CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

dieselFoam --> Janaf Error, what are the root causes?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 1, 2010, 16:40
Default dieselFoam --> Janaf Error, what are the root causes?
  #1
New Member
 
Paul
Join Date: Mar 2009
Posts: 19
Rep Power: 8
pajofego is on a distinguished road
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
pajofego is offline   Reply With Quote

Old   December 2, 2010, 06:59
Default
  #2
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
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.
nakul is offline   Reply With Quote

Old   December 2, 2010, 16:13
Default
  #3
New Member
 
Paul
Join Date: Mar 2009
Posts: 19
Rep Power: 8
pajofego is on a distinguished road
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)
       );
Here is the output of checkMesh. The mesh was done with gmsh. Regarding the output of the checkMesh I cannot find any advises.

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
If more informations are needed please let me know. Thanks and best regards.
pajofego
pajofego is offline   Reply With Quote

Old   December 3, 2010, 02:42
Default
  #4
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
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.
nakul is offline   Reply With Quote

Old   December 7, 2010, 10:35
Default
  #5
Senior Member
 
Rickard
Join Date: May 2010
Location: Lund, Skåne, Sweden
Posts: 143
Rep Power: 7
Rickard.Solsjo is on a distinguished road
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.
Rickard.Solsjo is offline   Reply With Quote

Old   December 7, 2010, 16:22
Default
  #6
New Member
 
Paul
Join Date: Mar 2009
Posts: 19
Rep Power: 8
pajofego is on a distinguished road
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
pajofego is offline   Reply With Quote

Old   December 12, 2010, 08:11
Default
  #7
New Member
 
Paul
Join Date: Mar 2009
Posts: 19
Rep Power: 8
pajofego is on a distinguished road
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
Enclosed you can find some pictures about my case and geometry. At simulation time 0.00275 (dt = 5e-5) the envolving of the spray seems to works well, also the time step is stable. Near by the simulation time 0.00335 the timestep gets smaller (5.19677e-08) and I got high velocity gradients at the wall. Take a look on the pictures. So my question is, what I'm doing wrong?

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
Thanks in advance
pajofego
Attached Images
File Type: png geometry.png (6.6 KB, 19 views)
File Type: png mesh_gmsh.png (30.5 KB, 20 views)
File Type: png vel_0_00275sec.png (22.5 KB, 22 views)
File Type: png vel_0_00335sec_unscaled.png (31.5 KB, 23 views)
File Type: png vel_0_00335sec_scaled.png (18.0 KB, 16 views)
pajofego is offline   Reply With Quote

Old   December 12, 2010, 09:05
Default
  #8
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
This error comes from this line in dieselFoam.C
Code:
           volScalarField tk =
                Cmix*sqrt(turbulence->muEff()/rho/turbulence->epsilon());
it means that either the viscosity or epsilon is negative.
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);
That will fix the error you are seeing, but I cant say if it will fix your problem.
niklas is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
OpenFOAM-1.7.0 for CentOS/RHEL/SL 5.x 64bit released linnemann OpenFOAM Installation 66 October 26, 2013 13:04
Installation problem with ParaView 3.8.0 on openSUSE 11.2 aero_ OpenFOAM Paraview & paraFoam 14 August 2, 2010 18:13
DieselFoam and temperature out of janaf range hoogland OpenFOAM Running, Solving & CFD 4 December 9, 2009 11:04
MPI PROBLEMS gtg627e OpenFOAM Running, Solving & CFD 20 October 5, 2007 04:02


All times are GMT -4. The time now is 17:25.