[zippostyle]

Dear all,

I currently am performing internal flow simulations of piping systems. Simulations involve a small pipe in the middle of a larger pipe. Holes in the side of the smaller pipe make flow go to the larger one (no reflux since the pressure in the smaller pipe is higher).

In terms of laminar or turbulent flow, the following can be said:
- Internal flow of the small pipe is originally laminar
- Internal flow of the larger pipe is originally laminar
- Flow exitting through the small side-holes has speeds which give laminar flow in through the side-holes
- The above speed is high enough to induce turbulence in the large pipe

After performing several simulations, both laminar and turbulent, I got different answers:

- Using a steady state laminar model, the problem does not converge;
- Using a steady state turbulence model, the problem does converge;
- Uing a transient laminar model, the problem converges but results show an inconsistent flow pattern not commonly seen in laminar flow

My question to you is: does this have to do with a periodic detachment from the small pipe or turbulence in the larger pipe or something else completely? And what is considered to be the right approach in modelling technique here?

attached you'll find the goemetry

Thanks in advance!

[flotus1]

"Laminar" is not a model. You are solving the Navier-Stokes equations directly, i.e. performing a DNS. This of course requires adequate resolution of the spatial and temporal scales of the flow.
If you can not afford a proper DNS, LES is the next logical step if you want to go beyond a RANS approach.

Uing a transient laminar model, the problem converges but results show an inconsistent flow pattern not commonly seen in laminar flow

Some pictures of the flow fields you are referring to might help.

[FMDenaro]

I agree...
if your problem has a quite small lenght scale you can afford a DNS. No additional hypothesis on the regime of the flow are required, only a grid enough fine to resolve up to at least the Taylor micro-scale

[zippostyle]

Thank you for the fast reply,

I am familiar with the usage and considerations involved with regard to difference between Laminar and Turbulent (RANS/LES/DNS) flow modelling. Perhaps model was not the right term to describe the used equation.
What i ment was when i solve the system using the laminar flow solver, the steady state simulation does not converge, but a transient simulation does, while giving an assymetrical velocity field (i am expecting a symmetrical velocity field).

Furthermore, the turbulence equation i am using is the spalart-allmaras eddy viscosity one. relatively small geometry permit solving the viscous sub-layer (maximum y+ is kept around 2.3). Using LES or DNS is however not possible due to limited computational power and time.

To give you some more information concerning this problem:

The average flow within the small pipe (D=0.65mm) is 1 m/s (resulting in a Re of 600 (laminar regime).
The average flow speed in the small holes (D=0.16mm) is 2 m/s (resulting in a Re of 0.3)
The average flow speed in the larger pipe (D=4.5mm) is 0.33 m/s (resulting in a Re of 500

When considering the 2 m/s entering the pipe of 4.5mm however, Re will move to the turbulent regime.

The dynamic viscosity of the model can be considered to be 1e-3 (water)

Which simulation approach should then be considered?


Attached you'll find the velocity fields of both the transient laminar and the steady state turbulence model

[FMDenaro]

You should be aware of the physics of your flow ... in an unsteady solution you cannot see a single snapshot...I immagine that you flow oscillate so that you have to:

1) let the solution run for some time, the arbitrary initial condition must be forgotten by the solution. Only after the numerical transient is finished you can see the physically correlated solution
2) Sampling of the solution over several time unit
3) statistical analysis fro the sample

[zippostyle]

@FMDenardo,

So what you mean is i have to 'average' my transient solution on basis of statistics? That was what i thought initially.
But in my oppinion it seems weird that this cannot be done by running the laminar solver in steady state. It should eventually be possible to avarage down an unsteady flow-field using a steady state simulation right?

Does in this case the a laminar simulation in transient mode gives me a correct solution, or should i run a turbulence model in transient mode to get a correct solution?

The geometry in this case kind of restricts proper determination of the Reynolds number, indicating laminar or turbulent flow.

Thanks in advance!

[flotus1]

It should eventually be possible to avarage down an unsteady flow-field using a steady state simulation right?

No, this assumption is wrong. You might get A solution with a steady-state solver, but not necessarily the same you would get from a time-average using a transient solver.

