CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   SonicTurbFoam initialisation (

anger April 6, 2006 05:09

Hi all, I have a problem ru
Hi all,

I have a problem running sonicTurbFoam.
I created initial fields (U, p, k, epsilon, phi) for a sonicTurbFoam calculation using simpleFoam. But when starting the calculation, the following error occurs:

Starting time loop

Mean and max Courant Numbers = 10.5008 inf
Time = 100.01

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
[2] --> FOAM FATAL ERROR : LHS and RHS of + have different dimensions
dimensions : [0 2 -1 0 0 0 0] + [1 -1 -1 0 0 0 0]
[2] From function operator+(const dimensionSet& ds1, const dimensionSet& ds2)
[2] in file dimensionSet/dimensionSet.C at line 357.
FOAM parallel run aborting

I'm aware that this has something to do with the
calculation of the viscosity. Is there any way to surpass this problem?

best regards,

hartinger April 6, 2006 07:40

Hi Thomas, you can't use th
Hi Thomas,

you can't use the results from simpleFoam directly in sonicTurbFoam. simpleFoam solves for 'specific pressure' (p/rho) [m^2/s^2], whereas sonicTurbFoam
solves for pressure [kg/(m*s^2)]. So the units don't match and would need to multiply the pressure with density and make sure the dimensions in the resulting Foam-file are correct.
And simpleFoam uses kinematic viscosity. Check what sonicTurbFoam uses.


anger April 6, 2006 09:15

Hello Markus, thanks for th
Hello Markus,

thanks for these hints. I actually had two errors in my setup which prevented sonicTurbFoam from running:
1. as you already pointed out, the dimension of p is different in simpleFoam and sonicTurbFoam
2. I had the face flux field p as starting condition, which also has the wrong dimensions.

Deleting this field and changing the dimensions of p did the trick.

Thanks for your help,

best regards

hartinger April 6, 2006 09:35

good, but just adjusting the d
good, but just adjusting the dimensions doesn't give the correct results.
you could modify the existing simpleFoam and create a new volScalarField pRho = p * rho


All times are GMT -4. The time now is 07:01.