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

Pressure instabilities at the bottom of the domain

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 30, 2013, 15:25
Default Pressure instabilities at the bottom of the domain
  #1
Member
 
Join Date: Jul 2010
Posts: 32
Rep Power: 6
MaryBau is on a distinguished road
Hi;

I am running a case similar to a half channel flow and I am having problems due to some pressure instabilities that form at the bottom of the domain. The deltaT becomes really really really small and eventually the simulation crashes.

It seems that the pressure instabilities happen at the processors boundaries (see pics). I first used the scotch method to decompose the domain and the pressure instabilities are exactly where several processors meet. I also tried to used the simple method to decompose the domain only in the vertical direction, but I guess since most of my cells are close to the bottom, the decomposition did not yield a "perfect" division of the domain in the vertical direction and I also end up with some (less) pressure instabilities.

Notes:

- I am using pisoFoam (adjustableTime), k-w SST-DES and k-w-DDES.
- Cyclic boundaries (inlet-outlet, front-back), no-slip at the bottom and slip at the top.
- My mesh has really small and refined cells at the bottom (y+~0.3). I am using preservePatches (inlet outlet front back);
- pRefCell is not located at the pressure instabilities.


Any suggestions of what could it be the problem or how can I troubleshot it?

Thanks in advance!!!
Attached Images
File Type: jpg scotchDecomposition.jpg (11.7 KB, 25 views)
File Type: jpg simpleDecomposition.jpg (12.1 KB, 21 views)
MaryBau is offline   Reply With Quote

Old   January 31, 2013, 10:22
Default
  #2
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
Can you post your files so that we can have a look at it in more details?
doubtsincfd is offline   Reply With Quote

Old   January 31, 2013, 14:55
Default
  #3
Member
 
Join Date: Jul 2010
Posts: 32
Rep Power: 6
MaryBau is on a distinguished road
Thanks a lot doubtsincfd!

Here are the files.
Attached Files
File Type: gz scotchDecompositionCase.tar.gz (5.3 KB, 3 views)
MaryBau is offline   Reply With Quote

Old   January 31, 2013, 16:58
Default
  #4
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
Quick question: What are the dimensions of the domain you are trying to simulate? Do you scale your mesh? Otherwise it 3000 m long domain
doubtsincfd is offline   Reply With Quote

Old   January 31, 2013, 17:01
Default
  #5
Member
 
Join Date: Jul 2010
Posts: 32
Rep Power: 6
MaryBau is on a distinguished road
Yes, it is a 3000m long domain.

I am doing atmospheric boundary layer simulations.
MaryBau is offline   Reply With Quote

Old   February 1, 2013, 17:35
Default
  #6
Member
 
Join Date: Jul 2010
Posts: 32
Rep Power: 6
MaryBau is on a distinguished road
Hi again;

I ran the same case, but this time without decomposing it, in a single core.

I still get those "pressure instabilities" (see pics). However, this time, the instabilities happen right at pRefCell.

I also checked the flux over the boundaries and it seems to be correct.

Flux at top = 0m^3/s [0 l/min]
Patch: front found on 1/1 processor(s)
Flux at front = 580.795708m^3/s [34847742.5 l/min]
Patch: back found on 1/1 processor(s)
Flux at back = -580.795708m^3/s [-34847742.5 l/min]
Patch: inlet found on 1/1 processor(s)
Flux at inlet = -1494831.5m^3/s [-8.96898898e+10 l/min]
Patch: outlet found on 1/1 processor(s)
Flux at outlet = 1494831.5m^3/s [8.96898898e+10 l/min]
Patch: bottom found on 1/1 processor(s)
Flux at bottom = 0m^3/s [0 l/min]

Any suggestions? Is this normal?

Thanks!!
Attached Images
File Type: jpg singleCore.jpg (13.4 KB, 11 views)
File Type: jpg singleCore_2ndPic.jpg (11.6 KB, 11 views)
MaryBau is offline   Reply With Quote

Old   February 19, 2013, 17:19
Default
  #7
Member
 
Join Date: Jul 2010
Posts: 32
Rep Power: 6
MaryBau is on a distinguished road
In case someone is having the same issue, I finally solved this problem. The trick was to modifying the solvers for p AND U in the fvSolution file.

I had GAMG for p which I believe is not good for really elongated cells (?) and PBiCG for the velocity. The pressure instabilities disappear when I changed the solvers to PCG for pressure and smoothSolver for the velocity.

So the solvers in my fvSolution file look like this:

Code:
solvers
{
    p
    {
	solver          PCG;
      	preconditioner  DIC;
        tolerance       1e-6; 
        relTol          0.01;
	minIter         5;
	// maxIter         100;
    }

    pFinal
    {
	solver          PCG;
      	preconditioner  DIC;
        tolerance       1e-6; //-7;
        relTol          0;
	minIter         5;
        // maxIter         100;
    }

    U
    {
        //solver          PBiCG;
        //preconditioner  DILU;
        tolerance	1e-6; //-15;
        relTol          0;
	solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         1;
        //maxIter		100;
	minIter 	1;
    }
    
    k
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-10;
        relTol          0;
        nSweeps         1;
        //maxIter		100;
	minIter 	1;

    }

    omega
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-10;
        relTol          0;
        nSweeps         1;
        //maxIter		100;
	minIter 	1;
    }
}
MaryBau 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
"Pressure Inlet" Boundary Setup Wijaya FLUENT 13 April 11, 2013 09:50
Pressure outlet BC help! eishinsnsayshin FLUENT 7 December 4, 2012 00:36
Pressure outlet boundary condition fluent_newbie FLUENT 0 December 2, 2011 00:51
transient simulation of a rotating rectangle icesniffer CFX 1 August 8, 2009 08:25
Pressure Rise Error emueller CFX 0 May 5, 2009 12:08


All times are GMT -4. The time now is 02:35.