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

simpleFoam - don't know where mass is going

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 19, 2016, 09:30
Default simpleFoam - don't know where mass is going
  #1
New Member
 
Katrin
Join Date: Jul 2016
Posts: 18
Rep Power: 3
highpressuretube is on a distinguished road
Hi all,

I am running a simpleFoam k-epsilon flow simulation. Attached is the flow inlet where the inlet diameter of 14,5mm goes down to 3,6mm.

General flow is set to 4l/min so I calculate
0,403722408160178 m/s inlet flow velocity
5,57m/s in the 3,6mm part..

However flow is only reaching 1,78m/s. What is happening there? Where is my mass going?

Problem is continued through the entire model, all steps show reduced velocity.

My p-File:

Code:
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
inlet
{
       type            zeroGradient;
}
outlet
{
        type            fixedValue; 
        value           uniform 0;
}
walls
{
        type            zeroGradient;
}
SYM
{
       type            empty;
}
}
My U file:
Code:
{
    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            fixedValue; 
        value           uniform (0.403722408160178 0.000000 0.000000);
}
outlet
{
       type            zeroGradient;
}
walls
{
        type            fixedValue; 
        value           uniform (0. 0. 0.);
}
SYM
{
       type            empty;
}
}
Any suggestions as to where to look for the error is welcome.

Thanks in advance,
highpressuretube
Attached Images
File Type: jpg Flow-InletSide.jpg (104.0 KB, 9 views)
File Type: jpg Flow-LastResiduals.jpg (62.7 KB, 7 views)
highpressuretube is offline   Reply With Quote

Old   October 19, 2016, 10:11
Default
  #2
Senior Member
 
floquation's Avatar
 
Kevin van As
Join Date: Sep 2014
Location: TU Delft, The Netherlands
Posts: 223
Rep Power: 12
floquation will become famous soon enough
Are you sure your simulation is 3D?

If your simulation is 2D, then you should expect an outlet velocity of (14.5*0.4*L)/(3.6*L)=~1.6 m/s.
Now, looking at your color figure, my eyes would say that the maximum velocity is reached at the beginning of the smaller tube, but it is in fact lower than the maximum value nearby the ending of this smaller tube.
1.6 m/s is slightly lower than 1.78 m/s, and could therefore very well be that value. (Again, I cannot perfectly see the value on a color figure - plot the velocity over a line and you can be sure of the precise value.)

Hence, are you sure your simulation is not in fact 2D?
floquation is offline   Reply With Quote

Old   October 20, 2016, 03:15
Default
  #3
New Member
 
Katrin
Join Date: Jul 2016
Posts: 18
Rep Power: 3
highpressuretube is on a distinguished road
Hi floquation,

you are soooo right. And I have been spending hours not seeing the woods because of all the trees blocking the view.

But then how would I need to scale my 2D model to be able to compare it to 3D measurements? (I wonder if it makes more sense to reduce to a rotationalsymmetric modell instead of a plane 2D...)

Thanks for the hint,
highpressuretube
highpressuretube is offline   Reply With Quote

Old   October 20, 2016, 08:41
Default
  #4
Senior Member
 
floquation's Avatar
 
Kevin van As
Join Date: Sep 2014
Location: TU Delft, The Netherlands
Posts: 223
Rep Power: 12
floquation will become famous soon enough
Quote:
Originally Posted by highpressuretube View Post
But then how would I need to scale my 2D model to be able to compare it to 3D measurements? (I wonder if it makes more sense to reduce to a rotationalsymmetric modell instead of a plane 2D...)
That depends on what you'd like to achieve.

If you just want to compare velocities, you should realise that velocities scale with the height of the channel in 2D, whereas they scale with the height squared in 3D.
Using a rotational symmetric model resolves this issue.

If you intend to go for turbulent simulations, you must realise that turbulent flows are not rotationally symmetric, hence a rotationally symmetric model wouldn't be very smart there.
In fact, turbulence is intrinsically 3D, requiring you to use a 3D mesh. If that is too computational intensive for your purposes, then 2D is probably still better than assuming rotational symmetry.
Either way, interpret 2D simulations with caution, as they assume one out of three dimensions to be infinitely long.
floquation is offline   Reply With Quote

Old   October 21, 2016, 07:17
Default
  #5
New Member
 
Katrin
Join Date: Jul 2016
Posts: 18
Rep Power: 3
highpressuretube is on a distinguished road
Hi floquation,

has to be 3D then.

Thanks for your thoughts,
highpressuretube
highpressuretube is offline   Reply With Quote

Old   October 21, 2016, 07:19
Default
  #6
New Member
 
Katrin
Join Date: Jul 2016
Posts: 18
Rep Power: 3
highpressuretube is on a distinguished road
How do I mark a thread as solved anyway?
highpressuretube is offline   Reply With Quote

Reply

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
Target Mass Flow Rate Nitin FLUENT 9 June 17, 2017 10:30
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
mass fraction of species Lilly FLUENT 3 July 25, 2011 05:00
Mass sources - help! Emmanuel Resch CD-adapco 11 May 29, 2008 10:20
Mass flux and mass flow rate us Phoenics 10 March 31, 2006 02:06


All times are GMT -4. The time now is 09:30.