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] [2] [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] [2] [2] From function operator+(const dimensionSet& ds1, const dimensionSet& ds2) [2] in file dimensionSet/dimensionSet.C at line 357. [2] 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, -Thomas |
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. regards markus |
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 -Thomas |
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 markus |
All times are GMT -4. The time now is 21:46. |