|
[Sponsors] |
October 24, 2017, 10:52 |
buoyancy Multiphase with Opening
|
#1 |
New Member
anon
Join Date: Oct 2017
Posts: 10
Rep Power: 8 |
Dear all,
I got trouble with a transient multiphase case (continueous domains). It includes - air (top) - cold water (middle) separated through a narrow gap from - hot water (bottom) air and water are different domains with a free surface in between. The hot water should mix up with the cold water and then heat up the air (there is also CHT around, but not interesting for the specific problem). Buoyancy is activated. With a closed volume everything is working fine but I do not want to cool down the hot water (represents a big domain where temperature change is negligible). Thus, I defined an opening at the bottom. The opening relative pressure is zero and the temperature is equal to the hot water temperature. Now, hot water flows back in and temperature stays constant. BUT the interface between air and cold water domain moves down, means the water level decreases. Of course, gravity does his job. Is there any trick to avoid this or can anyone recommend another workaround? |
|
October 24, 2017, 10:53 |
|
#2 |
New Member
anon
Join Date: Oct 2017
Posts: 10
Rep Power: 8 |
Code:
BOUNDARY: Opening Boundary Type = OPENING Interface Boundary = Off Location = F1049.1034 BOUNDARY CONDITIONS: FLOW DIRECTION: Option = Normal to Boundary Condition END FLOW REGIME: Option = Subsonic END HEAT TRANSFER: Opening Temperature = 98 [K] Option = Opening Temperature END MASS AND MOMENTUM: Option = Opening Pressure and Direction Relative Pressure = 0 [Pa] END END FLUID: Steam BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 0 END END END FLUID: Water BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 1 END END END END DOMAIN MODELS: BUOYANCY MODEL: Buoyancy Reference Density = 1 [kg m^-3] Gravity X Component = 0 [m s^-2] Gravity Y Component = -9.81 [m s^-2] Gravity Z Component = 0 [m s^-2] Option = Buoyant BUOYANCY REFERENCE LOCATION: Option = Automatic END END REFERENCE PRESSURE: Reference Pressure = 1 [atm] END END FLUID DEFINITION: Steam Material = Air Ideal Gas Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID DEFINITION: Water Material = Water Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID: Steam FLUID BUOYANCY MODEL: Option = Density Difference END END FLUID: Water FLUID BUOYANCY MODEL: Option = Density Difference END END HEAT TRANSFER MODEL: Homogeneous Model = True Option = Thermal Energy END TURBULENCE MODEL: Option = Laminar END END FLUID PAIR: Steam | Water INTERPHASE TRANSFER MODEL: Option = Free Surface END MASS TRANSFER: Option = None END SURFACE TENSION MODEL: Option = None END END |
|
October 24, 2017, 10:55 |
|
#3 |
New Member
anon
Join Date: Oct 2017
Posts: 10
Rep Power: 8 |
Maybe the picture helps to understand the problem. Displayed is the volume fraction of water. Over time it gets much worse.
|
|
October 24, 2017, 11:00 |
|
#4 |
New Member
Shrirang
Join Date: May 2016
Location: India
Posts: 18
Rep Power: 10 |
Why did you give an opening boundary condition?
How about defining the lower wall as wall with the hot water temperature? |
|
October 24, 2017, 11:05 |
|
#5 |
New Member
anon
Join Date: Oct 2017
Posts: 10
Rep Power: 8 |
Yep tried that as well. But only helped a little. In the end I had stratified water in the big volume (hot water has 98C and cold has 20C). Maybe I could define a wall heat flux depending on the average temperature in the hot volume but still it is not well distributed.
|
|
October 24, 2017, 11:11 |
|
#6 |
New Member
Shrirang
Join Date: May 2016
Location: India
Posts: 18
Rep Power: 10 |
Defining wall with the hot temperature should satisfy your need, as it is similar to having a fluid layer of that temperature at that position neglecting buoyancy.
|
|
October 24, 2017, 11:12 |
|
#7 | |
New Member
anon
Join Date: Oct 2017
Posts: 10
Rep Power: 8 |
Quote:
I am open for other ideas. I could also make the hot volume veeery big but i try to avoid this due to model size reasons. |
||
October 24, 2017, 11:19 |
|
#8 | |
New Member
anon
Join Date: Oct 2017
Posts: 10
Rep Power: 8 |
Quote:
Dont be confused by the additional temperature profiles in th solids and the slightly different geometry (top right and left). |
||
October 24, 2017, 11:35 |
|
#9 |
New Member
Shrirang
Join Date: May 2016
Location: India
Posts: 18
Rep Power: 10 |
You said that the hot water is a big domain physically. Is it modelled of the same scale?
If the cold water domain is very small in size, you wouldn't need any additional heat source other than initializing at high temperature. Are the size of domain in the simulation exactly scaled from the physical one you want to compare? |
|
October 25, 2017, 01:32 |
|
#10 |
New Member
anon
Join Date: Oct 2017
Posts: 10
Rep Power: 8 |
Nope. The warm zone is just a tiny part of the real volume. I only look at a small detail of the construction. Sure, I could make it bigger but I guess the problem would still persist.
|
|
October 25, 2017, 02:06 |
|
#11 |
New Member
Shrirang
Join Date: May 2016
Location: India
Posts: 18
Rep Power: 10 |
You can just have a quick hand calculation for energy balance before and after mixing and get an idea how much temperature to expect.
|
|
October 25, 2017, 07:32 |
|
#12 |
New Member
anon
Join Date: Oct 2017
Posts: 10
Rep Power: 8 |
Got a solution, at least for the next steps. I stop Mass and Momentum transfer over the interface from water to air and allow only thermal interface flux. Thus, it behaves like a wall.
Actually, I wanted to have evaporation and condensation in a later state of the model as well. So for that I need the interface flux and I will have to come back to problem. But for now, this should be fine. Btw: I also tried it with a heat source as function of warm water average temperature. But it is not mixing up perfectly. |
|
October 25, 2017, 11:55 |
|
#13 |
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14 |
Tips:
1) Solve the momentum and turbulence equations as homogeneous, but the energy equation as inhomogeneous. 2) For a better result switch everything (except turbulence) to inhomogeneous 3) The free surface sharpness is mesh dependent - refine the mesh where you expect the free surface to be 4) Make sure you're using the correct interfacial area density. If you get bubbly or droplet flow use the particle model. If it's all stratified use the free surface model. If its both then use the mixture model and define your own interfacial area density. 5) Couple volume fractions to the momentum and continuity equations for greater stability. This option is in solver control. 6) Use a specified blend factor of 1 as opposed to high resolution. 7) Thermal time scales are longer than molecular time scales. Freeze the flow fields and only solve the energy equation first to accelerate solution convergence. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Opening boundary condition for multiphase analysis in CFX | shivasluzz | CFX | 3 | May 15, 2015 09:49 |
Different buoyancy settings for multiphase flow | nga911 | CFX | 1 | August 14, 2014 06:44 |
Overflow Error in Multiphase Modelling with Two Continuous Fluids | ashtonJ | CFX | 6 | August 11, 2014 14:32 |
How to properly set up an opening in buoyancy driven problems | lavoz | CFX | 5 | July 23, 2014 06:06 |
Multiphase: Opening: prevent 1 Fluid of leaving the domain | m0h | CFX | 6 | November 23, 2013 10:17 |