4

1
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Chapter 4
Solver Settings
Introduction to CFX
Solver Settings
4

2
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Overview
•
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
4

3
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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
Initialization
Solver Settings
4

4
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Initialization
–
Setting Initial Values
•
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
4

5
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Initialization
–
Setting Initial Values
•
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
4

6
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Initialization
–
Using a Previous Solution
•
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
4

7
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
•
Edit the Solver Control object in the Outline tree
Solver Control
–
Editing
Solver Settings
4

8
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Control
–
Options
Solver Settings
4

9
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Advection Scheme
•
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
–
Often the dominant term
•
Three schemes are available,
High
Resolution
,
Upwind
and
Specified Blend
–
Discussed in more detail next
•
There is rarely any reason to change from the
default High Resolution scheme
Unsteady
Advection
Diffusion
Generation
Solver Settings
4

10
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Advection Scheme Theory
•
Solution data is stored at nodes, but variable values are required at
the control volume faces to calculate fluxes
•
The upstream nodal values (
f
u
p
) are interpolated to the integration
points (
f
ip
) on the control volume faces using:
–
Where is the variable gradient and is the vector between the
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
–
b
can have values between 0 and 1 …
f
i
p
f
u
p
b
f
r
+
=
f
f
i
p
f
u
p
b
f
r
+
=
Solver Settings
4

11
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Advection Scheme Theory
•
If
b
㴠=⁷攠来琠瑨攠
Upwind
advection
scheme, i.e. no correction
–
This is robust but only first order accurate
–
Sometimes useful for initial runs, but
usually not necessary
•
The
Specified Blend
scheme allows you to
specify
b
扥瑷敥渠〠0湤ㄠ⡩1攮e扥瑷敥渠湯
捯牲散瑩t渠異瑯畬t捯牲散瑩t温
–
But this is not guaranteed to be bounded,
meaning that when the correction is
included it can overshoot or undershoot
what is physically possible
•
The
High Resolution
scheme maximizes
b
throughout the flow domain while keeping
the solution bounded
f
i
p
f
u
p
b
f
r
+
=
Theory
High Resolution
Scheme
Upwind Scheme
b
=1.00
Flow is misaligned
with mesh
0
1
Solver Settings
4

12
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Turbulence Numerics
•
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
4

13
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Convergence Control
•
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
4

14
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Control
–
Timescale Background
Solver Settings
4

15
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Control
–
Timescale Selection
Solver Settings
4

16
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Timescale Selection
•
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/
(
楮i牡搯猩r楳i愠杯潤a捨潩捥
•
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
4

17
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Control
–
Timescale Control
Solver Settings
4

18
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Timescale Control
•
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
4

19
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
•
Local Timescale Factor
–
Timescale varies throughout the domain
–
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
Local Timescale =
Local Mesh Length Scale
Local Velocity Scale
Smaller Timescale in high
velocity and/or fine mesh regions
Solver Control
–
Timescale Control
Solver Settings
4

20
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Convergence Criteria
•
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
4

21
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Control
–
Residuals Theory
Solver Settings
4

22
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
•
Residual Type
–
MAX: Convergence based on maximum
residual anywhere
–
RMS: Convergence based on average
residual from all control volumes
–
Root Mean Square =
•
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
n
2
i
i
R
Solver Control
–
Residuals
Solver Settings
4

23
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Control
–
Conservation Target
•
The
Conservation Target
sets a target for the
global imbalances
•
The imbalances measure the overall
conservation of a quantity (mass, momentum,
energy) in the entire flow domain
Flux
Maximum
Out
Flux
In
Flux
Imbalance
%
•
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
4

24
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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
Solver Control
–
Elapsed Time and Interrupt Control
–
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
4

25
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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
Solver Control
–
Solid Timescale Control
•
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
4

26
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Control
–
Equation Class Settings
Solver Settings
4

27
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Output Controls
–
Results
•
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
4

28
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Frequency of output can be adjusted
Output Controls
–
Backup
•
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
Solver Settings
4

29
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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
Output Controls
–
Monitor
Solver Settings
4

30
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Manager
Solver Settings
4

31
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Manager
–
Defining a Run
Solver Settings
4

32
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Manager
–
Defining a Parallel Run
•
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
4

33
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Manager
–
Defining a Parallel Run
Solver Settings
4

34
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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 Manager
–
Define Run Advanced Controls
Solver Settings
4

35
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
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
Solver Manager
–
Define Run Advanced Controls
•
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
4

36
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Solver Manager
–
Interactive Solver Control
•
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
4

37
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
.out file
Monitor Plot
Solver Manager
–
Additional Solution Monitors
Right

click
•
By default monitor plots
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)
•
Normal (pressure)
–
Source terms …
New Monitor
Solver Settings
4

38
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
April 28, 2009
Inventory #002598
Training Manual
Start a new
Simulation
Monitor Run
in Progress
Monitor
Finished Run
Stop Current
Run
Save Current
Run
Switch
Residual Plot
between
RMS and
MAX
•
By dragging the cursor over any icon, the feature
description will appear
Solver Manager
–
Additional Icons
Comments 0
Log in to post a comment