42301.  \**/ Selecting physicsModel fluidSolidInteraction Selecting fluidSolidInterface method Aitken Selecting fluidModel icoFluid Selecting dynamicFvMesh dynamicMotionSolverFvMesh Selecting motion solver: velocityLaplacian Selecting motion diffusion: quadratic Selecting motion diffusion: inverseDistance g field not found in constant directory: initialising to zero Selecting solidModel nonLinearGeometryUpdatedLagrangian Selecting dynamicFvMesh staticFvMesh Creating fixedDisplacement boundary condition Creating solidTraction boundary condition limiter coefficient: 1 underrelaxation method: fixed Creating the mechanicalModel Selecting mechanical law neoHookeanElastic additionalMeshCorrection: false Selecting interfaceToInterfaceMapping GGI Courant Number mean: 2.74902e06 max: 0.00510776 velocity magnitude: 30 deltaT = 1.2e06 Time = 1.2e06 Setting traction on solid interfaces Interpolating face values using GGI Create GGI zonetozone interpolator interfacetointerface face error: 0.0847933 calcMasterPointAddressing() const Extended GGI, master point distance, max: 1e+15, avg: 3.5137e+11, min: 1.08721e14 > FOAM FATAL ERROR: Master point addressing is not correct From function GGIInterpolation::masterToSlavePointInterpolate(const Field<Type> pf) in file /home/philipp/foam/foamextend4.1/src/foam/lnInclude/GGIInterpolation.C at line 492. FOAM aborting Abgebrochen (Speicherabzug geschrieben) 

