|
[Sponsors] |
dieselFoam --> Janaf Error, what are the root causes? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 1, 2010, 15:40 |
dieselFoam --> Janaf Error, what are the root causes?
|
#1 |
New Member
Paul
Join Date: Mar 2009
Posts: 19
Rep Power: 17 |
Hello at all,
now I've spend a lot of time to understand how I can perform my own simulation with an injection similiar to the aachenBomb. So at first I run the aachenBomb test case and modified it to a different injected mass and mass rate. For the aachenBomb geometry it works. After this I decide to change the geometry to an cylindrical tube using a tet mesh. So this works also fine. But after modifying the tube to a more complex geometry I got the problem with the Janaf temperature error which is out of the specific range of 200 - 5000 K. Using a finer mesh this will not help. The simulation stops earlier then with a worst mesh? So the question is how I can identify the root cause of the Janaf Error? Is it related to the quality of the mesh? Which procedure you can recommend me to find the problem? Thanks in advance. pajofego |
|
December 2, 2010, 05:59 |
|
#2 |
Senior Member
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 16 |
Hi,
What exactly did you change? Did you only changed the domain or did you made some changes in BC and IC also? This error comes generally when something is wrong with your BC or mesh. If you are using the same BC as in the tutorial then have a look at your mesh. Run a "checkMesh" command and see what turns out. Also specify more details regarding your case, otherwise it would be difficult to advice. |
|
December 2, 2010, 15:13 |
|
#3 |
New Member
Paul
Join Date: Mar 2009
Posts: 19
Rep Power: 17 |
Hi,
in fact. I should give more informations about my case. I've only change the domain. The BC are all the same. That means like the tutorial all walls. Also I've change the Injector's properties - I would like to use a common rail injector: Code:
commonRailInjectorProps { position (0 0.0025 0); direction (0 1 0); diameter 1.73e-7; mass 0.4275e-06;//0.4275e-05; injectionPressure 5.0e+5; temperature 320; nParcels 5000; X ( 1.0 ); massFlowRateProfile ( (0 0) (0.0013 1.32e-6) (0.00135 1.32e-6) (0.0014 1.32e-6) (0.00145 1.32e-6) (0.0015 1.32e-6) (0.00155 1.32e-6) (0.0016 1.32e-6) (0.00165 1.32e-6) (0.0017 1.32e-6) (0.00175 1.32e-6) (0.0018 1.32e-6) (0.00185 1.32e-6) (0.0019 1.32e-6) (0.0025 0) ); Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 858010 faces: 9983705 internal faces: 9835631 cells: 4954834 boundary patches: 1 point zones: 0 face zones: 0 cell zones: 1 Overall number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 4954834 polyhedra: 0 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 Wall 148074 74039 ok (closed singly connected) Checking geometry... Overall domain bounding box (-0.06725 -0.017 -0.06725) (0.124412 0.2 0.06725) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (1.34258e-19 2.12949e-20 -1.44159e-20) OK. Max cell openness = 1.89982e-16 OK. Max aspect ratio = 10.3626 OK. Minumum face area = 1.96441e-08. Maximum face area = 4.53391e-06. Face area magnitudes OK. Min volume = 1.76279e-12. Max volume = 3.14575e-09. Total volume = 0.000710906. Cell volumes OK. Mesh non-orthogonality Max: 66.8448 average: 18.585 Non-orthogonality check OK. Face pyramids OK. Max skewness = 1.06135 OK. Mesh OK. End pajofego |
|
December 3, 2010, 01:42 |
|
#4 |
Senior Member
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 16 |
Hi,
It might be possible that problem is with your mesh. Your Max. non-orhtogonality, although OK, is a little high, in my opinion. Try to modify your mesh, if possible. Keep your maxCo to 0.1 and then try to run. Also if possible upload an image of your mesh, especially the areas where there is skewness and non-orthogonality. Also you may use first order schemes in your fvSchemes file. |
|
December 7, 2010, 09:35 |
|
#5 |
Senior Member
Rickard
Join Date: May 2010
Location: Lund, Skåne, Sweden
Posts: 143
Rep Power: 15 |
I had problems running before as well. You could try to increase the number of parcels you are injection. Okay you only have 0.something milligrams but i would still recommend at least 100 000 parcels, maybe more.
