Hello users,

I'm new to cfx and am running a fairly simple model (a solid cylinder with a fluid region inside of it). The model converges with no problems however when i come to post-process the results i have no results for the solid tube, only for the fluid region. The solid tube section does have a film externally however i don't think this is causing the problem.

Thanks for any advice.

Please post the CCL for your case to allow us to help. This is the text output you see at the top of the text window in CFX solver manager. We just need to see the bit near the top which describes the model setup - not all the residual values which get printed later.

Regards, andy

Hi Andy,

Thanks for your reply. Please see below the CCL as requested. As the model convergres without any obvious problems, I'm hoping that this may just be something simple. I've used the 'Air at 25 degrees' option for the fluid as I 'presume' that Air Ideal Gas is more for compressible flow scenarios.. Also, I noticed that my CCl doesn't contain geometry info - so I hope that I have given you the information which you referred to.

Thanks again, Gary.

LIBRARY:

MATERIAL: Air at 25 C

Material Description = Air at 25 C and 1 atm (dry)

Material Group = Air Data, Constant Property Gases

Option = Pure Substance

Thermodynamic State = Gas

PROPERTIES:

Option = General Material

Thermal Expansivity = 0.003356 [K^-1]

ABSORPTION COEFFICIENT:

Absorption Coefficient = 0.01 [m^-1]

Option = Value

END

DYNAMIC VISCOSITY:

Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1]

Option = Value

END

EQUATION OF STATE:

Density = 1.185 [kg m^-3]

Molar Mass = 28.96 [kg kmol^-1]

Option = Value

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

REFRACTIVE INDEX:

Option = Value

Refractive Index = 1.0 [m m^-1]

END

SCATTERING COEFFICIENT:

Option = Value

Scattering Coefficient = 0.0 [m^-1]

END

SPECIFIC HEAT CAPACITY:

Option = Value

Specific Heat Capacity = 1.0044E+03 [J kg^-1 K^-1]

Specific Heat Type = Constant Pressure

END

THERMAL CONDUCTIVITY:

Option = Value

Thermal Conductivity = 2.61E-02 [W m^-1 K^-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

REFERENCE STATE:

Option = Specified Point

Reference Specific Enthalpy = 0 [J/kg]

Reference Specific Entropy = 0 [J/kg/K]

Reference Temperature = 25 [C]

END

SPECIFIC HEAT CAPACITY:

Option = Value

Specific Heat Capacity = 4.34E+02 [J kg^-1 K^-1]

END

THERMAL CONDUCTIVITY:

Option = Value

Thermal Conductivity = 60.5 [W m^-1 K^-1]

END

END

END END FLOW:

SOLUTION UNITS:

Angle Units = [rad]

Length Units = [m]

Mass Units = [kg]

Solid Angle Units = [sr]

Temperature Units = [K]

Time Units = [s]

END

SIMULATION TYPE:

Option = Steady State

EXTERNAL SOLVER COUPLING:

Option = None

END

END

DOMAIN: ITube

Domain Type = Solid

Location = B10

Solids List = Steel

BOUNDARY: Default Fluid Solid Interface Side 1 1

Boundary Type = INTERFACE

Location = F15.10

BOUNDARY CONDITIONS:

HEAT TRANSFER:

Option = Conservative Interface Flux

END

END

END

BOUNDARY: Film

Boundary Type = WALL

Location = F11.10,F12.10,F13.10

BOUNDARY CONDITIONS:

HEAT TRANSFER:

Heat Transfer Coefficient = 10 [W m^-2 K^-1]

Option = Heat Transfer Coefficient

Outside Temperature = 19.6 [C]

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 = 19.6 [C]

END

END

END

SOLID MODELS:

HEAT TRANSFER MODEL:

Option = Thermal Energy

END

THERMAL RADIATION MODEL:

Option = None

END

END

END

DOMAIN: ITube_Air

Coord Frame = Coord 0

Domain Type = Fluid

Fluids List = Air at 25 C

Location = B14

BOUNDARY: Default Fluid Solid Interface Side 1

Boundary Type = INTERFACE

Location = F15.14

BOUNDARY CONDITIONS:

