[Manukamin_iisc]

Hello all,

I am currently carrying out compressible LES simulation of duct flows, with explicit time marching.

I need to add synethetic turbulence at the duct inflow to have a turbulent flow field within my domain. I know that there is a good amount of literature available out there that explains various methods to generate isotropic turbulence that can be added as velocity fluctuations to the required mean velocity at the inlet.

However, I am imposing a "pressure inlet" boundary condition, which means that I cannot now specify my inlet velocity. If I did so, the problem would become ill-posed. So I do not know how to add turbulent fluctuations now, given that I cannot specify my inlet velocity, but rather allow the velocity to develop for the given inlet and outlet pressure values.

I wasn't able to find any literature on this. Could anyone let me know how to get around this problem?

Cheers!

[FMDenaro]

Originally Posted by Manukamin_iisc

Hello all,

I am currently carrying out compressible LES simulation of duct flows, with explicit time marching.

I need to add synethetic turbulence at the duct inflow to have a turbulent flow field within my domain. I know that there is a good amount of literature available out there that explains various methods to generate isotropic turbulence that can be added as velocity fluctuations to the required mean velocity at the inlet.

However, I am imposing a "pressure inlet" boundary conditions, which means that I cannot now specify my inlet velocity. If I did so, the problem would become ill-posed. So I do not know how to add turbulent fluctuations now, given that I cannot specify my inlet velocity, but rather allow the velocity to develop for the given inlet and outlet pressure values.

I wasn't able to find any literature on this. Could anyone let me know how to get around this problem?

Cheers!

I suggest starting with an initial perturbed velocity field and let the inflow velocity developping...

You have read this paper ? https://www.researchgate.net/profile...f9296ad1de.pdf

[Manukamin_iisc]

Dear Dr. Denaro,

Yes I've tried your suggestion already. Here's what happens when I start with an initial disturbed velocity field:

The flow field within my domain has turbulent structures due to the the perturbed initial velocity field. And hence turbulence is sustained for a brief period. So far so good.

However, since I'm not adding any fluctuations at the inlet, although the developing inflow velocity is unsteady in nature, the unsteadiness slowly dies off since the pressure and density is fixed at the inlet (There is nothing that sustains this unsteadiness). once the flow field within is convected out, since the incoming flow is slowly becoming laminar, eventually, the entire flow field within the domain becomes laminar. I think I need to find a way to add pressure disturbances here instead of velocity! What do you think?

I'm aware of the Poinsot-Lele paper. In fact I've referred to it while implementing my characteristic boundary conditions. But it doesn't help me with this problem.

Regards,
Manu

[FMDenaro]

Originally Posted by Manukamin_iisc

Dear Dr. Denaro,

Yes I've tried your suggestion already. Here's what happens when I start with an initial disturbed velocity field:

The flow field within my domain has turbulent structures due to the the perturbed initial velocity field. And hence turbulence is sustained for a brief period. So far so good.

However, since I'm not adding any fluctuations at the inlet, although the developing inflow velocity is unsteady in nature, the unsteadiness slowly dies off since the pressure and density is fixed at the inlet (There is nothing that sustains this unsteadiness). once the flow field within is convected out, since the incoming flow is slowly becoming laminar, eventually, the entire flow field within the domain becomes laminar. I think I need to find a way to add pressure disturbances here instead of velocity! What do you think?

I'm aware of the Poinsot-Lele paper. In fact I've referred to it while implementing my characteristic boundary conditions. But it doesn't help me with this problem.

Regards,
Manu

be careful, in principle a laminar velocity inlet profile will develop unsteadiness after some lenght due to transition towards the local critical Re number... how about the lenght of your channel? Do you use a dinamic SGS model?
However, you can use a perturbation in the density and pressure at inflow, of course letting the suitable lenght to develop from numerical conditions.
Alternatively, you can perform a precurso simulation with periodic BCs and saving the solutions for using them as inflow

[Manukamin_iisc]

My simulation is at a very low Reynolds number of 2000 based on the duct width. My duct length is not sufficient either. Which is why it is hard to have natural transition of flow from laminar to turbulent state. However, in an experimental paper that I'm trying to simulate, the authors report a turbulent flow field at such a low Reynolds number due to wall roughness effect. Therefore, in order to mimic the experiments closely enough, I'm looking to add turbulence at the inflow artificially.

I think it is a very good idea to perform a precursor periodic channel flow simulation and feed that solution at the inflow. I'll try it out.

Thanks a lot for your suggestions!

[FMDenaro]

well, after a lenght ten times the height you reach Re=2 x 10^4 ... you should get an unsteady solution...I can suppose you have too dissipation in your code, maybe due to the numerical discretization, to the SGS model or to both!

[Manukamin_iisc]

That's right. If the duct length is long enough, I suppose I should get an unsteady solution.

By the way, we do not use the SGS model for sub-grid scale modelling in our lab. We use "explicit filtering method" as a sub-grid scale model. It is a very simple and elegant method to model the sub-grid scale structures. You might want to take a look at it:
http://scitation.aip.org/content/aip...1063/1.1586271

[FMDenaro]

Originally Posted by Manukamin_iisc

That's right. If the duct length is long enough, I suppose I should get an unsteady solution.

By the way, we do not use the SGS model for sub-grid scale modelling in our lab. We use "explicit filtering method" as a sub-grid scale model. It is a very simple and elegant method to model the sub-grid scale structures. You might want to take a look at it:
http://scitation.aip.org/content/aip...1063/1.1586271

I worked too with deconvolution-based approach, it can be shown that the recovering of the energy content (for smooth filter) is an SGS model, in the category of the scale similar model. You can see many details in the book of Sagaut. Also, have a look here

http://link.springer.com/book/10.100...-90-481-2819-8

[Manukamin_iisc]

Oh I see. That result sounds interesting! I'll read more about it. Thanks!