CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

SonicTurbFoam initialisation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 6, 2006, 05:09
Default Hi all, I have a problem ru
  #1
Member
 
Thomas Wolfanger
Join Date: Mar 2009
Location: South West Germany
Posts: 60
Rep Power: 8
anger is on a distinguished road
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
anger is offline   Reply With Quote

Old   April 6, 2006, 07:40
Default Hi Thomas, you can't use th
  #2
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 8
hartinger is on a distinguished road
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
hartinger is offline   Reply With Quote

Old   April 6, 2006, 09:15
Default Hello Markus, thanks for th
  #3
Member
 
Thomas Wolfanger
Join Date: Mar 2009
Location: South West Germany
Posts: 60
Rep Power: 8
anger is on a distinguished road
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
anger is offline   Reply With Quote

Old   April 6, 2006, 09:35
Default good, but just adjusting the d
  #4
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 8
hartinger is on a distinguished road
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
hartinger is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Global Initialisation Chirag CFX 1 July 21, 2008 08:54
Domain initialisation. KM CFX 2 October 12, 2007 15:27
Initialisation of my solution Gernot FLUENT 4 August 27, 2005 04:27
Initialisation Gernot FLUENT 1 August 22, 2005 14:17
UDF initialisation of DPM model Lasse Rosendahl FLUENT 0 December 11, 2000 10:08


All times are GMT -4. The time now is 04:22.