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

Artificial high velocities at the interface using interFoam

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

Like Tree9Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 15, 2012, 12:32
Default
  #21
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,754
Rep Power: 29
ngj will become famous soon enoughngj will become famous soon enough
Hi Joris

You could type

Code:
forAll(U, celli)
{
    if (alpha1[celli] < 0.01)
        U[celli] = vector::zero;
}
However, you ought to be careful as you are threading onto an extremely dangerous path. What you are doing here is equivalent to be removing energy from the system.

I do not have the solution to circumvent the high velocities, but I my case I have found the above approach to yield utterly wrong results.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   February 15, 2012, 14:10
Default
  #22
New Member
 
Join Date: May 2011
Posts: 15
Rep Power: 8
joris.hey is on a distinguished road
Thanks niels for your answer.

I'll try that tomorrow.

My case is the following : Water is flowing onto a slope by its own weigth. The bc are cyclic in the slope direction. The top boundary is set to athmosphere so the air is free to enter and leave the system.

AT time 0 it gives :



In reality, only a thin layer of air is moved by the flowing water, but it is quickly slow down upwards by the athmosphere.

As I set up a athmosphere bc, I guess it is not too important to loose energy from the air field. Only the water field matter for me (the pressure and velocity of water would contribute almost totally to the water depth level). I think Shallow water equation are derived from Navier Stokes taking a free velocity bc for the water surface. So in my case, air should influate a minimum the water surface. (maybe I should decrease a lot air viscosity for that?)
joris.hey is offline   Reply With Quote

Old   February 16, 2012, 03:51
Default
  #23
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,754
Rep Power: 29
ngj will become famous soon enoughngj will become famous soon enough
However, since you are removing energy from a system, where the Navier-Stokes equations are solved simultaneously for both air and water, then you indirectly removes energy from the water, since energy from the water will be used to re-accelerate the air. Work put into the air, which is then removed in subsequent time steps.

The approach could be working for your case; you merely have to exhibit extreme caution.

/ Niels
vsammartano likes this.
ngj is offline   Reply With Quote

Old   February 16, 2012, 04:14
Default
  #24
New Member
 
Join Date: May 2011
Posts: 15
Rep Power: 8
joris.hey is on a distinguished road
I see what you mean, I will be carefull though.

I 'll post later my rersults,

cheers
joris
joris.hey is offline   Reply With Quote

Old   May 5, 2014, 11:59
Default compile problem
  #25
New Member
 
Baek, Donghae
Join Date: Jan 2013
Location: Seoul
Posts: 24
Rep Power: 6
wes1204 is on a distinguished road
hello joris.hey

I got same problem.

did you solve it ???

please advise me
wes1204 is offline   Reply With Quote

Old   October 16, 2014, 17:18
Default To be sure
  #26
New Member
 
Remi Carmi
Join Date: Jul 2014
Posts: 15
Rep Power: 5
rcarmi is on a distinguished road
Quote:
Originally Posted by Bernhard View Post
I'd like to add something to this thread, since I encoutered similar problems for my case. This problems disappeared with reducing the density ratio in my case from 1000 to 10.

Since I don't like the clipping in the air velocity I was able to get better results by applying the argument of Brackbill ( http://www.sciencedirect.com/science...2199919290240Y ) for surface tension, on the additional source term in the Navier-Stokes equations resutling for the reformulation of the pressure.

Basically what I did, was replacing this (in pEqn.H and UEqn.H of interFoam)
Code:
- ghf*fvc::snGrad(rho)
By
Code:
- ghf*fvc::snGrad(rho)*2.0*fvc::interpolate(alpha1)
The argument by Brackbill is summarized as follows: as the interface thickness goes to zero, you can multiply the body force by a function that is 1 at the interface. Since \grad\rho is zero except at the interface and 2alpha1 is 1 there, I think this is justified (please correct me if I'm wrong)

For me it solved the issues with the high air velocities, and this implementation is at least more justified than just clipping U.