HEAT TRANSFER:

Option = Conservative Interface Flux

END

WALL INFLUENCE ON FLOW:

Option = No Slip

END

WALL ROUGHNESS:

Option = Smooth Wall

END

END

END

BOUNDARY: Fluid_Film_Bottom

Boundary Type = WALL

Location = F16.14

BOUNDARY CONDITIONS:

HEAT TRANSFER:

Heat Transfer Coefficient = 10 [W m^-2 K^-1]

Option = Heat Transfer Coefficient

Outside Temperature = 19.6 [C]

END

WALL INFLUENCE ON FLOW:

Option = No Slip

END

WALL ROUGHNESS:

Option = Smooth Wall

END

END

END

BOUNDARY: Fluid_Film_Top

Boundary Type = WALL

Location = F17.14

BOUNDARY CONDITIONS:

HEAT TRANSFER:

Heat Transfer Coefficient = 20 [W m^-2 K^-1]

Option = Heat Transfer Coefficient

Outside Temperature = 19.6 [C]

END

WALL INFLUENCE ON FLOW:

Option = No Slip

END

WALL ROUGHNESS:

Option = Smooth Wall

END

END

END

BOUNDARY: Flux

Boundary Type = WALL

Location = F18.14

BOUNDARY CONDITIONS:

HEAT TRANSFER:

Option = Adiabatic

END

WALL INFLUENCE ON FLOW:

Option = No Slip

END

WALL ROUGHNESS:

Option = Smooth Wall

END

END

BOUNDARY SOURCE:

SOURCES:

EQUATION SOURCE: energy

Flux = 46.358 [W m^-2]

Option = Flux

END

END

END

END

DOMAIN MODELS:

BUOYANCY MODEL:

Buoyancy Reference Temperature = 19.6 [C]

Gravity X Component = 0 [m s^-2]

Gravity Y Component = 0 [m s^-2]

Gravity Z Component = -9.81 [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 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

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

K:

Option = Automatic

END

STATIC PRESSURE:

Option = Automatic with Value

Relative Pressure = 1 [atm]

END

TEMPERATURE:

Option = Automatic with Value

Temperature = 292.6 [K]

END

END

END

END

DOMAIN INTERFACE: Default Fluid Solid Interface

Boundary List1 = Default Fluid Solid Interface Side 1 1

Boundary List2 = Default Fluid Solid Interface 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 = 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

EPSILON:

Option = Automatic

END

K:

Option = Automatic

END

STATIC PRESSURE:

Option = Automatic with Value

Relative Pressure = 1 [atm]

END

TEMPERATURE:

Option = Automatic with Value

Temperature = 19.6 [C]

END

END

END

OUTPUT CONTROL:

RESULTS:

File Compression Level = Default

Option = Standard

END

END

SOLVER CONTROL:

ADVECTION SCHEME:

Option = High Resolution

END

CONVERGENCE CONTROL:

Length Scale Option = Conservative

Maximum Number of Iterations = 150

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 = 11.0

Results Version = 11.0 END EXECUTION CONTROL:

INTERPOLATOR STEP CONTROL:

Runtime Priority = Standard

EXECUTABLE SELECTION:

Double Precision = Off

END

MEMORY CONTROL:

Memory Allocation Factor = 1.0

END

END

PARALLEL HOST LIBRARY:

HOST DEFINITION: gb002ws0295

Host Architecture String = winnt

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:

Definition File = T:/Development/1. R&D Projects/DU004594 - analysis \

development/005 Engineering/3D Thermal Analysis/Analysis \

Files/Convection/Perdido I-Tube/WoS.def

Interpolate Initial Values = Off

Run Mode = Full

END

SOLVER STEP CONTROL:

Runtime Priority = Standard

EXECUTABLE SELECTION:

Double Precision = Off

END

LICENSE CONTROL:

Preferred License = 35

Shared License Port = 1601

END

MEMORY CONTROL:

Memory Allocation Factor = 1.0

END

PARALLEL ENVIRONMENT:

Number of Processes = 1

Start Method = Serial

END

END END

Just an aside, your convergence criteria is not very strict. Be careful with these results.

