[Carno]

Hi Friends,

I want to give pressure jump in OF with respect to flow rate. This is basically fan curve (Pr. vs Q) which I want to enter. Based on the system resistance the flow rate through the fan will be set.

When I try to do that through cyclic BC, it takes table only wrt to time not in terms of velocity or flow. This is quite possible in other commercial tools.

Is there any workaround on this? Please help.

Thnaks
Carno

[tomf]

Hi,

You need to use the "fan" boundary in your pressure file:

    Fan_master
    {
        type            fan;
        patchType       cyclic;
        jumpTable       table   
        (// PressureJump vs mean velocity format: ( "mean velocity" "pressure jump")
            (  1   250)    
            ( 2   200 )   
            ( 4  150 )  
            ( 6.5   100 )  
            ( 7.5   50 )   
            ( 8  0.01 )                                                                   
        );
        outOfBounds clamp;
        value           $internalField;
    }
    Fan_slave
    {
        type            fan;
        patchType       cyclic;
        value           $internalField;
    }

Fan direction is in the normal direction of the master patch.
Cheers,
Tom

[Carno]

Thanks Tom,

I will check that.
But in that, how Openfoam will know that the table is of velocity vs deltaP?

Thanks Again...

Best regards,
Carno

[tomf]

Hi,

Check the source code of the fan boundary condition.

Regards,
Tom

[Carno]

Originally Posted by tomf

Hi,

Check the source code of the fan boundary condition.

Regards,
Tom

Thanks for the reply Tom. I will look into the code as suggested.
I apologize for asking again. Why did you comment the line

// PressureJump vs mean velocity format: ( "mean velocity" "pressure jump")

Thanks again

[tomf]

Hi Carno

I did it just to give you this hint. I originally did it for myself.
It was not meant to give you confusion, to the contrary actually.

Regards,
Tom

[Carno]

My Problem is solved thanks.
Now I have different question about the direction of it.

I have used following script in p file.

fan_master    
{        
	type            fan;		
	patchType 	cyclic;		
	f List<scalar>    3(3 3 -2);	
	value uniform 0;    
}	
fan_slave 
{        
	type            fan;		
	patchType 	cyclic;		
	f List<scalar>    3(3 3 -2);	
	value uniform 0;    
}

How to set the direction of the flow? In other words how to reverse the direction if required?
If the flow happens from master to slave, how to identify which side is the master and slave?

Thanks again..

[tomf]

Hi,

It depends on the orientation of the master patch. If you flip it (the normal direction), the direction of the fan will change. I am just not sure how to do it in OpenFOAM directly. I prepare my cases using ANSA, where I can easily flip the orientation of such a patch. Probably the slave will have to be flipped as well. I think that the master is always the first entry in constant/polyMesh/boundary.

Regards,
Tom