[Nurzhan]

Hi Guys,

I am trying to set a thermal conductivity as a full tensor so it varies based on one of the directions (X, Y, and Z). In order to set a magnitude of the conductivity, I looked at material properties and changed the magnitude there. However, my conductivity is described by three functions of temperature, each function per direction.

I believe there is an easy way to do it, but I am failing to find the solution.

Could you please help me?

Cheers,
Nurzhan

[ghorrocks]

Use a CEL expression, interpolation function or junction box rountine.

[Opaque]

Based on the mathematical formalism for heat conduction, thermal conductivity cannot be a vector. It is a second order tensor, that for isotropic materials reduces to scalar.

In the case of anisotropic thermal conduction, ANSYS CFX has a hidden feature to input the orthotropic conductivities (principal values on a specific orientation of the material) , or the full tensor.

You can search this forum for "Thermal Conductivity X".. Otherwise, you should probably contact ANSYS CFX support for help.

Either of those values can be set using CEL expression, interpolation functions or via user Fortran junction boxes.

[Nurzhan]

Thank you very much for your responses!

Cheers,
Nurzhan

[Nurzhan]

Hi Glenn/Opaque,

I managed to set thermal conductivity as a full tensor using CEL as you advised me. However, the same way does not work for electrical conductivity.

The error looks like that:

ERROR
CCL validation failed with message:
Error: Invalid Option parameter 'Orthotropic Cartesian Components'

Any ideas how to get over this problem?

The feeling is like ANSYS intentionally stopping people to use electrical conductivity as a vector value. What do you think?

Thank you in advance!
Nurzhan

[ghorrocks]

Thermal conductivity is not a vector. Opaque explained that very well.

As the anisotropic thermal conductivity is a hidden feature that means it is not a supported feature. This means it has not completed all testing, may not be accurate or correctly implemented. For many of these cases it is because the introduction of this additional flexibility introduces additional terms into the modelled equations which CFX does not model. It is then user beware when you decide to use them.

So no, it is unlikely that ANSYS has removed anisotropic electrical conductivity. Why would they develop it then remove it? What is far more likely is that it can introduce additional difficulties into the modelled equations and CFX has not got a model to handle that yet.

[Nurzhan]

Originally Posted by Opaque

Based on the mathematical formalism for heat conduction, thermal conductivity cannot be a vector. It is a second order tensor, that for isotropic materials reduces to scalar.

In the case of anisotropic thermal conduction, ANSYS CFX has a hidden feature to input the orthotropic conductivities (principal values on a specific orientation of the material) , or the full tensor.

You can search this forum for "Thermal Conductivity X".. Otherwise, you should probably contact ANSYS CFX support for help.

Either of those values can be set using CEL expression, interpolation functions or via user Fortran junction boxes.

Hi Opaque,

I used your suggestion to set thermal conductivity for an anisotropic material, using an orthotropic coordinates option (shown below), it worked for me. Thanks!

THERMAL CONDUCTIVITY:
Option = Orthotropic Cartesian Components
Thermal Conductivity X Component= # [W m^-1 K^-1]
Thermal Conductivity Y Component= # [W m^-1 K^-1]
Thermal Conductivity Z Component= # [W m^-1 K^-1]
END

However, I tried to use the same method to set electrical conductivity for an anisotropic material, and it didn't work. Do you have any idea how to handle this problem?

Thanks in advance,
Nurzhan

[ghorrocks]

I do not think CFX can handle anisotropic electrical conductivity. Don't forget the anisotropic thermal conductivity is just a beta feature so is not fully supported.

[Opaque]

There are hidden ways to access the anisotropic diffusion model for several equations. If you contact ANSYS CFX, they can provide you with the following beta re-configuration of the electrical conductivity settings:

RULES:
  SINGLETON: ELECTRICAL CONDUCTIVITY
    Description = Hold the details for an advanced description of \
                  Electrical Conductivity.
    Solver Name = CONELEC
    Context Rule = Option
    Essential Parameter List = Option
    Allowed Option List = \
      Value, \
      Orthotropic Cartesian Components
    CONTEXT: Value
      Essential Parameter List = \
       Electrical Conductivity
    END
    CONTEXT: Orthotropic Cartesian Components
      Essential Parameter List = \
        Electrical Conductivity X Component, \
        Electrical Conductivity Y Component, \
        Electrical Conductivity Z Component
    END
  END
  PARAMETER: Electrical Conductivity X Component
    Parameter Type        = Real
    Quantity Type         = Electrical Conductivity
    Dynamic Reread Item   = Yes
    Solver Name           = CONELEC-1
    Group Membership      = VECTOR, CONELEC, 1
  END
  PARAMETER: Electrical Conductivity Y Component
    Parameter Type        = Real
    Quantity Type         = Electrical Conductivity
    Dynamic Reread Item   = Yes
    Solver Name           = CONELEC-2
    Group Membership      = VECTOR, CONELEC, 2
  END
  PARAMETER: Electrical Conductivity Z Component
    Parameter Type        = Real
    Quantity Type         = Electrical Conductivity
    Dynamic Reread Item   = Yes
    Solver Name           = CONELEC-3
    Group Membership      = VECTOR, CONELEC, 3
  END
END

