[Martin_D]

Hello everybody.
I am currently simulating natural convection of a multicomponent mixture (helium, air and water vapor) induced by heat sources inside a pressurized conatainment.
So far my results are quite unrealistic since it is evident that the fluids inside are mixing at a high rate due to gravitational/bouyancy effects. The natural convection that should occur due to mixture heating is miniscule so far.

I am using the k-epsilon model for turbulence modeling. I have also compared cases with different dissipation coefficients and different Schmidt numbers (1 and 100) but the results are still the same - rapid mixing and degradation of a helium cloud (positioned at the top of the vessel) due to fluid flow which is moving downward to fast.
I would like to know if anyone knows how can I manage the process of such rapid mixing?

Thank you all in advance.

[ghorrocks]

General points are covered in the FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Something is causing an unrealistically high fluid motion from your description. You have to look into the details of your setup to find it.

[Martin_D]

The mesh metrics are good. I have tried different settings in the buoyancy turbulence tab (production, production and dissipatin, changing values of Sc number and dissipation coefficient), advection and turbulence schemes. My timestep value varies from 0.05 to 0.04 s, which is sufficiently small since the fluid velocities are relatively small.

I have also made a similar mesh (extruded model whereas the main simulation is based on a cillindrical/revolved model). The mesh metrics are excellent. I have enabled buoyancy,changed intial conditions from standard room temperature and pressure to the same conditions that are given from the experiment. The results are similar then before. The helium cloud at the top of the room degrades and moves towards the floor within 10 seconds.

From this facts follows that the mesh is not the problem. The initial conditions that I have used are the same as those that were used in a different simulation but still calculating the same physical phenomenon.

[ghorrocks]

The mesh metrics are good.

Different types of simulation require different mesh quality to work. Making sweeping statements like this is dangerous.

My timestep value varies from 0.05 to 0.04 s, which is sufficiently small since the fluid velocities are relatively small.

Another frequently made comment which is usually wrong. Time step size should be set based on a sensitivity study, not by what you think is small enough.

Can you post an image of what you are modeling?

[Martin_D]

Thank you for your help so far but all the statements above are made based on the articles I have studied to make such a simulation. I am well aware that the end result of a simulation depends on multiple factors, settings, initial conditions etc.
But the main topic of the thread remains the same. What else could I change to make my simulation a bit more realistic?

[ghorrocks]

So far you have only provided general details about your simulation, so all I can do is give general suggestions. If you want more specific comments you will have to describe what you are modelling in more detail. Post an image and attach the CCL.

[Martin_D]

I am modeling natural convection (caused by a heat source) in a pressurized containment. To be more specific, I am researching the degradation of a helium cloud which is situated at the top of the containment volume.
Because I had difficulties with the original case I created a simple case of a room which has a wall surrounding it to see which settings in CFX-Pre are causing unrealistic results for my type of simulation. This case actually serves me as a sensitivity analysis to find out why the helium cloud degrades too fast (which is occurring in when using both grids). Within approx. 10 seconds the helium cloud deforms and falls to the bottom of the room/vessel. Experimental data (taken inside the vessel) shows that the helium cloud does not dissolve for about 100 seconds.