I am facing a similar problem and I have tried all the solutions mentioned :

alpha1*div(rhophi,U) => well then the air flow is not transported and saturates where it is generated.
U air to 0 or a percentage of the solution value (that should work but it does not to violent a create instability)
I tried increasing the density : it is a bit better
I tried also to do higher rho and Brackbill.

What was your final solution Bernhard?
are you still doing the alpha1*div and the increasing rho plus blackbill?

Thanks
Remi
rcarmi is offline   Reply With Quote

Old   November 7, 2014, 07:52
Default
  #27
Member
 
Yuanchuan Liu
Join Date: Oct 2012
Posts: 30
Rep Power: 6
SailorLiu is on a distinguished road
Hi Remi,

I have been bothered by this problem for quite a long time. Which of those solutions mentioned in the earlier posts works best for you?
Cheers,

Yuanchuan Liu
SailorLiu is offline   Reply With Quote

Old   November 7, 2014, 15:13
Default
  #28
New Member
 
Remi Carmi
Join Date: Jul 2014
Posts: 15
Rep Power: 5
rcarmi is on a distinguished road
Hi Yuanchuan,

I will increase the density of the air. But that depends on what you are trying to do?

My problem was when putting an object near the interface and moving it. Then I have vorticity (shedding) generated by the object (chose your frame it happens if you put a flow or move the object). And when the vorticity reaches the interface it kind of generates fast flow in the easy to transport air. Making it thicker (just rho_water / rho_air =100 is still big) really reduce this not necessary transport. Killing the flow in air is definitely not a good idea.

Now that I think about it, would making a viscosity gradient help? (high viscosity as you move up in the air to dissipate the energy or just higher air viscosity to damp the transport, it is kind of what people do just by making the grid more loose in the air? numerical viscosity is bigger!).

Let me know what is your final call.

Best

Remi
rcarmi is offline   Reply With Quote

Old   November 7, 2014, 15:44
Default
  #29
Member
 
Yuanchuan Liu
Join Date: Oct 2012
Posts: 30
Rep Power: 6
SailorLiu is on a distinguished road
Hi Remi,

If I understand you correctly, you offer two ways to mitigate the effects of air convection:
1. Increase air density so that it is not so easy for air to transport.
2. Increase air viscosity so that even if high velocity occurs it will damp out quickly.
These two methods might work for my current case where a cylinder with a horinzontal thick plate oscillates vertically in xoz plane since air is not important here. Besides, I do not need to change the code, which is fine.
However, if I later want to take into account the aerodynamic force acting on the object, altering the properties of the air phase might be improper as air becomes important in this case. Of course, all the methods mentioned in this thread will change the real physics and are actually based on the assumption that air does not play a major part in my cases. I am wondering if there is any way to solve this problem without the need to alter the original problem. Really curious about how commercial solvers deal with this problem.
Anyway, thanks very much for sharing your thoughts with me. I will try them to see if they will make a difference.

Cheers,

Yuanchuan
SailorLiu is offline   Reply With Quote

Old   October 2, 2015, 04:49
Default a RANS in air only
  #30
New Member
 
Remi Carmi
Join Date: Jul 2014
Posts: 15
Rep Power: 5
rcarmi is on a distinguished road
Hi all,

I am still playing with this problem. I have recently tried a new idea. I activate turbulence in Air only. I created a new k-E RASModel where I use the scalar alpha1 to turn it on or off whether I am in air or water. This is quite convenient but might be wrong since I am in 2D. It however gives rather good results somehow in my case (at least qualitatively compares well with my experiments) I have a manually oscillating pincher near a free surface.

Any other comments on your side?


Best

Rmi
rcarmi is offline   Reply With Quote

Old   October 23, 2015, 04:42
Default
  #31
Member
 
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 95
Rep Power: 10
rcastilla is on a distinguished road
Quote:
Originally Posted by ngj View Post
Hi Joris

You could type

Code:
forAll(U, celli)
{
    if (alpha1[celli] < 0.01)
        U[celli] = vector::zero;
}
However, you ought to be careful as you are threading onto an extremely dangerous path. What you are doing here is equivalent to be removing energy from the system.

