[dasith0001]

Hi Foamers,

I am trying to simulate an effect of fan, and I am using ''accelerationSource'' fvModel. I am using OpenFoam10

The fvModel works fine if I include 'halfCosineRamp' but I cannot see any changes to velocity field when I change it to ''constant''.

I am assuming the fan would exert a constant acceleration to the fluid. Would you take a look into the file ?

PHP Code:

accelerationSource1
{
    type            accelerationSource;

    selectionMode   cellZone;
    cellZone        rotor;

    U               U;

    velocity        scale;            //constant; //uniform;
    value           (0 0 10);

 
    scale
    {
        type         constant;     //one;  //halfCosineRamp;  //constant; 
                                      //halfCosineRamp; uniform constant
        value        1;
        
        //start           0;
        //duration        100;
    }
} 


Also, is this the 'right' fvModel to simulated the 'effect of the fan' ?

Thank you
Dasith

[JNSN]

Hi Dasith,


the accelerationSource does not have any effect when using constant as scaling function. Having a look at the code you can see, that the acceleration is calculated by the difference of velocity between the time steps:

const vector dU =
        velocity_->value(mesh().time().timeToUserTime(t))
      - velocity_->value(mesh().time().timeToUserTime(t - dt));
 const vector a = dU/mesh().time().deltaTValue();

which gives zero acceleration for a constant scale.

I suggest you have a look at the actuationDiskSource in order to model the effect of a fan.

Best,
Jan

[dasith0001]

Hi Jan,

Thank you very much for the response.

ok, it makes sense now.

Hmm, I've been looking into actuationDiskSource as well, but is it not something to be use for a turbine, where the rotor is driven by wind? fan, is other way around.

PHP Code:

rotor
{
    type            actuationDiskSource;
    active          on;
    selectionMode   cellZone;
    cellZone        rotor;

    actuationDiskSourceCoeffs
    {

    selectionMode   cellZone;
    cellZone        rotor;

        fields          (U);        // names of fields to apply source
        diskDir         (0 0 1);   // disk direction
        Cp              0.9;        // power coefficient
        Ct              0.9;        // thrust coefficient
        diskArea        0.00001;        // disk area
        upstreamPoint   (0.65 0 1.82);    // upstream point
    }
} 


There is thread on this, but that either do not explain much,
Basic use of actuationDiskSource

And this'' Changing rotorDiskSource from source to sink '' also suggest actuationDisk might behave as a turbine.

'rotorDisk' might be my only option?

It is very hard to find any explanations/clarity of on OpenFOAM fvModels/fvOptions in general, whilst those remains very important. I would really appreciate if anyone could shred more light

Thank you
Dasith

[JNSN]

Hi, I have never used the OpenFOAM Implementation. But for my understanding the actuationDisk acts Like a driven Propeller, e.g. behind a ship. That means the flow is accelerated die to the implied thrust of the Rotor.