CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Initial Residual for p too high! (https://www.cfd-online.com/Forums/openfoam-solving/114088-initial-residual-p-too-high.html)

nikesh March 5, 2013 04:58

Initial Residual for p too high!
 
1 Attachment(s)
Hi all,

I am simulating a simple 2D flat plate flow in OpenFoam using simpleFOAM to validate a new turbulence model that I would like to implement here. This new turbulence model is a slight modification of the kOmegaSST model which includes few new terms into the nut equation.

Results from kOmegaSST model are all OK! However, when I use this new model for the same grid, my initial pressure residuals oscillate around a pretty high value, at around 0.03 while the initial U,k and omega residuals are all at a reasonable convergence criterion, at around 10^-5.

This is not making much sense to me. Because, after some iterations(about 6~7,000) when I extract the results (even without reaching the convergence tolerance) and compare, they don't yet seem so weird or deviating highly from that of the SST's results.

I have checked my code numerous times, doesn't seem to have any problems in there.

Could there be a problem with the solvers I chose?

I am as well wondering how the p-residual is calculated in simpleFOAM.

I would highly appreciate any insights into this!

Thanks!
Nikesh

These are my settings and I've used the same for kOmegaSST (in the pic attached).

immortality March 5, 2013 05:17

hi
Test for one or two order lower p tolernces than U,...
1e-9 or 1e-10

nikesh March 5, 2013 06:23

Thanks!
Tried, yet not much of a difference.

andrei.cimpoeru March 9, 2013 16:51

Hi


Basically I am having the same problem.... I just want to ask you if you managed to do it in the end. I am simulating the flow over an aerofoil using k omega sst and simpleFoam with wall functions..........
Have you got any ideas?


Thanks

Andrei

nikesh March 10, 2013 01:35

Hii Andrei,
Well, I am still stuck with the same problem. Obviously higher p-residual means mass is not being conserved so well somewhere in the cells. You might want to look into your boundary conditions once more. Basically that is what I am trying to do too. And the schemes and type of mesh you are using for airfoil flow.

andrei.cimpoeru March 10, 2013 07:28

Hi

Ok I understand . I am using k omega sst , wall functions and simpleFoam solver ..... I have changed my boundary conditions many times still nothing......for example how you o file looks like and something that I don't understand : how do you calculate
the turbulent kinetic energy K and the rate of dissipation W(omega).......

thanks

Andrei

chegdan March 10, 2013 10:56

Nick,

There are some strategies that I would try to get these residuals down to something you would like.
  1. Lower your pressure relTol by an order of magnitude compared to U i.e. relTol = 0.001 for P and relTol = 0.01 for U.
  2. Without knowing the mesh you are using you may need to increase the nonorthogonal corrector by 1 or 2. if you are using a tet mesh...then there are many things you can do.
  3. Use first order schemes to start with (you will move to higher order ones later)
  4. Obtain an initital velocity field with potentialFoam
  5. Using simpleFoam, the intial condition from potentialFoam, and first order schemes...turn turbulence OFF and once convergence seems to bottom out, turn turbulence on while the simulation is running
  6. Once a steady-state is obtained, stop the simulation, switch to second order schemes and restart the simulation with turbulence on and see if that helps

There are a lot of other strategies that you can try, but this one might be sufficient. Without knowing more details like divergence schemes; mesh structure and checkmesh results; y+ values; and boundary conditions there is not much to add on my part.

I would look at the thread http://www.cfd-online.com/Forums/ope...-problems.html and then move on to a search of the forum. There are many threads about simpleFoam convergence...but my list of threads is not in front of me right now. good luck.

immortality March 15, 2013 05:17

how can decrease the initial residuals for p in unsteady problems when relaxations are not applicable?

teodm May 25, 2017 02:52

Hello guys,

I am running a simulation of a flow over two wings. My simulation is 3d.I check the mesh and there is no error. I am using freestream bc and wall functions. Solver is simplefoam and turbulence model spalart almaras dudes. The problem is when I ran with coarse mesh the solution converge but when I ran with finer mesh the pressure residuals don't fall under 10^-5 they stop at about 2*10^-4.I used snappyhexmesh for the mesh. Any advice would be useful thank you in advance.

Thodoris

andrei.cimpoeru May 25, 2017 03:58

Quote:

Originally Posted by teodm (Post 650205)
Hello guys,

I am running a simulation of a flow over two wings. My simulation is 3d.I check the mesh and there is no error. I am using freestream bc and wall functions. Solver is simplefoam and turbulence model spalart almaras dudes. The problem is when I ran with coarse mesh the solution converge but when I ran with finer mesh the pressure residuals don't fall under 10^-5 they stop at about 2*10^-4.I used snappyhexmesh for the mesh. Any advice would be useful thank you in advance.

Thodoris

Having low residuals it does not mean that you simulation is physical. It is quite obvious that when you increase the mesh resolution to have higher residuals since you are capturing more physics. The best thing to do is to plot pressure and friction on your wings or lift and and drag and check you the results change as you increase the mesh resolution. Also check your y+ value for Spalart model. Cheers

teodm May 25, 2017 17:40

1 Attachment(s)
Andrei,
Thank you a lot for your answer.I am trying to calculate the cl, cd but i am having troubles because of my geometry, which consists two wings in the same but opposite angle of attack (+- 8 degrees) so i am having problems with the normals. I hope you have an idea to face this problem.I am attaching my geometry.

Thank you very much in advance.

andrei.cimpoeru May 26, 2017 06:53

Quote:

Originally Posted by teodm (Post 650303)
Andrei,
Thank you a lot for your answer.I am trying to calculate the cl, cd but i am having troubles because of my geometry, which consists two wings in the same but opposite angle of attack (+- 8 degrees) so i am having problems with the normals. I hope you have an idea to face this problem.I am attaching my geometry.

Thank you very much in advance.

You can ask the solver to dump CL and CD for you. But instead of calculating for both configs why are you not simplifying the problem by doing just one wing starting form -8 angle of attack to +20 in order to understand the flow field. Then you can probably have a look at much more complex configs.

Cheers


All times are GMT -4. The time now is 12:14.