[escodonic]

I am doing a two phase flow simulation with VOF.
As an inlet BC I'm using the "variableHeightFlowRateInletVelocity".

As inputs OpenFoam requires the volumetric flow rate and the phase-fraction field.

When running some cases I can see that the water free surface elevation can change in time. I assume that if the height increases, the velocity should decrease, and always the volumetric flow rate is constant.

Somebody knows how that BC works? How OpenFoam makes the change of velocity and height in time?

Thanks

[CUnsworth]

Hello,
I would also like clarity on this question, and in addition how the lower and upper bounds work.
are they set heights(mm or m)? fractions of the inlet boundary scale? percentage? variation from initial conditions?
Chris.

[sharonyue]

Originally Posted by escodonic

I am doing a two phase flow simulation with VOF.
As an inlet BC I'm using the "variableHeightFlowRateInletVelocity".

As inputs OpenFoam requires the volumetric flow rate and the phase-fraction field.

When running some cases I can see that the water free surface elevation can change in time. I assume that if the height increases, the velocity should decrease, and always the volumetric flow rate is constant.

Somebody knows how that BC works? How OpenFoam makes the change of velocity and height in time?

Thanks

Hi,

here is the code:

scalarField alphap =
        patch().lookupPatchField<volScalarField, scalar>("alpha1");

    alphap = max(alphap, scalar(0));
    alphap = min(alphap, scalar(1));

    // a simpler way of doing this would be nice
    scalar avgU = -flowRate_/gSum(patch().magSf()*alphap);

    vectorField n(patch().nf());

    operator==(n*avgU*alphap);

where n is to make it a vector. And avgU is:


Then U in every patch cell will be:

[buesinaw]

If I understand correctly, together the variableHeightFlowRate boundary condition can be used in the "alpha.water" file and the variableHeightFlowRateInletVelocity boundary condition can be used in the "U" file to apply a volumetric flow rate to a boundary of a two-phase (air/water) open-channel flow problem. It appears that there's no control over how much of the specified volumetric flow is assigned to water and how much is assigned to air. In an open-channel flow problem the user typically wants to specify the volumetric flow rate of just the water, not the air. Can one use these boundary conditions to specify that the volumetric inflow is the volumetric inflow of water only?

[indy07cz]

Originally Posted by buesinaw

If I understand correctly, together the variableHeightFlowRate boundary condition can be used in the "alpha.water" file and the variableHeightFlowRateInletVelocity boundary condition can be used in the "U" file to apply a volumetric flow rate to a boundary of a two-phase (air/water) open-channel flow problem. It appears that there's no control over how much of the specified volumetric flow is assigned to water and how much is assigned to air. In an open-channel flow problem the user typically wants to specify the volumetric flow rate of just the water, not the air. Can one use these boundary conditions to specify that the volumetric inflow is the volumetric inflow of water only?

I used theese BC's for spillway study and it worked as you expect - volumetric inflow=volumetric inflow of water. Just check spillway in FOAM_tutorials. Or you can separate inlet into 2 parts: one for water and one for air and then use other BC's.

[hwangpo]

The variableHeightFlowRate boundary condition provides a phase fraction condition based on the local flow conditions, whereby the values are constrained to lay between user-specified upper and lower bounds. The behaviour is described by:
if alpha > upperBound:
- apply a fixed value condition, with a uniform level of the upper bound
if lower bound <= alpha <= upper bound: - apply a zero-gradient condition
if alpha < lowerBound:
- apply a fixed value condition, with a uniform level of the lower bound.
Thus, the lowerBound and upperBound should be given.

The variableHeightFlowRateInletVelocity boundary condition provides a velocity boundary condition for multiphase flow based on a user-specified volumetric flow rate.
The flow rate is made proportional to the phase fraction alpha at each face of the patch and alpha is ensured to be bound between 0 and 1. The flowRate and alpha terms should be provided.

Hope this helps.

[alfa.fauzi]

Hi everyone,


I have a question regarding an inlet angle when using variableHeightFlowRateInletVelocity BC for interFoam. Is there a way to setup an angle? I know that it is easy to setup an angle using velocity vector component within standard inlet BC e.g. using fixedValue uniform (Usin45 Ucos45 0) for an angle of 45 degree between x&y direction.



However I'm not sure how it works with variableHeightFlowRateInletVelocity although there is the vector component uniform (0 0 0). Is it only by changing the value inside the bracket?



As an example if I want a 45 degree between x & y direction, is it simply by writing the followings?



type variableHeightFlowRateInletVelocity;
flowRate 109.15; //(m3/s)
alpha alpha.water;
value uniform (109.15*sin45 109.15*cos45 0);



Hope someone answers my question. Thanks!


Regards,
Alfa

[indy07cz]

Hi, I'm not sure but I think that value here is just placeholder. Just try and you will see.

[Mahmoud Abbaszadeh]

Hi All,

I would like to use variableHeightFlowRateInletVelocity BC. In this scenario, we can define a constant flow discharge across the inlet boundary. I'm wondering if we can use a non-uniform flow discharge at the inlet boundary?

I tried to use the topoSetDict and set non-uniform values at the inlet. However, after a few time steps, the depth at the inlet increases to satisfy the fixed flow discharge. As a result, the non-uniform velocity will only affect a fraction of the initialized cellZone that was determined in the toposetDict.

Anyone has an idea how to deal with it?

Thanks in advance.