CFD Simulation Setup Checklist: What to Define Before You Run

The cost of "Garbage In, Garbage Out" in Computational Fluid Dynamics (CFD) is high. A single poor assumption or an ill-posed boundary condition can ruin an otherwise perfect mesh, leading to divergence, unphysical results, or wasted compute time. Pre-simulation planning is often more critical than the actual solver run time.

If you follow this checklist before hitting compute, you will drastically reduce the chances of encountering a diverging solution or producing misleading data.

Disclaimer: This checklist is a general guideline. Always consult your specific solver documentation and validate against empirical data. Engineering judgment is strictly required.

---

Phase 1: Problem Definition

Before launching your CAD or meshing software, explicitly define your physics and goals:

• Goal: What specific engineering question are you trying to answer? (e.g., "What is the pressure drop across the valve?" or "Does the wing stall at 15 degrees angle of attack?").
• Fluid Properties: What are the density ($\rho$), dynamic viscosity ($\mu$), and thermal conductivity ($k$) of your fluid? Are they constant, temperature-dependent, or pressure-dependent?
• Flow Regime: Is the flow compressible or incompressible? Calculate your Mach number ($Ma$).
• Turbulence: What is the expected Reynolds number ($Re$)? Will the flow be strictly laminar, or fully turbulent? Tool: Estimate your bulk flow characteristics using our Reynolds Number Calculator.
• Time Dependence: Is the physics fundamentally steady-state, or do you expect transient behavior (e.g., vortex shedding, fluctuating loads)?

Phase 2: Geometry & Domain

A simulation is only as good as its geometric inputs. Clean up your CAD models to prevent meshing failures and artificial flow restriction:

• Defeaturing: Have you removed small fillets, chamfers, nuts, and bolts that do not significantly affect the bulk flow?
• Fluid Volume: Is the fluid volume properly extracted? Ensure there are no microscopic gaps or overlapping surfaces.
• Symmetry: Can the geometry and expected flow field be modeled using a symmetry plane to reduce computational cost?
• Domain Sizing: Placing boundaries too close to the region of interest artificially restricts the flow.
  • Upstream: Is the inlet far enough upstream (typically 5-10 characteristic lengths) to allow flow to fully develop?
  • Downstream: Is the outlet far enough downstream (typically 10-20 characteristic lengths) to capture the entire wake and prevent reversed flow?
  • Far-field/Walls: For external aerodynamics, is the bounding box sufficiently large (e.g., 20x the object size) to prevent artificial wind-tunnel blockage effects?

Phase 3: Meshing Strategy

A high-quality mesh is the foundation of a converging simulation:

• Cell Type Choice: Are you using hexahedral, tetrahedral, or polyhedral cells? Have you aligned the mesh with the primary flow direction where possible?
• Mesh Quality Checks: Poor cell quality leads directly to numerical diffusion and divergence. Before exporting the mesh:
  • Skewness: Is the maximum skewness below 0.95 (preferably below 0.85 for most cells)?
  • Orthogonal Quality: Is the minimum orthogonal quality above 0.1?
  • Aspect Ratio: Have you avoided extreme aspect ratios (e.g., > 1000) except inside properly aligned boundary layer inflation layers?
• Boundary Layer Resolution: The near-wall region dictates shear stress and heat transfer.
  • If using a turbulence model that resolves the viscous sublayer (like SST $k-\omega$), ensure $y^+ \approx 1$.
  • If using wall functions, ensure your $y^+$ is in the log-law region ($30 < y^+ < 300$). Tool: Use our y+ First Cell Height Calculator and Boundary Layer Thickness Calculator to plan your inflation layers. Further Reading: How to Estimate y+ and First Cell Height
• Grid Independence Planning: Do you have a plan to generate coarse, medium, and fine meshes to verify that your results do not depend on the grid resolution? Tool: Plan for the Grid Convergence Index.

