Show Posts

This section allows you to view all posts made by this member. Note that you can only see posts made in areas you currently have access to.


Messages - william

Pages: 1 ... 3 4 [5] 6 7 ... 11
61
For modeling gas-solid fluidized beds, I recommend that you do not use any turbulence model. Please run your cases laminar.

In any gas-solid fluidized bed, including bubbling beds, turbulent beds, risers etc, the main force balance is between the drag of the gas on the particles and the buoyant weight of the particles, unlike the case of single phase flow where the wall friction is the major factor influencing pressure drop.
Agrawal et al. (2001) and, Srivatsava and Sundaresan (2003) argue that in the case of dense gas-solid flows, where the inertia of the solids is much higher than the gas, the deviatoric part of the gas-phase stress plays a negligible role, and hence the role of the gas-phase viscosity, both laminar and turbulent, is negligible.

62
To get transient mass flow rate data, you need to use the surface monitor functionality under Solution->Monitors..

Let's say, you want to write out mass flow rate through the outlet face every time step.

You will click on the Monitors branch in the tree and then click the Create/Edit button under the Surface Monitors group. A window will pop up where you will select the "Mass Flow Rate" under type and select the zone you want the flow rate on.

Next, check the Write checkbox and enter a file name. Below it, you will select the write frequency. Select it to every time step or what do you think is best for you.

This completes the setting up of the monitors.

As the simulation proceeds, it will keep writing data to this file that you can open and view to make sure it is writing the correct data. Also, if you select two or more zones at the same time then the value will be the net value. If you want to store flow rates for different surfaces separately, you will create a monitor for each following the above procedure.

63
This error message is due to the solution monitor (Velocity magnitude of mixture), which no longer have access to mixture velocity when you use Eulerian Model. When you use VOF model, velocity is shared between phases and you have the mixture velocity in the drop-down list.

So, after changing to the Eulerian model, you need to reset the monitors if you have set it already. If you check this monitor after changing the model, you can see that Phase and sub-field variable drop-down list is blank. Select appropriate field variable and the individual phases.

64
Below are the 2 steps needed to set-up a mass flow-inlet with a 30 degrees rotation (or swirl).

FIRST STEP: Define the axial direction

Before setting the boundary condition, one has to ensure that the 'axial' direction as referred in the boundary condition is correctly setup. The axial direction of your system must be equal to the axial direction as defined by the solver.

This direction can be found (and modified) under define -> boundary conditions -> regions corresponding to a fluid-zone.
Look for the motion tab for the rotation-axis direction panel: X,
Y and Z define the direction of the 'axial direction'.

FLUENT Default:
2D: X is the axial direction (i.e. X = 1, Y = 0)
3D: Z is the axial direction (i.e. X = 0, Y = 0 and Z = 1)

Once the axial direction is defined, we can go to the second step and define the boundary condition

STEP 2: Define the rotation angle

We will assume that the radial flow direction is 0.
If the angle of swirl is 30 degrees, we have an axial component Vx = V * cos(30) and a tangential component Vtheta = V * sin(30).

Hence, the input should be the following:

Coordinate system: cylindrical

Radial Component of Flow Direction: 0
Tangential Component of Flow Direction: sin(30) (enter 0.5)
Axial Component of Flow Direction: cos(30) (enter 0.866)

65
If you are experiencing convergence difficulties while running a case with periodic boundaries and a specified mass flow rate, these are a few things you can try to improve the convergence behaviour.

(1) Mesh Requirement: Mesh plays an important role in the case convergence. The mesh in the periodic faces should be exactly same. You should link the periodic edge or face mesh. The convergence will be better if the meshes near to the periodic faces are also exactly same. If you use the sizing function, make sure that the mesh is same in the nearby region also, otherwise use uniform mesh.

(2) URF: Start the simulation with smaller URF values. Pr- 0.2, dens- 0.5, body force- 0.5, mom- 0.3, all turbulent URF- 0.4. You can increase the URF gradually with convergence.

(3) Initial Pressure gradient: The following command sets the pressure gradient value to zero:

(rpsetvar 'periodic/pressure-derivative 0)

Include this command in Solve->Execute Commands and execute at every iteration. Enable this command for first 30-50 iterations. After 50 iterations, disable this and the calculated beta will be updated. This sometimes helps convergence.


66
CFX solves for the Navier Stokes equations including viscosity. To obtain the Euler equation solution, you can set a very low Dynamic Viscosity value, say, 1e-12 kg/m/s, the 'laminar' turbulence model option and isothermal flow. In addition you should set the 'Free Slip Wall' option at all walls.


