[Madhatter92]

I am simulating the flow of gas closed in a pressure vessel due to cooling (Natural Convection). I am attaching the images of my geometry and mesh. I have chosen Steel as Solid Domain and Air Ideal Gas as the Fluid. In the Fluid Model, Buoyancy is switched on. I want to give the boundary condition that the cooler absorbs 9W of power at 80K at the Cold End. How can I apply this boundary condition?
I have done one simulation without giving the cooling power as the input and setting the boundary condition at the cold end as Isothermal 80K wall. Kindly help me.

CCL of simulation without cooling power:

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 = 28.96 [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:
Angle Units = [rad]
Length Units = [m]
Mass Units = [kg]
Solid Angle Units = [sr]
Temperature Units = [K]
Time Units = [s]
END
ANALYSIS TYPE:
Option = Steady State
EXTERNAL SOLVER COUPLING:
Option = None
END
END
DOMAIN: Cryocooler
Coord Frame = Coord 0
Domain Type = Solid
Location = CRYOCOOLER
BOUNDARY: Cold End
Boundary Type = WALL
Location = CRYOCOOLER_COLD_END_2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Fixed Temperature = 80 [K]
Option = Fixed Temperature
END
END
END
BOUNDARY: Cryocooler Default
Boundary Type = WALL
Location = CRYOCOOLER_INNER_WALL
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
END
END
BOUNDARY: Default Fluid Solid Interface in Cryocooler Side 1
Boundary Type = INTERFACE
Location = CRYOCOOLER_OUTER_WALL_1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Upper End
Boundary Type = WALL
Location = CRYOCOOLER_TOP_END_2
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
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
DOMAIN: Fluid
Coord Frame = Coord 0
Domain Type = Fluid
Location = FLUID
BOUNDARY: Default Fluid Solid Interface in Fluid Side 1
Boundary Type = INTERFACE
Location = CRYOCOOLER_OUTER_WALL_2,Primitive 2D,Primitive 2D \
B,Primitive 2D D,Primitive 2D N,Primitive 2D O,Primitive 2D \
P,Primitive 2D Q
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 Default
Boundary Type = WALL
Location = CRYOCOOLER_COLD_END_1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Fixed Temperature = 80 [K]
Option = Fixed Temperature
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1.1416 [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 = Thermal Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
Option = Scalable
END
END
END
DOMAIN: Metal
Coord Frame = Coord 0
Domain Type = Solid
Location = METAL
BOUNDARY: Default Fluid Solid Interface in Metal Side 1
Boundary Type = INTERFACE
Location = Primitive 2D A,Primitive 2D C,Primitive 2D G,Primitive 2D \
J,Primitive 2D K,Primitive 2D L,Primitive 2D M
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Metal Default
Boundary Type = WALL
Location = Primitive 2D H,Primitive 2D I
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
END
END
BOUNDARY: 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
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
DOMAIN INTERFACE: Default Fluid Solid Interface
Boundary List1 = Default Fluid Solid Interface in Cryocooler Side \
1,Default Fluid Solid Interface in Metal Side 1
Boundary List2 = Default Fluid Solid Interface in Fluid Side 1
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
OUTPUT CONTROL:
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = First Order
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 500
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 = On
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
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: prathameshpc
Remote Host Name = PRATHAMESH-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:\Study\M.Tech. Project\10-12-2015 \
Simulation\Simulation 3.0.0\Simulation 3.0.0.def
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

[ghorrocks]

A good clear question. Thank you for spending the time to write a good question.

You are modelling this as a steady state simulation. If you wish to do this you will need to use a solid time scale factor to accelerate convergence in the solid domain. But you will probably have problems with this and will require a transient simulation to get convergence. Natural convection simulations usually do not have a steady state answer (even if the conditions are steady state).

Also:
You are using air but say you are modelling nitrogren. The difference is small but it is easy to correct so you might as well. Use the molecular weight, Cp and thermal conductivity of nitrogen. Also note that as you are at cryogenic temperatures the room temperature values in CFX by default will be a long way off.

Also note that steel material properties vary quite a bit over these temperature ranges too. As the steel ranges in temperature from 80K to 300K you probably want a variable properties model to be accurate over this wide range.

You are using k-e turbulence model. I would recommend SST as the general purpose turbulence model instead of k-e. But it is your choice, there probably won't be much difference.

You are using a thermal energy model for the fluid. This will not take into account effects do to the gas expanding and contracting. In other words, to model the fluid as an ideal gas you will need to use the "Total Energy" heat transfer model.

What controls the pressure of this device? Is it kept at 1 bar pressure, or does it increase or decrease from there as the device is sealed and the gas wants to expand or contract?

[Madhatter92]

Thanks for the reply!

What controls the pressure of this device? Is it kept at 1 bar pressure, or does it increase or decrease from there as the device is sealed and the gas wants to expand or contract?

