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

Pressure instability with rhoSimpleFoam

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

Like Tree1Likes
  • 1 Post By Chris Lucas

Reply
 
LinkBack Thread Tools Display Modes
Old   September 30, 2011, 08:13
Default Pressure instability with rhoSimpleFoam
  #1
New Member
 
Philipp Hofemeier
Join Date: Sep 2011
Location: Freiberg, Germany
Posts: 7
Rep Power: 5
philipp. is on a distinguished road
Dear all,


for my diploma thesis I am simulating a subsonic flow (Ma = 0.5) through a convergent divergent (De Laval) nozzle. For this purpose I choose to use the rhoSimpleFoam solver in OF 1.7.1. It works fine with some meshes. But on others it is not converging.


To me it appears as if it is due to the aspect ratio for the cells. To show this I uploaded two identical cases. One has a high aspect ratio (a low resolution in flow direction → see the blockMeshDict). This mesh works fine and gives a good solution in comparison to theoretical calculations (http://dl.dropbox.com/u/24363809/Lav...soltion.tar.gz).
The other has a low aspect ratio which means a high resolution in stream direction (http://dl.dropbox.com/u/24363809/Lav...soltion.tar.gz). Surprisingly this mesh does not converge although the mesh resolution is higher. The results show that the temperature and the velocity are quite stable and only the pressure is oscillating (as seen in the case folder).
Besides the mesh the cases are completely identical. In order to solve the problem I tried several measures:


  • change of the discretization methods to limited, higher order schemes
  • change of the boundary and initial conditions
  • nonOrthogonalCorrectiors from 0 up to 10
  • I used the k-Epsilon and the k-Omega model
  • change of the relaxation factors


Non of these measures could stabilize the solution. All in all I would be grateful if somebody could help me solve the problem or explain why the rhoSimpleFoam solver cannot converge on the mesh with higher resolution.
Furthermore, I would like to know if anybody ever used the rhoSimpleFoam solver on a tetrahedral mesh. Since I ran some calculation on different tetra meshes and all of them did not converge.


Thanks for your help!


Philipp
philipp. is offline   Reply With Quote

Old   October 3, 2011, 01:43
Lightbulb
  #2
Member
 
kiran Ambilpur
Join Date: Jun 2010
Posts: 34
Rep Power: 7
kiran is on a distinguished road
Send a message via Skype™ to kiran
Hi phillip

use SonicFoam solver instead of rhosimplefoam.

all we require is a compressible and turbulent solver.

I fell like u will not get any issues with this solver

Regards
Kiran Ambilpur
kiran is offline   Reply With Quote

Old   October 3, 2011, 06:10
Default
  #3
New Member
 
Philipp Hofemeier
Join Date: Sep 2011
Location: Freiberg, Germany
Posts: 7
Rep Power: 5
philipp. is on a distinguished road
Hello Kiran!

Thanks for your reply. However, to me the sonicFoam solver seems not to be the right solver for my problem. When you check the user guide it says that the sonicFoam is a "Transient solver for trans-sonic/supersonic, laminar or turbulent flow of a compressible gas". But I got a subsonic (and steady) problem to solve. Anyway, I will try it and let you know about my results.

Philipp
philipp. is offline   Reply With Quote

Old   October 4, 2011, 13:22
Default
  #4
New Member
 
Philipp Hofemeier
Join Date: Sep 2011
Location: Freiberg, Germany
Posts: 7
Rep Power: 5
philipp. is on a distinguished road
Hi,

I tried the sonicFoam solver. By initialising "good" (fully converged) initial conditions the solver gives good results otherwise the solver needs long time to stabilize. However, the performance is not very good since I only need the steady state solution. Additionally, isn't sonicFoam an inviscid solver? For further applications I need to use a viscid solver.

Has anybody some more experience with rhoSimpleFoam, especially on tetrahedral meshes?

Regards, Philipp
philipp. is offline   Reply With Quote

Old   October 5, 2011, 02:56
Post
  #5
Senior Member
 
Christian Lucas
Join Date: Aug 2009
Location: Braunschweig, Germany
Posts: 198
Rep Power: 7
Chris Lucas is on a distinguished road
Hi

it will be difficult getting a solution using a steady state solver for your problem. So my suggestion, don't spend more time on rhoSimpleFoam.