67
CFX / Re: Boiling calculations with an energy model for the vapour
« on: May 12, 2012, 11:44:17 AM »
This may be due to an energy source term being included twice. The problem can be ameliorated by setting the Nusselt number on the zero resistance side to a high value. It is however better to set the vapour to be isothermal.

68
In inviscid flow simulation, the drag force is set to zero, so the particle would not be moved by surrounding fluid flow. The particle will only be moved by initial velocity. That's why when you set non-zero initial velocity, the particle moves forward. In viscous fluid flow without interaction with continuous phase, the particle will be moved with local fluid velocity. In viscous fluid flow with interaction with continuous phase, the particle will be moved by the drag force which depends on the relative velocity between fluid and the particle.

When the option of interaction with continuous phase is on, the particle mass flow rate value on the injection panel needs to be specified, so as to calculate the momentum exchange between particle and fluid accurately.

69
Wall Heat Flux is only defined on Wall Boundaries and on the fluid side of Fluid-Solid Interfaces. You should use this variable when calculating heat flux through Wall boundaries. If you perform the following calculation in CFX-Post:
areaInt(Wall Heat Flux)@MyWallBoundary, using a Direction of None
you will find that this matches the values printed near the end of the .out file under "Boundary Flow and Total Source Term Summary" for Energy. This is the best and the most accurate method, since Wall Heat Flux comes directly from the Solver.
Heat Flux is calculated by CFX-Post, it is not output from the Solver. You can use this variable to calculate heat flow on other boundaries and 2D regions (inlets and outlets for example).

On a wall boundary, you should get the same value for Wall Heat Flux and Heat Flux. There may be small differences since Wall Heat Flux is stored on vertices and Heat Flux is stored on the integration points.
In general, you should use Wall Heat Flux for calculations on Wall boundaries and Heat Flux on other boundaries.

70
Create the fluid and solid domains in the usual way. If you are solving a rotating problem, your fluid domain should be setup as a rotating domain while the solid domain must be stationary.
Do not create any wall boundary conditions on these surfaces. Create fluid-solid domain interfaces in the usual way. Once you have create the domain interface, you will see that CFX-Pre has automatically created some boundary conditions for the fluid and the solid side. You can then edit the fluid side boundary condition and set a wall velocity, or a counter rotating wall, or leave the walls as stationary as required. A stationary wall is always stationary with respect the the local domain.

71
The set up has 3 domains, a one fluid domain, a solid domain and a 2 fluid domain. Energy transfer is coupled across them by CHT.
In the 2 fluid domain there are 2 energy equations, in the other two only one. Unfortunately the energy subsystem has been set up
with only one energy equation allowed for. This is due to the fact that the one fluid domain comes first ! This should be griped.
A work around is to alter the domain order so that the 2 fluid domain comes first.

72
For steady-state problems, the CFX-Solver uses a robust, fully implicit formulation so that relatively large timesteps can be selected accelerating the convergence to steady-state as fast as possible. However, if the timestep is too large the resulting convergence behaviour will be ¿bouncy¿. If this is observed, then the first thing you should try is to reduce the timestep size, say, by a factor of four. If there is no noticeable improvement, then the convergence problem may be caused by another factor. Note that if the timestep is too small, then convergence will be very slow.
Note that also depending on your initial guess, a significantly smaller timestep may be required for the first few iterations of a problem.


In addition to the advice in the following sections, you will probably require a small physical timestep for the following situations:
- poor mesh quality
- transonic flow
- large regions of separated flow
- Openings with simultaneous inflow and outflow
- Free Surface flows (in these cases it is often sufficient to use a smaller timestep only for the Volume Fraction equations)
- Multiphase flows.


In order to set an appropriate Physical timestep size, you must check which phenomena is dominating your flow:

1) Advection dominated flows

The physical timestep size should be some fraction of a length scale divided by a velocity scale. A good approximation is the Dynamical Time for the flow. This is the time taken for a point in the flow to make its way through the fluid domain. For many simulations a reasonable estimate is easy to make based on the length of the fluid domain and the mean velocity, for example ?t = L / 2U

If the domain contains largely varying velocity and length scales, you should try to estimate an average value. If you get divergence, check in the Output File that your timestep size is not larger than the Advection Time Scale value given in the Average Scale Information at the end of the run. A ¿small¿ timestep can beconsidered to be less than 1/3 the smallest length/velocity_scale in the simulation. Values higher than this can be considered a ¿large¿ timestep.


