FSI: Pressure and Normal Force don't match with expected values
 

Hello everyone,

I'm currently working on slosh damping in a cylindrical tank. I try to set a two-ways FSI model to study the impact of a vibrating latex membrane located on the bottom of the tank on free-surface waves.

To start progressively, I am trying to run a simulation without any forced motion for the membrane. I want to check the deformation of this 1mm thick membrane due to the water weight.

The problem is that the pressure in the bottom of the tank and the normal force on the interface are not what could be expected with a simple hydrostatic model.

When I do the math, I obtain an expected 22N force and a +1545Pa relative pressure. But the simulation gives me: a -0.05N force and a -2Pa.

I already performed a simulation with just the CFD and I obtained the expected values, and I keep the same CFD setup for the FSI simulation so I really don't know what is wrong.

Any ideas are welcomed!

Thank you,
Geraud.

Do you have gravity vector defined? And are you pulling out Absolute Pressure as your pressure?

Yes, I have selected the buoyancy model for the fluid and I monitor the pressure (not the absolute pressure) with CFD-Post, on the interface and in the fluid.

CEL:
EXPRESSIONS:
DenWater = 997 [kg m^-3]
InitPressure = DenWater*g*(UpH-z)*VFWater
UpH = 0.158[m]
VFAir = 1-VFWater
VFWater = step((z-UpH)/1[m])
END
END
MATERIAL: Air Ideal Gas
Material Description = Air Ideal Gas (constant Cp)
Material Group = Air Data, Calorically Perfect Ideal Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Molar Mass = 28.96 [kg kmol^-1]
Option = Ideal Gas
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 = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 2.61E-2 [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
END
END
MATERIAL: Water
Material Description = Water (liquid)
Material Group = Water Data, Constant Property Liquids
Option = Pure Substance
Thermodynamic State = Liquid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 997.0 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 4181.7 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0.0 [J/kg]
Reference Specific Entropy = 0.0 [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 8.899E-4 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 0.6069 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 1.0 [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 = 2.57E-04 [K^-1]
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:
ANSYS Input File = ds.dat
Option = ANSYS MultiField
COUPLING TIME CONTROL:
COUPLING INITIAL TIME:
Option = Automatic
END
COUPLING TIME DURATION:
Option = Total Time
Total Time = 1 [s]
END
COUPLING TIME STEPS:
Option = Timesteps
Timesteps = 0.00001 [s]
END
END
END
INITIAL TIME:
Option = Coupling Initial Time
END
TIME DURATION:
Option = Coupling Time Duration
END
TIME STEPS:
Option = Coupling Timesteps
END
END
DOMAIN: Fluid
Coord Frame = Coord 0
Domain Type = Fluid
Location = part fluid
BOUNDARY: InterfaceMembrane
Boundary Type = WALL
Location = interfacemembrane Shadow
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
MESH MOTION:
ANSYS Interface = FSIN_1
Option = ANSYS MultiField
Receive from ANSYS = Total Mesh Displacement
Send to ANSYS = Total Force
END
END
END
BOUNDARY: Opening
Boundary Type = OPENING
Location = opening
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Entrainment
Relative Pressure = 0 [Pa]
END
MESH MOTION:
Option = Stationary
END
END
FLUID: Air
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 1
END
END
END
FLUID: Water
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 0
END
END
END
END
BOUNDARY: Wall
Boundary Type = WALL
Location = wall
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
MESH MOTION:
Option = Stationary
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1.185 [kg m^-3]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = 0 [m s^-2]
Gravity Z Component = -g
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Option = Automatic
END
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = Regions of Motion Specified
MESH MOTION MODEL:
