Surface tension driven flows: interFoam vs. multiphaseInterFoam

dzordz · October 25, 2018, 08:46

Greetings!

I wanted to discuss a topic that I have not seen talked about on these forums. The difference between interFoam and multiphaseInterFoam for surface tension driven flows. In my work I am simulating breaks up of a water jet. I have been using for a while multiphaseInterFoam solver but recently changed to interFoam solver. The main difference I noticed that the two solvers do not behave in the same way. The point of breakup differs for both solvers. Took me some time to figure it out and I just wanted to share if anyone else has the same issues or does not know which one to use.

So the code implementation for surface tension force (STF)looks like this:
INTER FOAM: $STF_{if} = \sigma \kappa \nabla \alpha_{1}$
MULTIPHASEINTERFOAM: $STF_{mif} = \sigma \kappa (\alpha_{2} \nabla \alpha_{1} - \alpha_{1} \nabla \alpha_{2})$

The issues is the two implementations are identical theoretically but surely not the same numerically. Problem occurs with the calculation of gradient of discontinuous volumetric alpha fields (this is a known issue in OpenFoam, and the erroneous calculations lead to spurious currents development.)
$\nabla \alpha^{numerical} = \nabla \alpha^{theoretical} + e(\nabla \alpha)$
$\alpha_{2} = 1 - \alpha_{1}$
$\nabla \alpha^{theoretical}_{1}+\nabla \alpha^{theoretical}_{2} = 0$

Looking only at gradient (STFif) and the brackets (STFmif) and using the previous three relations we get to the end result:

$STF_{if} \propto \nabla \alpha_{1}^{theoretical} + e(\nabla \alpha_{1})$

$STF_{mif} \propto \nabla \alpha_{1}^{theoretical} + e(\nabla \alpha_{1}) - \alpha_{1}(e(\nabla \alpha_{1})+e(\nabla \alpha_{2}))$

It can be seen that there is an extra error term, which makes calculating with multiphaseInterFoam worse. In my case the reduction of stf in mif makes the jet longer. There is of course the same error coming out of curvature K, which has the same issue of calculating gradients, calculation of which was omitted from here for clarity. Hopefully the error calculation reduces with implementation of new numerical techniques like the one from Scheufler & Roenby (Accurate and efficient surface reconstruction from volume fraction data on general meshes) and the two solvers produce equal solutions.

The question I have is does anybody know why surface tension is implemented in such way? Any literature on surface tension terms in momentum equation in mixture model would be much appreciated.

Cheers

mAlletto · October 30, 2018, 08:00

There are two references in https://openfoamwiki.net/index.php/InterFoam which i found usefull.

vivek05 · October 31, 2018, 22:26

Hi dzordz & Michael Alletto
I am also simulating liquid jet breakup using interFoam solver. In my case, the liquid jet is not even showing any sign of breakup, but small oscillation or perturbation are happening at the liquid jet surface. I don't know exactly what causes this problem. I tried with different mesh size. Could anyone help to find out this problem?

Thank you,

Zhicheng YUAN · December 22, 2021, 02:57

Form my point of view, MFIF can be used for a system more than three fluids. If only two phases are present in a cell, then $\nabla \alpha_1 = - \nabla \alpha_2$. With \alpha_1=1-\alpha_2, we will get the equation used by interFOAM.

