time step continuity error, fvScheme

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

 May 11, 2010, 09:23 time step continuity error, fvScheme #1 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi, I am working on a 3D Mesh(4 million cells-300MBsize). I am using simpleFoam (turbulent modeling-similar to the one given in tutorials//incompressible/simpleFoam/pitzDaily ). I have changed the Boundary conditions according to the problem statement.(NOTE: for modeling wall -'wedge' constraint is used..for rotational periodic). I am getting the following error. ------------------------------------------------------------------------ Create time Create mesh for time = 0 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting RAS turbulence model kEpsilon kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; sigmaEps 1.3; } Starting time loop Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0897376, No DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0695567, No DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0733983, No DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00982204, No It erations 951 time step continuity errors : sum local = 9.06009e-05, global = -6.32167e-06, cu mulative = -6.32167e-06 #0 Foam::error:rintStack(Foam::Ostream&) in "/usr/logau/expsm/OpenFOAM/OpenFO AM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/usr/logau/expsm/OpenFOAM/OpenFOAM-1.6/ lib/linux64GccDPOpt/libOpenFOAM.so" #2 ?? in "/lib64/libc.so.6" #3 void Foam::magSqr, Foam::fvPatchField, Foam::volMes h>(Foam::GeometricField&, Foam::Geome tricField, Foam::fvPatchField, Foam::volMesh> const&) i n "/usr/logau/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleR ASModels.so" #4 Foam::tmp > Foam::magSqr, Foam::fvPatchField, Foam::volMesh>(Foam:: tmp, Foam::fvPatchField, Foam::vol Mesh> > const&) in "/usr/logau/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/l ibincompressibleRASModels.so" #5 Foam::incompressible::RASModels::kEpsilon::correct () in "/usr/logau/expsm/Op enFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so" #6 main in "/usr/logau/expsm/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccD POpt/simpleFoam" #7 __libc_start_main in "/lib64/libc.so.6" #8 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start. S:116 floating decimal point exception --------------------------------------------------------------------- Could anyone please tell what may the problem? Thank You, Achinta Last edited by achinta; May 11, 2010 at 09:59.

 May 11, 2010, 09:30 Solution which I tried #2 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi once again, I tried following techniques..None of them worked. 1.Reduce time step. 2.Increase value of epsilon 3.Reduce relaxation factor. 4.Modify fvScheme. 5.Modify fvSolution. 6.reduce inlet velocity. Please suggest anyother methods. Thank You, Achinta

 May 11, 2010, 16:18 #3 Member   Alan Russell Join Date: Aug 2009 Location: Boise, Idaho USA Posts: 61 Rep Power: 10 I think you have something wrong with your setup - like the wrong kind of boundary conditions or something like that. The time step continuity is just the first error that's getting posted. First, make sure all the boundaries in the /0 directory files (U, p, epsilon ...) are the same type as what's stated in the /constant/polymesh/boundary file. For example, if in the boundary file you have a inlet patch called minX, and an outlet patch maxX, then /0/p needs to have the right conditions on these patches (typically zeroGradient at the inlet and uniform 0 at the outlet. Your error happened after the time step continuity check and before k and epsilon. I would check the k file boundaries first. The tutorial will help you figure this out. Some errors in OF tell you exactly where the problem is, and some are a bit more cryptic. Make sure you are running simpleFoam from the main case directory and not /system or /constant - that will give you errors also. If you want to temporarily simplify the solver, go in /constant/RASProperties and set turbulence off. The solver will skip k and epsilon, and might tell you exactly where the problem is - if the solver runs properly, then your k or epsilon files in /0 are the problem. So, I would start by checking boundary conditions, and if you don't find the problem turn turbulence off. If you need a 3d tutorial for an example, use motorBike (it runs simpleFoam with k-epsilon turbulence). Good luck, Alan

 May 12, 2010, 02:43 #4 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 Make sure your epsilon is not initialized with 0.

 May 12, 2010, 08:28 #5 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi Santhosh, K and epsilon are initialized to .000605 and .0003532 respectively. Is there a probability of Boundary conditions mistake? or with the mesh ? Thank you Cheers, Achinta Last edited by achinta; May 12, 2010 at 08:45.