Grid: http://postimage.org/image/gy0fvmb6l/

CCL:
&replace FLOW: Flow Analysis 1
ANALYSIS TYPE:
Option = Transient
EXTERNAL SOLVER COUPLING:
Option = None
END
INITIAL TIME:
Option = Automatic with Value
Time = 0 [s]
END
TIME DURATION:
Option = Total Time
Total Time = 10 [s]
END
TIME STEPS:
Option = Timesteps
Timesteps = 0.05 [s]
END
END
DOMAIN INTERFACE: Default Fluid Fluid Interface
Boundary List1 = Default Fluid Fluid Interface Side 1 1
Boundary List2 = Default Fluid Fluid Interface in He atm Side 1
Filter Domain List1 = AirSteam atm
Filter Domain List2 = He atm
Interface Region List1 = F100.106
Interface Region List2 = F100.105
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = None
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = None
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: Default Fluid Solid Interface
Boundary List1 = Default Fluid Solid Interface in He atm Side 1,Default Fluid Solid Interface in VPZr Side 1
Boundary List2 = Default Fluid Solid Interface in zunanja stena Side 2
Filter Domain List1 = AirSteam atm,He atm
Filter Domain List2 = wall
Interface Region List1 = F101.105,F102.105,F98.106,F99.106
Interface Region List2 = F101.104,F102.104,F98.104,F99.104
Interface Type = Fluid Solid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = None
END
PITCH CHANGE:
Option = None
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN: AirSteam atm
Coord Frame = Coord 0
Domain Type = Fluid
Location = B106
BOUNDARY: Default Fluid Fluid Interface Side 1 1
Boundary Type = INTERFACE
Interface Boundary = On
Location = F100.106
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Default Fluid Solid Interface in VPZr Side 1
Boundary Type = INTERFACE
Interface Boundary = On
Location = F98.106,F99.106
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL CONTACT MODEL:
Option = Use Volume Fraction
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: gsk2zg
Boundary Type = WALL
Create Other Side = Off
Interface Boundary = Off
Location = F97.106
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL CONTACT MODEL:
Option = Use Volume Fraction
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: sim21
Boundary Type = SYMMETRY
Interface Boundary = Off
Location = sim21
END
BOUNDARY: sim22
Boundary Type = SYMMETRY
Interface Boundary = Off
Location = sim22
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 0.2 [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:
Cartesian Coordinates = 0.0[m],0.0[m],0.0[m]
Option = Cartesian Coordinates
END
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1.013 [bar]
END
END
FLUID DEFINITION: air
Material = Air at STP
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: helij
Material = He at STP
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: steam
Material = Water Vapour at 100 C
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: air
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
FLUID: helij
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
FLUID: steam
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
HEAT TRANSFER MODEL:
Homogeneous Model = On
Option = Total Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Homogeneous Model = On
Option = k epsilon
BUOYANCY TURBULENCE:
Option = Production
END
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Scalable
END
END
FLUID PAIR: air | helij
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
MOMENTUM TRANSFER:
DRAG FORCE:
Drag Coefficient = 0.44
Option = Drag Coefficient
END
END
END
FLUID PAIR: air | steam
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
MOMENTUM TRANSFER:
DRAG FORCE:
Drag Coefficient = 0.44
Option = Drag Coefficient
END
END
END
FLUID PAIR: helij | steam
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
MOMENTUM TRANSFER:
DRAG FORCE:
Drag Coefficient = 0.44
Option = Drag Coefficient
END
END
END
INITIALISATION:
Coord Frame = Coord 0
Option = Automatic
FLUID: air
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 1
END
END
END
FLUID: helij
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
FLUID: steam
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
INITIAL CONDITIONS:
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = 0.187 [bar]
END
TEMPERATURE:
Option = Automatic with Value
Temperature = Tzac
END
TURBULENCE INITIAL CONDITIONS:
Option = k and Epsilon
EPSILON:
Epsilon = 1e-06 [m^2 s^-3]
Option = Automatic with Value
END
K:
Option = Automatic with Value
k = 1e-06 [m^2 s^-2]
END
END
END
END
MULTIPHASE MODELS:
Homogeneous Model = False
FREE SURFACE MODEL:
Option = None
END
END
END
DOMAIN: He atm
Coord Frame = Coord 0
Domain Type = Fluid
Location = B105
BOUNDARY: Default Fluid Fluid Interface in He atm Side 1
Boundary Type = INTERFACE
Interface Boundary = On
Location = F100.105
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Default Fluid Solid Interface in He atm Side 1
Boundary Type = INTERFACE
Interface Boundary = On
Location = F101.105,F102.105
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL CONTACT MODEL:
