Outflow condition CfX-Fluent
 

Hi All ;
till now no response about the equivalent of outflow condition to setup a BC in CFX Pre witch means ( a zero first derivative of all variables flow ). this conditition is used in fluent.

this is the post of a CFD user .

I'm moving from Fluent to CFX. There is this boundary condition in Fluent named outfow where the solver sets the normal derivative of flow variables to zero for that boundary edge. How is it possible to use this boundary condition in CFX. As far as I've understood there is only INLET, OUTLET, OPENING, WALL and SYMMETRY boundary conditions in CFX. Any help is really appreciated.

many thanks.

Incompressible or compressible flow? If compressible, sub-sonic or supersonic?

incompressible and sub-sonic flow.

The outlet in CFX is similar. It can be set up to use zero gradient on all parameters except pressure which needs to be defined.

how can I set up CFX outlet to use a zero gradient on all parameters ?
more details please.

That is a symmetry plane.

You have to define at least one parameter at an outlet.

Dr. Horrocks,

I'm a little confused by your statement here regarding a symmetry plane BC in CFX. I don't see how it could be used as an outlet BC since it requires zero normal velocity at the symmetry plane in addition to zero normal gradients of all variables.

It is my understanding that, in Fluent, you can specify a "outflow" boundary condition which specifies a zero diffusion flux for all flow variables along with an overall mass balance correction. From the Fluent User's Guide, Section 7.3.2: The CFX documentation I have read does not seem to address how this could be implimented. Do you have any insight that you could share?

I'll add that this question also relates to a previous topic:

http://www.cfd-online.com/Forums/cfx...w-b-c-cfx.html

This issue is that, when modeling pipe flow, I often don't know the pressure. How is it possible to specify a velocity or mass flow rate at the inlet along with zero gradients in all variables at the outlet?

The comment was "zero gradient on all parameters". That is a symmetry plane, but I guess the symmetry plane has the additional constraint of no flow normal to it. I guess a bit cheeky of me to change the subject like that but the question was not very specific.

No, you need to specify pressure at the outlet in your case. But for incompressible flows the pressure is relative anyway, so the outlet just becomes a reference pressure. You obviously need to be more careful in compressible flows.

Dear All
What is the best outlet boundary condition for transonic(subsonic inlet and outlet but transonic passage) compressor and in general transonic turbomachines? why?
I would like to have specified inlet mass flow rate. I use total pressure(because of more stable and better convergence behavior than inlet mass flow rate) at inlet but by applying static pressure at outlet, desired mass flow rate is not be obtained.

For a multiphase-phase change (condensation) flow (compressible flow) inside a tube, I know pressure, temperature and mass flow rate (initially all gas) at inlet only.
What should I use as an outlet boundary condition?

P.S I have experimentally determined pressure drop too.

Then you know the exit pressure, so use that for the exit pressure boundary and see if the simulation gets the correct pressure drop as a validation of the simulation.

I would like to explain my case with you.

I have a multiphase (liquid water-vapor) fluid flow through a tube.
The inlet conditions are 3.02MPa, 0.210Kg/s @ 240.47K (saturated vapor).

The tube outer surface is surrounded by 100C water at 1 atm (saturated liquid water) which I am not simulating for now. I simply put the tube wall temperature and the solid domain to be isothermal @ 100C.

The outlet conditions of the tube are actually required part of solution. But I have the experimental pressure drop across the tube to be of magnitude 7.25KPa.


I am trying to transient simulate the condensation of the flow using CFX and IAPWS water database. (water liq. and water vap. are defined for appropriate range along with their homogenous mxtr.)

Tube fluid domain reference pressure is put as 3.02MPa.
Now, my question is, should I use pressure inlet with 0MPa static relative pressure and pressure outlet with -7.25KPa static relative pressure?
Domain will be initialized with 0MPa relative static pressure.

If so, how can I validate the pressure drop if I am supplying the same information to CFX by myself? Also, how will CFX know about the mass flow rate information available for inlet?

Thank You in advance for you guidance.

Sorry, I did not explain fully. Use a mass flow rate boundary for your inlet and a pressure boundary for your outlet. Then the pressure drop can be compared against your experimental results as a validation.

Thank You for your response.

But can you please comment on pressure initialization in the flow domain?

If I initialize the domain with static relative pressure 0MPa (reference pressure already set as 3.02MPa), am I fixing the pressure drop making the problem over-constraint?

Your experiment has the inlet pressure 3.02MPa so your outlet is about 3.013MPa.

If you use 3.02MPa as the reference pressure then your outlet pressure boundary should be -7.25kPa and your inlet mass flow rate should be 0.210kg/s @ 240.47K (saturated vapor). Using 0Pa everywhere as your initial condition would make sense.

No this is not over constraining the pressure. From your initial guess the inlet pressure will vary until it reaches the inlet pressure it predicts from the flow rate you specify. If your simulation is accurate the inlet pressure (relative) should be 0Pa. But any simulation error or inaccuracy will result in that inlet pressure deviating from 0Pa, so it is not over constrained.

Thank You for your response

So do you mean that the inlet pressure will adjust itself (starting from initial guess) throughout the transient simulation time until I stop the simulation (as soon as required pressure drop is achieved)?

If I put the guess value exactly equal to the required pressure drop, then I am getting error just after 1st iteration (momentum terms are crazy (of the order of 10^19)).

What do you think, should I use little higher or lower guess value than real (3.02MPa abs i.e. 0MPa relative) pressure?

The initial condition is just that, it is just an initial condition. The solver will then adjust the variables available to what it thinks will happen.

Small changes in the initial conditions sometimes have an affect on the result. Fluid mechanics is full of examples where small changes in initial conditions makes big changes in the resulting flow field - look at the butterfly effect, turbulence, chaos theory etc.

If your momentum terms are so large then you are having problems with numerical stability. See the FAQ which discusses numerical stability for convergence problems: https://www.cfd-online.com/Wiki/Ansy...gence_criteria