 May 12, 2010, 08:44 #6 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi Alan, 1) Boundary conditions in /0 are of the same type as stated in boundary file. 2)k values seems to be fine,, --------------------------------------------------------------------------------- dimensions [0 2 -2 0 0 0 0]; internalField uniform 0.000605; boundaryField { INLET_AIR { type fixedValue; value uniform 0.000605; } OUTLET { type zeroGradient; } SYM1 { type kqRWallFunction; value uniform 0.000605; } SYM2 { type kqRWallFunction; value uniform 0.000605; } WALL { type kqRWallFunction; value uniform 0.000605; } INLET_GAS { type fixedValue; value uniform 0.000605; } -------------------------------------------------------------------------------------------------------- 3) I turned the turbulence off. It solved 1 time step completely(earlier it showed error while solving 1st time step. But there was error in 2nd time step.. ------------------------------------------- Create time Create mesh for time = 0 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting RAS turbulence model kEpsilon kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; sigmaEps 1.3; } Starting time loop Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0146234, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.05305, No I terations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.052276, No Iterations 1 DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00989021, No It erations 664 time step continuity errors : sum local = 0.00162561, global = -0.000143816, cum ulative = -0.000143816 ExecutionTime = 147.82 s ClockTime = 149 s Time = 2 #0 Foam::error:rintStack(Foam::Ostream&) in "/usr/defoe/expsm/OpenFOAM/OpenFO AM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/ lib/linux64GccDPOpt/libOpenFOAM.so" #2 ?? in "/lib64/libc.so.6" #3 void Foam::fvc::surfaceIntegrate >(Foam::Field >&, Foam::GeometricField, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux 64GccDPOpt/libfiniteVolume.so" #4 Foam::tmp, Foam::fvPatchField, Foa m::volMesh> > Foam::fvc::surfaceIntegrate >(Foam::Geometric Field, Foam::fvsPatchField, Foam::surfaceMesh> const&) in " /usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so" #5 Foam::tmp, Foam::fvPatchField, Foa m::volMesh> > Foam::fvc::surfaceIntegrate >(Foam::tmp, Foam::fvsPatchField, Foam::surfaceMesh> > const&) in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfinite Volume.so" #6 Foam::fv::gaussDivScheme >::fvcDiv(Foam::GeometricField , Foam::fvPatchField, Foam::volMesh> const&) in "/usr/defoe /expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so" #7 Foam::tmp, Foam ::Tensor >::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div >(Foam::GeometricField, Foam::fvPatchFie ld, Foam::volMesh> const&, Foam::word const&) in "/usr/defoe/expsm/OpenFOAM/Open FOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so" #8 Foam::tmp, Foam ::Tensor >::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div >(Foam::GeometricField, Foam::fvPatchFie ld, Foam::volMesh> const&) in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux6 4GccDPOpt/libincompressibleRASModels.so" #9 Foam::incompressible::RASModels::kEpsilon::divDevR eff(Foam::GeometricField, Foam::fvPatchField, Foam::volMesh>&) const in "/usr/defoe/e xpsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so" #10 main in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64Gcc DPOpt/simpleFoam" #11 __libc_start_main in "/lib64/libc.so.6" #12 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start .S:116 Floating decimal point exception ----------------------------------------------------------------------------------- Is k epsilon model good enough for 3D model(Gas turbine combustion model)? Most of the errors mention /OpenFOAM-1.6/lib/linux64GccDPOpt dirctory.... Is there any mistake in set up files? Or is there is anything wrong with mesh? Thank You Cheers, Achinta

 May 12, 2010, 09:05 #7 New Member   Christian Join Date: Feb 2010 Location: Payerne, Switzerland Posts: 9 Rep Power: 9 Hey, There is probably something wrong with the physic of your flow but to visualize that you need more time steps. In order to perform more time step you can decrease your relaxation factor in system/fvSolution or better change your numerical schemes in system/fvSchemes for example switch your laplacianSchemes to Gauss linear limited 0.6 for all variables and your divSchemes for U to Gauss limitedLinearV 1. Hope that it would be enough to get more time steps. Best regards Christian

 May 12, 2010, 12:01 #8 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi Christian, I have used wedge boundary condition (for rotational periodic condition) for my cylinder wall. Could that be a source of the problem? My mesh is 3D. Thank You Achinta

 May 12, 2010, 12:42 #9 New Member   Christian Join Date: Feb 2010 Location: Payerne, Switzerland Posts: 9 Rep Power: 9 Hi Achinta, I m sorry but it is out of my knowledge, I am currently working with MRFSimpleFoam (but without periodic condition) and I also have to deal with the floating point exception errors. But with more time steps you would be able to visualize the flow in Paraview (stay in the Euler case) and maybe you will find the problem. Christian

