Heat Transfert, mixing problem
 

Hello the CFD community !

I have a problem with a simple heat transfer. I have a pipe with oil going through the top to the bottom (T = 70°C) and inside I have 3 coils with water inside (T = 20°C). (See Picture)

I've followed the tutorial number 16 "Heat Transfert from a Heating Coil" part number 2 with the Dry Steam. Otherwise in my case I have 2 different fluids : Oil and Water.
I have created 2 Domains, 2 fluids (Oil and Water).
Fluid Models : Multiphase ->Homogeneous Model ; Heat Tranfer --> Homogeneous Model, Thermal Energy
Fluid Pair Models : Mass Tranfer --> None

Heat Tranfert with an Interface for the wall of the 3 coils. No Slip Wall, Heat Transfer : Conservative Interface Flux. Interface Model : Thin Material --> Steel --> 1 mm.
For my 2 inlets I did not forget to enter that I have only 1 fluid (ie volume fraction = 1).

First Problem, when I want to solve my Simulation, there is an error because there are 3 isolated fluid regions. I tried to figure out the Problem with DesignModeler by checking the Connection between the small pipes and the "U" but everything seems to be ok. (I merely used the tool Sweep with a circle and a "U" line)
So I decided to use expert Parameters to disable the control of isolated regions (maybe it is not a good idea but I wanted to have some results to figure out what could be the Problem).

Finally I have a result but there is material Transfer between oil and water (see Picture).

I hope I have well explained my Problem, tell me if not !
What do you think ? Is there something I forgot with the CFX file or is there a Problem with the geometry ? The error with the isolated Region is maybe not a small Problem...

Wazdq

I would recommend you activate the expert parameter to disable isolated volume checking. Then you should be able to set oil in the outer region and water in the inner region with no need for a multiphase model. Then you will not get problems with the fluids mixing.

Do you have any multiphase effects? Such as boiling, condensation, air bubbles, particles or anything like that?

Hello ghorrocks,

I've checked and I don't think that I have a multiphase problem. The temperature of the water is between 20 and 23°C and I have created the oil like a liquid and its temperature is between 67 and 70°C. Except if I am wrong, no Problem of condensation or boiling.

With regard to the Reynolds, I have calculated the velocity of the Oil and the Water in order that to have Re(W) = 2000 and Re(O)=1000 so between Turbulent and Laminar Regime. No air bubble I think or ?

Just for Information the velocity of the oil is 0.0039 m/s and the water is 0.0714 m/s. (the properties of the oil is not so different from the water but I would like later to increase the viscosity of the oil until 1000mPas).

I have changed a Parameters:
Domain : Fluid Pair Models : Interphase Transfer : Option --> None (instead of Mixture Model).
The result is different but I still have a mixture. "Good" point is : the maximum value of the water mass fraction in the outOil is 10^-6.

Wazdq

Edit : I have increased the Reynolds number for the Oil (1500) to see what could happen. Now the Maximum value of the water mass fraction in the OutOil is 10^-13. So maybe you were right and there was some air bubbles or something else during the simulation and the software tried to "fill" theses areas with water.

OK, good. So it looks like you have single phase water and single phase oil.

The Reynolds number tells you whether you are likely to be turbulent or not and nothing about air bubbles. For those Reynolds Numbers it does appear as if you are in the transitional regime. But you will have to find out whether bubbles are present from elsewhere.

My recommendation is to use the allow isolated volumes option and then use a different single phase model for water and oil. Then you do not need to use a multiphase model and will have no need to set multiphase parameters like interphase transfer option.

Hello ghorrocks,

I have followed your recommendation and I have used the laminar model for the Oil (I have changed the Reynolds number with 200) and k-eps model (I will use SST after) for the Water. I hope that it was what you wanted. There is still a mixing (The max volume fraction of the water in OutOil is 10^-8 and the max volume fraction of the oil in OutWater is 10^-2) but there is something interesting (see pictures).

I have used the tool Contour at the 3 Interfaces. One Picture is with the volume fraction of the water and the other is with the oil. As you can see at the beginning of the pipe the water is mix with the oil... I have checked the Table and my CFX file and I have entered that I have 0 for volume fraction of Oil in InWater.
The inlets are at the top right and it seems that there is a transfert between the wall (volume fraction = 1 for the oil at the bottom).
Therefore I do not know if it is a good or a bad things in the sense that maybe I entered something wrong in the CFX file or something else.

Wazdq

This is the third time I have said this: I recommend you activate the allow isolated volumes option and then specify a single phase fluid in the water and oil domain. If you don't understand what I am saying please say so.

Maybe I misunderstood what you wanted me to do, to allow isolated volumes option do I have to go to Expert Parameters and "disable the control of isolated regions" ?

If not, I am sorry I do not know how to allow this option. I would be glad if you help me !

Wazdq

I have not done this for a while, but I think the process is:
* set the disable isolated volumes check expert parameter
* define two fluids, one water, one oil
* You should now be able to use just water for one domain and just oil for the other domain. These are both single phase fluids, so there is no possibility of mixing.

Problem solved ! Two Domains with two differents fluids, so no mixing at all !

Thank you very much ghorrocks :)

I wish you a nice day/evening !

Wazdq