CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (http://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   flowRateInletVelocity (http://www.cfd-online.com/Forums/openfoam-pre-processing/97966-flowrateinletvelocity.html)

samiam1000 February 29, 2012 09:58

flowRateInletVelocity
 
Dear All,

I am trying to use the flowRateInletVelocity BC. There is something that I can not understand: what does the `value' field mean?

The code looks like this:
Code:

inlet
{
type        flowRateInletVelocity;
flowRate    0.2;        // Volumetric/mass flow rate [m3/s or kg/s]
value      uniform (0 0 0); // placeholder
}

And what about the value (0 0 0)? What does placeholder stand for?

Thanks,

Samuele

romant March 1, 2012 02:27

Quote:

Originally Posted by samiam1000 (Post 346914)
Dear All,

I am trying to use the flowRateInletVelocity BC. There is something that I can not understand: what does the `value' field mean?

The code looks like this:
Code:

inlet
{
type        flowRateInletVelocity;
flowRate    0.2;        // Volumetric/mass flow rate [m3/s or kg/s]
value      uniform (0 0 0); // placeholder
}

And what about the value (0 0 0)? What does placeholder stand for?

Thanks,

Samuele

The value field is a part of every boundary condition, since they derive from the same basic boundary condition. placeholder means just that. you need it in order for OF to use the boundary condition, but it doesn't really matter what you set it to.

samiam1000 March 1, 2012 02:42

Thanks for ansering.

I have a doubt: isn't that right that those values are the component of the u vector that is used if we have a revers-flux through that surface?

Thanks a lot,

Samuele

romant March 1, 2012 02:46

Quote:

Originally Posted by samiam1000 (Post 347018)
Thanks for ansering.

I have a doubt: isn't that right that those values are the component of the u vector that is used if we have a revers-flux through that surface?

Thanks a lot,

Samuele


In the source code it doesn't say anything about that and it gives that the flux is always normal and inwards from the patch.

Code:

Description
    Describes a volumetric/mass flow normal vector boundary condition by its
    magnitude as an integral over its area.

    The basis of the patch (volumetric or mass) is determined by the
    dimensions of the flux, phi.
    The current density is used to correct the velocity when applying the
    mass basis.

    Example of the boundary condition specification:
    \verbatim
    inlet
    {
        type        flowRateInletVelocity;
        flowRate    0.2;        // Volumetric/mass flow rate [m3/s or kg/s]
        value      uniform (0 0 0); // placeholder
    }
    \endverbatim

Note
    - The value is positive inwards
    - May not work correctly for transonic inlets
    - Strange behaviour with potentialFoam since the U equation is not solved


samiam1000 March 1, 2012 03:03

Dear Roman,

pardon the huge number of messages I am writing, but I would like to better und this point.

I many read the code many times. There's a point that I can not understand: why should we specify something that does not have any effects on our simulation?

Could you try to explain this?

Sorry if I am teasing you. I am just to try to und.

Have a good day,

Samuele

romant March 1, 2012 03:08

Quote:

Originally Posted by samiam1000 (Post 347021)
Dear Roman,

pardon the huge number of messages I am writing, but I would like to better und this point.

I many read the code many times. There's a point that I can not understand: why should we specify something that does not have any effects on our simulation?

Could you try to explain this?

Sorry if I am teasing you. I am just to try to und.

Have a good day,

Samuele


Hej,

OpenFOAM is based on C++ where new classes and libraries, such as boundary conditions can be derived from previous ones, which also means that they take input parameters and internal values with them. In this case this means that the new class flowRateInletVelocity, which is based on fixedValueFvPatchVectorField, also inherited the value component.

This in turn means that the value variable is part of flowRateInletVelocity and therefore must be specified, otherwise the class is missing an input, even though the variable is never used. Just try it without the variable and you will notice that it won't run.

samiam1000 March 1, 2012 03:12

Thanks Roman,

thank you very much.

I perfectly understand what you mean. And I completely agree with you. I haven't thought about that.

By the way - though I am afraid I am going off topic - is there `a point' in which I am asked to insert the value of velocity that are used just in case of a reverse flow somewhere?

Thanks again,

Samuele

anon_a March 1, 2012 03:53

I think that the "value" field is also needed because it's read by paraview.
At least I think that paraview crashes if I delete that field.
In the beginning it does not make a lot of sense I guess.

Ahmed Khattab March 4, 2012 13:58

where could i find such this file for all cases?
 
Quote:

Originally Posted by romant (Post 347020)
In the source code it doesn't say anything about that and it gives that the flux is always normal and inwards from the patch.

Code:

Description
    Describes a volumetric/mass flow normal vector boundary condition by its
    magnitude as an integral over its area.

    The basis of the patch (volumetric or mass) is determined by the
    dimensions of the flux, phi.
    The current density is used to correct the velocity when applying the
    mass basis.

    Example of the boundary condition specification:
    \verbatim
    inlet
    {
        type        flowRateInletVelocity;
        flowRate    0.2;        // Volumetric/mass flow rate [m3/s or kg/s]
        value      uniform (0 0 0); // placeholder
    }
    \endverbatim

Note
    - The value is positive inwards
    - May not work correctly for transonic inlets
    - Strange behaviour with potentialFoam since the U equation is not solved


please roman could you tell me the directory where this file exists?

romant March 5, 2012 01:41

Quote:

Originally Posted by rebel ahmed (Post 347580)
please roman could you tell me the directory where this file exists?

You can find it under $FOAM_SRC/finiteVolume/fields/fvPatchFields/derived/flowRateInletVelocity/flowRateInletVelocityFvPatchVectorField.H



Ahmed Khattab March 5, 2012 10:11

thanks roman for your swift reply

Ahmed Khattab March 5, 2012 10:11

solvers
 
roman,
i searched for discription for another type, slip type but this is the only description available. is there is moer detailed description.

Description
Foam::slipFvPatchField

is this available discription for solvers also?, if yes where?

ntchuyen August 13, 2013 04:42

Dear all guys,

I used the type flowRateInletVelocity in my case for the velocity field at the inlet. The solver ran well. However this error occured when I open the paraView.

"--> FOAM FATAL IO ERROR:
Please supply either 'volumetricFlowRate' or 'massFlowRate' and 'rho'"

I've used OpenFOAM version 2.1.1.

Can you instruct me to repair it?

Best regard.


All times are GMT -4. The time now is 09:29.