Periodic Boundary Conditions
 

Hi all, I am new to fluent and this forum, so please pardon me if i am asking something too simple and straight forward.

I am investigating flow characteristics through a pipe of a certain repeated geometry and hence the use of the periodic boundary condition.

Since i am dealing with laminar, incompressible flow, I only specified the inlet mass flow rate and the temperature.

One parameter of interest is the pressure drop across this small part of the whole configuration.

After solving for 10000 iterations, the pressure at the outlet is the same as that of the inlet.

I am clueless as to why this is so.

Are the periodic boundaries applied axially or radially? What outlet condition have you used? Pressure outlet or outflow?

Tranlational (axial) periodic conditions were used. Correct me if i am wrong, with mass flow rate bring specified, the boundary condition specified is velocity inlet right? Pressure based solver used.

You cannot use translational periodics along the length of the pipe. If the pipe is long and straight and has periodicity radially then I would suggest to use rotational periodics to reduce the cell count and define an inlet and outlet. In this way you will be able to detect a pressure loss along its length.

Isn't rotational periodics for propellers? The repetition is along the length of the pipe, and hence the choice to use translational periodic conditions. I'm sorry, confused here.

A pipe isn't translational-periodic, because you are always dealing with flow development effects at the enterance. (also, if it was, completely translationally periodic, what would be the point of simulating?)

A pipe is rotational periodic, around the central axis. If the pipe is smooth, you can even model it as a 2-d axisymmetric geometry.

I have nothing more to add to the reply of CeesH. It is spot on.

Firstly, thank you very much for all your replies.

but hmm... i think that you guys may has misunderstood what i was trying to model.

the pipe i am trying to analyse has a sine wave like geometry, with 12 periods in the streamwise direction (direction of flow).

as the developing region is small, it can be assumed that fully developed flow will be observed in most of the the length of the pipe.

hence, instead of meshing 12 sine waves, i just want to model 1 wave with translational periodic boundary conditions.

periodic zone (inlet)
shadow zone (outlet)

what i wish to do is to check the pressure drop for 1 wave and try to extrapolate the information for the entire length.

however, after determining the mass flow rate, i get the ave pressure on the inlet = pressure on the outlet.

laminar flow, pressure based solver.

this should not be the case as there should be some pressure drop in 1 wave, and for 12 waves, the pressure drop should be 12 times more.

for the entire array of 70 channels, it should be approximately be 70 x 12 x delta P for 1 wave.

That is my understanding.

The strange thing is that when i started with a coarse grid, there is pressure drop observed. as i refined the grid, it disappeared some how. with that, there is no way i can do my grid convergence test.

You cannot use translational periodics for this problem. Even with translational periodics then for your problem you still need a defined inlet and a defined outlet as well as the translation periodic boundaries. You will have to model the 12 waves. However if the waves are in one plane then you could split the model in half and have a symmetry plane. This will reduce the cell count.

Hi!
In my opinion this is true from a geometrical point of view, but there could be secondary flows inside the pipe, which can determine pressure drop: I think you'd better to simulate the whole geometry.

noted with great thanks.

will investigate further.

I don't see why this would not work. Maybe I don't get you right. Can you post a small picture of the "1-sine" domain, with some captions?

Yes, it is possible to simulate a translational periodic bc; you need to specify the mass flow across the periodic boundary (which is a known value in this case) and a "first guess" for pressure gradient.
The translational periodic is valid only for fully developed flow: if this is the case then it can be simulated.

Yes, that's what I think, too. And since his approximation is:
"as the developing region is small, it can be assumed that fully developed flow will be observed in most of the the length of the pipe."
this is a valid approach...

Thank you all once again for your replies.

It seems that there isnt a problem with the assumption which i have made, rather i think that the problem lies with the possibility that my result may not have converged.

I have attached images of the stream lines and the plots of the residuals of 2 different grid resolution.

High resolution is about 8x that of the low res one.

https://www.dropbox.com/sh/pgdjf1ivi...WnZpguz7a?dl=0
for the high resolution one, the mass flow rate at the outlet does not match the one which i have specified in the boundary condition.

any suggestions as to how i could reduce the iteration count?

Hey CZL, why the energy equation? If the temperatur changes along the pipe, there is no way this can be periodic. Or am I wrong?

Some thoughts on the statements in this thread:

1) Translational periodic boundary conditions can be used even for straight pipe flows
This simply implies that the flow is fully-developed, an assumption that may be valid at least for some part of the geometry we are dealing with here.
And of course we have to assume that the fluid we are dealing with is incompressible.

2) Fluent is able to deal with temperature variations even for straight pipes with translational periodic boundary conditions applied. The temperature is rescaled at the "inlet" based on the temperature value you provide at the periodic interface. Again, this only works with constant-density fluids.
Basically the same procedure as with a pressure gradient along a translational periodic flow.
Periodic flow with heat transfer is even one of the basic tutorials for Fluent.

Since the energy equation does not seem to converge very well in your cases, try decreasing the under-relaxation factor for this equation (->Solution controls)
The other equations seem to converge perfectly at least on the coarse grid.
If convergence is too slow on the finer grid, try interpolating the solution from the coarse grid as an initial condition for the fine grid. (File -> Interpolate)

thanks for the inputs!

will try to do as suggested.

I used energy equation to track how this passive geometry is better in terms of transferring heat rather that the straight case as the curvature kind of induces fluid mixing, enhancing heat transfer.

That means that the absolute values of the solution is not of concern, rather delta T will be taken note of.

My understanding is that if delta T is better than the conventional straight geometry, it will definitely also be better in the developing region due to the flow profile and hence, this be concluded to be overall more efficient...

does it sound logical? i mean is this method applicable?

Sounds reasonable.
But keep in mind that the curved geometry not only enhances heat transfer compared to a straight channel, it also increases pressure loss and might be quite difficult to manufacture.
So if pressure loss is a relevant factor check that your method is better than simply a longer straight channel.

Thanks flotus, good to know.