[Sakun]

Hello everyone,

I simulating 0.7 mach number simulation for a single compressor blade using rhoPimpleFoam. Simulation is pressure based so i just have to set up INLET flow direction and OUTLET flow direction. I have already set up INLET flow (45.83 degrees)direction using "pressureDirectedInletVelocity" but i don't know any boundary condition to set up OUTLET flow direction which is 6.22.



Can i get some suggestion for this issue

Thank you very much for your time,

/*--------------------------------*- C++ -*----------------------------------* \
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2112                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    INLET
    {
	
		type pressureDirectedInletVelocity;
		inletDirection uniform (0.631623456 -0.775275312 0); //geometric inlet angle is 50.83
		value uniform (0 0 0);
		
    }

	OUTLET
    {
       
		
	type            pressureInletOutletVelocity;
        inletValue      uniform (0 0 0);
        value           uniform (0 0 0);

			
    }

    CASCADE
    {
        type            noSlip;
    }
	
	"(TOP|BOTTOM)"
	{
		type            cyclicAMI;
	}

	frontAndBackPlanes
    {
        type            empty;
    }

    
}


// ************************************************************************* //

[alexvaleije]

Hi,

Although I haven't played with it, maybe you can try with pressureDirectedInletOutletVelocity, setting the outflow direction properly.

I'll let you the link with the definition:

https://www.openfoam.com/documentati...8H_source.html

Let me know if it works. Regards,

Originally Posted by Sakun

Hello everyone,

I simulating 0.7 mach number simulation for a single compressor blade using rhoPimpleFoam. Simulation is pressure based so i just have to set up INLET flow direction and OUTLET flow direction. I have already set up INLET flow (45.83 degrees)direction using "pressureDirectedInletVelocity" but i don't know any boundary condition to set up OUTLET flow direction which is 6.22.



Can i get some suggestion for this issue

Thank you very much for your time,

/*--------------------------------*- C++ -*----------------------------------* \
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2112                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    INLET
    {
	
		type pressureDirectedInletVelocity;
		inletDirection uniform (0.631623456 -0.775275312 0); //geometric inlet angle is 50.83
		value uniform (0 0 0);
		
    }

	OUTLET
    {
       
		
	type            pressureInletOutletVelocity;
        inletValue      uniform (0 0 0);
        value           uniform (0 0 0);

			
    }

    CASCADE
    {
        type            noSlip;
    }
	
	"(TOP|BOTTOM)"
	{
		type            cyclicAMI;
	}

	frontAndBackPlanes
    {
        type            empty;
    }

    
}


// ************************************************************************* //

[Sakun]

Originally Posted by alexvaleije

Hi,

Although I haven't played with it, maybe you can try with pressureDirectedInletOutletVelocity, setting the outflow direction properly.

I'll let you the link with the definition:

https://www.openfoam.com/documentati...8H_source.html

Let me know if it works. Regards,

Hi ,


Thank you very much for the reply. I had this boundary condition in my mind but since it said "inletDirection" again, i thought it only works with INLETs

{         type                pressureDirectedInletOutletVelocity;
           phi                  phi;         

           rho                  rho;         

           inletDirection  uniform (1 0 0);         

           value               uniform 0;
 }

If i want to apply 6.22 degrees to the OUTLET flow direction, is this correct ?

{         type             pressureDirectedInletOutletVelocity;         

           phi               phi;         

           rho               rho;         

            inletDirection  uniform (0.9941 0.1083 0);//[cos6.22 sin6.22 0]      

            value            uniform 0;    
 
}

Thank you very much again for your kind suggestions.

[alexvaleije]

Hi Sakun,

As far as I understand, I would proceed as you have written.

In any case, if you have any concern whether this is going to work and your case is too big, you can create a simple straight channel and try there the boundary conditions. The case only needs to have inlet, outlet and walls and it will run almost inmediately.

Best regards,

Originally Posted by Sakun

Hi ,


Thank you very much for the reply. I had this boundary condition in my mind but since it said "inletDirection" again, i thought it only works with INLETs

{         type                pressureDirectedInletOutletVelocity;
           phi                  phi;         

           rho                  rho;         

           inletDirection  uniform (1 0 0);         

           value               uniform 0;
 }

If i want to apply 6.22 degrees to the OUTLET flow direction, is this correct ?

{         type             pressureDirectedInletOutletVelocity;         

           phi               phi;         

           rho               rho;         

            inletDirection  uniform (0.9941 0.1083 0);//[cos6.22 sin6.22 0]      

            value            uniform 0;    
 
}

Thank you very much again for your kind suggestions.

[Yann]

Hello,

Originally Posted by alexvaleije

Although I haven't played with it, maybe you can try with pressureDirectedInletOutletVelocity, setting the outflow direction properly.

I don't think this will allow to set an outflow direction. The BC description is pretty straightforward:

This velocity inlet/outlet boundary condition is applied to velocity
boundaries where the pressure is specified. A zero-gradient condition is
applied for outflow (as defined by the flux); for inflow, the velocity
is obtained from the flux with the specified inlet direction.

Sign conventions:
- positive flux (out of domain): apply zero-gradient condition
- negative flux (into of domain): derive from the flux with specified
direction

The direction is only used for inflow. For outflow it's just zeroGradient.

Regards,
Yann

[Sakun]

Originally Posted by alexvaleije

Hi Sakun,

As far as I understand, I would proceed as you have written.

In any case, if you have any concern whether this is going to work and your case is too big, you can create a simple straight channel and try there the boundary conditions. The case only needs to have inlet, outlet and walls and it will run almost inmediately.

Best regards,

Hi Alejandro,


I can't really make it straight at the OUTLET becasue this is turbomachinery simulation and i had to follow the exact domain shape that my reference paper has (i have attached a picture of doamin from my reference paper)


Best regards,
Sakun

[Sakun]

Originally Posted by Yann

Hello,



I don't think this will allow to set an outflow direction. The BC description is pretty straightforward:





The direction is only used for inflow. For outflow it's just zeroGradient.

Regards,
Yann

Hi Yann,


Thank you very much for your kind response my isseue, i higly appriciate that


In that case i can either use "pressureDirectedInletOutletVelocity" or "pressureDirectedInletVelocity" for the INLET and use "zeroGradient" for the OUTLET ?


Best regards,
Sakun

[Yann]

Originally Posted by Sakun

In that case i can either use "pressureDirectedInletOutletVelocity" or "pressureDirectedInletVelocity" for the INLET and use "zeroGradient" for the OUTLET ?

Hello Sakun,

Yes it sounds good. I guess you won't have backflow at the inlet, so pressureDirectedInletVelocity should do the job.

Cheers,
Yann

[Sakun]

Originally Posted by Yann

Hello Sakun,

Yes it sounds good. I guess you won't have backflow at the inlet, so pressureDirectedInletVelocity should do the job.

Cheers,
Yann

Hi Yann,


Thank you very much for the suggestion, i will work on you suggestion



Since i have periodic boundary conditions for TOP and BOTTOM (attached picture) flow is extremely unsteady (go beyond 300 m/s) and it affects the stablity of the simulation too much .
So hopefully i guess zeroGradient in the OUTLET boundary condition would do the work.


Best regards,
Sakun