About sonicFoam, I see no reason against this solver. You might want to consider changing the energy equation to a total energy equation, might increase stability.

Solving the total energy equation

If your simulations are too slow, try rhoPimpleFoam, but have a look at the continuity error and mass imbalance in your system. You should not relax the density and, in the last internal iteration, the pressure.

About some of the points in your first post:

"change of the discretization methods to limited, higher order schemes"
--> use upwind!

"nonOrthogonalCorrectiors from 0 up to 10"
--> Do you have a strongly nonOrthogonal grid? If not, you don't need so many nonOrthogonalCorrectiors


Best Regards,
Christian



mm.abdollahzadeh likes this.
Chris Lucas is offline   Reply With Quote

Old   October 5, 2011, 14:08
Default
  #6
New Member
 
Phil
Join Date: Mar 2011
Location: West Des Moines, Iowa, U.S.A.
Posts: 5
Rep Power: 6
peob is on a distinguished road
Philipp,

I took your Laval-fineResolution case and ran it with version-2.0.1.
I was able to repeat the same behavior you observed.

Then I dropped the relaxation factor on "rho" from 0.05 down to 0.01, and the solution converged. Note that I didn't change anything other than the relaxation factor for "rho".

I've attached the fvSolution file and an image showing the convergence I obtained.

I also tried to increase the relaxation factor on "rho" after it converged, and the residuals rose right back up to what you were observing with "rho 0.05;".

I have no idea why the relaxation factor for "rho" should be so low... especially after the solution converges.

Phil
Attached Images
File Type: jpg Laval-fineResolution.jpg (64.5 KB, 98 views)
Attached Files
File Type: txt fvSolution.txt (1.7 KB, 66 views)
peob is offline   Reply With Quote

Old   October 6, 2011, 09:44
Default
  #7
New Member
 
Philipp Hofemeier
Join Date: Sep 2011
Location: Freiberg, Germany
Posts: 7
Rep Power: 5
philipp. is on a distinguished road
Hey Phil,

I also observed the same behavior when I initialized a converged solution. But with a relaxation factor of 0.01 for rho seems to work well even on a tetra mesh! When I was playing with the relaxation factors I just changed the factors for p and U .
So thank you very much!

Regards, Philipp
philipp. is offline   Reply With Quote

Old   July 27, 2015, 09:31
Default
  #8
New Member
 
Christa
Join Date: Apr 2011
Posts: 27
Rep Power: 6
user_of_cfx is on a distinguished road
Quote:
Originally Posted by Chris Lucas View Post
Hi

If your simulations are too slow, try rhoPimpleFoam, but have a look at the continuity error and mass imbalance in your system. You should not relax the density and, in the last internal iteration, the pressure.

Hi Christian,

I am struggling with rhoPimpleFoam at the moment, my pressure specifically will not converge (sum local = ~ 0.6) after trying several mesh resolutions, boundary conditions, fvSchemes and fvSolutions adjusted based on advice in this forum (mostly Gauss upwind schemes with GAMG solver for pressure), and the results I output before the simulation crashes look funny. I am very new to OpenFOAM and any advice (or directing me to another post on this forum I may have missed?) on things to look out for when using rhoPimpleFoam will be greatly appreciated.

I am not posting my problem just yet because I know for a fact I have not tried everything yet. I am only looking for general tips.

Thanks,

Christa
user_of_cfx is offline   Reply With Quote

Reply

Tags
compressible flow, laval nozzel, rhosimplefoam, tetra mesh

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
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
Pulsatile pressure inlet with pressure outlet a.lynchy FLUENT 3 March 23, 2012 14:45
Problem with rhoSimpleFoam : exploding enthalpy and density at the walls david39 OpenFOAM Running, Solving & CFD 6 January 18, 2011 12:49
Pressure in rhoSimpleFoam vitor OpenFOAM Running, Solving & CFD 2 September 16, 2010 11:49
Setting pressure and velocity in inlet Asghari FLUENT 5 September 22, 2006 13:23


All times are GMT -4. The time now is 20:32.