
[Sponsors] 
May 9, 2016, 03:46 
Error in using rhoSimpleFoam

#1 
New Member
Join Date: May 2016
Posts: 28
Rep Power: 2 
Hello again,
I am writing here again since OpenFOAM gives me an error and I have no idea how to solve. I am trying to solve the aerodynamic field around an airfoil with rhoSimpleFoam (I need also the temperature field): the mach number is 0.288. I prescribed total pressure and temperature at the inlet, static pressure and zero gradient temperature and velocity at the outlet, which seems to be the correct way. By the way, after three time steps, OpenFOAM returns this error: > FOAM FATAL ERROR: Maximum number of iterations exceeded From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const in file /u1/sales/OpenFOAM/OpenFOAM3.0.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. FOAM aborting I tried to change something in fvSchemes file, using limiters, but it doesn't work. Here you can find my case with the log: naca0012withTemp Thank you in advance for replying. Last edited by g.freeman; May 9, 2016 at 04:49. 

May 9, 2016, 06:53 

#2 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
Hello,
the problem here is that OpenFOAM can not calculate the temperature field out of the enthalpy field. If I remember correctly the temperature field is calculated in the thermo  model based on the enthalpy and vice versa. If for any reason the enthalpy / temperature field diverges the result is that message. For that a) check your simulation before the error; b) check if you underrelax the necessary fields and c) use upwind scheme first. I can imagine that your mesh causes the problem (some cell).
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

May 12, 2016, 03:52 

#3  
New Member
Join Date: May 2016
Posts: 28
Rep Power: 2 
Quote:
I did what you suggest and it seems it is all ok; I was using upwind scheme as default. I also changed the mesh (using a coarse and a better one) but the same error appears. With the coarse mesh it appears later, but it still appears. 

May 12, 2016, 05:59 

#4 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
Hi,
then there has to be something wrong. When does that error appear? The best way would be (really) to get the iterations before your solver blow up and check this with paraview. You should be able to see the cells where the problem starts.
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

May 12, 2016, 06:05 

#5  
New Member
Join Date: May 2016
Posts: 28
Rep Power: 2 
Quote:
as the log.rhoSimpleFoam reports, the error appears after just 3 iterations: Time = 3 smoothSolver: Solving for Ux, Initial residual = 0.210427, Final residual = 0.0024659, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 0.227503, Final residual = 0.00264876, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.990159, Final residual = 0.00557005, No Iterations 1 > FOAM FATAL ERROR: Maximum number of iterations exceeded From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const in file /u1/sales/OpenFOAM/OpenFOAM3.0.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. FOAM aborting #0 Foam::error:rintStack(Foam::Ostream&) in "/u1/ sales /OpenFOAM/OpenFOAM3.0.x/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/u1/ sales /OpenFOAM/OpenFOAM3.0.x/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so" #2 Foam::hePsiThermo<Foam:siThermo, Foam:ureMixture<Foam::constTransport<Foam::speci es::thermo<Foam::hConstThermo<Foam:erfectGas<Foa m::specie> >, Foam::sensibleEnthalpy> > > >::calculate() in "/u1/ sales /OpenFOAM/OpenFOAM3.0.x/platforms/linux64IccDPInt32Opt/lib/libfluidThermophysicalModels.so" #3 Foam::hePsiThermo<Foam:siThermo, Foam:ureMixture<Foam::constTransport<Foam::speci es::thermo<Foam::hConstThermo<Foam:erfectGas<Foa m::specie> >, Foam::sensibleEnthalpy> > > >::correct() in "/u1/ sales /OpenFOAM/OpenFOAM3.0.x/platforms/linux64IccDPInt32Opt/lib/libfluidThermophysicalModels.so" #4 ? in "/u1/ sales /OpenFOAM/OpenFOAM3.0.x/platforms/linux64IccDPInt32Opt/bin/rhoSimpleFoam" #5 __libc_start_main in "/lib64/libc.so.6" #6 ? in "/u1/ sales /OpenFOAM/OpenFOAM3.0.x/platforms/linux64IccDPInt32Opt/bin/rhoSimpleFoam" Abort I will try to use paraview and undestand which cell creates the problem now. Thank you for the help 

May 12, 2016, 06:27 

#6 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
Hi,
it is just a guess that you have problems on a cell. Maybe it is due to your boundary conditions, then you should find the problem on the boundary face. Save iteration 1 and 2 and check it out. Also check your mass conservation and other stuff. To get a better idea it could help to underrelax with 0.05 to get more iterations (then you will get more data for postprocessing).
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

