Fix Reynolds Number in a periodic flow
 

Hello to everyone,

I am trying to emulate the flow through periodic hills. Here is the case:
http://qnet-ercoftac.cfms.org.uk/w/i...3-30_Test_Case
But I am testing the effect of RANS simulations (k-omega and k-omegaSST) in these flow condition, using the solver simpleFoam in a 2D case.

To solve the case I am applying cyclic BC on the inlet and the outlet of the flow, without convergence problems.

However, I need to fix a Reynolds value to my simulation, with the reference velocity equal to the average velocity on the top of the second hill.

I am having problems to fix this value with the cyclic BC. When I initialize my internal field the final values diverge from the Reynolds Number I want to my case.

Any idea of how could I fix my average outlet velocity profile and then the Reynolds number with this Cyclic BC. Or how I should initialize better the internal field.

I have tried to simulate the flow as non-periodic Hill with the velocity profile of the experimental data of the reference in the inlet, and then map the fields to my Cyclic BC case. I have also tried to initialize the fields with a uniform value.

Any ideas of what should I do?

Thank you for your help.

I don't know how you tried to set the Re number. It is mostly best to change the viscosity rather than the velocity.

Thank you for your answer

Yes I have already try to set the viscosity to fix the Reynolds of my initial field. But the problem is that in the final field the velocity profile changes, changing then the value of the Reynolds Number according to the case criteria.

If exist a possibility of modifying dynamically the viscosity instead the velocity field, I will also like to know it. Please.

The main intention of this thread is try to find a way to fix the Reynolds number in the periodic simulation.

Any ideas?

Thank you for your answer

Yes I have already try to set the viscosity to fix the Reynolds of my initial field. But the problem is that in the final field the velocity profile changes, changing then the value of the Reynolds Number according to the case criteria.

If exist a possibility of modifying dynamically the viscosity instead the velocity field, I will also like to know it. Please.

The main intention of this thread is try to find a way to fix the Reynolds number in the periodic simulation.

Any ideas?

To be a nitpicker: There doesn't exist a Reynolds number for your geometry. Osborne Reynolds worked with tubes.

His law of similarity may be used for quite a lot (nearly all?) problems, of course. But you have to *define*, what the Reynolds-like number in your case should be. If the viscosity is constant, you need a characteristic length and a characteristic velocity for that. If the geometry is similar in mathematical sense you may select any of the length measures for analysis of changing.
As you mentioned, the selection of a characteristic velocity may be harder. I don't understand your problem in full extend, and don't know where and under which circumstances the velocity changes. Often used values are the free stream velocity o the inlet velocity at pipe and channel streams. You have to select on velocity which fits your model. It may be, that you "see" this velocity first after you finished your simulation. This is not a problem per se. The only flaw is that you don't have round values lik Re=1000 but have to live with something like Re=973 or Re=1059.

Sent from my GM 5 Plus d using CFD Online Forum mobile app

Hi

did you try the fvOption meanVelocityForce? There you can fix the mean value of the velocity of your flow.

Implementing cyclic (translational) boundary condition in OpenFOAM
 

There are two ways in which we can run translational periodic boundary condition cases. (Read this)

1. By fixing pressure gradient (mass flow rate will be varying in unsteady case)
2. By fixing mass flow rate (pressure gradient will be varying in unsteady case)

Second case represent constant Re case.
This can be implemented by using fvOption utility meanVelocityForce.
Please go through channel395 tutorial for more details regarding implemention of above mentioned method.

Hello Luttappy. Any idea how to fix pressure gradient instead of mass flow rate in a periodic boundary condition problem ?

Hi,


please check the semiImplicitSource



https://github.com/OpenFOAM/OpenFOAM...ImplicitSource


There, just use the explicit term for adding the pressure gradient, if I remember well>


U ( (dpdx dpdy dpdz) 0)


Please take a look to the sign of the gradient, otherwise your flow will be oriented in the other sense.

I will check that out. thanks for the quick reply.