2) Buoyancy driven flows

The maximum physical timestep size may be estimated using the following relationship:
?t_max ~ sqrt(L / (ß g ?T))

where:
L is a length scale associated with the vertical temperature gradient
?T is the temperature variation in the fluid
ß is the thermal expansivity of the fluid
g isthe gravitational acceleration.


3) Free surface flows

The timestep for free surface flows should be based on a L/U (Length/Velocity) scale. The length scale should be a geometric length scale. The velocity scale should be the maximum of a representative flow velocity and a buoyant velocity, which is given by:
U_buoyant = sqrt(g L)

In addition, it is often helpful to reduce the timestep for the volume fraction equations by an order of magnitude below that of the other equations.


4) Multiphase Flow (Inhomogeneous)

For bubble columns, use first a fraction of the bubble rise time for a total of one rise time, then increase the timestep to a fraction of the fluid circulation time. If species mass transfer is modelled, it can take a considerable amount of time for some species to come to equilibrium. Try setting the timestep size for the mass fraction equations to a large value if convergence is very slow for this equation class.

For dilute particle cases, use a fraction of the dynamical timescale for the momenta. This is essentially a fluid travel time through or around the region of interest.
If volume fraction convergence is slow, then the timescale for these equations can be increased suitably.


5) Combustion

It is often useful to apply a largertime step to temperature and species than the remaining equations. Try starting with a relatively large timestep to let the material sweep through the domain. You can reduce the timestep later to achieve better resolution of the simulation conditions, and therefore convergence.
When using the Finite Rate Chemistry model, using a timestep that is too large at the beginning may cause the solver to fail due to reaction rates not converging. Under these circumstances, the timestep must be reduced.



Finally, note that it may happen that simulations which are run in steady state mode will have difficulty converging, and no matter what action you take regarding mesh quality and timestep size, the solution does not converge. This could be an indication of transient behaviour. If you have run a steady state calculation and you see oscillatory behaviour of the residual plots, you can test to see if you are observing a transient effect by reducing/increasing the timestep size by a known factors. If the period of oscillation of the residual plot changes by changes the timestep size, then the phenomenon is most likely a numerical effect. If the period stays the same, then it is probably a transient effect.

73
A Stationary Domain with rotating walls is only valid if the wall motion is entirely tangential. If there is any normal component to the wall motion, the fluid will not "feel" the pushing effect of the wall, so this is not a valid set up. For example, in rotating machines the blades have a significant normal component so they must be modeled using a Rotating Domain and stationary walls (relative to the rotating domain).
In applications where the wall motion is purely tangential, then either method is valid, but one is usually preferred for numerical reasons. If the flow is mainly rotating at a magnitude similar to the rotating wall velocity then the Rotating Domain is preferred. If the axial/radial velocity in the majority of the domain is dominant, then a Stationary Domain with rotating walls should be used.

74
CFX / Re: How can I apply my profile?
« on: May 11, 2012, 10:55:44 PM »
In cases where a separate velocity field is specified for different fluids, clicking "Generate Values" on the profile boundary condition form does not automatically enter the velocity profile. You must do this manually, by entering an expression. For example: myprofile.Velocity u(x,y,z) can be entered for the velocity, where "myprofile" is the name of the profile, and "Velocity u" is the name of the U Velocity variable in your profile data file.

75
The ccl below uses the CEL expression CombEff to adjust the heating values:

LIBRARY:
MATERIAL: Methane Air WD1
Option = Variable Composition Mixture
Reactions List = Methane Air WD1
END # MATERIAL Methane Air WD1
MATERIAL : CH4 # Methane
Option = Pure Substance
PROPERTIES :
Option = Ideal Gas
Molar Mass = 16.04 [kg kmol^-1]
Dynamic Viscosity = 11.1E-06 [kg m^-1 s^-1]
Thermal Conductivity = 343E-04 [W m^-1 K^-1]
Thermal Expansivity = 3.35E-03 [K^-1]
Refractive Index = 1.
Reference Pressure = 1. [atm]
Reference Temperature = 25 [C]
Reference Specific Enthalpy = -74.87310 [kJ mol^-1] / 16.04 [kg kmol^-1]
Reference Specific Entropy = 186.2 [J mol^-1 K^-1] / 16.04 [kg kmol^-1]
SPECIFIC HEAT CAPACITY:
Option = NASA Format
Temperature Limit List = 300 [K], 5000 [K], 1000 [K]
NASA Coefficient List = \
NASACoeff21, NASACoeff22, NASACoeff23, \
NASACoeff24, NASACoeff25, NASACoeff26, \
NASACoeff27, \
NASACoeff11, NASACoeff12, NASACoeff13, \
NASACoeff14, NASACoeff15, NASACoeff16, \
NASACoeff17
END #SPECIFIC HEAT CAPACITY
#
# Boiling point (1 atm) = 111.66 [K]
# Critical Temperature = 190.58 [K]
# Critical Pressure = 4.604E+06 [Pa]
#
END #PROPERTIES
END #MATERIAL


