[UebertreibeR]

This error is caused when the solver tries to find T from h (or another energy variable). The task is to find T from known h when h = cp(T) * T and this is solved by a simple Newton-approach.


T is estimated and then re-calculated until convergence is reached. Bad estimates can lead to negative temperatures and cause the error. It's not always easy to find out why the estimated T is bad, but some possible reasons have been mentioned previously:
- bad mesh
- bad interpolation schemes
- bad thermophysical properties

[RebelYoung]

It occurred in rhoC and rhoP solvers.
The temperature limiter in fvOption does not work, because I add the minMax functions in controlDict. The minimum temperature in the fields is not negative.

In my case , the error happened after about 30-100 time steps. So the negative initial temperature is in the sub-iteration.

I can not find a solution so far...

[RebelYoung]

Originally Posted by UebertreibeR

This error is caused when the solver tries to find T from h (or another energy variable). The task is to find T from known h when h = cp(T) * T and this is solved by a simple Newton-approach.


T is estimated and then re-calculated until convergence is reached. Bad estimates can lead to negative temperatures and cause the error. It's not always easy to find out why the estimated T is bad, but some possible reasons have been mentioned previously:
- bad mesh
- bad interpolation schemes
- bad thermophysical properties

Thank you for your suggestions.
As your advice, in rhoCentralFoam solver, it solves rho and rhoE for estimating the temperature, which has the equation "e=cv*T" . For the normalized gas , the Cv is constant.
So the negative initial temperature means the energy is negative?

[Niko_choko]

Can confirm that changing mesh did work for me too.

[jdw135]

I am having the same issue, but I don't have a mesh problem. My entire domain is uniform spacing in a rectangular grid, so there is no change in mesh size, aspect ratio, or skewness. The solution runs fine with coarser grids, but my current grid is in no way over-refined, as edge length is 1 mm. I am doing LES in rhoPimpleFoam.

[jdw135]

As a follow-up, I noticed that for my grid the max Courant number was approaching 1 when I would get the error. I reduced the dt and solved my issue.

[bineet_aero]

Originally Posted by vs1

I get the same error when i set turbulence to laminar but with other turbulence models the error is gone.

opposite for me, no such error for laminar simulations but i get the error for turbulent ones !!

[saidc.]

Hi,

I'm having same problem in LES, I tried with refined mesh but the result is the same again. Also when i added temperature limit in fvOption it stops iterrate after like 200 iterates. Maybe the problem is in my boundary conditions. I'm open any suggestion. Files attached.

Kind regards
Said.

checkMesh

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           34125
    faces:            386106
    internal faces:   380986
    cells:            191773
    faces per cell:   4
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       2

Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    191773
    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                  
    inlet               214      128      ok (non-closed singly connected)  
    outlet              242      142      ok (non-closed singly connected)  
    wall                4664     2372     ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-0.025 -0.125 -0.025) (0.025 0.125 0.025)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (8.44415e-17 -7.50933e-17 5.0822e-18) OK.
    Max cell openness = 2.41502e-16 OK.
    Max aspect ratio = 5.2589 OK.
    Minimum face area = 1.47893e-07. Maximum face area = 3.61292e-05.  Face area magnitudes OK.
    Min volume = 2.65313e-11. Max volume = 6.60658e-08.  Total volume = 0.000625.  Cell volumes OK.
    Mesh non-orthogonality Max: 53.9367 average: 14.5269
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.518146 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

[jcoelho5]

Originally Posted by bineet_aero

opposite for me, no such error for laminar simulations but i get the error for turbulent ones !!

Same here. Did you solve it? Any tip?

[zhuangli]

Hi Tobias,
I got into trouble with the negative temperature, could you give me some advice to deal with it?
Thanks in advance!


_______
Kind regards!
Zhuangli

[Mahdi2010]

Originally Posted by zhuangli

Hi Tobias,
I got into trouble with the negative temperature, could you give me some advice to deal with it?
Thanks in advance!


_______
Kind regards!
Zhuangli

This functionObject may help to prevent negative T in compressible solvers:

fvOptions limitTemperature crashing in compressibleInterFoam

[zhuangli]

Originally Posted by Mahdi2010

This functionObject may help to prevent negative T in compressible solvers:

fvOptions limitTemperature crashing in compressibleInterFoam

Thank U Mahdi.

[Mars409]

I ran buoyantSimpleFoam with Boussinesq as the EoS but it crashed at Time=3 for ‘negative initial temperature T0=-24’ error. fvOptions limitT solves it, but the resulting flow pattern is unphysical. I would like to trace back in the code to find out what causes T0 < 0 (T0 is given as a fixed number in the EquationOfState subdict in constant/thermophysicalProperties as one of the requisite parameters for the Boussinesq EoS.)



My question: How to trace back from the thermol.H at line 300 (grep -r 'Negative initial temperature T0' reports it as the only place where this text appears under src/) through the source codes?


thermol.H is at https://cpp.openfoam.org/v9/thermoI_8H_source.html




td p { orphans: 0; widows: 0; background: transparent }p { line-height: 115%; margin-bottom: 0.1in; background: transparent }

[ERKSMAFA]

Originally Posted by saiguruprasad

I was having the same problem and changing the mesh got rid of the problem.

Make sure that there is no sudden change in mesh spacings.

I had the same issue even though I created a quality mesh. After seeing this message I replaced my mesh file with one with better orthagonal quality. My problem was solved with the new mesh file.

Thanks for your help.

[suoCFD]

Originally Posted by ERKSMAFA

I tried changing the mesh multiple times and it finally worked.

Sorry for my bad English.

I deal with an analysis using foamMultiRun. fluid solvers for fluid regions, solid solvers for solid regions. I had the same issue for fluid region (Negative initial value).

Firstly, I removed the radiation model which was added to the fluid from another tutorial case. Secondly, I adjusted p_rgh conditions accurately. Now, there is no error as negative initial value.
I will try to add radiation model in the future but how I dont know.