[zippostyle]

Ok, so what I understand from your point of view is to run the simulation with the use of the laminar equation (so no turbulence model) on unknown (local) Reynolds numbers (of which i know several being in the turbulent or transitional regime) with the Y+ being 2.3 in transient mode?
The fluctuations in the results (e.g. velocity field) are then defined by the largest lengthscales in the grid (and thus dependent on grid size), resulting in an 'almost but not quite' correct DNS simulation? Taylor lengthscale could be achieved by refining my mesh by a factor of 4 then.

Or am I seeing this completely wrong? And should I in this case use a transitional or fully turbulent model to take into account the higher Y+ values in the grid?

We're getting there, just a few more steps!
Thanks in advance!

[FMDenaro]

Originally Posted by zippostyle

@FMDenardo,

So what you mean is i have to 'average' my transient solution on basis of statistics? That was what i thought initially.
But in my oppinion it seems weird that this cannot be done by running the laminar solver in steady state. It should eventually be possible to avarage down an unsteady flow-field using a steady state simulation right?

Does in this case the a laminar simulation in transient mode gives me a correct solution, or should i run a turbulence model in transient mode to get a correct solution?

The geometry in this case kind of restricts proper determination of the Reynolds number, indicating laminar or turbulent flow.

Thanks in advance!

Sorry to say that you are quite confused in these issues... steady laminar is due to the fact that the time derivatives of the pointwise variables vanish while a statistical steady state is obtained when the ensemble/time average does not depend on time.
Furthermore, if you run a DNS you are already running a transient case for a turbulent flow.

[FMDenaro]

Originally Posted by zippostyle

Ok, so what I understand from your point of view is to run the simulation with the use of the laminar equation (so no turbulence model) on unknown (local) Reynolds numbers (of which i know several being in the turbulent or transitional regime) with the Y+ being 2.3 in transient mode?
The fluctuations in the results (e.g. velocity field) are then defined by the largest lengthscales in the grid (and thus dependent on grid size), resulting in an 'almost but not quite' correct DNS simulation? Taylor lengthscale could be achieved by refining my mesh by a factor of 4 then.

Or am I seeing this completely wrong? And should I in this case use a transitional or fully turbulent model to take into account the higher Y+ values in the grid?

We're getting there, just a few more steps!
Thanks in advance!

what about your Reynolds number referred as to the integral lenght scale? Running a DNS means that your computational grid is so fine to achieve a cell Reynolds number of O(1). Otherwise if you cell Re number is greater you are practically running a no-model LES.

[zippostyle]

Originally Posted by FMDenaro

what about your Reynolds number referred as to the integral lenght scale? Running a DNS means that your computational grid is so fine to achieve a cell Reynolds number of O(1). Otherwise if you cell Re number is greater you are practically running a no-model LES.

You are refering to a no-model LES. What is then the difference between applying the LES approach and solving the Navier-stokes directly with the use of the 'laminar' approach. If the viscous sublayer is fully resolved with the Y+ being <5
They will both only take into account the turbulent lenght scales which can be resolved by the grid.

[FMDenaro]

Originally Posted by zippostyle

You are refering to a no-model LES. What is then the difference between applying the LES approach and solving the Navier-stokes directly with the use of the 'laminar' approach. If the viscous sublayer is fully resolved with the Y+ being <5
They will both only take into account the turbulent lenght scales which can be resolved by the grid.

There exists no laminar approach ... It exists a solution of the NS equations and we define "laminar" If it describes some specific features.
If you have a resolved boundary layer and everywhere the Cell Reynolds number is O(1) then a no-model LES is actually a DNS.

[zippostyle]

But what is then the difference in terms of results between the approximated (approximated due to the grid size) solution of the NS equations and a LES turbulence model? Is there even a difference?

[FMDenaro]

Originally Posted by zippostyle

But what is then the difference in terms of results between the approximated (approximated due to the grid size) solution of the NS equations and a LES turbulence model? Is there even a difference?

Yes, the LES solution provides a locally filtered variable, without energy content at high wavenumbers while the DNS provides the solution with the full range of wavenumbers.
Practicallly, the DNS solution is much more rich of details of the small flow structures

[zippostyle]

But what if the DNS does not account for these smallest flow structures because the mesh does not resolve all the way down to Taylor lengthscales?

