# Closed Domain Buoyancy Flow Problem

 Register Blogs Members List Search Today's Posts Mark Forums Read June 10, 2016, 08:38 Closed Domain Buoyancy Flow Problem
#1
New Member

Join Date: Jan 2016
Location: India
Posts: 14
Rep Power: 9 I am modelling the cooling of Nitrogen gas by a cryocooler. The cryocooler body has not been modelled separately. Its been considered as a part of outer Stainless Steel vessel. The fluid domain is closed and the flow occurs only due to the density variation of the fluid. The gas is contained in a Stainless Steel vessel. I have made half geometry and given symmetry condition to reduce the computation time. The cold end of the cryocooler is at 150 K temperature. The outer walls are exposed to atmosphere at 300 K temperature. The geometry is 3D and the cut section is shown in attachment. Meshing was done in ICEM CFD. (Delaunay mesh with 3 prism layers).

I have the experimental data with me regarding the temperature at certain points and I need to verify the same using the simulations. But the problem is that I dont seem to observe any temperature field development in the fluid domain after running the simulation. The residuals also dont go below 1E-4. I am attaching the images of geometry, mesh, results, residuals and also CCL. Kindly help me.

LIBRARY:
MATERIAL: Air Ideal Gas
Material Description = Air Ideal Gas (constant Cp)
Material Group = Air Data,Calorically Perfect Ideal Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Molar Mass = 28 [kg kmol^-1]
Option = Ideal Gas
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 1.0044E+03 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0. [J/kg]
Reference Specific Entropy = 0. [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 2.61E-2 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 0.01 [m^-1]
Option = Value
END
SCATTERING COEFFICIENT:
Option = Value
Scattering Coefficient = 0.0 [m^-1]
END
REFRACTIVE INDEX:
Option = Value
Refractive Index = 1.0 [m m^-1]
END
END
END
MATERIAL: Steel
Material Group = CHT Solids, Particle Solids
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 7854 [kg m^-3]
Molar Mass = 55.85 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 4.34E+02 [J kg^-1 K^-1]
END
REFERENCE STATE:
Option = Specified Point
Reference Specific Enthalpy = 0 [J/kg]
Reference Specific Entropy = 0 [J/kg/K]
Reference Temperature = 25 [C]
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 60.5 [W m^-1 K^-1]
END
END
END
END
FLOW: Flow Analysis 1
SOLUTION UNITS:
Length Units = [m]
Mass Units = [kg]
Solid Angle Units = [sr]
Temperature Units = [K]
Time Units = [s]
END
ANALYSIS TYPE:
EXTERNAL SOLVER COUPLING:
Option = None
END
END
DOMAIN: Fluid
Coord Frame = Coord 0
Domain Type = Fluid
Location = FLUID
BOUNDARY: Cold End Fluid
Boundary Type = WALL
Location = COLD_END_1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Fixed Temperature = 151.47 [K]
Option = Fixed Temperature
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Default Fluid Solid Interface Side 1
Boundary Type = INTERFACE
Location = CRYO_WALLS_1,FLUID_BOTTOM_2,FLUID_WALL_2,Primitive \
2D,Primitive 2D B
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Fluid Symmetry
Boundary Type = SYMMETRY
Location = FLUID_SYMMETRY
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1.69335 [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
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
FLUID DEFINITION: Fluid 1
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = Total Energy
END
Option = None
END
TURBULENCE MODEL:
Option = SST
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Automatic
END
END
INITIALISATION:
Option = Automatic
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
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = 1 [bar]
END
TEMPERATURE:
Option = Automatic with Value
Temperature = 300 [K]
END
TURBULENCE INITIAL CONDITIONS:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
END
DOMAIN: Metal
Coord Frame = Coord 0
Domain Type = Solid
Location = STEEL
BOUNDARY: Cold End Metal
Boundary Type = WALL
Location = COLD_END_2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Fixed Temperature = 151.47 [K]
Option = Fixed Temperature
END
END
END
BOUNDARY: Default Fluid Solid Interface Side 2
Boundary Type = INTERFACE
Location = CRYO_WALLS_2,FLUID_BOTTOM_1,FLUID_WALL_1,Primitive 2D \
A,Primitive 2D C
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Metal Symmetry
Boundary Type = SYMMETRY
Location = METAL_SYMMETRY
END
BOUNDARY: Outer Walls
Boundary Type = WALL
Location = OUTER_WALLS
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Fixed Temperature = 300 [K]
Option = Fixed Temperature
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 = 300 [K]
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
Option = None
END
END
END
DOMAIN INTERFACE: Default Fluid Solid Interface
Boundary List1 = Default Fluid Solid Interface Side 1
Boundary List2 = Default Fluid Solid Interface Side 2
Interface Type = Fluid Solid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = None
END
HEAT TRANSFER:
Option = Conservative Interface Flux
HEAT TRANSFER INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = None
END
END
MESH CONNECTION:
Option = Automatic
END
END
OUTPUT CONTROL:
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = First Order
Option = Upwind
END
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 5000
Minimum Number of Iterations = 1
Solid Timescale Control = Auto Timescale
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END
CONVERGENCE CRITERIA:
Residual Target = 1.E-4
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = Yes
END
END
END
COMMAND FILE:
Version = 15.0
Results Version = 15.0
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = Off
END
INTERPOLATOR STEP CONTROL:
Runtime Priority = Standard
DOMAIN SEARCH CONTROL:
Bounding Box Tolerance = 0.01
END
INTERPOLATION MODEL CONTROL:
Enforce Strict Name Mapping for Phases = Off
Mesh Deformation Option = Automatic
Particle Relocalisation Tolerance = 0.01
END
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: profmdatreypc
Remote Host Name = PROFMDATREY-PC
Host Architecture String = winnt-amd64
Installation Root = C:\Program Files\ANSYS Inc\v%v\CFX
END
END
PARTITIONER STEP CONTROL:
Multidomain Option = Independent Partitioning
Runtime Priority = Standard
EXECUTABLE SELECTION:
Use Large Problem Partitioner = Off
END
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
END
END
RUN DEFINITION:
Run Mode = Full
Solver Input File = E:\Prathamesh\Cavity\Simulation 94.2.def
INITIAL VALUES SPECIFICATION:
INITIAL VALUES CONTROL:
Continue History From = Initial Values 1
Use Mesh From = Solver Input File
END
INITIAL VALUES: Initial Values 1
File Name = E:\Prathamesh\Cavity\Simulation 94.2_002.res
Option = Results File
END
END
END
SOLVER STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARALLEL ENVIRONMENT:
Number of Processes = 1
Start Method = Serial
END
END
END
END
Attached Images Geometry.jpg (38.6 KB, 42 views) Mesh.jpg (117.3 KB, 40 views) Temperature Contour.jpg (167.0 KB, 35 views) Velocity Vector.jpg (49.5 KB, 31 views) Residuals.png (17.8 KB, 36 views)   June 10, 2016, 18:06 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,487 Rep Power: 140    FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria Also, I suspect you need to run this model for longer physical time to get the temperature field to develop.   June 11, 2016, 05:04 #3 New Member   Prathamesh Phadke Join Date: Jan 2016 Location: India Posts: 14 Rep Power: 9 Thanks ghorrocks! I will try to implement your suggestions and will report back which works.    June 20, 2016, 13:51 #4 New Member   Prathamesh Phadke Join Date: Jan 2016 Location: India Posts: 14 Rep Power: 9 I was doing a pretty stupid mistake. The mesh was not scaled properly. It was created in millimetres but imported as metres. Thats why the temperature field was not developing.   June 20, 2016, 14:01 #5
New Member