I do not have the solution to circumvent the high velocities, but I my case I have found the above approach to yield utterly wrong results.

Best regards,

Niels
Hi,

I would like to make my modest contribution to this interesting subject. I agree that it is not the perfect solution but, nevertheless, it is better than getting kinetic turbulent energy divergence.

On the other hand, I have tested this loop and
1.- It is very slow
2.- It does not work with decomposed cases, since it only loops over the cells in the local processor

I suggest this solution for the velocity correction:

Code:
Info<< "Umax : " << max(mag(U)).value() << " U average: " << average(mag(U)).value() << endl;
 
U *= 1/(1+exp(-1000*(alpha1-scalar(0.1))));

Info<< "Update U" << endl;
Info<< "Umax : " << max(mag(U)).value() << " U average: " << average(mag(U)).value() << endl;
It is just an approximation to the Heaviside step function for the alpha1 scalar. The parameters can be changed in order to make it steeper and to modify the threshold value of alpha1

It is faster than the forAll loop, and it works fine in decomposed case.

Now I am thinking on how to modify this function so that it does not put to zero all the values of velocity where alpha1<0.1 but only the "peak" values, lowering them to an average velocity value. Any suggestion will be welcome.

Robert
rcastilla is offline   Reply With Quote

Old   October 24, 2015, 13:12
Default
  #32
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,020
Blog Entries: 39
Rep Power: 109
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Greetings to all!

I'm finding this issue with artificially high velocities very strange. I've taken a quick look into the whole thread and I couldn't find a single test case for this issue.

Can anyone provide a simple test case that demonstrates this?
Because I suspect that the problem for this has another origin, namely initialization problems, such as described here: http://www.cfd-online.com/Forums/ope...tml#post404292 - post #7

Best regards,
Bruno
vsammartano likes this.
__________________
wyldckat is offline   Reply With Quote

Old   October 29, 2015, 21:33
Default
  #33
New Member
 
Matej Muller
Join Date: Oct 2011
Location: Slovenia
Posts: 23
Rep Power: 7
matejmuller is on a distinguished road
Hi Remi!

How did you manage to activate the turbulence in air only? (by the way... shouldn't you activate it in water only?) I'm having troubles with using lookup for alpha1 in the turbulence model. When I use

Code:
const volScalarField& alpha1 = mesh_.lookupObject<volScalarField>("alpha1");
the turbulence model compiles fine, but when running interFoam I get the error:

Code:
--> FOAM FATAL ERROR:

    request for volScalarField alpha1_ from objectRegistry region0 failed
    available objects of type volScalarField are

15
(
alpha.water_0
interfaceProperties:K
nut
alpha.water
rho
k
p_rgh
nu
gh
nu1
p
rho_0
nu2
alpha.air
epsilon
)


    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting
If I use alpha.water instead of alpha1 it doesn't compile... Did you had similar problems?

Thanks, Matej

Last edited by matejmuller; October 29, 2015 at 22:37.
matejmuller is offline   Reply With Quote

Old   October 31, 2015, 10:56
Default
  #34
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,020
Blog Entries: 39
Rep Power: 109
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Quick answer:
Quote:
Originally Posted by matejmuller View Post
If I use alpha.water instead of alpha1 it doesn't compile... Did you had similar problems?
My guess is that you did this:
Code:
const volScalarField& alpha.water = mesh_.lookupObject<volScalarField>("alpha.water");
which is incorrect..

Try using this:
Code:
const volScalarField& alpha1 = mesh_.lookupObject<volScalarField>("alpha.water");
wyldckat is offline   Reply With Quote

Old   November 6, 2015, 07:30
Default
  #35
New Member
 
Dominik Schmidt
Join Date: Mar 2014
Posts: 11
Rep Power: 5
dschmidt is on a distinguished road
Quote:
I've taken a quick look into the whole thread and I couldn't find a single test case for this issue

Dear wyldckat,

those interfacial-velocities occur e.g. in mutliphaseEulerFoam (2.3.x), too.

