Design

1. ANSYS Fluent Introduction Course
Some Best Practice Guidelines…
by Tomer Avraham
Senior CFD specialist
All About CFD

2. CFD Modeling Goals
• Modeling goals are strongly dependent upon the following:
⮚Results to be achieved.
⮚Simplifying assumptions to be made and whether they actually can be made.
⮚Physical models to be included and the exploration of their range of validity.
⮚Regarding the above, retain an expected accuracy considering the statistical measures
achieved.
⮚Retain how quickly the results are to be achieved.
Remember:
• All of the above goals interact with each other. Finding the an optimum is achieved only by weighing each of
the goals (no free lunch…).

3. CFD Workflow
1. Define the model problem at hand according to CFD modeling goals.
2. Perform pre-calculation to establish a better understanding of the problem at hand, achieving bounds and
a route for exploration.
3. Simplify the model geometry to account for approximations (e.g. symmetry/periodic) and exclude CFD
passive features (e.g. bolts).
4. Define a domain to include only physical result. Realizable/synthetic boundary conditions should be
accommodated.
5. Define mesh resolution to according to appropriate features (computer resources, physics, numerical
description, turbulence and other physics models, prediction of high gradients, etc…).

4. CFD Workflow
6. Set up the solver:
⮚Select appropriate physical models (turbulence, combustion, radiation, multiphase,
etc…) to conform with the physics of the model problem.
⮚Define material properties for solid/fluid/mixture to conform with the physics model.
⮚Prescribe operating and boundary conditions to conform with physics of the model
problem and the definition of the domain.
⮚Prescribe initial conditions or initial values based on an “educated guess” or previous
solution.
⮚Set up the solver type (density or pressure based and steady or transient).
⮚Choose an solution algorithm (pressure-velocity coupling for formulation and flux
methodology for pressure and density based solvers respectively) to conform with the
physics of the model problem.
⮚Set up spatial and/or temporal discretization according to the level of accuracy to be
achieved and tune the solution controls (under-relaxation factors, intrinsic iteration
loops, multigrid) to promote convergence or accelerate convergence (tradeoff).
7. Set up solution monitors of both equation residuals and key quantitative measurements.

5. CFD Workflow
6. Compute the solution by iteratively solving the discretized conservation equations until convergence is
achieved (changes in solution variables monitored by residuals, overall imbalances minimization and
unchanged quantities of interest).
7. Examine the results assisting specialized post-processing tools:
⮚Overall pattern produce physical results.
⮚Key features according to the physics of the model problem are resolved.
⮚Flux balances are conform.
⮚Comparison of integral quantities (e.g. drag or lift) and flow statistics (according to
applicable level deemed by the physical model) such as: mean velocity profile (first order
statistics), R.M.S. profile (first order statistics), PSD(one-point spectral analysis), correlations
(two-point spectral analysis), etc…
8. Consider revising the model:
⮚Physical models: resolving physical features.
⮚Boundary/initial conditions: adequate domain, switch to prescribed realizable BC/IC, adjust
boundary zones values.
⮚Mesh: replace topology, revise boundary-layer description, change resolution, etc…).
Repeat

6. Geometry Repair and Simplification
Why Repair?
• Several translation methods available
to enable data exchange with
CAD/CAE systems
– Direct Integration/CAD Readers
– Import of generic CAD formats
(IGES, ACIS etc)
• Translation can:
– Return incomplete, corrupt, or
disconnected geometry
• Requires repair
– Return geometry details
unnecessary for CAE analysis
• Requires defeaturing
How to Fix?
• Geometry cleanup
– Processes required to prepare
geometry for meshing
• Fix incomplete or corrupt
geometry and connect
disconnected geometry
• Remove unnecessary details
(defeaturing)
• Decompose geometry into
meshable sections

7. • Many potential issues
• Missing faces
• Sliver faces
• Hard edges
• Small edges
• Sharp angles
• Others …
These issues must be fixed to
• Create watertight volume bodies
• Prevent meshing issues
Typical Geometry Translation Issues
Missing faces Sliver faces
Hard Edges Small edges Sharp angles