If you copy the rules above into a, say, aniso_eleccon.ccl, you can use along the cfx5solve command line as

cfx5solve -def MyAnisoCase.def -ccl aniso_eleccon.ccl .....

Keep in mind that is not even beta, so you may have to validate the results carefully.

[Nurzhan]

Thank you, guys! I do not know how to express my feelings right now - I really appreciate your help.

Regards,
Nurzhan

[Nurzhan]

Hi Opaque,

I have been trying to apply the additional rules, written above to my simple simulation. However, I get an error saying that there is an "Error reading Command Language data from memory". I tried my simulation without the additional rules and the simulation worked fine. I decided to describe the procedure of my simulation below.

1) Setting all paramters in cfx pre (electrical conductivity specified as isotropic) and cube.def file is created:

# State file created: 2015/10/01 13:39:12
# CFX-14.5 build 2012.09.19-21.47

LIBRARY:
ADDITIONAL VARIABLE: Electric Power
Option = Definition
Tensor Type = SCALAR
Units = [W m^-3]
Variable Type = Volumetric
END
MATERIAL: Solid
Material Description = Aluminium
Material Group = User
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 2700 [kg m^-3]
Molar Mass = 1.0 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 0.91 [J kg^-1 K^-1]
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 237 [W m^-1 K^-1]
END
ELECTRICAL CONDUCTIVITY:
Electrical Conductivity = 5 [S m^-1]
Option = Value
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 = Transient
EXTERNAL SOLVER COUPLING:
Option = None
END
INITIAL TIME:
Option = Automatic with Value
Time = 0 [s]
END
TIME DURATION:
Option = Total Time
Total Time = 100 [s]
END
TIME STEPS:
Option = Timesteps
Timesteps = 0.1 [s]
END
END
DOMAIN: Cube
Coord Frame = Coord 0
Domain Type = Solid
Location = solid
BOUNDARY: Ground
Boundary Type = WALL
Location = ground
BOUNDARY CONDITIONS:
ELECTRIC FIELD:
Option = Ground
END
HEAT TRANSFER:
Option = Adiabatic
END
END
END
BOUNDARY: High Voltage
Boundary Type = WALL
Location = highvoltage
BOUNDARY CONDITIONS:
ELECTRIC FIELD:
Option = Voltage
Voltage = 10 [V]
END
HEAT TRANSFER:
Option = Adiabatic
END
END
END
BOUNDARY: Insulated Surfaces
Boundary Type = WALL
Location = externalsurfaces
BOUNDARY CONDITIONS:
ELECTRIC FIELD:
Option = Zero Flux
END
HEAT TRANSFER:
Option = Adiabatic
END
END
END
DOMAIN MODELS:
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
END
SOLID DEFINITION: Solid 1
Material = Solid
Option = Material Library
MORPHOLOGY:
Option = Continuous Solid
END
END
SOLID MODELS:
ADDITIONAL VARIABLE: Electric Power
Additional Variable Value = Current Density X *Electric Field X + \
Current Density Y *Electric Field Y + Current Density Z *Electric \
Field Z
Option = Algebraic Equation
END
ELECTROMAGNETIC MODEL:
ELECTRIC FIELD MODEL:
Option = Electric Potential
END
MAGNETIC FIELD MODEL:
Option = None
END
END
HEAT TRANSFER MODEL:
Option = Thermal Energy
END
THERMAL RADIATION MODEL:
Option = None
END
END
END
INITIALISATION:
Option = Automatic
INITIAL CONDITIONS:
ELECTRIC POTENTIAL:
Electric Potential = 0 [V]
Option = Automatic with Value
END
TEMPERATURE:
Option = Automatic with Value
Temperature = 0 [C]
END
END
END
OUTPUT CONTROL:
MONITOR OBJECTS:
Monitor Coefficient Loop Convergence = On
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR RESIDUALS:
Option = Full
END
MONITOR TOTALS:
Option = Full
END
END
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 = Electric Power,Electric Field,Electrical \
Conductivity,Current Density,Temperature
OUTPUT FREQUENCY:
Option = Timestep Interval
Timestep Interval = 50
END
END
END
SOLVER CONTROL:
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Maximum Number of Coefficient Loops = 40
Minimum Number of Coefficient Loops = 1
Timescale Control = Coefficient Loops
END
CONVERGENCE CRITERIA:
Residual Target = 0.000001
Residual Type = RMS
END
TRANSIENT SCHEME:
Option = Second Order Backward Euler
TIMESTEP INITIALISATION:
Option = Automatic
END
END
END
END
COMMAND FILE:
Version = 14.5
END

