Hi,

I am trying to solve for an additional variable that obeys a poissons equation using CFX-11. CFX couples this equation to that of momentum and continuity. Is there a way to solve this variable after solving momentum and continuity, essentially de-coupling this variable.

Anil

In the expert parameters, set

"solve additional variable = f" "solve fluids = t" "solve turbulence = t" "solve energy = t"

the solver will not solve your AV equation but will continue solving for the rest. When you run is complete, either edit the .res file using the def editor in Solver Manager or write a new .def file with the flag set to "solve additional variable = t" and set the others to 'f', then restart the analysis to solve your AV equation.

-CycLone

Dear Anil,

Are you concerned with the solution, or with the "performance"/speed? The solution will be the same in any case.

Unfortunately, there is not mechanism (exposed to the user) to move a particular equation set to the solver post-processing stage (like NOx modeling does). A workaround (for steady state though) is to run the case w/o the AV and later restart the solution with the AV.

Hope this helps, Opaque

Hi Guys,

Thanks for your responses. The momentum and continuity equations provide BC for the poissons equation. So what I want to do is: time =t Step 1: Solve for momentum and continuity. Step 2: Use the velocity and solve the poissons equation Step 3: time = t +dt

Anil

What are solving for with the Poisson equation?

The poissons equation solves for a scalar variable (instantaneous pressure) generated by a moving boundary. The velocity from the momentum equation generates the velocity of the boundary, this is followed by solving for the instantaenous pressure, kind of like a pressure wave equation.

Your idea of changing the expert parameters could be used as: (1) Turn scalar variable =f and solve for velocity and pressure. (2) Change this parameter=t in the next time step and turn off velocity and pressure. repeat this cycle.

So the physical time = 0.5* CFX time.

Anil

Dear Anil,

For transient simulations, I think you have no choice but to solve the equation with the defaults settings.

There is nothing wrong with the solution, except for the extra effort of solving for every coefficient loop. However, solving the Poisson (though you said is a wave equation, not Poisson) after the Cont+Mom equations are converged still requires several coefficient loops for the AV equation since it will not be solved in 1 iteration.

The workaround explained by "Mr. Cyclone" works well for steady runs, but it is not trivial for transient simulations.

Please contact your help representative, and place a request for additional solution controls such as this one.

Opaque

Hi Anil,

If you are moving the boundary, there is no need to do this. CFX will solve for the pressure wave caused by the boundary motion. If the fluid is incompressible, this will tranlate into an instantaneous change in pressure. If the fluid is compressilbe and the timestep is large you'll have a similar effect and if the timestep is small, you'll see the wave propegate.

-CycLone

Hi Opaque and Cyclone,

I would look into the reccomendations you guys have made and post my findings later today.

Thanks once again for your guidance

Anil