Cfx12 04 solver

Chapter 4

Solver Settings

Introduction to CFX

ANSYS, Inc. Proprietary April 28, 2009
© 2009 ANSYS, Inc. All rights reserved. 4-1 Inventory #002598

Solver Settings
Overview Training Manual

• Initialization

• Solver Control

• Output Control

• Solver Manager

Note: This chapter considers solver settings for steady-state simulations.
Settings specific to transient simulation are discussed in a later chapter.


Solver Settings
Initialization Training Manual

• Iterative solution procedures require that all solution variables are
assigned initial values before calculating a solution

• A good initial guess can reduce the solution time

• In some cases a poor initial guess may cause the solver to fail
during the first few iterations

• The initial values can be set in 3 ways:
1. Solver automatically calculates the initial values
2. Initial values are entered by the user
3. Initial values are obtained from a previous solution

• Initial values can be set on a per-domain basis or globally for all
domains

Solver Settings
Initialization – Setting Initial Values Training Manual

• Insert Global Initialisation
from the toolbar or by right-
clicking on Flow Analysis 1

• Edit each Domain to set initial
values on a per-domain basis
– When both are defined the
domain settings take
precedence
– Solid domain must have
initial conditions set on a per-
domain basis


Solver Settings
Initialization – Setting Initial Values Training Manual

• The Automatic option means that the
CFX-Solver will calculate an initial value
for the solved variable unless a previous
results file is provided
– Will be based on boundary condition
values and domain settings

• The Automatic with Value option means
that the specified value will be used
unless a previous results file is provided
– Can use a constant value or an expression


Solver Settings
Initialization – Using a Previous Solution Training Manual

• To use a previous solution as the
initial guess enable the Initial Values
Specification toggle when launching
the Solver
– You can provide multiple initial values
files
• When simulating a system you can
provide previous solutions for each
component of the system as the initial
guess
• Usually each file would correspond to a
separate region of space
• It is best if domains in the Solver Input
File do not overlap with multiple initial
values files


Solver Settings
Solver Control – Editing Training Manual

• Edit the Solver Control object in the Outline tree


Solver Settings
Solver Control – Options Training Manual

• The Solver Control panel contains
various controls that influence the
behavior of the solver

• These controls are important for the
accuracy of the solution, the stability of
the solver and the length of time it takes
to obtain a solution


Solver Settings
Solver Control – Advection Scheme Training Manual

Generation
• The Advection Scheme refers to the way the
advection term in the transport equations is
modeled numerically
– i.e. the term that accounts for bulk fluid motion

Diffusion
– Often the dominant term

Advection

• Three schemes are available, High
Resolution, Upwind and Specified Blend
– Discussed in more detail next
Unsteady

• There is rarely any reason to change from the
default High Resolution scheme


Solver Settings
Solver Control – Advection Scheme Theory Training Manual

• Solution data is stored at nodes, but variable values are required
at the control volume faces to calculate fluxes

• The upstream nodal values (φ up) are interpolated to the integration
points (φ ip) on the control volume faces using:

φip = φup + β ∇φ ⋅ ∆r

– Where ∇φ is the variable gradient ∇φ ⋅ ∆r is the vector between the
φip = φup + β and
upstream node and the integration point
– In other words, the ip value is equal to the upstream value plus a
correction due to the gradient
– β can have values between 0 and 1 …


Solver Settings
Solver Control – Advection Scheme Theory Training Manual

Flow is misaligned
φip = φup + β ∇φ ⋅ ∆r with mesh
Theory

1
• If β = 0 we get the Upwind advection
scheme, i.e. no correction 0
– This is robust but only first order accurate
– Sometimes useful for initial runs, but
usually not necessary
Upwind Scheme

• The Specified Blend scheme allows you to
specify β between 0 and 1 (i.e. between no
correction up to full correction)
– But this is not guaranteed to be bounded,
β=1.00
meaning that when the correction is
included it can overshoot or undershoot
what is physically possible

• The High Resolution scheme maximizes β High Resolution
throughout the flow domain while keeping Scheme
the solution bounded

Solver Settings
Solver Control – Turbulence Numerics Training Manual

• Regardless of the Advection Scheme
selection, the Turbulence equations
default to the First Order (Upwind)
scheme
– Usually this is sufficient

• The High Resolution scheme can be
selected for additional accuracy
– Can give better accuracy in boundary
layers on unstructured meshes


