[ovie]

Hi:

I have a set up where a slug of liquid (water) is suspended in a vertical capillary channel open to the atmosphere at both ends. Experimental results from our lab shows that the liquid is unable to flow under its weight without agitating the channel. However, when I run simulations using interFoam for the set up, the liquid easily flows under the influence of gravity (see attached file for 2D case).

I guess the question is should the no-slip boundary condition be used in this case or should it be replaced by some friction dependent bc that accounts for the effect of a static friction barrier that must be overcome before liquid starts flowing?

Thanks.

[wyldckat]

Greetings Ovie,

I haven't managed to look into this, but I'm still curious... I'm making a note to come back to this in a few days.

Anyway, my guess is that you did not initialize properly the pressure field. The other possibilities that come to mind are:

• Mesh isn't good enough.
• The dimensions of the tube might be incorrect.
• The alpha contact angle algorithm should be able to handle this. Did you follow the same steps as in the "capillaryTube" tutorial case?

By the way, you might want to try and initially run the simulation without gravity or with the vector perpendicular to the tube wall, for a few seconds. Then after the simulation stops, change the gravity vector and then continue the simulation from the last time snapshot.


Best regards,
Bruno

[ovie]

Originally Posted by wyldckat

Greetings Ovie,

I haven't managed to look into this, but I'm still curious... I'm making a note to come back to this in a few days.

Anyway, my guess is that you did not initialize properly the pressure field. The other possibilities that come to mind are:

• Mesh isn't good enough.
• The dimensions of the tube might be incorrect.
• The alpha contact angle algorithm should be able to handle this. Did you follow the same steps as in the "capillaryTube" tutorial case?

By the way, you might want to try and initially run the simulation without gravity or with the vector perpendicular to the tube wall, for a few seconds. Then after the simulation stops, change the gravity vector and then continue the simulation from the last time snapshot.


Best regards,
Bruno

Hi Bruno: thanks for your feedback.

The set up for the 2-D version of this problem is adapted directly from the "Capillary Rise" tutorial - so i used the same set of the initial conditions. I also retained the same mesh resolution as was used in the tutorial. The dimensions have been double checked and they are ok too.

The suggestion to turn off gravity at first sounds good. I would try this out and let you know the outcome.

Thanks again!

[ovie]

Originally Posted by ovie

Hi Bruno: thanks for your feedback.

The set up for the 2-D version of this problem is adapted directly from the "Capillary Rise" tutorial - so i used the same set of the initial conditions. I also retained the same mesh resolution as was used in the tutorial. The dimensions have been double checked and they are ok too.

The suggestion to turn off gravity at first sounds good. I would try this out and let you know the outcome.

Thanks again!

Hi:

I just repeated the simulations with/without gravity. The case with gravity was ok i.e. liquid remains suspended in capillary channel. I ran this for enough time to ensure the solution is stable. Then I restarted with gravity turned on and the liquid slug starts flowing downwards. The liquid slug has a volume of 5microL and the channel volume is 70microL. The velocities from the interFoam solution approach values from Poiseuille flow which is really high for channels of this dimension. I dont think these results are correct.

Thanks.

[wyldckat]

Hi Ovie,

Mmm... I think you might be hitting the limitation mentioned on these posts:

• http://www.cfd-online.com/Forums/ope...tml#post433969 post #2
• http://www.cfd-online.com/Forums/ope...tml#post455220 post #20
• http://www.cfd-online.com/Forums/ope...tml#post453034 post #16

Last but not least, as mentioned on the post #15 on the last thread, you might want to:

Originally Posted by wyldckat

try contacting OpenCFD's support http://www.openfoam.com/support/ - at the very least, they can give you a straight answer if this can be simulated with the current version of OpenFOAM and how much it would cost to implement this is, in case it doesn't have this feature yet.

Best regards,
Bruno

[wyldckat]

Hi Ovie,

I finally managed to give a look into this. Just to be clear, I'm not an expert on this, but I believe that you can't use a constant alpha angle, given that it oscillates that much.

You'll need to search more about this, but the "dynamicAlphaContactAngle" seems to be what you should be using for the walls. For example (a somewhat bad one I tried):

    walls
    {
        type           dynamicAlphaContactAngle;
        theta0         45;
        uTheta         10;
        thetaA         10;
        thetaR         60;
        limit          gradient;
        value          uniform 0;
    }

For the meaning of each variable, the source code at "$FOAM_SRC/transportModels/twoPhaseProperties/alphaContactAngle/dynamicAlphaContactAngle/dynamicAlphaContactAngleFvPatchScalarField.H" has these comments:

        //- Equilibrium contact angle
        scalar theta0_;

        //- Dynamic contact angle velocity scale
        scalar uTheta_;

        //- Limiting advancing contact angle
        scalar thetaA_;

        //- Limiting receeding contact angle
        scalar thetaR_;

Best regards,
Bruno

[ovie]

Originally Posted by wyldckat

Hi Ovie,

I finally managed to give a look into this. Just to be clear, I'm not an expert on this, but I believe that you can't use a constant alpha angle, given that it oscillates that much.

You'll need to search more about this, but the "dynamicAlphaContactAngle" seems to be what you should be using for the walls. For example (a somewhat bad one I tried):

    walls
    {
        type           dynamicAlphaContactAngle;
        theta0         45;
        uTheta         10;
        thetaA         10;
        thetaR         60;
        limit          gradient;
        value          uniform 0;
    }

For the meaning of each variable, the source code at "$FOAM_SRC/transportModels/twoPhaseProperties/alphaContactAngle/dynamicAlphaContactAngle/dynamicAlphaContactAngleFvPatchScalarField.H" has these comments:

        //- Equilibrium contact angle
        scalar theta0_;

        //- Dynamic contact angle velocity scale
        scalar uTheta_;

        //- Limiting advancing contact angle
        scalar thetaA_;

        //- Limiting receeding contact angle
        scalar thetaR_;

Best regards,
Bruno

Hi Bruno:

Thanks for looking into this. I would implement the dynamic contact angle BC and let you know the results.

Thanks again!

[wyldckat]

Hi Ovie,

I forgot to mention that you might need to do some more research on this topic, as implied by this paper: Impacting droplets: dynamic contact angle modelling in OpenFOAM® - this paper indicates that another model had to be implemented by the paper's authors in order to better simulate the following:

The spreading and receding behavior of simulated water droplets impacting onto automobile wind shields or aircraft wings is not only determined by their initial conditions, but also influenced by the evolution of the contact angle throughout the impact scenario.

In your case, it's sort of the opposite and yet the same: although the droplet is meant to be stuck in the same place, the initial condition makes it wobble and leads to the observed motion. If the wobbling was better contained by the contact angle model, then it might not move.

Best regards,
Bruno

[ovie]

Great! Thanks!

[lumasci]

Originally Posted by wyldckat

Impacting droplets: dynamic contact angle modelling in OpenFOAM® - this paper indicates that another model had to be implemented by the paper's authors in order to better simulate the following

Hi,


Old topic, I know, but still a current topic.


Did anyone try to implement the Kistler model for theta_dyn?


I am having issues with a droplet rolling down an inclined plane.