Phase 4: Physics & Boundary Conditions

Ensure your physics models represent reality and your boundary conditions are mathematically well-posed:

• Turbulence Models: Select a model suited for your physics. Note: There is no single "best" model.
  • $k-\epsilon$: Often suitable for free-shear flows and fully turbulent internal flows.
  • SST $k-\omega$: Often preferred for adverse pressure gradients and flow separation, provided the near-wall mesh is adequately refined.
• Inlet & Outlet BCs: Are your boundary conditions placed in regions of calm, uniform flow? Have you avoided over-constraining the domain (e.g., specifying mass flow at both the inlet and outlet in an incompressible flow)?
  • Best Practice: Use a Velocity/Mass Flow Inlet with a Static Pressure Outlet.
  • Avoid placing outlets in regions of strong recirculation, which can cause "reversed flow" instability.
• Turbulence BCs: Have you provided realistic turbulent intensity and length scales at the inlets? Guessing 5% intensity everywhere is often inaccurate. Tool: Use our Inlet Turbulence Boundary Conditions Calculator to define realistic values.
• Wall Conditions: Are the walls set to no-slip? Have you defined appropriate thermal boundary conditions (adiabatic, fixed temperature, or heat flux)?
• Initial Conditions: A good initial guess prevents immediate divergence on iteration 1.
  • Have you initialized the flow field with realistic values?
  • Consider using hybrid initialization or computing from the main inlet to establish a realistic baseline velocity and pressure field before starting the solver.

Phase 5: Solver & Numerics

Match the solver numerics to your accuracy and stability requirements:

• Discretization Schemes: Are you using at least Second-Order Upwind for momentum and energy equations to minimize numerical diffusion? (First-order may be used temporarily for initial stability, but should not be used for final results).
• Pressure-Velocity Coupling: For steady-state incompressible flows, is the coupling scheme appropriate (e.g., SIMPLE or SIMPLEC for steady flows, PISO for transient)?
• Steady-State Solver Controls & Relaxation: If using a steady-state pressure-based solver, have you verified the Under-Relaxation Factors (URFs)? If the solution diverges early, lowering momentum and pressure URFs can improve stability. However, lowering URFs too much can lead to "false convergence" where residuals drop artificially without finding the physical solution. Watch out for stability warning signs such as severe oscillations, divergence, reversed flow at outlets, or growing mass imbalance.
• Transient Time-Stepping Strategy: For transient simulations, your time step ($\Delta t$) must be small enough to resolve the fastest-moving flow features. The relationship between mesh size ($\Delta x$), velocity scale ($U$), and time step is governed by the Courant (CFL) number.
  • Explicit Solvers: Ensuring the Courant number is strictly $CFL < 1$ is an absolute requirement for mathematical stability. If the solver diverges, you must either decrease the time step or locally coarsen the mesh.
  • Implicit Solvers: A higher CFL (e.g., 5-50) may be numerically stable, but temporal accuracy will degrade if the time step is too large to capture the relevant physical scales. Always perform a time-step independence study. Workflow: Estimate your velocity scale using the Reynolds Number Calculator, verify your mesh size using the Grid Convergence Index Calculator, and then plan your time step using the Courant Number Calculator.

Phase 6: Convergence & Validation

Define how you will know when the simulation is finished and if the data is reliable:

• Residual Targets: Have you set strict residual monitors (e.g., $10^{-4}$ to $10^{-5}$ for standard flows, tighter for energy/heat transfer)? A flat residual curve indicates the solver is stuck, not converged.
• Monitor Points: Did you set up point or surface monitors for key engineering values (e.g., drag coefficient, average outlet temperature, or pressure drop)?
  • Rule of Thumb: A simulation is generally considered converged only when both residuals drop to acceptable levels and the critical engineering monitors flatten out over many iterations. Further Reading: CFD Convergence: Why Residuals Are Not Enough
• Mass Balance: Does mass flow in equal mass flow out exactly? The net mass imbalance should ideally be less than 0.1% of the total inlet mass flow.
• Comparison Against Empirical Data: Do you have experimental validation data or analytical solutions to compare against your CFD results?

Conclusion & Summary Checklist

Before clicking "Calculate", review this summary checklist:

| Phase | Check | | :--- | :--- | | Problem | Flow regime (Compressible/Incompressible, Steady/Transient) defined. | | Geometry | Geometry cleaned, defeatured, and fluid volume extracted. | | Domain | Domain extended sufficiently upstream and downstream to avoid artificial boundary effects. | | Mesh | Boundary layer meshed to appropriate $y^+$ target. Mesh quality metrics within solver limits. | | Physics | Material properties, operating conditions, and turbulence models verified. | | Boundary | Boundary conditions are mathematically well-posed (no conflicting mass constraints). | | Solver | Spatial discretization set to 2nd Order. | | Convergence| Engineering monitors (Drag, Pressure Drop, etc.) created alongside residual monitors. | | Initial | Flow field initialized with realistic values. |

Following these steps rigorously will not guarantee a perfect simulation on the first try, but it will significantly reduce unforced errors and save hours of debugging diverged runs.