Solver Settings
Solver Control – Convergence Control Training Manual

• The Solver will finish when it reaches Max.
Iterations unless convergence is achieved
sooner
– If Max. Iterations is reached you may not have
a converged solution
– Can be useful to set Max. Iterations to a large
number

• When the Solver finishes you should always
check why it finished

• Fluid Timescale Control sets the timescale in
a steady-state simulation …


Solver Settings
Solver Control – Timescale Background Training Manual

• ANSYS CFX employs the so called False Transient Algorithm
– A timescale is used to move the solution towards the final answer

• In a steady-state simulation the timescale provides relaxation of the
equation non-linearities

• A steady-state simulation is a “transient” evolution of the flow from the
initial guess to the steady-state conditions
– Converged solution is independent of the timescale used

Initial Guess
50 iterations
100 iterations
150 iterations

Final Solution


Solver Settings
Solver Control – Timescale Selection Training Manual

• For obtaining successful
convergence, the selection of the
timescale plays an important role

– If the timescale is too large, the
convergence becomes bouncy or
may even lead to the failure of the
Solver

– If the timescale is too small, the
convergence will be very slow and
the solution may not be fully
accurate


Solver Settings
Solver Control – Timescale Selection Training Manual

• For advection dominated flow, a fraction of the fluid residence time is
often a good estimate for the timescale
– A timescale of 1/3 of (Length Scale / Velocity Scale) is often optimal
– May need a smaller timescale for the first few iterations and for complex
physics, transonic flow,…..

• For rotating machines, 1/ω (ω in rad/s) is a good choice

• For buoyancy driven flows, the timescale should be based on a
function of gravity, thermal expansivity, temperature difference and
length scale (see documentation)


Solver Settings
Solver Control – Timescale Control Training Manual

• Timescale Control can be Auto Timescale,
Physical Timescale or Local Timescale
Factor

• Physical Timescale

– Specify the timescale. Usually a constant but
can also be variable via an expression

– Can often set a better timescale than Auto
Timescale would produce – faster
convergence


Solver Settings

• Auto Timescale
– The Solver calculates a timescale based on
boundary / initial conditions or current solution
and domain length scale

– Use a Conservative or Aggressive estimate for
the domain length scale, or a specified value

– Timescale is re-calculated and updated every
few iterations as the flow field changes

– Can set a Maximum Timescale to provide an
upper limit

– Tends to produce a conservative timescale

– Timescale factor (default = 1) is a multiplier
which can be changed to adjust the
automatically calculated timescale

Solver Settings

• Local Timescale Factor
– Timescale varies throughout the domain

Local Mesh Length Scale
Local Timescale =
Local Velocity Scale

Smaller Timescale in high
velocity and/or fine mesh regions
– Can accelerate convergence when vastly different local velocity scales exist
• E.g. a jet entering a plenum
– Best used on fairly uniform meshes, since small element will have a small
timescale which can slow convergence
– Local Timescale Factor is a multiplier of the local timescale
– Never use as final solution; always finish off with a constant timescale

Solver Settings
Solver Control – Convergence Criteria Training Manual

• Convergence Criteria settings determine
when the solution is considered converged
and hence when the Solver will stop
– Assuming Max. Iterations is not reached

• Residuals are a measure of how accurately
the set of equations have been solved
– Since we are iterating towards a solution, we never
get the exact solution to the equations
– Lower residuals mean a more accurate solution to
the set of equations (more on the next slide)
– Do not confuse accurately solving the equations
with overall solution accuracy – the equations may
or may not be a good representation of the true
system!
– Residuals are just one measure of accuracy and
should be combined with other measures:
• Monitor Points (ch. 8) and Imbalances (below)


Solver Settings
Solver Control – Residuals Theory Training Manual

• The continuous governing equations are discretized into a set of linear
equations that can be solved. The set of linear equations can be written in
the form:
[A] [Φ] = [b]

where [A] is the coefficient matrix and [Φ] is the solution variable

• If the equation were solved exactly we would have:

[A] [Φ] - [b] = [0]

• The residual vector [R] is the error in the numerical solution:

[A] [Φ] - [b] = [R]

• Since each control volume has a residual we usually look at the RMS
average or the maximum normalized residual


