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

chtMultiRegionSimpleFoam - Stabilise mass flux in a sub-divided channel

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

Like Tree1Likes
  • 1 Post By billie

Reply
 
LinkBack Thread Tools Display Modes
Old   April 25, 2013, 06:42
Default chtMultiRegionSimpleFoam - Stabilise mass flux in a sub-divided channel
  #1
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
When solving the flow through a sub-divided channel the mass fluxes should be equal in all divisions. However the mass fluxes in the individual splits diverge from the expected distribution after some iterations.

Case geometry:
geometry.jpg
Starting from one inlet the channel is split up into eight separate channels (Here the mass flux is measured). Four of them are combined again to the two outlets.


Mesh:
detail.jpg
The mesh consists of prismatic layers and a tetrahedra core mesh. The mesh seems coarse but this way I get quicker results. The problem occurs as well with a mesh triple the size.


Output from checkMesh:
log.checkMesh.txt

Contents of fvSchemes and fvSolution for the fluid domain:
fvSchemes.txt
I have not a lot experience with different schemes so I just used the defaults from the heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater tutorial. Maybe there is room for improvement here.

fvSolution.txt
Here I already tried to lower the residual tolerances, add one NonOrthogonalCorrector and to under-relax a lot without success.

Last edited by billie; April 25, 2013 at 16:12.
billie is offline   Reply With Quote

Old   April 25, 2013, 06:45
Default
  #2
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
Adding further information in a second post as only five attachments are allowed per post.

Output from chtMultiRegionSimpleFoam:
log.chtMultiRegionSimpleFoam.txt
This is the output from the first iterations and some at iteration number 200.

Mass flux of the different splits:
mass_flux_splits.png

Mass flux of the two outlets:
mass_flux_outlet.png


Is there a way to stabilise the system to avoid the divergence of the mass flux?
billie is offline   Reply With Quote

Old   April 25, 2013, 08:21
Default
  #3
New Member
 
ignacio's Avatar
 
Ignacio Gallego
Join Date: Jan 2013
Posts: 25
Rep Power: 4
ignacio is on a distinguished road
Hello Daniel,

The difference might be due to the asymmetry of the mesh.
Why don't you create one half and then mirror the other? You just have to include a file called mirrorMeshDict.
Also check the gravity direction!

You are using a One-Equation turbulent model right? Why don't you change to a more accurate two-equation method?

Cheers
ignacio is offline   Reply With Quote

Old   April 25, 2013, 08:55
Default
  #4
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
Hello Ignacio,

thank you for your answer.

Quote:
Originally Posted by ignacio View Post
The difference might be due to the asymmetry of the mesh.
Why don't you create one half and then mirror the other? You just have to include a file called mirrorMeshDict.
This is just a simple model to test the simulation. For the real model it is not possible to mirror the mesh.

Quote:
Originally Posted by ignacio View Post
Also check the gravity direction!
Gravity is applied in z-direction (the blue arrow from the coordinate system on the pictures) which should be fine.

Quote:
Originally Posted by ignacio View Post
You are using a One-Equation turbulent model right? Why don't you change to a more accurate two-equation method?
I would like to stick with Spalart-Allmaras because I am comparing with another solver and the only turbulence model they have in common is this one.

Last edited by billie; May 12, 2013 at 12:44.
billie is offline   Reply With Quote

Old   April 26, 2013, 03:53
Default
  #5
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
I forgot to add some information about the boundary conditions applied.

At the inlet there is constant velocity and zeroGradient pressure. For the outflows there is zeroGradient velocity and constant pressure.
billie is offline   Reply With Quote

Old   April 28, 2013, 12:03
Default
  #6
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
Nobody who can give me any hint here?

The mass flux on the inlet is 0.5kg/s so it should split to approximately 0.0625kg/s in the eight sub-divisions and 0.25kg/s should reach the two outlets. From the charts in the second post one can see that the mass fluxes in the individual channels as well as in the outlets diverge completely. Split 1-4 get high and 5-8 even negative. The total mass balance is correct but the individual flows are unrealistic.

I am trying to compare with another software which does not have this problem, so I think there must be anything wrong with my setup.
billie is offline   Reply With Quote

Old   May 14, 2013, 10:11
Default
  #7
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
I found the reason for the extreme mass imbalance. If I increase the number of iterations the system balances after a high number of iterations. First of all refining the mesh and improving the mesh quality helps to some degree. The most influential factor however is relaxation. Until now I applied the same relaxation values for pressure and velocity. Lets say U = 0.6 and p = 0.6. Reducing both values only has the effect that it takes longer to converge but the imbalance remains the same. However under-relaxing velocity more than pressure greatly reduces the imbalance (U = 0.3, p = 0,7 like in the cht tutorial). There is still an initial imbalance but it is lower in magnitude and it takes a lot less iterations until the imbalance is resolved.
nsf likes this.
billie is offline   Reply With Quote

Old   June 13, 2013, 13:28
Default
  #8
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
I also played a bit with different schemes and found that using leastSquares as gradScheme and corrected as snGradScheme also reduces the imbalance as well as the simulation time. The individual iterations take longer but with the faster convergence the overall simulation time is reduced.
billie 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
Fixed Outlet Mass Flux boundary condition? trex930 OpenFOAM Pre-Processing 2 June 30, 2010 21:44
mass flux units in kg/ms cfd~ Main CFD Forum 0 May 3, 2007 16:45
Calcuationg mass flux of a UDS? Derek FLUENT 0 March 20, 2006 08:58
mass flux correction at outflow boundaries Subhra Datta Main CFD Forum 2 November 24, 2003 14:11
total mass flux correction for compressible fluid? Francesco Di Maio Main CFD Forum 0 August 21, 2000 04:23


All times are GMT -4. The time now is 13:06.