(If I run the above code alone, I get an accurate result.)

However, when I apply the additional rules (a ccl file, named aniso_eleccon.ccl)

RULES:
SINGLETON: ELECTRICAL CONDUCTIVITY
Description = Hold the details for an advanced description of \
Electrical Conductivity.
Solver Name = CONELEC
Context Rule = Option
Essential Parameter List = Option
Allowed Option List = \
Value, \
Orthotropic Cartesian Components
CONTEXT: Value
Essential Parameter List = \
Electrical Conductivity
END
CONTEXT: Orthotropic Cartesian Components
Essential Parameter List = \
Electrical Conductivity X Component, \
Electrical Conductivity Y Component, \
Electrical Conductivity Z Component
END
END
PARAMETER: Electrical Conductivity X Component
Parameter Type = Real
Quantity Type = Electrical Conductivity
Dynamic Reread Item = Yes
Solver Name = CONELEC-1
Group Membership = VECTOR, CONELEC, 1
END
PARAMETER: Electrical Conductivity Y Component
Parameter Type = Real
Quantity Type = Electrical Conductivity
Dynamic Reread Item = Yes
Solver Name = CONELEC-2
Group Membership = VECTOR, CONELEC, 2
END
PARAMETER: Electrical Conductivity Z Component
Parameter Type = Real
Quantity Type = Electrical Conductivity
Dynamic Reread Item = Yes
Solver Name = CONELEC-3
Group Membership = VECTOR, CONELEC, 3
END
END

and change the electrical conductivity using the following code (a ccl file, named solid.ccl):

LIBRARY:
&replace MATERIAL: Solid
Material Description = Aluminium
Material Group = User
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 2700 [kg m^-3]
Molar Mass = 1.0 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 0.91 [J kg^-1 K^-1]
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 237 [W m^-1 K^-1]
END
ELECTRICAL CONDUCTIVITY:
Option = Orthotropic Cartesian Components
Electrical Conductivity X Component = 5 [S m^-1]
Electrical Conductivity Y Component = 0 [S m^-1]
Electrical Conductivity Z Component = 0 [S m^-1]
END
END
END
END

Then I get the error.

I run all three codes using through the command line

cfx5solve -def cube.def -ccl aniso_eleccon.ccl -ccl solid.ccl

I checked the RULES file, where written that

The solver supports anisotropic electric conductivity as well, additional rules are needed. Translation in tt.txt is ready.

I did not want to bother you again and tried to figure out the problem myself. However, I cannot find a clue. I also do not have a direct access to ANSYS commercial portal and support, as I am a student.

Thanks for taking your time to read this.

Regards,
Nurzhan

[Nurzhan]

Hi, guys!

Sorry for coming back to this old post, but I really need your help.

I am facing a problem with setting electrical conductivity for orthotropic cylindrical coordinates, where a value set per each direction is a temperature dependent expression.

Everything works well with the above code, kindly provided by Opaque, if the values set for each Cartesian direction are constants. (Opaque, thank you very much for your code! It helped me a lot!)

However, when I try to re-write the rules for cylindrical coordinates, I get an error.

Could you please at least tell me any reference material, where a process of changing rules is described?

Thank you in advance!

[Opaque]

If you look into the installation directory for the RULES, you should find the existing rules for Orthotropic Cylindrical Components used for the Thermal Conductivity.

You should be able to create/add the Electrical Conductivity r/Theta/Axial Component parameters. Do not forget to include an AXIS DEFINITION as well.

[Nurzhan]

Thank you, Opaque, for the reply!