Solver Settings
Solver Control – Residuals Training Manual

• Residual Type
– MAX: Convergence based on maximum
residual anywhere
– RMS: Convergence based on average
residual from all control volumes

– Root Mean Square = ∑R
i
i
2

n

• Residual Target
– For reasonable convergence MAX residuals
should be 1.0E-3, RMS should be at least
1.0E-4
– The targets dependent on the accuracy
needed
• Lower values may be needed for greater
accuracy


Solver Settings
Solver Control – Conservation Target Training Manual

• The Conservation Target sets a target for the
global imbalances
Flux In − Flux Out
% Imbalance =
Maximum Flux

• The imbalances measure the overall
conservation of a quantity (mass, momentum,
energy) in the entire flow domain
• Clearly in a converged solution Flux In should equal Flux Out

• It’s good practice to set a Conservation Target and/or monitor the
imbalances during the run

• When set, the Solver must meet both the Residual and Conservation Target
before stopping (assuming Max. Iterations is not reached)

• Set a target of 0.01 (1%) or less
– Flux In – Flux Out < 1%


Solver Settings
Solver Control – Elapsed Time and Interrupt Control Training Manual

• Elapsed Time Control
– Can specify the maximum wall clock time
for a run
– Solver will stop after this amount of time
regardless of whether it has converged

• Interrupt Control
– Can specify other criteria for stopping
the Solver based on logical CEL
expressions
– When the expression returns true the
solver will stop
• Any value >= 0.5 is true
– Examples
• If temperature exceeds a specified value
if(areaAve(T)@wall>200[C],1,0)
• If mesh quality drops below a specified value in a moving mesh case
– More on logical expressions in the CEL lecture


Solver Settings
Solver Control – Solid Timescale Control Training Manual

• This option is only available when a solid
domain is included in the simulation

• The Solid Timescale should be selected such
that it is MUCH larger than the fluid timescale
(100 times larger is typical)
– the energy equation is usually very stable in the
solid zone
– solid timescales are typically much larger than
fluid timescales

• The fluid timescale is estimated using Length Scale / Velocity Scale

• The solid timescale is automatically calculated as function of the length
scale, thermal conductivity, density and specific heat capacity
– Or you can choose the Physical Timescale option and provide a timescale
directly


Solver Settings
Solver Control – Equation Class Settings Training Manual

• The Equation Class Settings tab is an
advanced option that can be used to
set Solver controls on an equation
specific basis
– Not usually needed
– Will override the controls set on Basic
Settings for the selected equation

• Advanced Options
– Advanced solver control options
– Rarely needed


Solver Settings
Output Controls – Results Training Manual

• The Output Control settings control the output
produced by the Solver
– The Trn Results, Trn Stats and Export tab only apply to
transient simulations and are covered in the Transient
chapter

• The Results tab controls the final .res file
– Generally do not use the Selected Variables (or None!)
option since it probably won’t contain enough
information to restart the run later
– Output Equation Residuals is useful if you need to
check where convergence problems are occurring
– Extra Output Variables List
contains variables that are not
written to the standard results
file
• E.g. Vorticity


Solver Settings
Output Controls – Backup Training Manual

• The Backup tab controls if and when
backup results files are automatically
written by the Solver

• Recommend for long Solver runs in case
of power failure, network interruptions, etc

• Option:
– Standard: Like a full results file
– Essential: Allows a clean solver restart
– Smallest: Can restart the solver, but there’ll
be a jump in the residuals
– Selected Variables: Not recommended

• Can also manually request a backup file
from the Solver Manager at any time

Frequency of output can be adjusted


Solver Settings
Output Controls – Monitor Training Manual

• The Monitor tab allows you to create Monitor
Points
– These are used to track values of interest as
the Solver runs

• The Cartesian Coordinates Option is used to
track the value of a variable at a specific X, Y,
Z location

• The Expression Option is used to monitor the
values of a CEL expression
– E.g. Calculate the area average of Cp at the
inlet boundary: areaAve(Cp)@inlet
– E.g. Mass flow of particular fluid through an
outlet: oil.massFlow()@outlet

• In steady-state simulations you should create
monitor points for quantities of interest
– One measure of convergence is when these
values are no longer changing


Solver Settings
Solver Manager Training Manual

• The CFX-Solver Manager is a graphical user interface used to:
– Define a run
– Control the CFX-Solver interactively
– View information about the emerging solution
– Export data


