Author Topic: How do I specify Boundary Conditions correctly in CFX?  (Read 10504 times)

Offline pitney1

  • Jr. Member
  • **
  • Posts: 65
  • Reputation: +0/-0
  • Searching for solution
    • View Profile
How do I specify Boundary Conditions correctly in CFX?
« on: February 13, 2012, 09:16:26 PM »
I am new to CFX, how do I specify Boundary Conditions correctly?

Thank you.

Offline william

  • Full Member
  • ***
  • Posts: 159
  • Reputation: +15/-0
  • Know it, share it.
    • View Profile
Re: How do I specify Boundary Conditions correctly in CFX?
« Reply #1 on: February 13, 2012, 09:18:07 PM »
For a given computational domain, boundary conditions can be given that over-specify or under-specify the setup. This usually results in non-physical solutions or failure of the solution to converge. It is important, therefore, to understand the meaning of well-posed boundary conditions.

An example of an over-specified setup is a constant area duct, with a specified fluid velocity at the inlet, and a different velocity specified at the outlet. Clearly, both conditions cannot be physically satisfied in the absence of a mass source for an isochoric fluid.
An example of an under-specified setup is that of a closed box for which only heat flux boundary conditions were specified. In this case, the temperature level is not constrained and, while the solution may converge, the resultant temperature level would be unpredictable.

The best way to determine if the boundary conditions are well posed is to ask the question: Could the configuration I have set be physically recreated in a laboratory?. In the first example above, this is clearly not possible. In the second example, no matter how good the insulation of the boundary there would eventually be some heat flow from or into the environment that would serve to set the temperature level.

Recommended Configurations of Boundary Conditions:

The following combinations of boundary conditions are all valid configurations commonly used in CFX-5. They are listed from the most robust option to the least robust:

- Most Robust: Velocity/Mass Flow at an Inlet; Static Pressure at an Outlet. The Inlet total pressure is an implicit result of the prediction.
- Robust: Total Pressure at an Inlet; Velocity/Mass Flow at an Outlet. The static pressure at the Outlet and the velocity at the Inlet are part of the solution.
- Sensitive to Initial Guess: Total Pressure at an Inlet; Static Pressure at an Outlet. The system mass flow is part of the solution.
- Very Unreliable: Static Pressure at an Inlet; Static Pressure at anOutlet. This combination is not recommended, as the inlet total pressure level and the mass flow are both an implicit result of the prediction (the boundary condition combination is a very weak constraint on the system).
- Not Possible: Total Pressure cannot be specified at an Outlet. The total pressure boundary condition is unconditionally unstable when the fluid flows out of the domain where the total pressure is specified.With more than two inflows or outflows, the other openings should be of the boundary condition type Opening. This is because the flow at these other boundaries could in general be in or out, and the direction will be part of the solution.

Using Inlets, Outlets and Openings:

If at an Outlet Boundary Condition you see the CFX-Solver is trying to enforce outflow by erecting temporary walls on the boundary mesh faces to prevent inflow occurring (you will get a warning message in the output file), it may be due to a numerical problem or to a real phenomenon.

If you suspect that the problem is a numerical one and it persists, then you can overcome this by temporarily replacing the Inlet/Outlet boundary condition with a pressure specified Opening. Temporary walls are not erected with the Opening type boundary, as both inflow and outflow are allowed (although you may have to specify information that is used if the flow becomes locally inflow). Restart the solver, and once the solution is further converged, the original boundary condition can be restored.

If you suspect that a real phenomenon is causing the inflow, for example, a recirculation region near an Outlet, then two options are available to you:

- Move the Outlet to a region well away from this influence by, perhaps, extending the flow domain further downstream. A good rule of thumb is to place the boundary a distance downstream which is at least 10 times the height of the last obstacle.
- Alternatively, you may have reasons to want to maintain the location of that boundary, in which case you can use an Opening to describe subsonic flow where simultaneous inflow and outflow may occur. Generally, however, it should be noted that defining the boundary of your computational domain to cross a flow recirculation region is not a good idea. You are making a poor approximation of what is happening just outside the Opening by not modelling it.
« Last Edit: February 13, 2012, 09:22:48 PM by william »