|
[Sponsors] |
sonicFoam "prism" tutorial not working when inlet velocity is increased |
View Poll Results: what should be the first check to fix "negative initial temperature" error | |||
0 folder |
![]() ![]() ![]() ![]() |
2 | 50.00% |
constant folder |
![]() ![]() ![]() ![]() |
1 | 25.00% |
system folder |
![]() ![]() ![]() ![]() |
1 | 25.00% |
Voters: 4. You may not vote on this poll |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Dumbledore
Join Date: Jun 2019
Posts: 10
Rep Power: 7 ![]() |
hello foamDudes
I took up a tutorial case $FOAM_TUTORIALS/compressible/sonicFoam/RAS/prism the default inlet velocity boundary condition in the tutorial was 650(which is M =1.89) In 0 folder i have changed velocity from (650 0 0) to (1030 0 0) at inlet, top and bottom wall boundaries to get to Mach 3 over the prism, i havent changed anything else and then this error shows up while i try to run it: HTML Code:
Time = 3.25e-05 Courant Number mean: 0.056095 max: 0.45764 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 PIMPLE: iteration 1 smoothSolver: Solving for Ux, Initial residual = 0.00361405, Final residual = 1.25973e-07, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0121551, Final residual = 5.68609e-07, No Iterations 2 smoothSolver: Solving for e, Initial residual = 0.00566519, Final residual = 3.57166e-07, No Iterations 2 --> FOAM FATAL ERROR: Negative initial temperature T0: -32.7705 From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hConstThermo<Foam::perfectGas<Foam::specie> >; Type = Foam::sensibleInternalEnergy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy>] in file /home/pawan/OpenFOAM/OpenFOAM-v1812/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 54. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&)sh: 1: addr2line: not found addr2line failed #1 Foam::error::abort()sh: 1: addr2line: not found addr2line failed #2 Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy>::TEs(double, double, double) constsh: 1: addr2line: not found addr2line failed #3 Foam::hePsiThermo<Foam::psiThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, bool)sh: 1: addr2line: not found addr2line failed #4 Foam::hePsiThermo<Foam::psiThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct()sh: 1: addr2line: not found addr2line failed #5 ?sh: 1: addr2line: not found addr2line failed #6 __libc_start_mainsh: 1: addr2line: not found addr2line failed #7 ?sh: 1: addr2line: not found addr2line failed Aborted (core dumped) (i have later changed k and epsilon values in 0 folder but still the same story) Last edited by hemanthgrylls; July 16, 2019 at 08:23. Reason: typos |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Member
Giovanni Medici
Join Date: Mar 2014
Posts: 47
Rep Power: 12 ![]() |
Apparently you reach nonphysical temperatures, this several different reasons may lead to this behavior.
In order to assess it several infos are missing from your post:
During the first part of the computation, the flow develops and hence it may reach very strong gradients (in particular near the object of interest). Hence by introducing temperature limiters, a decrease convergence / flow development rate can be expected, but overall computation stability shall be stiffer. |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Gavin Ridley
Join Date: Jan 2019
Location: Tennessee, USA
Posts: 25
Rep Power: 7 ![]() |
Seeing as how your timestep is good in this case, my bet is that you're using a scheme for temperature which can oscillate in the presence of sharp gradients, leading to zero temperatures. You can check if this is the issue by changing the temperature scheme to upwind.
|
|
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Dumbledore
Join Date: Jun 2019
Posts: 10
Rep Power: 7 ![]() |
I have resolved this issue successfully, by replacing the mesh, i just made a bad mesh! reducing the time step also dint work.
I suggest everyone to use ICEMCFD instead of doing blind meshing inside Mesh button of Ansys workbench. make sure aspect ratio is less than 20 in the regions away from the wall, there is no issue with cells with aspect ratio of even 200 closer to the walls. a greatman once said: "One who owns the Mesh, owns the solution" Openfoam is not like fluent, it does not have robust automated adjustments which can manage divergence issues. In OF we need to tweak the schemes and paramaters a bit but the end result that OF gives you is more reliable is what i feel. cheers! thanks a lot for the replies |
|
![]() |
![]() |
![]() |
Tags |
sonicfoam, supersonic flows |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
serial udf to parallel udf | radioss | Fluent UDF and Scheme Programming | 10 | January 19, 2019 08:56 |
Defined inlet velocity is different with inlet velocity on CFX post | jonpewpew | CFX | 2 | November 2, 2017 16:40 |
Setting Density for Velocity Inlet Face | arkie87 | FLUENT | 0 | November 7, 2012 15:15 |
Velocity inlet boundary condition for porous medium | Chander | CFX | 3 | March 11, 2012 21:18 |
UDF paraboloid velocity inlet | Ronak Shah | FLUENT | 0 | June 4, 2003 09:44 |