Domain Imbalance
Hi,
I am new user of CFX. I am doing transient simulation of two heat source(with same dimension) located bottom side of inside of a rectangular area.Top of the rectangular area(1mx1mx1m) is open, 4 wall is insulated and bottom is also insulated.Distance between two heat sources is 28cm. I tried to do simulation in different way but I found that domain imbalance in Pmass is always 200%. I also tried to do above simulation on steady state (this is not my target) but results again showed that domain imbalance Pmass 200%. For convenience I attached the CCL ++    CFX Command Language for Run    ++ 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 EQUATION OF STATE: Density = 1.185 [kg m^3] Molar Mass = 28.96 [kg kmol^1] Option = Value 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 = 1.831E05 [kg m^1 s^1] Option = Value END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 2.61E02 [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 THERMAL EXPANSIVITY: Option = Value Thermal Expansivity = 0.003356 [K^1] END END END MATERIAL: Air at 27 C Material Description = Air at 27 C (dry) Material Group = Air Data,Constant Property Gases Option = Pure Substance Thermodynamic State = Gas PROPERTIES: Option = General Material EQUATION OF STATE: Density = 1.1777 [kg m^3] Molar Mass = 28.96 [kg kmol^1] Option = Value END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 1005 [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^1] Reference Specific Entropy = 0 [J kg^1 K^1] Reference Temperature = 300 [K] END DYNAMIC VISCOSITY: Dynamic Viscosity = 1.983e05 [kg m^1 s^1] Option = Value END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 0.02619 [W m^1 K^1] END ABSORPTION COEFFICIENT: Absorption Coefficient = 0.01 [m^1] Option = Value END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0. [m^1] END REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 END THERMAL EXPANSIVITY: Option = Value Thermal Expansivity = 0.003356 [K^1] END END END END FLOW: Transient Analysis 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 = 1000 [s] END TIME STEPS: Option = Timesteps Timesteps = 0.581899 [s] END END DOMAIN: Two Heat Sources Coord Frame = Coord 0 Domain Type = Fluid Location = B46 BOUNDARY: Atm Boundary Type = OUTLET Location = F48.46 BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Normal Speed = 0 [m s^1] Option = Normal Speed END END END BOUNDARY: Bottom Boundary Type = WALL Location = F47.46 BOUNDARY CONDITIONS: HEAT TRANSFER: Option = Adiabatic END MASS AND MOMENTUM: Option = No Slip Wall END END END BOUNDARY: Vent 1 Boundary Type = INLET Location = F138.46 BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END HEAT TRANSFER: Option = Static Temperature Static Temperature = 298.644619578 [K] END MASS AND MOMENTUM: Normal Speed = 0.0841895 [m s^1] Option = Normal Speed END END END BOUNDARY: Vent 2 Boundary Type = INLET Location = F137.46 BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END HEAT TRANSFER: Option = Static Temperature Static Temperature = 298.644619578 [K] END MASS AND MOMENTUM: Normal Speed = 0.0841895 [m s^1] Option = Normal Speed END END END BOUNDARY: Wall Boundary Type = WALL Location = F49.46,F50.46,F51.46,F52.46 BOUNDARY CONDITIONS: HEAT TRANSFER: Option = Adiabatic END MASS AND MOMENTUM: Option = No Slip Wall END END END DOMAIN MODELS: BUOYANCY MODEL: Buoyancy Reference Temperature = 300 [K] 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 DEFINITION: Fluid 1 Material = Air at 25 C 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 = Laminar END 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 [atm] END TEMPERATURE: Option = Automatic with Value Temperature = 300 [K] END END END OUTPUT CONTROL: 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 = Temperature,Velocity OUTPUT FREQUENCY: Option = Time Interval Time Interval = 0.5 [s] END END END SOLVER CONTROL: ADVECTION SCHEME: Option = High Resolution END BODY FORCES: Body Force Averaging Type = VolumeWeighted END CONVERGENCE CONTROL: Maximum Number of Coefficient Loops = 5 Minimum Number of Coefficient Loops = 1 Timescale Control = Coefficient Loops END CONVERGENCE CRITERIA: Residual Target = 1.E4 Residual Type = RMS END TRANSIENT SCHEME: Option = Second Order Backward Euler TIMESTEP INITIALISATION: Option = Automatic END END END END COMMAND FILE: Version = 12.1 Results Version = 12.1 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: fmcv42s 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 = kway Option = MeTiS Partition Size Rule = Automatic END END RUN DEFINITION: Run Mode = Full Solver Input File = C:\Documents and Settings\jc218370\Local \ Settings\Temp\2HS28CMUPDATE1_1052_Working\dp0\CFX\CFX\Work1\Fluid \ Flow.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 ================================================== ==================== Boundary Flow and Total Source Term Summary ================================================== ==================== ++  UMom  ++ Boundary : Atm 1.6471E06 Boundary : Bottom 1.3208E06 Boundary : Vent 1 1.0866E08 Boundary : Vent 2 2.0033E08 Boundary : Wall 4.7055E06 Neg Accumulation : Two Heat Sources 5.1746E09  Domain Imbalance : 4.3935E06 Domain Imbalance, in %: 0.0177 % ++  VMom  ++ Boundary : Atm 3.5500E07 Boundary : Bottom 3.6152E07 Boundary : Vent 1 2.6344E09 Boundary : Vent 2 7.1901E09 Boundary : Wall 4.2817E06 Neg Accumulation : Two Heat Sources 3.1277E07  Domain Imbalance : 4.5911E06 Domain Imbalance, in %: 0.0185 % ++  WMom  ++ Boundary : Atm 5.9300E05 Boundary : Bottom 2.4246E02 Boundary : Vent 1 2.6491E04 Boundary : Vent 2 2.6527E04 Boundary : Wall 1.2362E06 Domain Src (Pos) : Two Heat Sources 2.4839E02 Neg Accumulation : Two Heat Sources 2.6798E07  Domain Imbalance : 4.8673E06 Domain Imbalance, in %: 0.0196 % ++  PMass  ++ Boundary : Vent 1 8.0007E04 Boundary : Vent 2 8.0007E04  Domain Imbalance : 1.6001E03 Domain Imbalance, in %: 200.0000 % ++  HEnergy  ++ Boundary : Vent 1 3.9746E01 Boundary : Vent 2 3.9746E01 Neg Accumulation : Two Heat Sources 7.9492E01  Domain Imbalance : 1.0729E06 Domain Imbalance, in %: 0.0001 % I run this test 1000s and time step is 0.58s. Now I am confused whether my simulation is ok or not.If not how can i improve my simulation results.What is the error in my simulation? In addition I want added that CFX manager screen showed that the results was converged successfully. I need anybodys good comment on my querry Thanks in advance. HMR 
velocity inlet and velocity outlet is numerically not advantageous. Check your boundaries and the according chapters in the help

