# SonicTurbFoam initialisation

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 6, 2006, 05:09 Hi all, I have a problem ru #1 Member   Thomas Wolfanger Join Date: Mar 2009 Location: South West Germany Posts: 60 Rep Power: 9 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

 April 6, 2006, 07:40 Hi Thomas, you can't use th #2 Senior Member   Markus Hartinger Join Date: Mar 2009 Posts: 102 Rep Power: 9 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

 April 6, 2006, 09:15 Hello Markus, thanks for th #3 Member   Thomas Wolfanger Join Date: Mar 2009 Location: South West Germany Posts: 60 Rep Power: 9 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

 April 6, 2006, 09:35 good, but just adjusting the d #4 Senior Member   Markus Hartinger Join Date: Mar 2009 Posts: 102 Rep Power: 9 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Chirag CFX 1 July 21, 2008 08:54 KM CFX 2 October 12, 2007 15:27 Gernot FLUENT 4 August 27, 2005 04:27 Gernot FLUENT 1 August 22, 2005 14:17 Lasse Rosendahl FLUENT 0 December 11, 2000 10:08

All times are GMT -4. The time now is 18:43.

 Contact Us - CFD Online - Top