[Mehrez]

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

[FMDenaro]

what about your flow problem and Re number? Are you solving in DNS? have you numerical viscosity due to upwind?

[Mehrez]

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

[FMDenaro]

Are you using low order upwind schemes?

[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.

[FMDenaro]

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

[Mehrez]

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

[praveen]

You may have to add some disturbance to induce unsteadiness. E.g., perturb the initial condition by a small amount.

[Mehrez]

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

[praveen]

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.

[luoan]

Originally Posted by Mehrez

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

Hi,I'm learning about it now.Can you share me how you implement dimensionless Navier? THX
Does it build with weak form PDE ?