Option = Use Volume Fraction
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: gsk1zg
Boundary Type = WALL
Create Other Side = Off
Interface Boundary = Off
Location = F103.105
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL CONTACT MODEL:
Option = Use Volume Fraction
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: sim11
Boundary Type = SYMMETRY
Interface Boundary = Off
Location = sim11
END
BOUNDARY: sim12
Boundary Type = SYMMETRY
Interface Boundary = Off
Location = sim12
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 0.2 [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:
Cartesian Coordinates = 0.0[m],0.0[m],0.0[m]
Option = Cartesian Coordinates
END
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1.013 [bar]
END
END
FLUID DEFINITION: air
Material = Air at STP
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: helij
Material = He at STP
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: steam
Material = Water Vapour at 100 C
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: air
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
FLUID: helij
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
FLUID: steam
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
HEAT TRANSFER MODEL:
Homogeneous Model = On
Option = Total Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Homogeneous Model = On
Option = k epsilon
BUOYANCY TURBULENCE:
Option = Production
END
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Scalable
END
END
FLUID PAIR: air | helij
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
MOMENTUM TRANSFER:
DRAG FORCE:
Drag Coefficient = 0.44
Option = Drag Coefficient
END
END
END
FLUID PAIR: air | steam
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
MOMENTUM TRANSFER:
DRAG FORCE:
Drag Coefficient = 0.44
Option = Drag Coefficient
END
END
END
FLUID PAIR: helij | steam
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
MOMENTUM TRANSFER:
DRAG FORCE:
Drag Coefficient = 0.44
Option = Drag Coefficient
END
END
END
INITIALISATION:
Coord Frame = Coord 0
Option = Automatic
FLUID: air
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
FLUID: helij
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 1
END
END
END
FLUID: steam
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
INITIAL CONDITIONS:
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = 0.187 [bar]
END
TEMPERATURE:
Option = Automatic with Value
Temperature = Tzac
END
TURBULENCE INITIAL CONDITIONS:
Option = k and Epsilon
EPSILON:
Epsilon = 1e-06 [m^2 s^-3]
Option = Automatic with Value
END
K:
Option = Automatic with Value
k = 1e-06 [m^2 s^-2]
END
END
END
END
MULTIPHASE MODELS:
Homogeneous Model = False
FREE SURFACE MODEL:
Option = None
END
END
END
DOMAIN: wall
Coord Frame = Coord 0
Domain Type = Solid
Location = B104
BOUNDARY: Default Fluid Solid Interface in zunanja stena Side 2
Boundary Type = INTERFACE
Interface Boundary = On
Location = F101.104,F102.104,F98.104,F99.104
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: sim31
Boundary Type = SYMMETRY
Interface Boundary = Off
Location = sim31
END
BOUNDARY: sim32
Boundary Type = SYMMETRY
Interface Boundary = Off
Location = sim32
END
BOUNDARY: wall Default
Boundary Type = WALL
Create Other Side = Off
Interface Boundary = Off
Location = F103.104,F97.104
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
END
END
BOUNDARY: zunanje stene
Boundary Type = WALL
Create Other Side = Off
Interface Boundary = Off
Location = zunanje stene
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
END
END
DOMAIN MODELS:
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
END
INITIALISATION:
Option = Automatic
INITIAL CONDITIONS:
TEMPERATURE:
Option = Automatic with Value
Temperature = Tzac
END
END
END
SOLID DEFINITION: Solid 1
Material = Steel
Option = Material Library
MORPHOLOGY:
Option = Continuous Solid
END
END
SOLID MODELS:
HEAT TRANSFER MODEL:
Option = Thermal Energy
END
THERMAL RADIATION MODEL:
Option = None
END
END
END
OUTPUT CONTROL:
RESULTS:
File Compression Level = Default
Option = Standard
END
TRANSIENT RESULTS: Transient Results 1
File Compression Level = Default
Include Mesh = No
Option = Selected Variables
Output Variables List = Absolute Pressure,helij.Total Density,helij.Total Temperature,helij.Velocity,helij.Velocity u,helij.Velocity v,helij.Velocity w,helij.Volume Fraction,helij.Vorticity
OUTPUT FREQUENCY:
Option = Timestep Interval
Timestep Interval = 5
END
END
END
SOLUTION UNITS:
Angle Units = [rad]
Length Units = [m]
Mass Units = [kg]
Solid Angle Units = [sr]
Temperature Units = [K]
Time Units = [s]
END
SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Maximum Number of Coefficient Loops = 5
Minimum Number of Coefficient Loops = 3
Timescale Control = Coefficient Loops
END
CONVERGENCE CRITERIA:
Residual Target = 1.E-4
Residual Type = RMS
END
TRANSIENT SCHEME:
Option = Second Order Backward Euler
TIMESTEP INITIALISATION:
Option = Automatic
END
END
END
END