Gary,

I did not find inlet & outlet for the fluid domain, all the boundaries of domain, ITube_Air, are walls. What is your analysis target? Just to get the temp. distribution on the walls?

Rikio

Gary,

I cannot see any particlar problems here.

1) When you run the problem, do you see a tab on the Solver Manager for the energy equation? Do you see residuals for the enthalpy (H) and temperature (T) in the solver output?

2) How are you post-processing it? What happens if you put a plane through the tube, passing through both the solid and the air domains; then define a contour on this plane (being careful to select either 'All Domains' or both the solid and air domains are selected in the definition of the contour, and select Temperature for the variable? (Sorry if this is too obvious - but you did say you're new to CFX...)

3) In multi-domain problems, I think CFXPost asks if it should load results from all domains (or just some of them) when you load the results file. This is useful for large models - but in your case make sure you load them all here! (You can tell it not to ask again about this in the future - so don't worry if you do not see this message)

Regards, andy2o

Hello Craig, Rikio and Andy2o. Thank you for your posts.

Craig, with regards to the convergence criteria, if I remember correctly I used the default settings with residual target set at 1E-04; perhaps this could be reduced, unless it was other parameters which you were referring to?

Rikio, my intention is to model an enclosed volume using the buoyancy option to model the temperature distribution within the volume. As far as I am aware, I don't need to specify an inlet and outlet?? If you think my method for achieving this is incorrect, then please feel free to comment or suggest otherwise.

Andy, no those instrustions aren't too basic as this is the first simulation I've run with CFX. Actually I had already tried what you have suggested (creating a plane through both the solid and fluid domains) although this still doesn't seem to give me results for the solid tube section. I have also made sure that the two domains are selected for post processing when prompted. When solving, the residuals for enthalpy and temperature appear to be reducing without 'problems'.I'm beginning to think that maybe its a default setting somewhere that I may have adjusted, I may try recreating the simulation and trying again... While talking about post processing, is there a preferred package that CFX users use, or do most generally use CFX-post itself?

Thanks again, gary.

You're correct - the RMS residual < 10e-4 is the default, but if you read the documentation you'll find they suggest you should have MAX residaul < 10e-4 (or less, 5e-5 for example) for accurate results. That isn't the cause of your current problem though, as CFX Post should display your results (accurate or not), but it is worth knowing.

What about the fluid results? Do they look sensible? Sensible temperatures (you're not getting millions of degrees C?!)? If so, it sounds like CFX is solving OK. So, it sounds like you must be having problems with CFX Post. I suggest you start from scratch in CFX POST (close it down, restart it and don't use any saved state files you've made). Perhaps look at the tutorials - there's one with a heater coil which includes solid materials - why not do that tutorial for guidance?

Obviously some variables, such as velocity, are not output for the solid region - so make sure you use variables that are defined in the solid region to create your plots.

Good luck. Do you have a CFX support contract? Why not give them a call? Otherwise perhaps someone else will pipe up with an answer, because I've never hit a problem like this before myself.

Andy

Success! I decided to stick with my idea that the problem must be something simple as everything else seemed correct and there were no convergence problems. My post-processing choice was the value of 'total temperature' and for some reason this doesn't give any results for the solid region. If i change this to simply 'temperature', the results are there...! If you can explain what the difference is then that would be great as I can't find it in the manual...

Further to your question, yes I do have a CFX/workbench contact (was helpful with a couple of design modeller problems)

Thanks, gary.

Gary,

There is no "Total Temperature" in a solid. It just exists in fluid domain, because it should be calculated based on static temperature and velocity. Obviously, no velocity in solid domain.

Rikio

Hi Rikio,

That makes sense, thanks for your reply and help with this problem.

Gary.