Mixed convection means buoyancy-influenced convective flow and heat transfer

Since you are satisfying the conservation equations I don't see why you couldn't use a segregated scheme. But someone more knowledgeable may have something to say.

well, their manual also does not provide much detail, the only thing that i could gather from their manual is , cfx descetise equations for u, v,w, p same as segregated solver, but when it solves it solves them coupled, that is, put all the coefficients of u v w p in a single matrix and create megha matrix and solve it with AMG with ILU preconditioner. so in a way it little better segregated solver. (well i must say this is what i gathered from first glance on their manual and i might be wrong, someone who uses CFX can correct me).

and if this is correct then only this coupled solver can work well with incompressible flow (as the pressure decouples at mach goes to zero).

here is excerpt from CFX 5 Manualwhich only shows that the coupled solver ag is talking , CFX is not talking about it )

The linear set of equations that arise by applying the Finite Volume Method to all elements in the domain are discrete conservation equations. The system of equations can be written in the form:

sigma(a_i * phi_i) = b_i

where f is the solution, b the right hand side, a the coefficients of the equation, i is the identifying number of the finite volume or node in question, and nb means �g neighbour�h, but also includes the central coefficient multiplying the solution at the ith location. The node may have any number of such neighbours, so that the method is equally applicable to both structured and unstructured meshes. The set of these, for all finite volumes constitutes the whole linear equation system. For a scalar equation (e.g. enthalpy or turbulent kinetic energy), each ai nb, fnb and bi is a single number. For the coupled, 3D mass-momentum equation set they are a (4 x 4) matrix or a (4 x 1) vector, which can be expressed as:

[here MAtrix_an = a matrix made up all the coefficients of u,v,w,p]

It is at the equation level that the coupling in question is retained and at no point are any of the rows of the matrix treated any differently (e.g. different solution algorithms for momentum versus mass). The advantages of such a coupled treatment over a non-coupled or segregated approach are several: robustness, efficiency, generality and simplicity. These advantages all combine to make the coupled solver an extremely powerful feature of any CFD code. The principal drawback is the high storage needed for all the coefficients.

yes, as i gathered from fluent manual that they can solve it with segregated solver, but because of decoupling of flow and heat transfer equations they suggest to use coupled solver (so according to them choice is users what he wants to use).

I'm CFX user but I'm not strong in the background theories. Just a question.... Is coupled solver referred to the way we solve u,v,w,p numerically? ie. whether the equations are solved in one lots or step-by-step (I'm too lazy to find the right term but you know what I mean if you come across the steps in segregated approach)

I don't think there should be any difference on how the equation is being discretized in these two approaches... again not sure about this. Maybe someone can tell us more.......... I'm dealing with incompressible flow most of time (thanks god..) and so not sure about the compressible one.....

On the way, CFX only solve u,v,w,p coupledly but not the energy & turbulence equations..... So... Can I say it's "not a fully coupled solver"? I read somewhereelse saying that there's not much advantage to include the energy & turbulence equations in the coupled solver.......

Okay....You're talking about the problem of coupled solver for compressible flow, aren't you? I don't have much experience with it.... so not sure about this.

CFX doesn't include energy equation in the coupled solver....I think.....but they still say it's more robust and better than the segregated aprroach... So are you sure it has no advantage at all to use coupled solver in incompressible, isothermal flow?

Hope we're talking about the same subject here..... ha..... I'm a bit confused right now....

yes, solving them together is what we meant by coupled, but then the approach could be different. the way fluent decretise equations for coupled solver is very different from CFX (i have just glanced into cfx5.5 so i might be wrong), but the way fluent descretise the equations , fluent is bound to get into trouble when it goes to incompressibel flow.

this is what fluent manual says: {

The Navier-Stokes equations as expressed in Equation 26.4-1 become (numerically) very stiff at low Mach number due to the disparity between the fluid velocity and the acoustic speed (speed of sound). This is also true for incompressible flows, regardless of the fluid velocity, because acoustic waves travel infinitely fast in an incompressible fluid (speed of sound is infinite). The numerical stiffness of the equations under these conditions results in poor convergence rates. This difficulty is overcome in FLUENT's coupled solver by employing a technique called (time-derivative) preconditioning [ 371].

}

so it is clear that they acknowledge the problem mentioned by ag.

difference due to descretisation could be important, but that depends upon cases to cases, and not always true. (its really difficult to tell much about cfx since they do not tell it in much detail and underlying confusion remains)

well as CFX boasts about it, according to them their coupled solver is always better than any segregated solver. And i mostly agree with this part that coupled approach is better than segregated approach if can be used.

the only thing i was mentioning is when memory is an issue, one has to go to segregated solver, i mean for the cases where i have difficulty in running with segregated due to memory, i think thinking of coupled solver in those places is foolish thing. and when cases are smaller, one can use coupled solvers without any prob,

With velocity and pressure as your primitive variables, momentum and mass do not decouple. Also, for rotating cases, the velocity components themselves are coupled together.

Regarding memory, in principle coupled solvers do require more memory than segregated ones. But comparing with segregated solvers depends on how carefully memory is managed by a particular solver. For example, CFX is routinely used on cases with tens of millions of elements despite having a coupled solver.