[ghorrocks]

Some comments:

* Why is there a fluid fluid interface? This looks like it can be done as a single domain.
* Is this a CHT simulation as well? If you are looking at the mixing of the He cloud why does CHT matter?
* Shouldn't your gravity vector be y=-9.81 [m/s]? You seem to have gravity in the wrong direction.
* Are you sure this simulation is turbulent? Have you checked the relevant non-dimensional numbers?
* (This is a big mistake) You are modelling this as a multiphase model. But there is only a single phase, being gas. You should be modelling this as a multi-component mixture. Read the documentation on the definition of multiphase and multicomponent mixtures as the difference is critical - as you will find out when you try it.
* Why are you restricting it to 3-5 coeff loops per time step? Let it use a good number for a maximum and don't bother with a minimum.

[Martin_D]

1) Is there any other way to model the helium cloud?
(I was thinking about writing a CEL expression of the helium mass concentration/fraction distribution but so far my knowledge about CFX is poor.)

2) The main simulation involves a steel compartment (cylinder) inside the vessel. Also the outer walls of the containment are made of steel so I have to assume that a part of the heat energy gets stored in the walls and the cylinder. That is why I have to consider the calorific effects of the inner and outer structure.

3) Fixed the gravity

4) Over time natural convection is is expected to occur due to heating of the surfaces inside the vessel. Based on previous simulations made and research done on similar cases the flow that occurs is considered turbulent.

5) Looked at the tutorials (properly this time) and changed the settings.

6) I have chosen this setting based on the modeling guide in ANSYS help: "A value of 3 iterations per timestep should be sufficient for most single phase simulations, and values higher than 5 are unlikely to improve accuracy. In multiphase cases, the default value of 10 iterations per timestep may be more appropriate."

Here is the link for the actual mesh that I will be using: http://postimage.org/image/q2gjrz0l5/


Thank you very much for your help. I appreciate it.

[ghorrocks]

1) Yes. Model the entire fluid domain as a single domain. Then use a CEL expression to set the initial condition, using a function of space. For instance Helium.mass fraction=if(z>10[m],1.0,0.0) sets the mass fraction of He to 1.0 above z=10m.

2) If you are interested in heat effects then fair enough, model the casing.

3)

4) OK, if you know the flow is turbulent then model it as turbulent. But I would still work out the relevant non-dimensional numbers to determine if you are just turbulent or strongly turbulent. If you are just turbulent I would probably not use a turbulence model and use a laminar model. But if strongly turbulent I would use a turbulence model.

5) This will dramatically change the results. You are now saying molecular diffusion is the mixing process, rather than "particles" of one gas inside the other. Obviously this particle assumption is rubbish, and hence your initial results are totally wrong.

6) No, you have taken the doco comments the wrong way. You should use a min of 3 and a max of 5 as targets for adaptive time stepping, with limit values (which is what you set) of around 10 max and no minimum. Then the simulation will automatically find its time step size in the ideal range.

7) With regards your mesh: This looks like a 2D axisymmetric model, so try to generate the mesh to be a single element thick. It can be diffiicult to convince Workbench to do this sometimes (it does have a mind of its own for these things....), but it will significantly speed you simulation up if you do.

[Martin_D]

Mr. Horrocks,
thank you for the advice and especially you time for helping me out.
I have implemented (almost) all of the above settings in my simulation.

I have another question regarding the initial conditions and CEL expressions.
I have experimental values for the initial conditions for He mass fraction which vary with height. For example: from 5 to 6 meters the mass fraction goes from 0 to 0.005 and from 6 to 7 meters it goes from 0.005 to 0.095. What I would like to do is to implement this data or write a CEL expression that would describe the He mass fraction gradient as it is shown on the diagram in the picture:

http://postimg.org/image/y5ry85pfn/

Can I use a for loop in the CEL expression? I was going through the CEL manual but couldn't find any explanation or examples for such a case.

[ghorrocks]

CEL does not have for loops. Your function is easy to implement as a 1D interpolation function with height (y) as the input variable.

[oj.bulmer]

If you are are having problems of quality of mesh at the axis, you can chop off the edge at the axis. Often there are spurious results at the axis due to this bad quality zone. After chopping off the edge, there won't be a sharp corner and specify the resultant small wall as symmetry or free slip wall.

OJ

[Martin_D]

OJ I already did that at the beginning (which I forgot to mention)
Thanks for the heads up anyway.