8. • Repair Holes
Typical Geometry Simplification Issues
Holes in a solid body Holes removed
Use SpaceClaim power
selection!
Hole in a surface body Hole removed

9. Meshing: Fluent Mesh Workflow
• CAD Import
• CFD Surface Mesh
• With curvature and proximity according to geometry
• Surface Mesh
• Separate Faces, Merge and Rename, set initial BC
• Set Scoped Size Field
• Remesh globally and/or locally
• Diagnostics & Repair
• For skewed faces - geometry local remesh recommended
• Volumetric Region
• Change types and names
• Automesh
• Inflation
• Start with default settings and investigate
• Cell Correction if Needed
• Auto-node move

10. Fix Connectivity/Quality Global Remesh Local Remesh

11. Meshing Best Practice Guidelines

12. Meshing Best Practice Guidelines – Skewness:
• Skewness Triangles/Tet:
Equilateral volume deviation:
• Skewness Hexa/Prism/Pyramids:
Normalized angle deviation:
• Mesh Quality:
• Skewness < 0.9 for the volumetric mesh (require surface mesh skewness <0.7).
• Consider defeaturing of areas susceptible for unavoidable highly skewed mesh such
as created by low spatial angle of intersecting surfaces.

13. Meshing Best Practice Guidelines – Aspect Ratio and Smoothness:
• Aspect ratio in 2D is according to length/height ratio and in 3D according to the area ratio or that
between circumscribed to inscribed circles.
• “High” aspect ratio is acceptable for instances where no high cross-stream gradient exists (such as
boundary layers)
• Smoothness is checked in the solver as part of the Volume Adaptation function.

14. Meshing Best Practice Guidelines – Topology

15. Solver: Pressure-Based Vs. Density-Based

16. Pressure Based Solver Best Practice Guidelines
⮚Pressure-based is the default and should be used for most problems. Handles the range of Mach numbers
from 0 to ~2-3
⮚Density-based is normally only used for higher Mach numbers, or for specialized cases such as capturing
interacting shock.
⮚Pressure-based segregated “projection algorithms” (SIMPLE/SIMPLEC/PISO) may be controled to stabilize
convergence through “under-relaxation” factors, taking in mind that this shall in turn decelerate the
convergence process.
⮚Pressure-based coupled algorithm may be controlled for stabilization by reducing the courant number
from 200 (default) to 10-50 (flow dependent).
⮚Better stabilization of the convergence process (especially for high aspect-ratio meshes) of the pressure-
based coupled solver is achieved by using the pseudo-transient option while in the Advanced… option for
Run Calculation checking for Length Scale Method the Conservative option for internal flow and the User
Specified (with characteristic length scale of the geometry such as plate length) for external flows.

17. Pressure Based Solver Best Practice Guidelines
⮚One may promote convergence by initially applying a segregated algorithm such as SIMPLE (with or
without reduced under-relaxation factors) then after a seeming initial trend towards residual convergence
switch to a coupled algorithm to accelerate convergence.

18. Density Based Solver Best Practice Guidelines
⮚The density-based solver is applicable when there is a strong coupling, or interdependence, between
density, energy, momentum, and/or species.
⮚The density-based solver may be implicit or explicit. Explicit methods calculate the state of a system at a
later time from the state of the system at the current time, while implicit methods find a solution by
solving an equation involving both the current state of the system and the later one.
⮚The implicit option is slower to converge but is less sensitive to Courant-Friedrich-Levy (CFL)
condition. Implicit methods are used for problems arising in practice are stiff, for which the use of an
explicit method requires impractically small time steps due to harsh bounds on CFL number.
⮚Hence the implicit approach should be chosen for most density-based solver application applications such
as: High speed compressible flow with combustion, hypersonic flows, shock interactions, etc…
⮚Explicit approach is used for specialized cases where the characteristic time scale of the flow is on the
same order as the acoustic time scale (and so the boun on CFL number is obvious) for cases such as (e.g.
propagation of high-Mach shock waves).