After several days of trials and studying the 'RULES' file, I updated my rules file. Opaque, could you please have a look at the below code:

Description = Hold the details for an advanced description of \
                  Electrical Conductivity.
    Solver Name = CONELEC
    Context Rule = Option
    Essential Parameter List = Option
    Allowed Option List = \
      Value, \
      Orthotropic Cylindrical Components
    CONTEXT: Value
      Essential Parameter List = \
       Electrical Conductivity
    END
    CONTEXT: Orthotropic Cylindrical Components
      Essential Parameter List = \
        Electrical Conductivity r Component, \
        Electrical Conductivity Theta Component, \
        Electrical Conductivity Axial Component
	  Essential Child List = AXIS DEFINITION
    END
  END
  PARAMETER: Electrical Conductivity r Component
    Parameter Type        = Real
    Quantity Type         = Electrical Conductivity
    Dependency List       = ANY
    Dynamic Reread Item   = Yes
    Solver Name           = CONELEC-1
    Lower Bound           = 0 [S m^-1]
    Group Membership      = VECCYL, CONELEC, 1
  END
  PARAMETER: Electrical Conductivity Theta Component
    Parameter Type        = Real
    Quantity Type         = Electrical Conductivity
    Dependency List       = ANY
    Dynamic Reread Item   = Yes
    Solver Name           = CONELEC-2
    Lower Bound           = 0 [S m^-1]
    Group Membership      = VECCYL, CONELEC, 2
  END
  PARAMETER: Electrical Conductivity Axial Component
    Parameter Type        = Real
    Quantity Type         = Electrical Conductivity
    Dependency List       = ANY
    Dynamic Reread Item   = Yes
    Solver Name           = CONELEC-3
    Lower Bound           = 0 [S m^-1]
    Group Membership      = VECCYL, CONELEC, 3
  END
END

I inserted "Dependency List = ANY" to my new code, so I can express conductivity as a function of temperature. In "Group Membership", I changed initial "VECTOR" to "VECCYL", as it is done for some other parameters in the 'RULES' file.

After using this code, I get the following error:

"ERROR #001100279 has occurred in subroutine ErrAction. Floating point exception: Zero divide."

Despite that, my code works fine with isotropic conductivity (it was validated with experimental data) and orthotropic conductivity expressed in Cartesian coordinates, where conductivity in each direction is constant. Hence, it makes me believe that the above code has a bug, which leads to that error.

Do you have any suggestions?

Cheers,

[Opaque]

Not sure what version of ANSYS CFX you are using, but for Thermal Conductivity r Component, the group membership is ORTCYL2, not VECCYL.

Similarly, the solver name should be 11, 22, and 33, not 1/2 or 3

Hope the above helps,

[Nurzhan]

Opaque, thank you for your time and the suggestions.

I didn't get that error this time, and the run was successful. Though, I will have to study the results first, to be sure that they are valid.

BTW, why did you wrote 'VECTOR' in 'Group Membership', when you described electrical conductivity in the Cartesian coordinates (the quote is below)?

Group Membership = VECTOR, CONELEC, 1

As, for thermal conductivity, when described in Cartesian coordinates, there need to be 'ORTTEN2'. That is why I substituted 'VECTOR' with 'VECCYL', when I re-wrote the code for Cylindrical coordinates.

Anyway, thanks a lot!

[Opaque]

My apologies for the typo.. Definitely a mistake. For Cartesian components, there is little difference between a vector, and a diagonal 2nd order tensor.

However, for cylindrical coordinates the orthotropic cylindrical components are not a diagonal 2nd order tensor in Cartesian coordinates; therefore, some mathematical manipulations required.

I will correct my local rules for Cartesian components. Thank you..

[DaveD!]

Originally Posted by Nurzhan

I inserted "Dependency List = ANY" to my new code, so I can express conductivity as a function of temperature. In "Group Membership", I changed initial "VECTOR" to "VECCYL", as it is done for some other parameters in the 'RULES' file.

After using this code, I get the following error:

"ERROR #001100279 has occurred in subroutine ErrAction. Floating point exception: Zero divide."

Despite that, my code works fine with isotropic conductivity (it was validated with experimental data) and orthotropic conductivity expressed in Cartesian coordinates, where conductivity in each direction is constant.

Hi Nurzhan,


I am facing the same problem as you. How did you solve the zero-division error when working with temperature dependent spatial electrical conductivities in Cartesian coordinates? Could you please paste your final file?


Thank you so much,
DaveD!

[DaveD!]

I found a solution, how to avoid the zero-division error (at least for my case). Obviously, when initializing the solution for the first time, there might be no temperature defined in every cell, leading to the error.
One workaround is to define constant values in x,y and z direction at first, and change them after the first iteration(s) to the temperature-dependent expression you actually have. That's all...

[Martin_Sz]

I think if U use fluent will be much easier to define various conductivity on various direction . On program U have various definition od materials