May 12, 2016, 08:50 

#7 
New Member
Join Date: May 2016
Posts: 28
Rep Power: 2 
So, even if I change my underelaxtion factors, it continues to work until t=3, at t=2 the values are in the expected range so it quite hard to detect which cells cause the divergence.
For the boundary condition, I checked which are to use in the book of Ferziger and Peric (computational methods for fluid dynamics) 

May 12, 2016, 10:28 

#8 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
Can you share your case? Sometimes is obvious where the problem is located but can not be analyzed without the case (:
Finally, most of the time it is due to cells but in your case it seems that there is something wrong with your BC or solversettings or sth. else.
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

May 12, 2016, 10:47 

#9  
New Member
Join Date: May 2016
Posts: 28
Rep Power: 2 
Quote:


May 12, 2016, 11:20 

#10 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
Hello,
I think you made a snappyHexMesh meshing and then extrude to 2d? Your mesh looks okay in the first view but the mesh around your airfoil is very bad (see picture). From one cell to the your layers you have a ratio that is too high. But that is not the main problem. The problem is related to your boundary conditions. P for inlet and outlet is similar (no pressure drop) and your velocity bc are wrong too. There is no flow and the system is not prescribed in good conditions. Either, fixed p at outlet and u at inlet or vice versa or set a pressure drop that force the flow... In addition the mesh should be corrected.
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

May 13, 2016, 08:03 

#11 
New Member
Join Date: May 2016
Posts: 28
Rep Power: 2 
Hello again,
first I will refine the mesh around the airfoil and the I'll trying to use the set of boundary condition you wrote. Thank you for all the help!! 

May 13, 2016, 08:13 

#12 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
I do not mean that you have to refine the mesh around your airfoil but the transision between layer and cells are too extreme.
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

May 16, 2016, 04:36 

#13 
New Member
Join Date: May 2016
Posts: 28
Rep Power: 2 
Hey all again,
so I changed my mesh in order to correct the AR, and set my boundary condition fixing the pressure at the outlet and the velocity at the inlet. The solution continues to work for more time step, but soon or later the same error as before appears. Also the forces are completely wrong respect to that I expect. Here there is my new case: naca0012heat_new 

May 16, 2016, 04:53 

#14 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
The layers are as bad as before.
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

May 17, 2016, 22:24 

#15 
Member
Peter
Join Date: Feb 2015
Location: California
Posts: 59
Rep Power: 3 
A few suggestions:
1) In addition to the mesh being a bit funky, your temperature BC's are really weird. Have a look at some of the rhoCentralFoam/rhoSimpleFoam tutorials. 2) try setting nNonOrthogonalCorrectors to around 3. 3) Some of your other BC's are just wrong (using inletOutlet for inlets... etc.; slip conditions for nonvectors...) 4) p BCs seem wrong as well. Ok, it's pretty clear that your BCs are just not right. Really think through what you are trying to achieve, and try to understand the meaning of each boundary condition. Also, start from a tutorial case (forwardStep, for example) and use that as a template to start from. Then build complexity incrementally (i.e., use a simple block rather than an airfoil at first and get that right, then add geometric complexity)  I think you'll find that working incrementally toward your goal will be much faster (and less frustrating) than trying lots of stuff and just seeing what sticks... Good luck! Kind regards, Peter 

May 18, 2016, 02:10 

#16 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
Are the bc still wrong? Did not check it again
one of the easiest cases to set up
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

July 4, 2016, 05:52 

#17 
Member
carno
Join Date: Mar 2009
Posts: 33
Rep Power: 9 
I am getting the same error in rhoSimpleFoam. I tried everything in the discussion.
Please help me. rhoSimpleFoam seems to be extremely picky. 

July 4, 2016, 05:54 

#18 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,555
Blog Entries: 6
Rep Power: 27 
Dear Carno,
no one knows what you did (you do not provide any information). How should the community help you ? If you did it like I said above it has to work. Otherwise I think your FOAM is not compiled correct and has errors.
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials, publications and videos on www.Holzmanncfd.de OpenFOAM Beginners should check out the new wiki on wiki.openfoam.com A list of some active OpenFOAM contributers can be found »here« A book about the basics of »Mathematics, Numerics, Derivations and OpenFOAM« can be found on www.Holzmanncfd.de 