CEL:
EXPRESSIONS:
#
# Combustion of methane: CH4 + 2O2 -> CO2 + 2H2O
#
Rgas = 8314.41 [J kmol^-1]
CombEff = 0.95
HoFCO2 = -393.5224 [kJ mol^-1]
HoFH2O = -241.8264 [kJ mol^-1]
HoFCH4 = -74.8731 [kJ mol^-1]
HeatofProducts = HoFCO2+2*HoFH2O
HeatofReaction = HeatofProducts-HoFCH4
#
# Modify heat of formation ofmethane to account for a
# combustion efficiency of less than 100% using Gordon
# & McBride (NASA) format for enthalpy polynomial
#
HoFCH4Mod = HeatofProducts-CombEff*HeatofReaction
#
NASACoeff11 = 0.07787415E+01
NASACoeff12 = 0.01747668E+00
NASACoeff13 = -0.02783409E-03
NASACoeff14 = 0.03049708E-06
NASACoeff15 = -0.01223931E-09
NASACoeff17 = 0.01372219E+03
Tref1 = 298.15
DHTref11 = NASACoeff11*Tref1 + NASACoeff12*Tref1^2/2 + \
NASACoeff13*Tref1^3/3 + NASACoeff14*Tref1^4/4 + \NASACoeff15*Tref1^5/5
Tref2 = 1000.0
DHTref12 = NASACoeff11*Tref2 + NASACoeff12*Tref2^2/2 + \
NASACoeff13*Tref2^3/3 + NASACoeff14*Tref2^4/4 + \
NASACoeff15*Tref2^5/5
NASACoeff16 = HoFCH4Mod/Rgas-DHTref11
# NASACoeff16 = -0.09825229E+05
#
# High temperature polynomial
#
NASACoeff21 = 0.01683479E+02
NASACoeff22 = 0.01023724E+00
NASACoeff23 = -0.03875129E-04
NASACoeff24 = 0.06785585E-08
NASACoeff25 = -0.04503423E-12
NASACoeff27 = 0.09623395E+02
DHTref22 = NASACoeff21*Tref2 + NASACoeff22*Tref2^2/2 + \
NASACoeff23*Tref2^3/3 + NASACoeff24*Tref2^4/4 + \
NASACoeff25*Tref2^5/5
# Ensure high T and low T polynomials match at Tref2
NASACoeff26 = DHTref12 + NASACoeff16 - DHTref22
# NASACoeff26 = -0.01008079E+06
#
END # EXPRESSIONS
END # CEL
END # LIBRARY


FLOW:

DOMAIN: Combustor
Location = Combustor
Coord Frame = Coord 0
Fluids List = Methane Air WD1
DOMAIN MODELS:
DOMAIN MOTION:
Option = Stationary
END # DOMAIN MOTION
BUOYANCY MODEL:
Option = Non Buoyant
END # BUOYANCY MODEL
REFERENCE PRESSURE:
Reference Pressure = 1.0133E5 [Pa]
END # REFERENCE PRESSURE
END # DOMAIN MODELS

FLUID MODELS:
TURBULENCE MODEL:
Option = k epsilon
END # TURBULENCE MODEL
TURBULENT WALL FUNCTIONS:
Option = Scalable
END # TURBULENT WALL FUNCTIONS
HEAT TRANSFER MODEL:
Option = Thermal Energy
END # HEAT TRANSFER MODEL
COMBUSTION MODEL:
Option = Eddy Dissipation
END # COMBUSTION MODEL
COMPONENT: CH4
Option = Transport Equation
END # COMPONENT CH4
COMPONENT: O2
Option = Transport EquationEND # COMPONENT O2
COMPONENT: CO2
Option = Transport Equation
END # COMPONENT CO2
COMPONENT: H2O
Option = Transport Equation
END # COMPONENT H2O
COMPONENT: N2
Option = Constraint
END # COMPONENT N2
THERMAL RADIATION MODEL:
Option = None
END # THERMAL RADIATION MODEL
END # FLUID MODELS

END # DOMAIN Combustor
END #FLOW

Pages: 1 ... 3 4 [5] 6 7 ... 11