CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Heat Transfert, mixing problem

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 2, 2016, 06:51
Default Heat Transfert, mixing problem
  #1
New Member
 
Antoine
Join Date: Aug 2016
Posts: 6
Rep Power: 8
Wazdq is on a distinguished road
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 = 70C) and inside I have 3 coils with water inside (T = 20C). (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
Attached Images
File Type: png Capture2.PNG (30.9 KB, 16 views)
File Type: png CFX 8.png (134.4 KB, 16 views)
Wazdq is offline   Reply With Quote

Old   November 2, 2016, 18:00
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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?
ghorrocks is offline   Reply With Quote

Old   November 3, 2016, 05:48
Default
  #3
New Member
 
Antoine
Join Date: Aug 2016
Posts: 6
Rep Power: 8
Wazdq is on a distinguished road
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 23C and I have created the oil like a liquid and its temperature is between 67 and 70C. 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.

Last edited by Wazdq; November 3, 2016 at 08:30.
Wazdq is offline   Reply With Quote

Old   November 3, 2016, 17:22
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Quote:
I've checked and I don't think that I have a multiphase problem. The temperature of the water is between 20 and 23C and I have created the oil like a liquid and its temperature is between 67 and 70C. Except if I am wrong, no Problem of condensation or boiling.
OK, good. So it looks like you have single phase water and single phase oil.

Quote:
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 ?
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.
ghorrocks is offline   Reply With Quote

Old   November 4, 2016, 09:37
Default
  #5
New Member
 
Antoine
Join Date: Aug 2016
Posts: 6
Rep Power: 8
Wazdq is on a distinguished road
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
Attached Images
File Type: png CFX 8.png (188.2 KB, 6 views)
File Type: png CFX 81.png (189.0 KB, 6 views)
Wazdq is offline   Reply With Quote

Old   November 5, 2016, 05:39
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   November 6, 2016, 09:40
Default
  #7
New Member
 
Antoine
Join Date: Aug 2016
Posts: 6
Rep Power: 8
Wazdq is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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
Wazdq is offline   Reply With Quote

Old   November 6, 2016, 19:24
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   November 7, 2016, 06:44
Default
  #9
New Member
 
Antoine
Join Date: Aug 2016
Posts: 6
Rep Power: 8
Wazdq is on a distinguished road
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
Wazdq is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Error - Solar absorber - Solar Thermal Radiation MichaelK CFX 12 September 1, 2016 06:15
Problem with snGrad() for heat flux. SKLee OpenFOAM Programming & Development 4 March 4, 2014 23:46
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 08:00
Heat transfer problem in ansys please help me please...!!!!!!! rm2052 CFX 1 March 14, 2010 18:51
Ansys CFX10: multiphase reaction heat problem CFDS CFX 1 September 21, 2006 00:09


All times are GMT -4. The time now is 11:20.