19. Spatial Discretization – Best Practice Guidelines

20. Spatial Discretization – Best Practice Guidelines

21. Time Dependent Problems - Best Practice Guidelines
⮚Time step should be chosen such that the residuals will reduce by three orders of magnitude.
⮚The Courant number serves as conservative estimate for time step (Typical values 1-10):
⮚Estimation according to generic problems:

22. Time Dependent Problems - Best Practice Guidelines
⮚Initial conditions are critically important. Perform a preliminary steady-state simulation that shall act as
initial conditions for the transient problem.
⮚Avoid including results for the first few time steps where before settling trend of the residuals is seeming.
⮚Select the number of iterations per time step to be around 20.
⮚Reduce the time step to achieve better conditions instead of increasing the number of iterations per time-
step.
⮚For pressure-based solver (that do not include: DO radiation, DPM, Mixture Multiphase, etc…)
convergence may be highly accelerated by invoking a Non-Iterative Time Advancement (NITA) algorithm
(Transient Formulation in Solution Methods).
⮚Use Data Sampling for Time Statistic to achieve the following (crucial for validation):

23. Modeling of Turbulence:
⮚ Three basic approaches according to fidelity level:

24. Modeling of Turbulence:
⮚ For RANS we solve time (or ensemble) averaged NSE:
Time/ensemble average

25. Modeling of Turbulence:
Reynolds Averaged Simulation (RANS)
⮚ Different turbulence models goal is to relate the unknown Reynolds stress tensor to the mean velocity
field (actually derivatives of the velocity field) and other flow related quantities. These models can be
divided into two main categories: (a) eddy-viscosity models and (b) non-eddy viscosity models. Eddy
viscosity models invoke the Boussinesq approximation that enforces a linear relationship between the
Reynolds stress tensor and the mean strain-rate tensor with a so-called scalar eddy viscosity serving as
the isotropic proportionality factor:
⮚ Since the eddy viscosity is a property of the flow rather than the fluid (in contrast to kinematic viscosity)
additional equations must be added to solve for the additional variable – Turbulent Model

26. Modeling of Turbulence – Best Practice Guidelines
⮚ Taken from ANSYS Fluent Course Recommendations:

27. Modeling of Turbulence – Best Practice Guidelines
⮚ Aim to achieve y+<5 for problem of which the viscous sub-layer integration is crucial (such as heat transfer,
drag calculation, etc…).
⮚ The number of layers for capturing the boundary-layer should be 10-20. This concern proceeds that of a
small y+.
⮚ Perform an initial calculation for the physical unit y needed to achieve an initial representation of the BL:

28. References
⮚ ANSYS FLUENT: Introductory FLUENT Notes
⮚ Turbulence Modeling for CFD (David C. Wilcox)
⮚ “ALL About CFD Blog…” - https://allaboutcfd-tomersblog.com/2020/04/02/all-about-cfd-index/
⮚ Large Eddy Simulation, Dynamic Model, and Applications - Charles Meneveau (Department of Mechanical Engineering Center
for Environmental and Applied Fluid Mechanics Johns Hopkins University)
⮚ Turbulence: Subgrid-Scale Modeling (Scholarpedia) doi:10.4249/scholarpedia.9489
⮚ Wall-modeled large eddy simulation resource (university of Maryland)
⮚ Turbulence Modeling Resource (NASA Langley Research Center)
⮚ Improved two-equation k-omega turbulence models for aerodynamic flows (F. Menter 1992)
⮚ Transition Modelling for Turbomachinery Flows (F. Menter, R.B. Langtry – ANSYS 2012)
⮚ Development of DDES and IDDES Formulations for the k-ω Shear Stress Transport Model (F. Menter, M. Gritskevich, A.
Gritskevich, J. Schütze)
⮚ The Scale-Adaptive Simulation Method for Unsteady Turbulent Flow Predictions. Part 1/2: Theory and Model
Description/Application to Complex Flows (F. Menter et al. 2010)
⮚ The DESIDER Project - http://cfd.mace.manchester.ac.uk/desider/index2.html
⮚ The State of the Art of Hybrid RANS/LES Modeling for the Simulation of Turbulent Flows (Bruno Chaouat 2017)
⮚ Introductory Lectures On Turbulence - Physics, Mathematics and Modeling (J. M. McDonough - University of Kentucky)

29. HAPPY
Contact:
Email:
Avr.Tomer@gmail.com
Mobile: 054-3551807