The gas is filled in the container at 1 atm pressure and then the container is sealed. Then the gas expands or contracts according to its temperature.

You are using air but say you are modelling nitrogren. The difference is small but it is easy to correct so you might as well. Use the molecular weight, Cp and thermal conductivity of nitrogen. Also note that as you are at cryogenic temperatures the room temperature values in CFX by default will be a long way off.

In one of my previous simulations I did use Nitrogen as the Fluid but did not find much difference in the result because air is about 70% N2. About the cryogenic properties of the fluid, my results show that the average bulk temperature of the fluid is about 200K. Thus I thought that the default properties would be ok.

From your reply I got the following which I had not considered previously:
1. To model the properties of Steel as temperature dependent
2. To use SST model for turbulence
3. To use Total energy model for fluid
4. To Model the problem as a transient problem.

I am attaching the temperature contour and Velocity Vector plot I got in the previous simulation. I will make the modifications suggested by you and again run the simulation and check whether the results vary.

The problem is I expected the temperatures to be much lower (just by intuition) which they are not. So I am rechecking by boundary conditions. Because one thing which I did not include in the previous simulation was the cooling power of the cooler (9 W at 80K). I dont know how to apply this boundary condition at the cold end.

Thanks for your help in advance!!

[Opaque]

Regarding your concern with the boundary condition for the cooler. Mathematically, it is not possible to enforce both conditions simultaneously for the energy equation. Either you model using a temperature specified condition, say 80 [K], or heat flux specified, say 9 [W] / area()@boundary.

Once either of the two cases has converged, you can check if the non-enforced condition has been met, or how far off the conditions are from the expected value.

Hope the above helps,

[ghorrocks]

And your mesh has no inflation layers are these will be necessary accurate results. But I would do all the basic model development on the coarse mesh you already have, and once that is working well you can refine your mesh to get the accuracy you require.

[evcelica]

Looks like you are doing a cryocooler's cold head? And have been told 9W at 80K is the operational point?

These Cryocoolers have a performance curve, for example, it may do 10W at 90K, and 8W at 70K. What I've done in the past is put this curve in as a function of temperature.

If you find this curve, You can write an expression that describes its cooling power and input it.
You can do a convective boundary condition with a heat transfer coefficient that is a function of temperature, or a heat flux or anything else that accurately represents it.

[Madhatter92]

Thank you Opaque for your insight. I will apply the boundary condition as suggested by you and evcelica.

[Madhatter92]

Originally Posted by ghorrocks

And your mesh has no inflation layers are these will be necessary accurate results. But I would do all the basic model development on the coarse mesh you already have, and once that is working well you can refine your mesh to get the accuracy you require.

Thanks for your suggestion. That is what I was planning. To get proper results on coarse mesh first then go for accuracy. I still dont know how to create inflation layers properly. But I will read about it and try it once my initial settings of the problem are correct.

[Madhatter92]

Originally Posted by evcelica

Looks like you are doing a cryocooler's cold head? And have been told 9W at 80K is the operational point?

These Cryocoolers have a performance curve, for example, it may do 10W at 90K, and 8W at 70K. What I've done in the past is put this curve in as a function of temperature.

If you find this curve, You can write an expression that describes its cooling power and input it.
You can do a convective boundary condition with a heat transfer coefficient that is a function of temperature, or a heat flux or anything else that accurately represents it.

Yes I am simulating the cooling of gas due to cryocooler. It is a coaxial stirling pulse tube cryocooler. We have the cryocooler in our lab and I can get its Cooling Power vs Temperature data.

What I did not get is -
I dont know the value of heat transfer coefficient or any equations which can be applied at the cold end of the cryocooler. So can you guide me about it? (I dont want the exact equation but a little guidance about applying the convective boundary condition)

Thanks for your help

[ghorrocks]

You do not need to define a heat transfer boundary condition at the cooler. As this is a solid/fluid simulation the simulation will automatically work out the heat transfer conditions for the interface. This assumes the cooler acts on the solid domain, not the fluid domain.

[Madhatter92]

Originally Posted by ghorrocks

You do not need to define a heat transfer boundary condition at the cooler. As this is a solid/fluid simulation the simulation will automatically work out the heat transfer conditions for the interface. This assumes the cooler acts on the solid domain, not the fluid domain.

I want to cool the gas, not the solid. I mean the solid is supposed to be cooling the gas.

[ghorrocks]

Yes, that is what I am talking about. The cooler acts on the steel and the heat is conducted through the steel from the hot fluid to the cooler. In this case you do not need to define a boundary condition at the steel/fluid interface as it is an internal interface.

The cooler face on the steel should probably be modelled as a heat flux (an option under wall boundaries), with a performance curve against temperature as previously mentioned.

[Madhatter92]

Ok. I understood now. Thanks a lot. I will do the same.