Option = Displacement Diffusion
MESH STIFFNESS:
Option = Increase near Small Volumes
Stiffness Model Exponent = 10
END
END
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
FLUID DEFINITION: Air
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: Water
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: Air
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
FLUID: Water
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
HEAT TRANSFER MODEL:
Fluid Temperature = 25 [C]
Homogeneous Model = True
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = Laminar
END
END
FLUID PAIR: Air | Water
INTERPHASE TRANSFER MODEL:
Option = None
END
MASS TRANSFER:
Option = None
END
SURFACE TENSION MODEL:
Option = None
END
END
MULTIPHASE MODELS:
Homogeneous Model = On
FREE SURFACE MODEL:
Option = Standard
END
END
END
INITIALISATION:
Option = Automatic
FLUID: Air
INITIAL CONDITIONS:
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = VFAir
END
END
END
FLUID: Water
INITIAL CONDITIONS:
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = VFWater
END
END
END
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 = InitPressure
END
END
END
OUTPUT CONTROL:
MONITOR OBJECTS:
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR POINT: Monitor Point 1
Cartesian Coordinates = 0 [m], 0 [m], 0.001 [m]
Domain Name = Fluid
Option = Cartesian Coordinates
Output Variables List = Absolute Pressure
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
Option = Standard
OUTPUT FREQUENCY:
Option = Every Timestep
END
END
END
SOLVER CONTROL:
ADVECTION SCHEME:
Option = High Resolution
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.E-4
Residual Type = RMS
END
EXTERNAL SOLVER COUPLING CONTROL:
COUPLING DATA TRANSFER CONTROL:
Convergence Target = 1e-2
Under Relaxation Factor = 0.75
END
COUPLING STEP CONTROL:
Maximum Number of Coupling Iterations = 10
Minimum Number of Coupling Iterations = 1
SOLUTION SEQUENCE CONTROL:
Solve ANSYS Fields = Before CFX Fields
END
END
END
MULTIPHASE CONTROL:
Volume Fraction Coupling = Coupled
END
TRANSIENT SCHEME:
Option = Second Order Backward Euler
TIMESTEP INITIALISATION:
Option = Automatic
END
END
END
END
COMMAND FILE:
Version = 14.0
Results Version = 14.0
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
MFX RUN CONTROL:
MFX RUN DEFINITION:
MFX Run Mode = Start ANSYS and CFX
Process ANSYS Input File = On
Restart ANSYS Run = Off
END
MFX SOLVER CONTROL:
ANSYS Installation Root = C:\Program Files\ANSYS Inc\v140\ansys
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: lb13207
Remote Host Name = LB132-07
Host Architecture String = winnt-amd64
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
Partition Weight Factors = 0.25000, 0.25000, 0.25000, 0.25000
END
END
RUN DEFINITION:
Run Mode = Full
Solver Input File = CFX.def
END
SOLVER STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARALLEL ENVIRONMENT:
Number of Processes = 4
Start Method = Platform MPI Local Parallel
Parallel Host List = lb13207*4
END
PROCESS COUPLING:
Process Name = CFX
Host Port = 50037
Host Name = LB132-07
END
END
END
END

Concerning Pressure difference:

I believe the hyrdostatic portion of the pressure in CFX is carried in Absolute Pressure and not in Pressure.

Actually, I was just checking the absolute pressure instead and I obtain: 101328Pa at the interface and inside the fluid. So no sign of the water weight there too.

In my limited time I looked at this, I think:



VFAir = 1-VFWater
VFWater = step((z-UpH)/1[m])

Based on VFWater the above CEL indicates to me that your z axis is pointing to the bottom of the screen.


InitPressure = DenWater*g*(UpH-z)*VFWater
UpH = 0.158[m]
and
BUOYANCY MODEL:
Buoyancy Reference Density = 1.185 [kg m^-3]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = 0 [m s^-2]
Gravity Z Component = -g
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Option = Automatic
END
indicates that your z axis is pointing to the top of the screen.

Fix them to be consistant. I suggest changing:

VFWater = step((UpH-z)/1[m])

Oh! I really did that?!

Shame on me! I don't know how I could missed it.

Thank you very much.
Geraud.