|
|
December 7, 2010, 15:22 |
|
#6 |
New Member
Paul
Join Date: Mar 2009
Posts: 19
Rep Power: 17 |
So, I've done improvements regarding the mesh. I tried to use a structed hex mesh in gmsh, which is not really simple. It was possible to reduce the max. skewness up to 0.35 and I was able to run a simulation for a cylindrical geometry with a hex mesh. Tet meshes doesn't work for my geometry. I will upload a picture of the meshes that I used an I will also start a simulation with an increased parcel number. What is the benefit using a increased parcel number.
Thanks pajofego |
|
December 12, 2010, 07:11 |
|
#7 |
New Member
Paul
Join Date: Mar 2009
Posts: 19
Rep Power: 17 |
Hello at all,
I came back with my problem, after done some improvements regarding the mesh. It stills will not work! That's the last iteration before I got a floating point exception, instead of an janaf error Code:
Number of parcels in system.... | 9959 Injected liquid mass........... | 4.275 mg Liquid Mass in system.......... | 3.8261 mg SMD, Dmax...................... | 88.5959 mu, 150.154 mu Added gas mass................. | 1.29834 mg Evaporation Continuity Error... | 0.849442 mg ExecutionTime = 2363.32 s ClockTime = 2397 s Courant Number mean: 8.40164e-05 max: 0.0557897 deltaT = 5.19677e-08 Time = 0.00335422 Evolving Spray Solving chemistry #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::sqrt(Foam::Field<double>&, Foam::UList<double> const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::sqrt<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/opt/openfoam171/applications/bin/linuxGccDPOpt/dieselFoam" #5 in "/opt/openfoam171/applications/bin/linuxGccDPOpt/dieselFoam" #6 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #7 in "/opt/openfoam171/applications/bin/linuxGccDPOpt/dieselFoam" Floating point exception Here the output of checkMesh: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 47660 faces: 134197 internal faces: 125723 cells: 43320 boundary patches: 1 point zones: 0 face zones: 0 cell zones: 1 Overall number of cells of each type: hexahedra: 43320 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 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 Wall 8474 8476 ok (closed singly connected) Checking geometry... Overall domain bounding box (-0.065 -0.065 -0.017) (0.065 0.065 0.06) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (-7.35605e-19 8.20756e-19 -7.23779e-19) OK. Max cell openness = 2.05763e-16 OK. Max aspect ratio = 10.8915 OK. Minumum face area = 1.12701e-06. Maximum face area = 1.15717e-05. Face area magnitudes OK. Min volume = 1.35242e-09. Max volume = 1.40514e-08. Total volume = 0.000394841. Cell volumes OK. Mesh non-orthogonality Max: 74.3926 average: 14.9572 *Number of severely non-orthogonal faces: 512. Non-orthogonality check OK. <<Writing 512 non-orthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 0.993807 OK. Mesh OK. End pajofego |
|
December 12, 2010, 08:05 |
|
#8 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
This error comes from this line in dieselFoam.C
Code:
volScalarField tk = Cmix*sqrt(turbulence->muEff()/rho/turbulence->epsilon()); You probably have some earlier warnings about bounding the epsilon equation. what you can do is to create a new field tk2 and limit that like below to calculate tk. Code:
volScalarField tk2 = turbulence->muEff()/rho/turbulence->epsilon(); tk2.max(1.0e-15); volScalarField tk = Cmix*sqrt(tk2); |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
DieselFoam and temperature out of janaf range | hoogland | OpenFOAM Running, Solving & CFD | 5 | January 28, 2016 12:30 |
OpenFOAM-1.7.0 for CentOS/RHEL/SL 5.x 64bit released | linnemann | OpenFOAM Installation | 66 | October 26, 2013 13:04 |
[OpenFOAM] Installation problem with ParaView 3.8.0 on openSUSE 11.2 | aero_ | ParaView | 14 | August 2, 2010 18:13 |
MPI PROBLEMS | gtg627e | OpenFOAM Running, Solving & CFD | 20 | October 5, 2007 04:02 |