Chapter 4 Solver Settings

1. Chapter 4Solver Settings Introduction to CFX

2. 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.

3. Initialization • 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: • Solver automatically calculates the initial values • 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

4. 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

5. 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

6. 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

7. Solver Control – Editing • Edit the Solver Control object in the Outline tree

8. 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

9. Unsteady Generation Advection Diffusion 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

10. 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 (fup) are interpolated to the integration points (fip) 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 …

11. Solver Control – Advection Scheme Theory Flow is misaligned with mesh Theory • 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 • 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 • The High Resolution scheme maximizes b throughout the flow domain while keeping the solution bounded 1 0 Upwind Scheme =1.00 High Resolution Scheme

12. 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

13. 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 …

14. Initial Guess 50 iterations 100 iterations 150 iterations Final Solution 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 • 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

15. 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

16. 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/ ( 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)

17. 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

18. 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

19. Solver Control – Timescale Control • 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 Mesh Length Scale Local Velocity Scale Local Timescale = Smaller Timescale in high velocity and/or fine mesh regions

20. 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)

21. Solver Control – Residuals Theory • 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

22. 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 = • 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

23. 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 • 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%

24. 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 • 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

25. Solver Control – Solid Timescale Control • 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

26. 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

27. 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 Listcontains variables that are notwritten to the standard resultsfile • E.g. Vorticity

28. 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 Frequency of output can be adjusted

29. 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

30. Solver Manager • 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

31. 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

32. 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

33. Solver Manager – Defining a Parallel Run • 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

34. 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

35. 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 • 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

36. 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

37. 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 .out file Monitor Plot

38. Solver Manager – Additional Icons • By dragging the cursor over any icon, the feature description will appear Start a new Simulation Switch Residual Plot between RMS and MAX Monitor Finished Run Stop Current Run Monitor Run in Progress Save Current Run