As a test case one can use the bubbleColumn tutorial.
To better study the behavior I modified U.air, an alpha.air/water in a way,
that there is no inflow of air.

inlet: alpha.air = 0 , alpha.water = 1
inlet: U.air = 0


As previously stated in the thread, when I reduce the density gradient of both phases,
the interface velocities disappear (e.g. 995 to 1000).

I already looked into the effects of e.g. surface tension&interface compression,
but the effect is only very little influenced by turning on VOF-interface compression with surface tension.

I also followed your advise and initialized the pressure field according to gravity/mass effects, but that did not make the velocities disappear, either.

//EDIT: My first funkySetField approach was based on the setFieldsDict setup. I now modified the blockMeshdict to create 100 cells in y-direction,
so it should be easier to initialize the correct pressure field. I'll update the post if I make any further progress

//EDIT2: With this initialization the pressure is dropping at the liquid-gas interface after one iteration, while liquid downflow and gas upward flow is indicated in the U-fields.
Case Files are attached.
It seems that the solver calculates the hydrostatic pressure, as if the first "liquid cell" is not fully acting with the liquid density onto the pressure, as the pressure drop,
is in the order of half a cell-height filled with water.

Comparing those results with a setup without pressure initialization, there is no significant improvement regarding the artificial velocities at the interface, thus here the pressure initialization might not help resolving the problem.


Code:
  expressions
 (
	pressureWater
	{
	 field p; 
	 expression "1000*9.81*(0.7-pos().y)+(1-0.7)*1*9.81"; 	
	 condition  "(pos().y<0.7) && (pos().y>=0)";
         keepPatches 1;
	}

	pressureAir
	{
	 field p; 
	 expression "1*9.81*(1-pos().y)"; 
	 condition  "(pos().y<1) && (pos().y>=0.7)"; 
         keepPatches 1; 
	}

 );


Another way to reduce the velocities is to use the implemented damping function of multiphaseEulerFoam,
as stated by Kent:
http://www.cfd-online.com/Forums/ope...tml#post396320

... but isn't this effecting the overall physics?

Might a damper only at the surface be a less powerful intervention?



//EDIT3:
http://openfoam.org/mantisbt/view.php?id=1379

Following this bug report, the currents at the interface seem to be a general issue in "stagnand" two phase flow?
Is there a general recommendation in cases were the interface currents are higher than the liquid velocities, e.g. induced by liquid natural convection?


Sincerely,
Dominik
Attached Files
File Type: zip bubbleColumn.23x.artificialVelocities.zip (88.2 KB, 5 views)

Last edited by dschmidt; November 9, 2015 at 12:22.
dschmidt is offline   Reply With Quote

Old   April 14, 2016, 03:24
Default
  #36
Member
 
YS
Join Date: Jan 2010
Posts: 80
Rep Power: 9
Ya_Squall2010 is on a distinguished road
I wonder is there any progress in addressing this issue?

portal: http://www.cfd-online.com/Forums/ope...tml#post594956
Ya_Squall2010 is offline   Reply With Quote

Old   April 14, 2016, 12:01
Default
  #37
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 218
Rep Power: 14
kwardle is on a distinguished road
Here is a related topic with some info.
http://www.cfd-online.com/Forums/ope...tml#post576093
wyldckat likes this.
kwardle 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
Wind turbine simulation Saturn CFX 45 February 8, 2016 05:42
InterFoam Artificially High Velocities andersson.j OpenFOAM Running, Solving & CFD 0 February 8, 2011 11:43
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12
Replace periodic by inlet-outlet pair lego CFX 3 November 5, 2002 21:09


All times are GMT -4. The time now is 00:49.