sorry no idea

Of course you can. As matter of fact, I think all commercial software can solve it and it is a good example to validate the code. All you need is to define geometry, fluid property and boundary conditions.

Yes, definitely as explained by Mr Shiuh-Hwa Shyu.

However, i suggest using CFX instead of Fluent. Both of these comercial softwares are sold by ANSYS and both have their advantages and disadvantages. After using both, i will suggest using CFX. The biggest advantage of Fluent over CFX is the usage of memory when running a simulation. On the contrary, CFX provides much more flexibility, options to run your simulations though it is memory intensive as compared with Fluent.

All CFD softwares will require both inlet and outlet conditions. From the Navier-Stokes formulation, the better is always to provide velocity field in inlet section and pressure field at outlet.

Now, this is not always so easy to determine those conditions, depending on your case. The different softwares will thus provide ways to provide different inputs, and will arrange to get back to this velocity/pressure conditions situation.

Back to your question, I am not sure to fully understand your issue:

- if your point is to model a fully developped flow by providing velocity profile, then as answered before, any CFD code will do that. But it will recalculate the velocity profile along the duct: your inlet profile might (will?) not be maintained.

- if for some reason, you want at all cost to keep your velocity profile along the duct axis, this is possible through the use of UDF (user defined function) in Fluent - other codes provide an equivalent. You can write one that will override the Navier-Stokes calculation and simply propagate the velocity field. Why someone would want to do that is however beyond my understanding.

And a final point: the solution is not only the velocity field. Pressure, turbulence, energy are also important to consider.

Mr Shiuh, I think we need to give inlet and out let conditions both. But I am trying to solve the elliptic equation on one cross section,

Dear Mazhar, I believe you mean the velocity component for the "one cross section." The point is that they are found while you have a pressure field. The inlet & outlet conditions are for the pressure. When I said "elliptic", I mean the pressure is elliptic in nature. In fact, pressure at both walls should also be specified. You can set pressure at the two walls as zero gradient.

Mazhar Iqbal, have you tried periodic boundary conditions to get fully develop flow.

Besides UDF tool you can provide a profile (see profile tool) of your inlet velocity and an outlet pressure. It´s very dificult to simulate two phase flow once the interface solid-liquid need to be modeled too. It should be cited that the Fluent´s advanced tutorial was developed in this area.

2 possibilities: if your flow is hydrodynamically fully developped with small coupling with other scalar calculated (heat or mass transfer), you can impose everywhere in the domain the analytical solution and calculate only the scalar. If you have no analytical solution to impose the better is to calculate the flow under the pressure outlet BC. If the section you are interested in has large change in hydrodynamics and if the domain frontier exit is near from changes region, you should add a "virtual long tube domain" at the end of the real domain to calculate to be allowed to impose pressure outlet condition.

The term "fully developed" usually refers to a rectilinear flow, which by definition means that the velocity field does not depend on the flow coordinate (say z); and has a single component of velocity in the z direction. This velocity component (say u) can depend on time and the coordinates orthogonal to the flow direction ( say x, and y). Such a velocity field automatically satisfies the continuity equation ( for incompressible flow). When you substitute the velocity field into the steady Navier Stokes equations with constant viscosity), you will obtain a Poisson equation for the velocity field u. The RHS is the known pressure gradient which is a constant.

If your channel is a rectangular duct, then the only boundary conditions you need to satisfy are the no slip condition(u=0) on the channel walls. In most cases this problem can be solved analytically, but can also be solved with most software packages ( MatLab, Mathematica, Fluent etc). If the duct walls do not conform to an orthogonal coordinate system, then you should look at using boundary fitted coordinates. The boundary conditions are the same but now your simple Poisson equation is more complicated, but can be readily solved using say a spectral collocation method.

The key assumptions for rectilinear flow are: (i) that the channel cross section does not vary in the flow direction (ii) your are far away from entrances and exits, both of which can induce flow variations in the flow direction, e.g. the well known entrance effects, the length of which depends on the Reynolds number. Exits effects are less troublesome as information of the flow is typically "washed down stream". Nonetheless because the equations are elliptic there is always some exit effect (though small) .

Finally, if the pressure gradient is time periodic, then using the rectilinear flow assumption, you can derive a Helmholtz equation for the amplitude of the time periodic flow.

Of course any software will do.Since the flow is "parabolic" the only BC's you need are at inlet and at solid walls.You DO NOT need BC at outlet.If you specify one you have overspecified the problem with well-known consequences.

You could use a velocity profile at the inlet (with periodic condition type). In case of turbulent flow initial values for the turbulence model should be specified.

PHOENICS, for example, allows you to type PARAB=T and the parabolic mode(i.e. marching integration ) allows you Not to specify outlet BC, which is the ONLY correct practise.

Thanks Brian for detailed answer, but i am novice in Fluent, I have solved the same problem using MATLAB and it is giving me good results.

Yes, I have Poisson equation which is given in the attached fie. I am working in annuls sector.

Now when i try to simulate using Fluent it requires the driving factor like pressure gradient, temperature difference or inlet velocity be specified.

Dear Mazhar,

This is what I can suggest you as I have tried this myself and find it quite satisfactory.

Take the channel as it is and simulate it only for fluid flow condition (I mean no energy equation)

Take sufficient long length of the duct and let the flow converge to desired criterion (say 1e-5). Once done, import the velocity profile at outlet to a file. Now for solving your case with fully developed boundary condition, start a fresh case and give at inlet the velocity profile which you may imported during previous solution.

Hope this helps.

thanks Deewakar I will try

Dear Mazhar,

in CFX and Fluent a fully developed condition is implemented by setting at the inlet cross-section "Inlet static Pressure" +  Zero Gradient in flow direction and in Turbulence. However, I suppose that a fully developed flow can be modeled in another way. You could perform two different simulations. In the first simulation you select a constant streamwise velocity at the inlet section and a static pressure condition at the outlet cross section. When the first simulation ends you can extract the velocity profile estimated at the outlet section and use this velocity profile as inlet boundary condition of a second simulation. Hope it helps! Cheers

If using CFX:

1) Make your domain (duct dimensions for the lateral boundaries, with a few elements in the streamwise direction)

2) use "Translational periodicity" between the "inlet" and "outlet" of the domain.

3) Set wall boundary conditions on the lateral bounds

3) Setup initial conditions. (analytical velocity turbulence profiles) (not super important but a good initial guess will speed the computation)

4) Create a "subdomain" (your whole mesh)

5) In that subdomain, set a "general momentum source" (Sx) equal to the pressure gradient needed to maintain your flow. 

I wanted to maintain a certain average velocity so I used the following:

Sx= ( areaAve(u)@IN - TargetU ) * density / 1[m]

but you can also set a constant value for the pressure gradient. 

6) RUN to convergence (may take many iterations) 

This will give the "fully developed" velocity and turbulence profiles for the chosen pressure gradient. 

I hope this helps!

( The periodicity condition is essentially an automated way to do Deewakar's method)

Dear friends,

I'm doing 2D-axisymmetric vertical flow boiling simulation through a simple circular pipe in FLUENT. For this I have to apply fully developed turbulent velocity profile at the inlet. First I run the simulation for single phase and obtained the fully developed velocity profile at outlet. My question is how this fully developed velocity profile can be correctly applied at inlet in next simulation?

Hello Ram and friends,

Were you able to apply the fully developed profile at inlet on your next simulation. Could you please share how you achieve that? 

Thanks!