I apply CFX4.3 to study the pure buoyancy driven flow in steady state, such as fire-induced airflow in the tunnel. But it's very difficult to get convergence result in steady state, especially for those with free boundary at both side. It's alway no convergence or divergence. I learned from the manual that it could only be achieved from real time stepping to the steady states with quite huge calculation time. But I can directly obtain the result with another commerical software PHOENICS.

That means it's not the physical problem that cause divergence in steady state. Could anybody tell me why it's so difficult to get in CFX4.3 or there are some special commands on solution, (such as under-relaxation factors, methods for p-v linked equations, difference scheme) set up in CFX4.3 to get the convergence result??

Some hints and tips and additional questions:

- set the number of iterations of enthalpy and scalar equations to 2 or 3. Set the underrelaxationfactor for enthalpy equal to 1 (=no underrelaxation). I think you might require a fairly good converged enthalpy-field.

- set the underrelaxationfactor for the velocity component with the same direction as 'g' to a low value like 0.1 or something.

- what is a free boundary at both sides? A pressure boundary? Then, have you implemented rho*g*h as static pressure over the height of the boundary by using USRBCS?

- what makes you think it will converge to a steady state? If conditions are laminar, it will allmost be impossible to find a steady state. I have once found a steady state at laminar conditions by using an underrelaxationfactor of 0.001 for the velocity with the same direction as 'g'.

- How did you implement the driving force? Bousinesq approach? Fully compressible? Calculating the forces by using USRBF.

Regs, Gert-Jan

Thanks very much. I will try the number of iteration of enthalpy and under-relaxation factors for velocity.

The free boundary condition is the pressure boundary conditions. Because the equation has subtract the hydrodynamic prssure in the momentum equations. I think the value of pressure boundary should be set to zero. Why using rpo*g*h?

It's truly a turbulent flow and I have tried it with PHENOICS, the result is quite good.

I apply the Bousinesq approach to imply the driving force. For the velocity is quite small comapre with acoustic.

- If the first pressure boundary is located at 0 m, the second at 10 m and the fluid is air, then you should set the relative pressure at the first pressure boundary equal to approx. (10-0)*1*9.81 Pa. The pressure at the second pressure boundary should be set to 0.

- How large are the density differences? If it exceeds 10 % it is better to use fully compressible flow.

- More important. Have you set the reference temperature to a proper value?

Regs, Gert-Jan

I have implied the new pressure boundary conditions as you say. It seems works. But I still have wonder why the other commerical software PHOENICS could do the same simulation without considering the variation of pressure at boundary with height?

Nevertheless, thank you very much!

Well, I don't know Phoenics but I think that Phoenics does it automatically. Click Fluid Dynamics!

Regs, Gert-Jan

I am not sure that I know all the background of your problem, nor that I have read all the previous e-mails about it, but I can confirm that ( I am a Fluent user as well):

1/ I have always found PHOENICS to be a lot more convincing in terms of convergence for buoyancy driven flows (due to SIMPLEST? Conjugate Gradient solver on temperature? Pressure-correction equation accounting for density variation? False-time step relaxation on velocities? I do not know ...).

2/ If you are using the "density difference" model for gravity forces, the pressure specification at the outlet boundary condition should NOT reflect the difference in height, for this model uses a reduced pressure formulation. I don't think that this is a "unique-to-Phoenics device", it actually is the case for most CFD general purpose softwares.

In other words, you should set "0" regardingless the location of the boundary condition.

CFX uses reduced pressure too:

Real pressure = standard reference pressure + reduced pressure.

So, the standard reference pressure (default = 1.013e5 Pa) is subtracted from all real pressures, leaving the reduced pressure as the variable to solve. The static pressure (rho*g*h), is part of the reduced pressure. Thus to solve the case correctly, the static pressure should be specified at the pressure boundaries.

Am I wrong? Gert-Jan

I agree witht the opinion of Miler. i have tried this type of two-dimensional simulations with CFX4 and self-developed program. The result is quite good with the pressure boundary condition set to 0, But the grid system needed for CFX must be very fine. Also the maximum pressure difference caused by density different is only about 10 Pa. If the height of building is 10m and we consider the reduced pressure at the boundary, the pressure different along the height is about 100 Pa, which dominate the flow inside the building. The result is very unrealistic.

Sorry, you could be wrong (but it could be me, so...).

I think there is a confusion between "reduced pressure" (which is the one I was talking about) and "relative pressure" to which you seem to refer to.

a/ The latter, as you say, is Prelative. By definition,

Prelative=Preal-Pzero_of_reference.

"Pzero_of_reference" is a CONSTANT (important), and "usually" people sets it to 1.013E5 Pa, for lots of processes take place at atmospheric pressure.

Thus the solved-term "P" (or "P1" for PHOENICS users or "Pstat" for FLUENT users) represents only this relative contribution (=Prelative), with the benefit of working with small numbers for pressure.

Indeed, when the real pressure value is important, (for the calculation of an ideal-gas density for example) the different codes usually authomatically add "Pzero_of_reference" to "Prelative" (i.e again, P, P1, or Pstat depending on which software you are using) to obtain the real pressure. Otherwise, as the pressure only intervins as a pressure gradient, the value of the Pzero_of_reference is irrelevant..

b/ The former, i.e the "reduced pressure" is something different, though it can be "combined" with the concept described above.

By nature the concept of "reduced pressure" is bonded to the concept of "perturbation density": "rho_pert"="rho-rho_ref", where "rho_ref" is usually chosen as the ambient fluid density.

This practice leads to the introduction of the the following source term in the momentum equations: "(rho_rho_ref)*g" , instead of the "full" gravity term "rho*g".

Then, the place of the pressure in the momentum equation can be taken by a "perturbation" pressure, which is what I have called so far "reduced pressure":

p_pert=preduced=preal-p_ref

By analogy with the two buoyancy source terms above (the "reduced" and the "full" ones), it can be seen that the reference pressure p_ref is NOT A CONSTANT, and must satisfy the hydorstatic equilibrium equation:

grad(p_ref)- rho_ref*g=0 (or maybe "+" instead of "-", I 'll have to check).

So, to be brief, the variation is height is included" (and therefore "hidden") in the term "P_ref".

The height should NOT be included in the value of the solved-variable "P" (or "P1", etc ...) at an aperture boundary condition.

Well, at least this is my understanding. It may be wrong ...

Please confirm with the User Support Team of your respective software.

The small book all CFX users might have about the CFX-4.3 Solver entitled: 'Summary of commands and keywords' tells me that the pressure as specified at a pressure boundary is the static pressure by default (page 15)!?!

It puzzles me..... I will run several cases to see what the different options will do.

To be continued, Gert-Jan

The equations that are being solved, indeed indicate that pressure should be equal to zero. The test cases I have run, confirm this too. So, you were right. No question about that.

Gert-Jan