|
[Sponsors] |
March 10, 2009, 11:23 |
No results for solid domain
|
#1 |
Guest
Posts: n/a
|
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. |
|
March 10, 2009, 16:12 |
Re: No results for solid domain
|
#2 |
Guest
Posts: n/a
|
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 |
|
March 11, 2009, 08:05 |
Re: No results for solid domain
|
#3 |
Guest
Posts: n/a
|
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 |
|
March 11, 2009, 16:52 |
Re: No results for solid domain
|
#4 |
Guest
Posts: n/a
|
Just an aside, your convergence criteria is not very strict. Be careful with these results.
|
|
March 11, 2009, 21:11 |
Re: No results for solid domain
|
#5 |
Guest
Posts: n/a
|
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 |
|
March 12, 2009, 03:23 |
Re: No results for solid domain
|
#6 |
Guest
Posts: n/a
|
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 |
|
March 12, 2009, 04:14 |
Re: No results for solid domain
|
#7 |
Guest
Posts: n/a
|
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. |
|
March 12, 2009, 08:06 |
Re: No results for solid domain
|
#8 |
Guest
Posts: n/a
|
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 |
|
March 12, 2009, 10:51 |
Re: No results for solid domain
|
#9 |
Guest
Posts: n/a
|
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. |
|
March 12, 2009, 20:20 |
Re: No results for solid domain
|
#10 |
Guest
Posts: n/a
|
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 |
|
March 13, 2009, 03:30 |
Re: No results for solid domain
|
#11 |
Guest
Posts: n/a
|
Hi Rikio,
That makes sense, thanks for your reply and help with this problem. Gary. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Generate a CFD domain from FEA results | Dave442 | Main CFD Forum | 0 | August 3, 2011 12:42 |
initialize 3D domain with 2D results | ivanbuz | FLUENT | 6 | September 3, 2009 18:19 |
CFX Solver Memory Error | mike | CFX | 1 | March 19, 2008 07:22 |
rotating domain in rotating domain, different axis | Robert Stringer | CFX | 3 | December 4, 2006 07:04 |
Solver error message!!! | IoSa | CFX | 1 | September 14, 2006 04:48 |