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

CavitatingFoam with a moving mesh mass conservation error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 26, 2007, 16:06
Default Dear all, I am trying to bu
  #1
New Member
 
Ido Silverman
Join Date: Mar 2009
Posts: 13
Rep Power: 7
idosil is on a distinguished road
Dear all,

I am trying to build a cavitation flow model with dynamic mesh. However, I have a mass conservation problem when I use a moving mesh. At first, I modified cavitatingFoam solver to have moving mesh, then I modified sonicFoamAutoMotion to include barotropic cavitating model as with cavitatingFoam. With both solvers I have the same problem. Mass do not conserve as soon as vapor fraction increases if I use a moving mesh. I have two test problems. The first is a close volume with a boundary condition of constant flow out on one of the boundaries. The conditions in the volume change from liquid to a mixture of liquid and vapor as the density and pressure decrease due to the flow out. In the other case, I use moving mesh to simulate the expansion of the volume in order to get similar density and pressure decrease. As before, the conditions change from one to two phases. However, there is a small increase of total mass even though the mass flux over the boundaries is zero (I have checked it with the surfaceIntegrate function.)
I would appreciate any help to locate the source of this error.
I attach three files with the solver based on sonicFoamAutoMotion and the two test problems.
cavSonicMoMFoam.tgz
decompressionSV15.tgz
decompressionDV15.tgz

Best regards,
Ido
idosil is offline   Reply With Quote

Old   November 26, 2007, 18:20
Default You have, of course, made sure
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,734
Rep Power: 20
hjasak will become famous soon enough
You have, of course, made sure that the mesh motion terms are added correctly to your momentum and pressure equation. Also, check the flux through moving walls to make sure you set up the boundary conditions correctly.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   November 27, 2007, 14:07
Default Dear Hrv, Thanks for the ad
  #3
New Member
 
Ido Silverman
Join Date: Mar 2009
Posts: 13
Rep Power: 7
idosil is on a distinguished road
Dear Hrv,

Thanks for the advice. I have checked the boundary conditions and the calculation of the fluxes on the face (I did surfaceInegrate to get the flux into each cell and then domainIntegrate to get the total flux in/out of the domain). For all practical purpose it was zero (if not exactly zero than in the order of 1e-20 or lower). Phi itself is practically zero on the domain boundaries (I print this field).
The error is probably due to inconsistent writing of the equations or in calculating one or some of the terms. However, I could not find it yet.
One problem I found with moving mesh is in the calculation of the time derivative of a field which has limiting values. For example, let look at the vapor fraction gamma which can be between zero and one only. The time derivative for Euler method with moving mesh is calculated as (gamma1 – gamma0*v0/v1)/dt where index 1 is for current conditions and 0 for previous time step. In any cell where gamma0=1 the multiplication of gamma by the volumes fraction is not correct. In most cases local conditions prevent change in gamma. The change in cell volume will influence the fluid by other parameters but not the volume fraction.
In the test problem this problem do not has any effect since for gamma=0 the multiplication has no effect. However, due to this problem I replaced the ddt(psi) term which appears in the original cavitatingFoam solver by the term (dPsi/dGamma)*ddt(gamma) (psi is function of gamma only, all other parameters are constants).

Best regards,
Ido
idosil is offline   Reply With Quote

Old   November 27, 2007, 17:27
Default Well Ido, that leaves only one
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,734
Rep Power: 20
hjasak will become famous soon enough
Well Ido, that leaves only one possibility: you did not account for mesh motion fluxes from phi after solving the pressure equation. Did you account for mesh motion when solving for phi and subtract mesh.phi() as appropriate?

There are two things you can check:
- volume conservation:
ddt(1) - div(mesh.phi()) = 0

- mass conservation, the usual way.

If both are satisfied, you will preserve boundedness on a moving mesh.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
Mass Conservation in LES Sas Main CFD Forum 3 July 6, 2007 10:37
Mass Conservation Prabhas FLUENT 0 December 5, 2006 01:15
mass conservation mange FLUENT 0 July 20, 2006 07:08
Mass Conservation in LES Jaswant Main CFD Forum 8 July 4, 2005 22:32
Mass Conservation Balaji FLUENT 0 May 11, 2005 07:16


All times are GMT -4. The time now is 10:18.