 May 13, 2010, 13:23 #10 Member   Alan Russell Join Date: Aug 2009 Location: Boise, Idaho USA Posts: 61 Rep Power: 10 Achinta, Can you modify your setup to temporarily remove the rotational periodic boundary condition? I agree with Christian, there's probably something wrong with the physics of the flow. I would try the default fvSchemes first. I had many crashes while experimenting with non-default fvSchemes after the default setup worked well. The basic approach is to simplify everything - coarse mesh, simple boundaries, default solutions, etc. This might let you run more time steps so you can look at the flow in ParaView. Once you get the simple version to work, start adding complexity until you get to the simulation you want (rotating boundaries, etc.). Alan

 May 14, 2010, 04:03 #11 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 Hi, Some hints, 1. check the quality of the mesh (checkMesh) 2. increase orthogonal correctors (system/fvSolution) 3. use potential foam to initialize 4. Reduce the relaxation factors (system/fvSolution) Regards, Santhosh.

 May 15, 2010, 06:20 #12 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi, I am using default fvschemes..and default fvsolution... The mesh is coarse too..and I have removed rotational periodic condition.. Same error this time too.. I am using prism cells near the wall.. Could that be a problem?..because its working fine for mesh without prism cells.. Isnt it strange? Is there a solution for this problem? Thank You, Kind regards, Achinta

 May 16, 2010, 11:26 #13 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 prism are always not good for CFD...what is your meshCheck is saying. As I already suggest increase the nonOrthogonalcorrector rather than default settings. santhosh

 May 17, 2010, 04:25 #14 Senior Member     Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,274 Rep Power: 23 How large is your time step and what is the corresponding Courant number?

 May 17, 2010, 07:50 #15 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi Santhosh, I increased nonorthogonal corrector to 20. But it didnt give results. I applied checkMesh. It gave 4 errors. ---------------------------------------- Mesh stats points: 72486 faces: 631844 internal faces: 613931 cells: 298120 boundary patches: 4 point zones: 0 face zones: 1 cell zones: 1 Overall number of cells of each type: hexahedra: 0 prisms: 53255 wedges: 0 pyramids: 30 tet wedges: 0 tetrahedra: 244825 polyhedra: 10 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology INLET 265 214 ok (non-closed singly connected) WALL 10658 5502 ok (non-closed singly connected) OUTLET 741 528 ok (non-closed singly connected) SYM 6249 3973 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (0 -0.05 -0.0500799) (0.5 0.05 5.21766e-10) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) ***Boundary openness (-5.64149e-13 1.37356e-13 -0.000140076) possible hole in boundary description. ***Open cells found, max cell openness: 1, number of open cells 46 <

 May 17, 2010, 07:54 #16 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi Anton, I am working on a steady-state problem. I am using default time-step of 1.( I had decreased it to .1 to see if it could work. But it failed.). Thank You. Regards, Achinta

 May 18, 2010, 03:03 #17 Senior Member     Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,274 Rep Power: 23 There is something wrong with your mesh. Read your blockMesh file carefully with the user manual page for axisymmetric meshes next to you. There shouldn't be no open cells and no incorrectly oriented faces. And since it looks like you are trying to build a pipe: You'll need inlet, outlet, wall (the curved surface) and wedge (both planes that intersect at the symmetry axis).

 May 18, 2010, 04:13 #18 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi, Is it necessary that the angle between the two wedge patches be 5 degrees? Can we use wedge boundary condition if the angle between the wedges is 180 degrees? Thank You. Regards, Achinta

 May 18, 2010, 06:49 #19 Senior Member     Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,274 Rep Power: 23 Why use a wedge if the angle is 180 degrees? Wouldn't symmetry be what you want in that case? Apart from that, no the angle doesn't necessarily have to be 5 degrees, see: http://www.cfd-online.com/Forums/ope...type-bcbs.html

 May 19, 2010, 06:51 #20 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi, The physics of the problem requires rotational periodic condition which is not possible with 'symmetryPlane'. So I need 'wedge'. Is there any other way to implement the rotational periodic condition? Regards, Achinta

 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 irishdave OpenFOAM Running, Solving & CFD 30 September 19, 2017 12:38 meangreen Main CFD Forum 5 August 27, 2009 12:32 gopala OpenFOAM Running, Solving & CFD 0 April 27, 2009 10:46 skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48 Sanjay Padhiar Main CFD Forum 1 March 31, 1999 12:32

All times are GMT -4. The time now is 08:23.