September 27, 2021, 11:04 

#10 
New Member
Philipp Conen
Join Date: Jul 2021
Location: Germany, NRW
Posts: 22
Rep Power: 3 
While cross reading this thread:
FSI simulation of a Wind Turbine I tried to increase the solid mesh. Switching the element size from 0.005mm to 0.001mm results in hugh mesh with 1.7 million cells. I was able to get rid of the mentioned error. But after one iteration the solver just stops without a foam error message, but a floating point exception (memory dump written). After some tries I get to know that:  With 0.002mm element size: Master point error  With 0.0015mm element size: Floating point exception Are there further ideas? Here are my logs: Code:
*\  =========    \\ / F ield  foamextend: Open Source CFD   \\ / O peration  Version: 4.1   \\ / A nd  Web: http://www.foamextend.org   \\/ M anipulation  For copyright notice see file Copyright  \**/ Build : 4.170b064d0f326 Exec : solids4Foam Date : Sep 27 2021 Time : 15:51:29 Host : "philippMS7A38" PID : 29337 CtrlDict : "/home/philipp/foam/philipp4.1/run/OF/2021_09_27/crossFlow_Own/system/controlDict" Case : /home/philipp/foam/philipp4.1/run/OF/2021_09_27/crossFlow_Own nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). allowSystemOperations : Disallowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time /**\  For further information on the solids4Foam toolbox implementations,   please see the following publications:     P. Cardiff, A Karac, P. De Jaeger, H. Jasak, J. Nagy, A. Ivankovic,   Z. Tukovic: An opensource finite volume toolbox for solid mechanics and   fluidsolid interaction simulations. arXiv:1808.10736v2, 2018, available   at https://arxiv.org/abs/1808.10736.     Z. Tukovic, A. Karac, P. Cardiff, H. Jasak, A. Ivankovic: OpenFOAM   finite volume solver for fluidsolid interaction. Transactions of   Famena, 42 (3), pp. 131, 2018, 10.21278/TOF.42301.  \**/ Selecting physicsModel fluidSolidInteraction Selecting fluidSolidInterface method Aitken Selecting fluidModel icoFluid Selecting dynamicFvMesh dynamicMotionSolverFvMesh Selecting motion solver: velocityLaplacian Selecting motion diffusion: quadratic Selecting motion diffusion: inverseDistance g field not found in constant directory: initialising to zero Selecting solidModel nonLinearGeometryUpdatedLagrangian Selecting dynamicFvMesh staticFvMesh Creating fixedDisplacement boundary condition Creating solidTraction boundary condition limiter coefficient: 1 underrelaxation method: fixed Creating the mechanicalModel Selecting mechanical law neoHookeanElastic additionalMeshCorrection: false Selecting interfaceToInterfaceMapping GGI Courant Number mean: 2.74902e06 max: 0.00510776 velocity magnitude: 30 deltaT = 1.2e06 Time = 1.2e06 Setting traction on solid interfaces Interpolating face values using GGI Create GGI zonetozone interpolator interfacetointerface face error: 0.145588 calcMasterPointAddressing() const Extended GGI, master point distance, max: 7.31739e05, avg: 1.08881e06, min: 1.68008e05 interfacetointerface point error: 7.31739e05 Number of uncovered master faces: 1 Number of uncovered slave faces: 3 Total force on fluid interface 0: (0 0 0) Total force on solid interface 0: (0 0 0) Evolving solid solver Solving the updated Lagrangian form of the momentum equation for DD setCellDisplacements: reading cellDisplacements Corr, res, relRes, matRes, iters Both residuals have converged 2, 0, 0, 0, 0 Interpolating point values using GGI Interpolating point values using GGI FSI relative residual1 norm for interface 0: 0 FSI residual2 norm for interface 0: 0 Time = 1.2e06, iteration: 1 Current fsi underrelaxation factor (fixed): 0.05 Maximal accumulated displacement of interface 0: 0 GAMG: Solving for cellMotionUx, Initial residual = 0, Final residual = 0, No Iterations 1 GAMG: Solving for cellMotionUy, Initial residual = 0, Final residual = 0, No Iterations 1 GAMG: Solving for cellMotionUz, Initial residual = 0, Final residual = 0, No Iterations 1 GAMG: Solving for cellMotionUx, Initial residual = 0, Final residual = 0, No Iterations 1 GAMG: Solving for cellMotionUy, Initial residual = 0, Final residual = 0, No Iterations 1 GAMG: Solving for cellMotionUz, Initial residual = 0, Final residual = 0, No Iterations 1 Evolving fluid model: icoFluid Courant Number mean: 3.29882e06 max: 0.00612931 velocity magnitude: 30 PISO: Operating solver in PISO mode DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 4.40629e08, No Iterations 1 DILUPBiCG: Solving for Uy: solution singularity DILUPBiCG: Solving for Uz: solution singularity GAMG: Solving for p, Initial residual = 1, Final residual = 6.34219e07, No Iterations 15 GAMG: Solving for p, Initial residual = 0.131569, Final residual = 8.61138e07, No Iterations 11 time step continuity errors : sum local = 1.53686e07, global = 2.84692e08, cumulative = 2.84692e08 GAMG: Solving for p, Initial residual = 0.0254475, Final residual = 8.75811e07, No Iterations 10 GAMG: Solving for p, Initial residual = 0.00591659, Final residual = 4.72096e07, No Iterations 9 time step continuity errors : sum local = 8.81695e08, global = 1.36805e08, cumulative = 4.21497e08 GAMG: Solving for p, Initial residual = 0.00166295, Final residual = 6.54635e07, No Iterations 7 GAMG: Solving for p, Initial residual = 0.000494962, Final residual = 8.44851e07, No Iterations 5 time step continuity errors : sum local = 1.57978e07, global = 3.92148e09, cumulative = 4.60711e08 Setting traction on solid interfaces Interpolating face values using GGI Total force on fluid interface 0: (3825.75 15123.4 21189.2) Total force on solid interface 0: (3833.97 15118.3 21186.4) Evolving solid solver Solving the updated Lagrangian form of the momentum equation for DD GleitkommaAusnahme (Speicherabzug geschrieben) 

June 4, 2022, 04:51 
Master point addressing is not correct!

#11  
New Member
Anas Muhamad Pauzi
Join Date: Nov 2019
Posts: 16
Rep Power: 5 
Hi Daniel Khazaei, Ali Shayegh, and respected readers,
I think I'm having the same problem. Quote:
Quote:
How can I restart this simulation again? Thank you ANAS 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Injection initialization generate a segmentation fault!!  zahrae  Fluent UDF and Scheme Programming  11  July 9, 2019 20:00 
Moving mesh  Niklas Wikstrom (Wikstrom)  OpenFOAM Running, Solving & CFD  122  June 15, 2014 07:20 
[blockMesh] BlockMeshmergePatchPairs  hjasak  OpenFOAM Meshing & Mesh Conversion  11  August 15, 2008 08:36 
[Gmsh] Gmsh and samplesurface  touf  OpenFOAM Meshing & Mesh Conversion  2  December 10, 2007 03:27 
CFX4.3 build analysis form  Chie Min  CFX  5  July 13, 2001 00:19 