[RobertC]

I am new to OpenFOAM, and am experimenting with various flavors of the solver, including OpenFOAM-6 and OpenFOAM-dev (CFD-Direct), and OpenFOAM-plus (ESI).

I am interested in compressible solvers, so for OpenFOAM-dev, I attemped to run the forward step problem ($FOAM_PROJECT_DIR/tutorials/compressible/rhoPimpleFoam/laminar/forwardStep) using rhoCentralFoam and rhoPimpleFoam. To my surprise, rhoPimpleFoam failed with the below error message. I am posting here to see if I am missing something simple, ahead of filing a bug report with CFD Direct. I greatly appreciate any help you can provide.

  Courant Number mean: 0.251275 max: 1.17915
  Time = 0.016s

  PIMPLE: Iteration 1
  diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
  smoothSolver:  Solving for Ux, Initial residual = 0.0764808, Final residual = 1.29e-06, No Iterations 1
  smoothSolver:  Solving for Uy, Initial residual = 0.064002, Final residual = 7.94223e-06, No Iterations 1
  smoothSolver:  Solving for e, Initial residual = 0.26368, Final residual = 4.9006e-06, No Iterations 3
  smoothSolver:  Solving for p, Initial residual = 0.0715941, Final residual = 6.77228e-08, No Iterations 2
  diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
  time step continuity errors : sum local = 1.94255e-09, global = 1.06042e-09, cumulative = 6.6211e-09
  PIMPLE: Iteration 2
  smoothSolver:  Solving for Ux, Initial residual = 0.00795199, Final residual = 9.99449e-11, No Iterations 1
  smoothSolver:  Solving for Uy, Initial residual = 0.021992, Final residual = 1.56364e-09, No Iterations 1
  smoothSolver:  Solving for e, Initial residual = 0.285134, Final residual = 2.3536e-08, No Iterations 2


  --> FOAM FATAL ERROR:
  Negative initial temperature T0: -3.09503

I see no such error using rhoCentralFoam, nor in OpenFOAM-6 using sonicFoam, nor in OpenFoam-plus using sonicFoam.

Looking at the git log, I see the following commit which may be related:

commit 3341f925108a759f58f06ce2fd865321af6dd6ca
Author: Henry Weller <http://openfoam.org>
Date: Wed Jun 6 11:07:45 2018 +0100

sonicFoam, sonicDyMFoam, sonicLiquidFoam: Functionality merged into rhoPimpleFoam

The sonicFoam, sonicDyMFoam and sonicLiquidFoam functionality has been merged
into the transonic option of the latest rhoPimpleFoam solver and the
corresponding tutorials moved into the rhoPimpleFoam tutorials directory.

To run rhoPimpleFoam in transonic mode set the transonic option in the
PIMPLE sub-dictionary of fvSolution:

PIMPLE
{
.
.
.
transonic yes;
}

I have checked, and the transonic option is indeed present in fvSolution for forwardStep.

FWIW, I am using OpenFOAM-dev at commit 38262243ccdd13bd936541d2373ccfd1974db597

[jsoln]

I concur that this case, as packaged in OpenFOAM 10 (installed 1 or 2 months ago from CFD Direct), encounters the negative temperature error. I can overcome the error when adding the following lines to the file 'system/controlDict'.

adjustTimeStep yes;
maxCo 0.7;
maxDeltaT 1;

However, the process time step becomes very small, ~2e-08.

[dlahaye]

Use limiter on T using https://www.openfoam.com/documentati...mperature.html

Nothing in rhoSimpleFoam prevents negative T values, especially in initial stages of convergence.

The issues has been repeated discussed in this forum.

Good luck.

[jsoln]

The issue I had was addressed by OpenFOAM.org Issue 3889.