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

Solution diverges at the corner of orthogonal mesh

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

Like Tree2Likes
  • 1 Post By tomf
  • 1 Post By Akshay

Reply
 
LinkBack Thread Tools Display Modes
Old   January 3, 2016, 21:07
Default Solution diverges at the corner of orthogonal mesh
  #1
New Member
 
Amir Abbas Aliabadi
Join Date: Mar 2013
Posts: 26
Rep Power: 5
amir.a.aliabadi is on a distinguished road
Hello Dear FOAMers,

I have been benefiting from this forum a lot, and would like to seek your help in my problem. I am simulating air flow in an urban canyon by establishing a pressure differential (0.5 divided by density) across the canyon and implementing cyclic boundary conditions on inlet/outlet as well as front/back of my domain. See pictures attached. I have a heated bottom (street) to 352.15 K, adiabatic walls, and ambient temperature and roof temperatures equal to 293.15 K.

I have compiled a solver to combine functionalities of buoyant boussinesq approximation, LES turbulence model, Pimple algorithm, and passive scalar transport. The mesh is generated using blockMesh and y+ is close to 1 to ensure the boundaries are resolved.

The code works fine except that in one cell in a corner, and only one corner of my orthogonal mesh, the solution for temperature starts diverging. The solver operates under PISO model, and I have tried under-relaxing pressure. But this problem persists no matter how hard I try.

Would anyone please make a suggestion? I have attached pictures of the mesh and the diverging corner. I have also attached all files from the solver as well as the case files...

I appreciate your help...
Amir
Attached Images
File Type: jpg Diverging Temperature at the Corner.jpg (34.2 KB, 42 views)
File Type: jpg Entire Domain.jpg (25.3 KB, 33 views)
Attached Files
File Type: gz passiveScalarBuoyantBoussinesqPimpleLESFoam.tar.gz (2.8 KB, 5 views)
File Type: gz canyon4.tar.gz (5.1 KB, 6 views)
amir.a.aliabadi is offline   Reply With Quote

Old   January 6, 2016, 06:45
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 302
Rep Power: 12
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi,

I suspect it may be related to the pRefCell that you set in fvSolution. Since you use cyclics on inlet and outlet you need to have a reference pressure somewhere. I guess your diverging cell is cell 0. Maybe it helps to use a pRefPoint somewhere in the center of the domain or in a location where the pressure is steady.

Code:
PIMPLE
{
    momentumPredictor no;
    nOuterCorrectors 1;
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
}
amir.a.aliabadi likes this.
tomf is offline   Reply With Quote

Old   January 6, 2016, 11:10
Default
  #3
New Member
 
Amir Abbas Aliabadi
Join Date: Mar 2013
Posts: 26
Rep Power: 5
amir.a.aliabadi is on a distinguished road
Hello Dear Tom,

Thank you for your effective suggestion and I appreciate your time. I changed the pRefCell to a middle point on the topLid of the domain with pRefValue of 0. The solution in the corner at pRefCell = 0 is now well behaved. However, the solution at and around the new pRefCell shows similar effect to the old corner cell. Again I get some cooling in the cell with starts to propagate in the neighbouring cells. I am wondering why this is happening at the pRefCell.

My colleague suggested having maximum temperature range in the entire domain up to 15 K for the use of Boussinesq approximation to be valid. I also ensure that for the PISO algorithm the Courant number is around 0.2. Do you think this may be cause by pRefCell being at the boundary? Shall I move this point to the centre of the domain somewhere?

Regards,
Amir
amir.a.aliabadi is offline   Reply With Quote

Old   January 6, 2016, 11:56
Default
  #4
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 302
Rep Power: 12
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Dear Amir,

Well at least we know that the error stems from the pRefCell. I suspect that if you change it to the middle of the domain you will have similar behavior. I know this has been discussed before on the forum (google site:cfd-online.com temperature anomaly pressure reference cell).

Best solution would probably to fix the pressure on a boundary, so the reference cell pressure is not set during the computation, but this may interfere with your cyclic pressure jump. I have not done something like this myself so unfortunately all I can do is give some pointers.

Regards,
Tom
tomf is offline   Reply With Quote

Old   January 6, 2016, 15:54
Default
  #5
New Member
 
Amir Abbas Aliabadi
Join Date: Mar 2013
Posts: 26
Rep Power: 5
amir.a.aliabadi is on a distinguished road
Hello Dear Tom,

Thank you for the follow up and referring me to other discussions. I found them very useful.

Regards,
Amir
amir.a.aliabadi is offline   Reply With Quote

Old   January 7, 2016, 10:38
Default
  #6
Member
 
Akshay Kumar
Join Date: Aug 2010
Location: India
Posts: 82
Rep Power: 7
Akshay is on a distinguished road
Hello Amir

I think Tom has pointed in the right direction. I would also suggest trying to run this case using a compressible solver. This would take out the Pressure referencing adjustment at the matrix level.
amir.a.aliabadi likes this.
Akshay is offline   Reply With Quote

Old   January 12, 2016, 17:19
Default
  #7
New Member
 
Amir Abbas Aliabadi
Join Date: Mar 2013
Posts: 26
Rep Power: 5
amir.a.aliabadi is on a distinguished road
Hello Dear Colleagues,

Let me thank you all for making such effective comments. So I moved to a compressible solver "buoyantPimpleFoam" provided by OpenFOAM with a tutorial under heatTransfer folder. This solver has the capability to be adapted to LES, which I successfully implemented. In order to get the cyclic inlet/outlet with a pressure jump working, I had to use the cyclic boundary condition "fixedJump" in OpenFOAM 3.0.1. Surprisingly the "fan" boundary condition does not work properly in this version of OpenFOAM, but the "fixedJump" is working suitably. I will post any other updates that I may find useful to other users with the same problem.

Regards,
Amir
amir.a.aliabadi 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
Star CCM Overset Mesh Error (Rotating Turbine) thezack CD-adapco 4 April 26, 2016 02:03
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
Converging the solution aja1345 FLUENT 10 June 26, 2015 18:00
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
Layers:problem with curvature giulio.topazio OpenFOAM Native Meshers: snappyHexMesh and Others 10 August 22, 2012 09:03


All times are GMT -4. The time now is 20:44.