[MelroseBing]

Hi everybody,
I'm simulating a chimney pipe with double exits in a building to obtain the resistance pressure drops versus velocities under constant temperature. I'm using the SST turbulence model and 15 layers of prism is grown in the mesh. Velocity inlet and opening outlet are given as the BCs.
CFX solver failed to converge and the monitor variable pressure drops oscillate. I have plotted a isosurface of velocity residual~1.0E-3 and remesh this region with refined grid, but the convergence problem still there. I also change to a physical timescale from 1s~5s (fluid residence time is about 15s) and it doesn't help, too. The only convergence is obtained by using upwind advection scheme, but this scheme is of poor accuray. Can anybody help me?

Detailed setup in CFX-Pre:
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: Domain 1
Coord Frame = Coord 0
Domain Type = Fluid
Location = EXT
BOUNDARY: inlet
Boundary Type = INLET
Location = INLET
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Normal Speed = 2.4 [m s^-1]
Option = Normal Speed
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: outlet
Boundary Type = OPENING
Location = OUTLET1,OUTLET2
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Entrainment
Relative Pressure = 0 [Pa]
PRESSURE OPTION:
Option = Opening Pressure
END
END
TURBULENCE:
Option = Zero Gradient
END
END
END
BOUNDARY: wall
Boundary Type = WALL
Location = WALL
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Rough Wall
Sand Grain Roughness Height = 0.046 [mm]
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
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:
Fluid Temperature = 39.4 [C]
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
END
OUTPUT CONTROL:
BACKUP RESULTS: Backup Results 1
File Compression Level = Default
Option = Standard
Output Equation Residuals = All
OUTPUT FREQUENCY:
Iteration Interval = 500
Option = Iteration Interval
END
END
MONITOR OBJECTS:
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR POINT: Monitor Point 1
Coord Frame = Coord 0
Expression Value = dp1
Option = Expression
END
MONITOR POINT: Monitor Point 2
Coord Frame = Coord 0
Expression Value = dp2
Option = Expression
END
MONITOR RESIDUALS:
Option = Full
END
MONITOR TOTALS:
Option = Full
END
END
RESULTS:
File Compression Level = Default
Option = Standard
Output Equation Residuals = All
END
END
SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 1000
Minimum Number of Iterations = 1
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END
CONVERGENCE CRITERIA:
Residual Target = 1e-06
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
END
END

[ghorrocks]

Two things are a give-away for what the problem is:
1) bluff edges which will cause gross separations
2) residuals which converge for a while but then flat-line with a periodic pattern.

This means you are getting transient flow behaviour. You cannot model this steady state, you will need to do a transient simulation.

[MelroseBing]

Originally Posted by ghorrocks

Two things are a give-away for what the problem is:
1) bluff edges which will cause gross separations
2) residuals which converge for a while but then flat-line with a periodic pattern.

This means you are getting transient flow behaviour. You cannot model this steady state, you will need to do a transient simulation.

Thank you for your reply Glenn. I will try the transient simulation and further update will be present.