[FMDenaro]

Originally Posted by zippostyle

But what if the DNS does not account for these smallest flow structures because the mesh does not resolve all the way down to Taylor lengthscales?

In case of an unresolved DNS you are practically using the so-called no-model LES.

[vidyadhar]

Hi!


Can any one please clarify a fundamental doubt:


If the solution to a heat transfer problem is expected to be a periodic variation of temperature at a point in the domain, then which of the following modelling strategies are correct:


1. Going for transient Turbulent analysis - expected to give periodic output

2. Going for steady state Turbulent analysis - this analysis leads to what output? Whether it gives the mean value of the result that was given by transient Turbulent analysis? Or would there by any convergence issues?
3. Going for steady Laminar analysis by continuously refining cell size in order to achieve convergence. Can I call this DNS.


Another question:
If I do not know the temperature variation at a point in the domain as Rayleigh number increases, then I am running simulation like below: Is it correct?


Q1. If I run my simulation with fine grid with steady Laminar analysis and convergence is achieved if the residuals are below a certain threshold and a physical parameter of interest is not varying with iterations, Then Can this simulation be called DNS as Rayleigh number keep on increasing?
Q2. What problem in results(eg. temperature at a point) do I face if I get convergence with steady laminar+fine grid as Ra keeps on increasing? Would it be correct or should I go for transient laminar analysis?


Thanks in advance!
vidyadhar

[LuckyTran]

If you know there will be periodic temperature variation then you should probably go for a transient simulation. You can run try to run a steady case and it might give you the mean if you only care about the mean. But it also might not give you the mean. And you probably will encounter convergence issues. It's better not to worry about these and give yourself headaches and just do a proper transient simulation.

You should be able to achieve a converged solution for any mesh whether it is coarse or fine. To properly call it DNS, your grid must be super fine to resolve all the length scales. On a super coarse grid, you can technically call it a DNS. But it would be a terrible DNS. It would also be the wrong result. It is like someone handing you an orange and telling you it's an apple. We all know it's not an apple.

[JonN]

Hi, I also think vidyadhar and zippostyle should do transient simulations.

For a unsteady heat transfer problem it makes no sense to perform a steady state simulation - no matter how fine the grid is resolved - as the solution will not lead to an accurate result.
As the temperature field will vary as a function of time, the heat transport coefficients compared to an implicitly time averaged solution (steady state sim) will be much higher in reality.

For the flow from the small to the large pipe, it can be initially expected that the solution will be transient if Re for the small orifices connecting the two pipes is > 100.
If the accuracy of a RANS simulation (Maybe k-omega-SST or sigma model for this case?) is not sufficient, there is no way around perfoming a LES (always transient).
To avoid very high spatial resolution, select a proper LES model.
The converged transient laminar solution obtained by zippostyle might be misleading, if the spatial resolution is not high enough to resolve all shear components of the flow.

When performing transient simulations, always make sure the time step is sufficiently small, to keep the Cell convective Courant number (CFL) <~1.

[vidyadhar]

Originally Posted by LuckyTran

If you know there will be periodic temperature variation then you should probably go for a transient simulation. You can run try to run a steady case and it might give you the mean if you only care about the mean. But it also might not give you the mean. And you probably will encounter convergence issues. It's better not to worry about these and give yourself headaches and just do a proper transient simulation.

You should be able to achieve a converged solution for any mesh whether it is coarse or fine. To properly call it DNS, your grid must be super fine to resolve all the length scales. On a super coarse grid, you can technically call it a DNS. But it would be a terrible DNS. It would also be the wrong result. It is like someone handing you an orange and telling you it's an apple. We all know it's not an apple.

Hello Lucky Tran,
Thank you for the reply.
If I want to simulate a natural convection problem over a heat sink, how can I decide that I have to use Laminar analysis or turbulent analysis when I change parameters like heat supply to the heat sink, dimensions of the heat sink etc.

If I have to do Laminar analysis, how to decide whether to chose steady state simulation or transient simulation.. if I am interested in steady state solution.


Thanks in advance!
vidyadhar