# Time dependent solver of unsteady Navier Stokes

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 May 17, 2014, 10:45 Time dependent solver of unsteady Navier Stokes #1 Member   Mehrez Join Date: Nov 2012 Location: Bordeaux, France Posts: 80 Rep Power: 6 Hi, I'm simulating flow of incompressible fluid in periodic media. I have implemented dimensionless Navier Stokes equations with Comsol PDE module. 1- I resolve my problem with a steady solver (for high Reynolds number which leads to unsteady flow). I get a good solution. 2- I use this steady solution as initial values for my unsteady solver. The problem is that the unsteady solver is giving me a steady solution (for high Re !). The solution is still the same as the steady solver solution. The unsteady solver : Direct MUMPS solver, Times: range(0,0.002,1), Time stepping method: BDF, Steps taken by solver: Strict, Error estimation: Exclude Algebraic. Can you advice me please how can I fix this problem ? Thanks in advance. Mehrez

 May 17, 2014, 11:20 #2 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,693 Rep Power: 33 what about your flow problem and Re number? Are you solving in DNS? have you numerical viscosity due to upwind?

 May 17, 2014, 11:47 #3 Member   Mehrez Join Date: Nov 2012 Location: Bordeaux, France Posts: 80 Rep Power: 6 Dear FMDenaro, Thank you for your help. My geometry is a 2D periodic square (fluid) with a solid square placed in its center. The fluid represents 75% of my geometry. The governing equations are the time dependent dimensionless Navier Stokes equations (DNS), so I have just to give the Re number. Boundary conditions: - no slip BC at the interface fluid/solid. - periodic BC, vertically and horizontally (The fluid is driven by a volumetric force F=(1,0) ). I ran simulations with Re equal to 200 but I get stationary solution ! (comparing to OpenFoam, Re=200 gives unsteady flow). Even for a very high Re number, the Comsol time dependent solver is still giving a steady solution. Thanks, Mehrez

 May 17, 2014, 17:37 #4 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,693 Rep Power: 33 Are you using low order upwind schemes?

 May 17, 2014, 20:29 #5 Member   Mehrez Join Date: Nov 2012 Location: Bordeaux, France Posts: 80 Rep Power: 6 If I'm not wrong a such scheme is used for stabilization ?, On Comsol I can use streamline upwind Petrov-Galerkin (SUGP) or GLS but trying to compute with and then without stabilization didn't change the results, I still have a stationary solution. I suspect a problem with my solver.

May 18, 2014, 04:04
#6
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,693
Rep Power: 33
Quote:
 Originally Posted by Mehrez If I'm not wrong a such scheme is used for stabilization ?, On Comsol I can use streamline upwind Petrov-Galerkin (SUGP) or GLS but trying to compute with and then without stabilization didn't change the results, I still have a stationary solution. I suspect a problem with my solver.

"stabilization" is not necessary for viscous flows provided you solve up to the viscous scales...generally, such terms comes from solution of Euler equation with the presence of shocks.
In your case the scheme can be too dissipative, try using a more refined grid or use second order time-space discretization

May 18, 2014, 12:52
#7
Member

Mehrez
Join Date: Nov 2012
Location: Bordeaux, France
Posts: 80
Rep Power: 6
Quote:
 Originally Posted by FMDenaro "stabilization" is not necessary for viscous flows provided you solve up to the viscous scales...generally, such terms comes from solution of Euler equation with the presence of shocks. In your case the scheme can be too dissipative, try using a more refined grid or use second order time-space discretization
Dear FMDenaro,
Thank you for these precisions.
If I have well understood the User's Manual, the upwind scheme is used to stabilize the solution (damp the oscillations), am I right ?
Which scheme do you think is too dissipative ?
I am not using a stabilization in my problem and I am solving with a BDF solver which uses backward differentiation formulas with order of accuracy varying from one (that is, backward Euler) to five.
For the velocity discritization, the order is 2 and 1 for pressure.
I can send you my Comsol model if you can run it.

Thank you for your help.

Best regards,

Mehrez

 May 18, 2014, 13:49 #8 Super Moderator     Praveen. C Join Date: Mar 2009 Location: Bangalore Posts: 256 Blog Entries: 6 Rep Power: 10 You may have to add some disturbance to induce unsteadiness. E.g., perturb the initial condition by a small amount. __________________ http://twitter.com/cfdlab

May 18, 2014, 14:08
#9
Member

Mehrez
Join Date: Nov 2012
Location: Bordeaux, France
Posts: 80
Rep Power: 6
Quote:
 Originally Posted by praveen You may have to add some disturbance to induce unsteadiness. E.g., perturb the initial condition by a small amount.
Hello dear Praveen,
I use as initial values in the Comsol time dependent solver the solution of the stationary solver. It means that I don't have any perturbation in the initial values.
On the other side, If I do the same procedure on OpenFoam with the icoFoam solver, the results are much more better and I have unsteady flow for high Reynolds number.

Thank you for your help,

Best regards,

Mehrez

 May 19, 2014, 05:01 #10 Super Moderator     Praveen. C Join Date: Mar 2009 Location: Bangalore Posts: 256 Blog Entries: 6 Rep Power: 10 It may happen that openfoam has some sort of asymmetry in the solution process which induces instabilities to develop. If it does not happen in comsol you have to add some disturbance yourself. Mehrez likes this. __________________ http://twitter.com/cfdlab

 Tags comsol, navier stoke solver, transient flow, unsteady flow

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post djbungee OpenFOAM Programming & Development 45 March 23, 2015 05:14 Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20 mbay101 OpenFOAM Running, Solving & CFD 13 December 28, 2013 14:12 danny123 OpenFOAM Programming & Development 8 September 6, 2013 02:34 jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24

All times are GMT -4. The time now is 22:35.

 Contact Us - CFD Online - Top