Rather than "not advantageous", I would say "physically impossible". Read the CFX documentation as joey says on boundary condition selection.

Thanks JOEY2007 and GLENN for your good comments, I have checked that some thing need to adjust in boundary conditions to get good result.
Regards HMR 
I have a question about Pmass imbalance.
I have a rotor spining ( 1/6=60° rotating domain with ciclic simetry) problem, it is a wentilated braking disk with cooling fins. Convergence of residuals is good and my monitor points are converging to some value (torque, avgHTC...), imbalances in the domain are all wery close to 0 but the Pmass imbalance jumps from +100 the frequency is somewhat timescale dependant. https://drive.google.com/open?id=0Bw...DBiTlItbjIxX1U in the figure there is all ~350 itterations. monitor points are constant at ~100 itter, all RMS residuals are under 1e4 but max residuals are above 1e2. I only have an opening tipe boundary condition and the flow is induced by rotors rotation, there is also heat transfer included and domain has properties of air ideal gas, SSTmodel with wery fine inflation layers is used for turbulence model. Is there a problem if Pmass is jumping +100? Can I change something to make it beter? I dont understand why it is jumping and how can my simulation still looks well converged. Thank you 
If you only have a single flow boundary then you cannot generally use imbalances. That is because the smallest net flow in or out the boundary (even if just cause by numerical noise) has nothing to balance it and so shows as 100% imbalance. And the next time step when the tiny flow is in the other direction the imbalance shows up as 100%. That is why imbalances is an optional convergence criteria  for some simulations it is meaningless.

All times are GMT 4. The time now is 01:13. 