October 25, 2018, 08:46	Surface tension driven flows: interFoam vs. multiphaseInterFoam	#1
dzordz Member Join Date: May 2016 Posts: 39 Rep Power: 9	Greetings! I wanted to discuss a topic that I have not seen talked about on these forums. The difference between interFoam and multiphaseInterFoam for surface tension driven flows. In my work I am simulating breaks up of a water jet. I have been using for a while multiphaseInterFoam solver but recently changed to interFoam solver. The main difference I noticed that the two solvers do not behave in the same way. The point of breakup differs for both solvers. Took me some time to figure it out and I just wanted to share if anyone else has the same issues or does not know which one to use. So the code implementation for surface tension force (STF)looks like this: INTER FOAM: $STF_{if} = \sigma \kappa \nabla \alpha_{1}$ MULTIPHASEINTERFOAM: $STF_{mif} = \sigma \kappa (\alpha_{2} \nabla \alpha_{1} - \alpha_{1} \nabla \alpha_{2})$ The issues is the two implementations are identical theoretically but surely not the same numerically. Problem occurs with the calculation of gradient of discontinuous volumetric alpha fields (this is a known issue in OpenFoam, and the erroneous calculations lead to spurious currents development.) $\nabla \alpha^{numerical} = \nabla \alpha^{theoretical} + e(\nabla \alpha)$ $\alpha_{2} = 1 - \alpha_{1}$ $\nabla \alpha^{theoretical}_{1}+\nabla \alpha^{theoretical}_{2} = 0$ Looking only at gradient (STFif) and the brackets (STFmif) and using the previous three relations we get to the end result: $STF_{if} \propto \nabla \alpha_{1}^{theoretical} + e(\nabla \alpha_{1})$ $STF_{mif} \propto \nabla \alpha_{1}^{theoretical} + e(\nabla \alpha_{1}) - \alpha_{1}(e(\nabla \alpha_{1})+e(\nabla \alpha_{2}))$ It can be seen that there is an extra error term, which makes calculating with multiphaseInterFoam worse. In my case the reduction of stf in mif makes the jet longer. There is of course the same error coming out of curvature K, which has the same issue of calculating gradients, calculation of which was omitted from here for clarity. Hopefully the error calculation reduces with implementation of new numerical techniques like the one from Scheufler & Roenby (Accurate and efficient surface reconstruction from volume fraction data on general meshes) and the two solvers produce equal solutions. The question I have is does anybody know why surface tension is implemented in such way? Any literature on surface tension terms in momentum equation in mixture model would be much appreciated. Cheers tom_flint2012, missios and yikui like this.

October 31, 2018, 22:26	interFoam	#3
vivek05 Member Vivek Join Date: Mar 2018 Location: India Posts: 54 Rep Power: 8	Hi dzordz & Michael Alletto I am also simulating liquid jet breakup using interFoam solver. In my case, the liquid jet is not even showing any sign of breakup, but small oscillation or perturbation are happening at the liquid jet surface. I don't know exactly what causes this problem. I tried with different mesh size. Could anyone help to find out this problem? Thank you,

December 22, 2021, 02:57		#4
Zhicheng YUAN New Member Zhicheng YUAN Join Date: Dec 2021 Posts: 2 Rep Power: 0	Form my point of view, MFIF can be used for a system more than three fluids. If only two phases are present in a cell, then $\nabla \alpha_1 = - \nabla \alpha_2$. With \alpha_1=1-\alpha_2, we will get the equation used by interFOAM. guin likes this. Last edited by Zhicheng YUAN; December 22, 2021 at 04:17.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
How to add Surface Tension in cavitatingFoam solver	jamestangx	OpenFOAM Programming & Development	1	April 6, 2016 16:39
Surface tension Interfoam	nb977	OpenFOAM Running, Solving & CFD	1	March 9, 2016 03:02
Help!! customize surface tension term in interFoam	w051cxw	OpenFOAM Running, Solving & CFD	0	February 12, 2016 01:15
interface tension question with interFoam solver	openTom	OpenFOAM Running, Solving & CFD	4	May 29, 2009 13:18
Modeling Free Surface Flows	Elliot Schwartz	Main CFD Forum	5	August 25, 1998 21:03

October 30, 2018, 08:00		#2
mAlletto Senior Member Michael Alletto Join Date: Jun 2018 Location: Bremen Posts: 615 Rep Power: 15	There are two references in https://openfoamwiki.net/index.php/InterFoam which i found usefull.