Join Date: Jan 2016
Location: India
Posts: 14
Rep Power: 9 Now that the temperature field is developing. There is one more problem. The geometry and boundary conditions are axis symmetric. I have converged the solutions till 1e-5. But the temperature field developed is not axis symmetric. It should be symmetric . I dont know what is causing this. I tried different mesh size to check whether it was mesh size issue. I also switched from delaunay mesh to octree mesh to check whether that affects. The developed temperature profile shifts randomly to left or right as shown in attached pictures. Kindly help me how do I get it to be close to symmetric.
Attached Images Run 2 octree_001.jpg (177.4 KB, 35 views) Run 3 octree_001.jpg (174.8 KB, 25 views) Run 4 octree_001.jpg (170.0 KB, 21 views) Run 5 octree_001.jpg (177.0 KB, 21 views)   June 20, 2016, 20:40 #6
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,487
Rep Power: 140    Quote:
 It should be symmetric . I dont know what is causing this.
Why should it be symmetric? Fluid mechanics often generates non-symmetric flow fields from symmetric geometries. Have a look at plumes, vortex streets and even turbulence. None of them are symmetric flows despite the simple geometry.

The images you show are the flow field I would expect in this configuration. It means that the flow is 3D transient, and not 2D axisymmetric steady state as the geometry might suggest.   June 20, 2016, 21:05 #7 New Member   Prathamesh Phadke Join Date: Jan 2016 Location: India Posts: 14 Rep Power: 9 Thanks Glen for your quick reply! Maybe my expectations for the field to be symmetrical are wrong. I have modelled the problem as 3D steady case. Now I will go for 3D Transient and see what happens to the field with respect to time. I will reply back what happens if it helps others.  Thread Tools Search this Thread Show Printable Version Email this Page Search this Thread: Advanced Search Display Modes Linear Mode Switch to Hybrid Mode Switch to Threaded Mode 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules Similar Threads Thread Thread Starter Forum Replies Last Post Nicole OpenFOAM Running, Solving & CFD 1 March 12, 2019 21:24 mukut OpenFOAM Meshing & Mesh Conversion 0 June 2, 2014 06:19 Mavier CFX 5 April 29, 2013 00:00 sunilpatil CFX 8 April 26, 2013 07:00 [DesignModeler] Flow Domain of DesignModeler swiss_zhang ANSYS Meshing & Geometry 0 June 9, 2011 07:13

All times are GMT -4. The time now is 01:53.