CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Bugs

TwoPhaseEulerFOAM application

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 16, 2006, 08:27
Default Description: The application
  #1
Senior Member
 
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 8
hemph is on a distinguished road
Description:
The application gives erroneous solution for the Ua-field when the particle-particle force is included (g0 > 0). If settling particles are simulated, the velocity of the particles does not approach zero as they reach the bottom of the domain.

Solution. The ppMagf-term in alphaEqn.H: should be divided by alphaf on row 26.

Old:
ppMagf = g0*rUaAf*min(exp(preAlphaExp*(alphaf - alphaMax)), expMax);

New:
ppMagf = 1.0/(rhoa*max(alphaf,SMALL))*g0*rUaAf*min(exp(preAlpha Exp*(alphaf - alphaMax)), expMax);

Also row 32 in alphaEqn.H needs to be changed.

Old:
alphaEqn -= fvm::laplacian(ppMagf, alpha);

New:
alphaEqn -= fvm::laplacian(alphaf*ppMagf, alpha);

Solver/Application:
twoPhaseEulerFoam

Source file:
alphaEqn.H

Testcase:
twoPhaseEulerFoamPack1D.tar.gz

Platform:
All

Version:
All

Notes:
The dimension of g0 is in Pascal in most references. In twoPhaseEulerFoam the dimensions of g0 is Pa/(kg/m3). To aid comparison between models, the ppMagf term should be divided by rho, as
ppMagf = 1.0/(rhoa*max(alphaf,SMALL))*g0*rUaAf*min(exp(preAlpha Exp*(alphaf - alphaMax)), expMax);

with a corresonding change to the dimensions of g0 in constant/ppProperties
hemph 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
TwoPhaseEulerFOAM application hemph OpenFOAM Bugs 35 November 6, 2011 02:06
TwoPhaseEulerFoam sara OpenFOAM Running, Solving & CFD 2 November 6, 2008 20:26
Bug in twoPhaseEulerFoam alberto OpenFOAM Bugs 2 May 20, 2008 21:25
TwoPhaseEulerFoam Bug alondono OpenFOAM Bugs 1 February 19, 2008 21:01
TwoPhaseEulerFoam newbee OpenFOAM 0 March 27, 2006 08:41


All times are GMT -4. The time now is 01:20.