CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   How to define the interface between two fluids (

TfG April 25, 2009 07:10

How to define the interface between two fluids

I am trying to model a tank which is half filled. Due to higher density water is is the fluid at the bottom part of the tank and air is above the water. I am simulating natural convection.

What I want to do is that at the interface the velocities of the air and water are the same in the plane of the interface but cannot penetrate one fluid in the other (i.e. normal velocity is zero). Also I want to set continuity of the heat transfer between the two fluids.

How should I model it? I did the mesh and I asig different fluids to each part, but I do not know how to model the interface. I tried with "interior" but it does not seem to work ( I get divergence and very strange patterns at the interface).

I would appreciate if somebody could help me with this,

thanks in advance

-mAx- April 25, 2009 09:36

Create two separated fluid volumes (connected), don't set any BC at the interface.
Once your model is set, then you initialize the whole domain, and you patch each one with the right vof-value.
Regarding the non-penetration, I think it should be done in the phase panel (interaction), but I am not sure

Ralf Schmidt April 25, 2009 10:13

take care, that between both fluids is only one face!!
If you have two volumes, that are simply attached to each other, and you define (one) interface at interior (or whatever else) Fluent will create a wall for that other interface!!

You can assure that by using in the face command field the "connect faces" button (looks like a plug). Select (all) faces of your domain and connect. That will cause all superposed faces to be joined.


-mAx- April 25, 2009 10:18


Originally Posted by Ralf Schmidt (Post 214157)
If you have two volumes, that are simply attached to each other, and you define (one) interface at interior (or whatever else) Fluent will create a wall for that other interface!!

If you split one volume into two volumes, the "interface" between the 2 volumes (connected) will be set automatically as interior (or internal).
It will set as wall, if the 2 volumes aren't connected (eg: 2 surfaces superposed)

TfG April 25, 2009 11:18

That is what I did, dont set any boundary at the interface (i.e. the same as to set interior condition). And yes, the faces were connected.

Are you suggesting me that I should use VOF model? Isn't any possibilitie to do it without it?


-mAx- April 25, 2009 12:01

I don't see other possibility else than multiphase (but I am not expert).
I did a similar calculation with a tank filled at the 2/3 with oil, and the rest with air, but without convection.
I solved it with multiphase

TfG April 25, 2009 14:23

Tried the VOF model and patch like you said but I get and error at the beginning of the second iteration:
Updating solution at time level N...
Global Courant Number : 560.10

Error: Global courant number is greater than 250.0. The
velocity field is probably diverging. Please check the solution
and reduce the time-step if necessary.
Error Object: ()

The no penetration thing I didn`t find anywhere....

-mAx- April 25, 2009 15:58

Go to the interaction panel

TfG April 26, 2009 05:45

I already did it, and defined my two phases (oil and air)... but, then in interaction there are only available two tabs to edit: Mass and Surface tension.... and nothing about no penetration.
I am pretty lost now... and I need this thing for my final project!

-mAx- April 26, 2009 05:51

on the 6.3 version there are more options like slip velocity between phases etc...

TfG April 26, 2009 06:55

Yes yes, Im running 6.3.26 and I have those tabs, but it says: this page is not applicable under current settings...

-mAx- April 26, 2009 07:01

Then check the help, maybe those tabs aren't available with multiphase.
Try mixture model.
But as I said, I am not expert

suryawanshi_nitin April 27, 2009 03:12

Dear friend
if u want to see only convection then make that interface to wall type in preprocessor and then import those two seperate volumes to fluen and to that wall & its shadow give 0 shear stress in x y & z direction so that proper convection pattern will form at interface (i.e wall) & model density with boussinesq model

regards Nitin

TfG April 27, 2009 04:31


Thanks for the answers, I will try that one.

Only two observations, first, on thermal boundaries I shoul set coupled right?
Second, I see shear stress 0 could be a reasonable assumption for the part of water. But for the air, shouldn't it be more like a non-slip condition (the air will have it difficult to "move" the water (forgetting waves...))?

Just wondering about it, but I am not expert so I may follow your advice and set shear 0 for both sides...

suryawanshi_nitin April 29, 2009 07:12

yes u r right but this will give u proper convection velocity pattern for heat transfer near the inerface (avoiding no slip on both sides of interface wall.
have u tried this??

Thank you

TfG April 29, 2009 13:29

Yes I tried with slip condition in both side and it seems to work fine, Thanks!

Still, do you think I should mantain lip conditions in the air part or no slip conditions?

suryawanshi_nitin April 30, 2009 01:02

with slip on air side will disturb ur convectopn (velocity pattern on air side )
if u want to see this just ceck it out..


TfG May 3, 2009 10:49

I tried setting slip for water side and no-slip for air side and the heat transfer in the interface is smaller than if I set slip for both sides (about 20% less).

The question is which result is more "real"... ?

All times are GMT -4. The time now is 17:50.