July 4, 2016, 06:53 

#19 
Member
carno
Join Date: Mar 2009
Posts: 33
Rep Power: 9 
Thanks for the reply.
I am sending information. It's a MRF problem. A 2m diameter fan is rotating with 250 rad/s. So the tip rotates around 250 m/s. I used Inlet BC : total pressure 1 bar Outlet BC: 1 bar static pressure Max nonortho cell is 64 (all tetra) Kindly guide how to paste code. I can paste the fVschemes and fvSolution here too. Check Mesh result: Code: Mesh stats points: 612835 faces: 5948384 internal faces: 5438852 cells: 2846809 faces per cell: 4 boundary patches: 5 point zones: 0 face zones: 0 cell zones: 3 Overall number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 2846809 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing 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 outlet 4494 2406 ok (nonclosed singly connected) walls 332050 166341 ok (nonclosed singly connected) walls_rotor 139415 69893 ok (nonclosed singly connected) walls_hub 29229 14802 ok (nonclosed singly connected) inlet 4344 2331 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0 1.02 1.02) (9 1.02 1.02) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (1.157218e015 2.861809e015 2.727448e017) OK. Max cell openness = 2.735671e016 OK. Max aspect ratio = 6.275062 OK. Minimum face area = 3.818967e006. Maximum face area = 0.005911771. Face area magnitudes OK. Min volume = 5.255555e009. Max volume = 0.0001364341. Total volume = 29.37645. Cell volumes OK. Mesh nonorthogonality Max: 65.20238 average: 16.78288 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.9447552 OK. Coupled point location match (average 0) OK. 

July 4, 2016, 07:02 

#20  
Member
carno
Join Date: Mar 2009
Posts: 33
Rep Power: 9 
Quote:
Code:
FoamFile { version 2.0; class dictionary; format ascii; location "system"; object fvSchemes; } ddtSchemes { default steadyState; } gradSchemes { default cellLimited leastSquares 1; grad(U) cellLimited leastSquares 1; } divSchemes { default bounded Gauss upwind; div(phi,U) bounded Gauss linearUpwind grad(U); div(phi,omega) bounded Gauss upwind; div(phi,k) bounded Gauss upwind; div(R) Gauss linear; div((muEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear limited 0.77; } interpolationSchemes { default linear; } snGradSchemes { default limited 0.77; } fluxRequired { default no; p ; } Code:
FoamFile { version 2.0; class dictionary; format ascii; location "system"; object fvSolution; } solvers { U { type coupled; tolerance (1.0E6 1.0E6 1.0E6); preconditioner DILU; solver PBiCCCG; relTol (0.1 0.1 0.1); maxIter 100; } omega { tolerance 1.0E6; preconditioner DILU; solver PBiCG; relTol 0.1; //maxIter 100; } k { tolerance 1.0E6; preconditioner DILU; solver PBiCG; relTol 0.1; //maxIter 100; } h { tolerance 1.0E6; preconditioner DILU; solver PBiCG; relTol 0.1; //maxIter 100; } p { nPostSweeps 1; solver GAMG; preconditioner DILU; smoother GaussSeidel; nFinalSweeps 0; nPreSweeps 0; nPostSweeps 2; nCellsInCoarsestLevel 1000; cacheAgglomeration true; minIter 3; maxIter 100; tolerance 1.0E4; agglomerator faceAreaPair; relTol 0.05; mergeLevels 1; } } SIMPLE { nNonOrthogonalCorrectors 3; pRefCell 0; pRefValue 0.0; transonic true; rhoMin rhoMin [1 3 0 0 0 0 0] 0.1; rhoMax rhoMax [1 3 0 0 0 0 0] 10.0; residualControl { U 1.0E4; omega 1.0E4; k 1.0E4; h 1.0E4; p 1.0E4; } } relaxationFactors { U 0.05; omega 0.05; k 0.05; rho 0.05; h 0.05; p 0.05; } potentialFlow { nNonOrthogonalCorrectors 10; pRefCell 0; pRefValue 0.0; } Code:
FoamFile { version 2.0; format binary; class volScalarField; location "0"; object p; } dimensions [1 1 2 0 0 0 0]; internalField uniform 100000.0; boundaryField { inlet { type totalPressure; p0 uniform 100000.0; gamma 1.4; rho rho; } outlet { type totalPressure; p0 uniform 100000.0; gamma 1.4; rho rho; } walls { type zeroGradient; } walls_hub { type zeroGradient; } walls_rotor { type zeroGradient; } } 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
rhoSimpleFoam angledDuctExplicitFixedCoeff tutorial fails in parallel  donQi  OpenFOAM Running, Solving & CFD  1  February 22, 2016 20:47 
Switching from simpleFoam to rhoSimpleFoam  sebastian  OpenFOAM  11  January 7, 2015 05:32 
rhoSimpleFoam. patchField error.  123  OpenFOAM Running, Solving & CFD  4  June 6, 2014 15:22 
transsonic nozzle with rhoSimpleFoam  Unseen  OpenFOAM Running, Solving & CFD  7  April 16, 2014 03:38 
Transonic rhoSimpleFoam Equations  eric.m.tridas  OpenFOAM  3  January 25, 2012 11:52 