CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

Inlet and Outlet b.c. based on mass flux

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 19, 2013, 09:01
Default Inlet and Outlet b.c. based on mass flux
  #1
Member
 
Hale
Join Date: May 2013
Posts: 53
Rep Power: 4
Hale is on a distinguished road
Hi foamers,




I'm trying to model a dropshaft (using interFoam solver) that contains
  • constant water flow at the inlet.
  • also constant water flow at the outlet which is equal to the fraction of water that is dropped.
I tried with
  • Inlet
    • U: type fixedValue;
      value uniform (-0.05 0 0);
    • P: type zeroGradient;
  • Outlet
    • U: type zeroGradient;
    • P: type fixedValue;
      value uniform 0;
These boundary conditions give some wrong results.
  1. Inlet: I calculated the velocity based on the constant water discharge. As I can see from the results the water has the expected velocity but the water level at (1) does not remain constant. The water level decreases as it drops down.
  2. Outlet: I constructed the U-shaped form so the water at location (2) is in balance with outlet so when the water drops the corresponding flux will go out from the outlet and therefore the water level would be constant at location (2). But it seems like the outlet boundary condition sucks the water and therefore I won't have constant water level at location (2) shown in figure below.
Figure below shows the set-up and the inlet/outlet boundaries.

Is there any way to define the boundaries based on mass flux? if yes how can I apply it to my case. I really appreciate any help and idea.
Attached Images
File Type: jpg dropshaft.jpg (29.2 KB, 63 views)
Hale is offline   Reply With Quote

Old   August 9, 2013, 00:13
Default
  #2
Member
 
India
Join Date: Oct 2012
Posts: 84
Rep Power: 4
mayank.dce2k7 is on a distinguished road
Hi Hale,

Did you find any solution to your problem. I am stuck on the same problem i.e applying boundary conditions based on mass flux?

Regards,
Mayank
mayank.dce2k7 is offline   Reply With Quote

Old   August 9, 2013, 02:26
Default
  #3
Member
 
Hale
Join Date: May 2013
Posts: 53
Rep Power: 4
Hale is on a distinguished road
Quote:
Originally Posted by mayank.dce2k7 View Post
Hi Hale,

Did you find any solution to your problem. I am stuck on the same problem i.e applying boundary conditions based on mass flux?

Regards,
Mayank

Hi Mayank,

yes I solved the problem. If you only want to define a boundary condition based on the mass flux then I recommend that you calculate the corresponding velocity (Q=U*A -> U = Q/A) and use the following for velocity and pressure

velocity

Code:
    inFlow 
    {
        type            fixedValue;
        value           uniform (xx 0 0);   // define the velocity 
     }
pressure

Code:
    inFlow           
    {
        type            buoyantPressure;
        value           uniform 0;
     }

This boundary condition gives a uniform velocity at the inlet. There is also another boundary condition where you directly can define the mass flux:

velocity

Code:
    inFlow
    {
        type            flowRateInletVelocity;   
        flowRate        xx;  // here you define the mass flux
        value           uniform (0 0 0);
    }
pressure

Code:
    inFlow           
    {
        type            buoyantPressure;
        value           uniform 0;
    }
This boundary condition gives the desired mass flux through the specified boundary but the velocity is not necessarily uniform. I'm not so sure about this boundary condition therefore I recommend you the first one.

If you want to know the mass flux through the boundaries then add this function to your controlDict

Code:
functions
{
    inletFlux
    {
        type            faceSource;
        functionObjectLibs ("libfieldFunctionObjects.so");
        outputControl   outputTime;
        log             true;
        // Output field values as well
        valueOutput     false;
        source          patch;
        sourceName      waterFlow;   // write the name of the boundary
        operation       sum;

        fields
        (
            rho phi alpha1     //define the quantities you want to be printed
        );
    }

    outletFlux
    {
        $inletFlux;
        sourceName      outlet;
    }

}
Remember that you should define your geometry in such a way that y=0 at the outlet otherwise it produces negative pressure. I had this problem with the previous post.

Hope this helps you
Hale is offline   Reply With Quote

Reply

Tags
boundary condition, constant height, interfoam

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mass flow inlet and pressure outlet issue nikhil FLUENT 5 December 11, 2013 13:30
Boudaries for bouynat driven flow with additional mass flux at inlet Charon CFX 2 April 27, 2013 08:02
mass flow inlet and pressure outlet with target mass flow rate Zigainer FLUENT 10 January 5, 2013 22:51
Net mass flow inlet vs outlet Nigui28 FLUENT 1 August 12, 2011 10:09
Mass flow inlet B.C. at exit... Jack Keays FLUENT 2 October 6, 2000 08:39


All times are GMT -4. The time now is 07:25.