Solver Settings
Solver Manager – Defining a Run Training Manual

• Define a new Solver run

• Solver Input File should be the .def file
– Can also pick .res, .bak or _full.trn files to restart a
previous incomplete run

• To make a physics change and restart a solution,
create a new .def file and provide it as the Solver
Input File then select the .res, .bak or _full.trn file
in the Initial Values Specification section
– If both files have the same physics, this is the same
as picking the .res/.bak/_full.trn file as the input file

• Use Mesh From selects which mesh to use. If the
meshes are identical can use either option,
otherwise:
– If you use the Solver Input File mesh, the Initial
Values solution is interpolated onto the input file
– If you use the Initial Values mesh only the physics
from the Solver Input File is used

• Continue History From carriers over convergence
history and iteration counters

Solver Settings
Solver Manager – Defining a Parallel Run Training Manual

• By default the Solver will run in serial
– A single solver process runs on the local
machine

• Set the Run Mode to one of the parallel options
to make use of multiple cores/processors
– Requires parallel licenses
– Allows you to divide a large CFD problem into
smaller partitions
• Faster solution times
• Solve larger problems by making use of memory
(RAM) on multiple machines

• The Local Parallel options should be used
when running on a single machine

• The Distributed Parallel options should be
used when running across multiple machines


Solver Settings
Solver Manager – Defining a Parallel Run Training Manual

• Serial

• Local Parallel

• Distributed Parallel

• Different communication methods are available (MPICH2, HP MPI, PVM)
– See documentation “When To Use MPI or PVM” for more details, but HP MPI is
recommended in most cases


Solver Settings
Solver Manager – Define Run Advanced Controls Training Manual

• The Show Advanced Control toggle enables the
Partitioner, Solver and Interpolator tabs

• On the Partitioner tab you can pick different
partitioning algorithms
– Partitioning is always a serial process
– Can be a problem for v.large cases since you
cannot distribute the memory load across multiple
machines
– The default MeTiS algorithm uses more memory
than others, so if you run out of memory use a
different method (see documentation for details)

• Multidomain Option:
– Independent Partitioning: Each domain is
partitioned into n partitions
– Coupled Partitioning: All domains are combined
and then partitioned into n partitions
• There’s a specific option for Transient Rotor Stator
cases


Solver Settings
Solver Manager – Define Run Advanced Controls Training Manual

• On the Solver tab you can select the Double
Precision option
– The solver will use more significant figures in its
calculations
– Doubles solver memory requirements
– Use when round-off error could be a problem – if
‘small’ variations in a variable are important,
where ‘small’ is relative to the global range of
that variable, e.g:
• Many Mesh Motion cases, since the motion is often
small relative to the size of the domain
• Most CHT cases, since thermal conductivity is
vastly different in the fluid and solid
• If you have a wide pressure range, but small
pressure changes are important
– Small values by themselves do not need DP

• The Solver estimates its memory requirements upfront
• Memory Alloc Factor is a multiplier for this estimate
– Use when the solver stops with an “Insufficient Memory Allocated” error


Solver Settings
Solver Manager – Interactive Solver Control Training Manual

• During a solution Edit Run in Progress lets you make changes on the fly
– Models generally cannot be changed, but timescales, BC’s, etc can


Solver Settings
Solver Manager – Additional Solution Monitors Training Manual

• By default monitor plots
New Monitor
are created showing the
RMS residuals for each
equation solved, plus one
plot for any monitor points
• Right-click to switch
between RMS and MAX
• Additional monitors can be
selected showing:
– Imbalances
– Boundary fluxes (FLOW)
– Boundary forces
• Tangential (viscous) Right-click
• Normal (pressure)
– Source terms …

Monitor Plot .out file


Solver Settings
Solver Manager – Additional Icons Training Manual

• By dragging the cursor over any icon, the feature
description will appear

Start a new Switch
Simulation
Residual Plot
between
Monitor Stop Current RMS and
Finished Run Run MAX

Monitor Run Save Current
in Progress Run

Cfx12 04 solver

Empfohlen

Empfohlen

Weitere ähnliche Inhalte

Was ist angesagt?

Was ist angesagt? (13)

Andere mochten auch

Andere mochten auch (16)

Kürzlich hochgeladen

Kürzlich hochgeladen (20)

Cfx12 04 solver

Hinweis der Redaktion