CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Setting Flow Direction in OUTLET

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Yann

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 4, 2023, 08:40
Post Setting Flow Direction in OUTLET
  #1
Senior Member
 
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 100
Rep Power: 6
Sakun is on a distinguished road
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,

Code:
/*--------------------------------*- 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;
    }

    
}


// ************************************************************************* //
Attached Images
File Type: png paper values.PNG (39.3 KB, 13 views)
Sakun is offline   Reply With Quote

Old   May 4, 2023, 13:04
Default
  #2
Member
 
Alejandro Valeije
Join Date: Nov 2014
Location: Spain
Posts: 52
Rep Power: 11
alexvaleije is on a distinguished road
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,

Quote:
Originally Posted by Sakun View Post
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,

Code:
/*--------------------------------*- 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 is offline   Reply With Quote

Old   May 4, 2023, 16:15
Default
  #3
Senior Member
 
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 100
Rep Power: 6
Sakun is on a distinguished road
Quote:
Originally Posted by alexvaleije View Post
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



Code:
{         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 ?


Code:
{         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.
Sakun is offline   Reply With Quote

Old   May 4, 2023, 16:45
Default
  #4
Member
 
Alejandro Valeije
Join Date: Nov 2014
Location: Spain
Posts: 52
Rep Power: 11
alexvaleije is on a distinguished road
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,

Quote:
Originally Posted by Sakun View Post
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



Code:
{         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 ?


Code:
{         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 is offline   Reply With Quote

Old   May 5, 2023, 03:35
Default
  #5
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,108
Rep Power: 26
Yann will become famous soon enough
Hello,

Quote:
Originally Posted by alexvaleije View Post
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:

Quote:
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.
Quote:
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
Yann is offline   Reply With Quote

Old   May 5, 2023, 16:15
Default
  #6
Senior Member
 
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 100
Rep Power: 6
Sakun is on a distinguished road
Quote:
Originally Posted by alexvaleije View Post
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
Attached Images
File Type: png Blade doamin shape.PNG (103.7 KB, 6 views)
Sakun is offline   Reply With Quote

Old   May 5, 2023, 16:19
Default
  #7
Senior Member
 
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 100
Rep Power: 6
Sakun is on a distinguished road
Quote:
Originally Posted by Yann View Post
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
Sakun is offline   Reply With Quote

Old   May 6, 2023, 04:54
Default
  #8
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,108
Rep Power: 26
Yann will become famous soon enough
Quote:
Originally Posted by Sakun View Post
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 likes this.
Yann is offline   Reply With Quote

Old   May 7, 2023, 07:06
Default
  #9
Senior Member
 
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 100
Rep Power: 6
Sakun is on a distinguished road
Quote:
Originally Posted by Yann View Post
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
Attached Images
File Type: jpg doamin shape.jpg (62.4 KB, 4 views)
Sakun is offline   Reply With Quote

Reply

Tags
flow direction, periodic boundaries, turbo machinery, unsteady compressible

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Simple Box - Gravity with Pressure Outlet - Unrealistic Reverse Flow pyccknn FLUENT 2 December 1, 2021 17:31
setting OUTLET flow rate equal to INLET flow rate spitchers OpenFOAM Programming & Development 0 March 22, 2018 06:33
Compressible Flow Pressure Outlet Back Flow okstatecheme OpenFOAM Running, Solving & CFD 1 March 21, 2018 08:11
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
Warning 097- AB Siemens 6 November 15, 2004 04:41


All times are GMT -4. The time now is 10:47.