How do you keep the continuity equation from becoming a simple divergence-free constraint in the limit of zero Mach number? Even if the continuity equation is written in terms of pressure the time derivative will still vanish in the incompressible limit unless some form of artificial compressibility is invoked, which is simply another form of preconditioning. Is there another way tie the equations together aside from preconditioning or utilizing a segregated scheme with a correction procedure? If there is I would love to get details on it.

About memory:

this is what CFX says {

Memory Usage

The CFX solver provides high memory efficiency. One million unstructured tetrahedral mesh element problems can be run in 400 MB RAM. The software intelligently uses the memory available in order to dynamically optimize the balance of resource usage against computational speed.

}

which makes sense, since 10 million floats take about 40 mb memory, and for each cell we roughly allocate around 50 floats. so by this simple math, for 1 million cells we have around 50 million floats to allocate, that is we need 5 x 40 mb memory = 400 mb roughly. and that is what CFX says. well so on a 3 gb ram machine, if we leave some ram for other processes we can roughly go till 6million cell case. (but ideal conditions do not come and i guess with CFX max size that you can run is around 4 million on a 3gb machine).

so if it comes to run tens of millions of cells as a case with normal machine you CAN NOT do, because, i think CFX says we use memory wisely , 'NOT create memory'. in nut shell, i don't find anything great in it. (so when you run tens of millions of cells, you use parallel machine, and so do other softwares).

ohh i made a simple mistake , i wrote:

5 x 40 mb memory = 400 mb,

instead of writing

5 x 40 mb memory = 200 mb

(and include the variables for faces after this, so total will be roughly 300mb).

For your info..... I've solved an incompressible flow problem with more than 6 million tet mesh in CFX before.... Takes a few GB of rams if I remember correctly....The solution doesn't converge if compared with coarse mesh though....... this is another issue but what I want to say is that CFX can certainly handle millions of cells...

well you din't mention how many GB of ram, and second thing about CFX can handle millions of cells, if it couldn't, they would not in business.

This depends on your control volume layout. I believe that Vanka used a coupled line solver for staggered meshes; I don't recall the reference but it was late 70's or early 80's. With a colocated grid, the continuity equation is modified by adding a pressure dissipation term to avoid checkerboarding (eg, Rhie-Chow); this introduces a kind of diffusion term on pressure into the continuity equation. Another option might be to replace continuity with the 'Pressure Poisson' equation, but I'm not personally aware of any work which has combined this with a coupled solver.

ag,

Be careful of categorising things in terms of what variables are being solved for and solution strategy (segregated vs. implict say), these are two mutually exclusive choices. You are correct though that if you solve for density, you are screwed in the incompressible limit.

CFX does not use pre-conditioning as you know it. It solves for u,v,w and p all at once. One matrix and RHS go into the linear solver, the solution corrections for u,v,w and p come out.

Mass and momentum equations are coupled using Rhie-Chow. Basically an artifical term is added to the continuity equation which behaves like a 4th order derivative on pressure with a coefficient in front of it that scales with 1/dx^3. There is a paper on this from the early 80s.

The coupled-implicit strategy in the CFX solver (TASCflow and CFX-5) was developed during the early/mid-80s at the University of Waterloo, Canada. Check for papers by Micheal Raw, George Raithby, Brad Hutchinson, Paul Galpin.

Neale.

I don't believe your statements about memory usage.

When you say memory is an issue with coupled vs. segregated what exactly are you comparing?? In some highly theoretical la la world coupled should use more than segregated. However, humans make many mistakes when typing in source code for a solver so whether this statement is true in the real world depends on who implemented the solvers.

Perhaps your coupled solver is poorly implemented?

Neale.

hi Neale, i think you will agree on one thing that any solver can not create memory on machine. So lets fix this fact first ( some cfx users seems to forget this).

now, lets fix another thing, that coupled solvers usually takes more memory than segregated solver ( even if we take CFX approach that is, put all the coefficients of u v w and p in one matrix, as you also mentioned, you are allocating 4 times a matrix than one matrix of segregated solver). So i think you will agree on this part too. ( that is a segregated CFX would take less memory than coupled CFX).

Now if i fix this two things, then all i said is thinking of coupled solver is impossible where i am finding running a segregated solver difficult due to memory.

read again what i wrote :

"the only thing i was mentioning is when memory is an issue, one has to go to segregated solver, i mean for the cases where i have difficulty in running with segregated due to memory, i think thinking of coupled solver in those places is foolish thing. and when cases are smaller, one can use coupled solvers without any prob,"

in the end , it really does not matter whether you agree with me or not, by using CFX you can not create memory ( u will use what is given to u) , its a fact.

You are assuming that anyone implementing a coupled solver also knows how to properly implement sparse matrix data structures. That is not always the case.

Hence, it is still possible that eventhough someone implements a segregated solver they still end up storing a bunch of zero values they don't need, which will still use more memory than a coupled solver.

There are other issues as well because the matrix is not the only storage you need (you need geometry, properties, derived variables, etc....). You have assumed that the matrix is the limiting factor. That is not always the case. Poor memory managment in the non-linear solve portion of a code can be really limiting.

Neale.