Transcript CFX12 04 Solver
Chapter 4 Solver Settings
Introduction to CFX
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-1 April 28, 2009 Inventory #002598
Solver Settings
Overview
•
Initialization
•
Solver Control
•
Output Control
•
Solver Manager
Training Manual
Note: This chapter considers solver settings for steady-state simulations. Settings specific to transient simulation are discussed in a later chapter.
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-2 April 28, 2009 Inventory #002598
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.
3.
Initial values are entered by the user Initial values are obtained from a previous solution
•
Initial values can be set on a per-domain basis or globally for all domains
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-3 April 28, 2009 Inventory #002598
Solver Settings
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-4
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-5
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-6
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Editing
•
Edit the Solver Control object in the Outline tree
Training Manual
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-7 April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Options
•
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
Training Manual
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-8 April 28, 2009 Inventory #002598
Solver Settings
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 Unsteady Advection Diffusion Generation
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-9
Training Manual
April 28, 2009 Inventory #002598
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 (
f
up ) are interpolated to the integration points (
f
ip
) on the control volume faces using:
– f
ip
= f
up
+
r
f
ip
= f
up
+
upstream node and the integration point
r
– –
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 …
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-10 April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Advection Scheme Theory
f
ip
= f
up
+
r
Flow is misaligned with mesh
•
If
b
= 0 we get the Upwind advection scheme, i.e. no correction
– –
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
b
between 0 and 1 (i.e. between no correction up to full correction)
–
But this is not guaranteed to be bounded, meaning that when the correction is included it can overshoot or undershoot what is physically possible
b =1.00
Training Manual
Theory
1 0
•
The High Resolution scheme maximizes
b
throughout the flow domain while keeping the solution bounded
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-11 High Resolution Scheme April 28, 2009 Inventory #002598
Solver Settings
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
Training Manual
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-12 April 28, 2009 Inventory #002598
Solver Settings
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 …
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-13
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Timescale Background
•
ANSYS CFX employs the so called False Transient Algorithm
–
A timescale is used to move the solution towards the final answer
Training Manual
•
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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-14 April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Timescale Selection
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-15
Training Manual
April 28, 2009 Inventory #002598
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/
(
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)
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-16 April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Timescale Control
•
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
Training Manual
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-17 April 28, 2009 Inventory #002598
Solver Settings
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
upper limit to provide an – Tends to produce a conservative timescale – Timescale factor (default = 1) is a multiplier which can be changed to adjust the automatically calculated timescale ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-18
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Timescale Control
•
Local Timescale Factor
– Timescale varies throughout the domain
Local Timescale = Local Mesh Length Scale Local Velocity Scale Training Manual
–
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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
; always finish off with a constant timescale 4-19 April 28, 2009 Inventory #002598
Solver Settings
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) ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-20
Training Manual
April 28, 2009 Inventory #002598
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-21 April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Residuals
•
Residual Type
–
MAX: Convergence based on maximum residual anywhere
– –
RMS: Convergence based on average residual from all control volumes Root Mean Square =
i R 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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-22
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Conservation Target
•
The Conservation Target sets a target for the global imbalances
% Imbalance Flux In Flux Out 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
Training Manual
•
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%
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-23 April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Elapsed Time and Interrupt Control
•
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
Training Manual
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-24 April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Solid Timescale Control
•
This option is only available when a solid domain is included in the simulation
Training Manual
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-25 April 28, 2009 Inventory #002598
Solver Settings
Solver Control – Equation Class Settings
•
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
Training Manual
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-26 April 28, 2009 Inventory #002598
Solver Settings
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-27
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
Output Controls – Backup
•
The Backup tab controls if and when backup results files are automatically written by the Solver
Training Manual
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-28 April 28, 2009 Inventory #002598
Solver Settings
Output Controls – Monitor
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-29
Training Manual
April 28, 2009 Inventory #002598
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-30 April 28, 2009 Inventory #002598
Solver Settings
Solver Manager – Defining a Run
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-31
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-32
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
Solver Manager – Defining a Parallel Run
•
Serial
•
Local Parallel
Training Manual
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-33 April 28, 2009 Inventory #002598
Solver Settings
Solver Manager – Define Run Advanced Controls
•
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-34
Training Manual
April 28, 2009 Inventory #002598
Solver Settings
Solver Manager – Define Run Advanced Controls
•
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
Training Manual
• •
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-35 April 28, 2009 Inventory #002598
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
ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-36 April 28, 2009 Inventory #002598
Solver Settings
Solver Manager – Additional Solution Monitors
• •
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
Right-click Monitor Plot ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-37
Training Manual
.out file April 28, 2009 Inventory #002598
Solver Settings
Solver Manager – Additional Icons
•
By dragging the cursor over any icon, the feature description will appear
Start a new Simulation Monitor Finished Run Stop Current Run
Training Manual
Switch Residual Plot between RMS and MAX Monitor Run in Progress ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.
4-38 Save Current Run April 28, 2009 Inventory #002598