Best Practices

Best Practices#

Guidelines for getting accurate, reliable results from Gradient Dynamics Studio.

Geometry Preparation#

Start with a Clean Geometry#

  • Always run geometry analysis before meshing — catch problems early

  • Use STEP format for CAD files — it preserves topology that helps meshing and surface identification

  • Simplify complex assemblies — remove small features (screws, bolts, labels) that don’t affect flow

  • Close gaps and holes — the geometry must be watertight for volume meshing

  • Remove internal surfaces — overlapping or duplicate faces cause cut-cell meshing errors

Geometry Scale#

  • Verify your geometry is in the correct units (meters)

  • A car should be ~4.5 m long, not 4500 (millimeters) or 0.0045 (micrometers)

  • Incorrect scale leads to wrong mesh sizes, Reynolds numbers, and results

Meshing#

Start Coarse, Then Refine#

  1. Coarse mesh first — Run a quick mesh (lower AMR levels) to verify the setup

  2. Check quality — Review cut-cell volume fractions and any flagged problem cells

  3. Refine — Increase AMR levels and regenerate

  4. Compare — Check that key quantities (Cd, pressure drop) change by < 5% between meshes

This “mesh independence study” ensures your results are not artifacts of the mesh resolution.

Near-Wall Resolution#

  • Use the y+ calculator to determine the appropriate near-wall AMR level for your flow speed and turbulence model

  • y+ ≈ 30 (wall-function RANS, medium surface refinement) works well for most external aerodynamics

  • y+ ≈ 1 (wall-resolved, fine or very fine surface refinement) is needed for LES, detailed heat transfer, or sensitive separation

  • Do not over-refine walls unnecessarily — each additional near-wall AMR level multiplies local cell count significantly

Refinement Zones#

  • Focus refinement where it matters — wakes, separation zones, stagnation regions

  • Don’t over-refine far-field regions — cells far from the geometry contribute little to accuracy

  • Avoid extreme level jumps — 2–3 AMR level difference between adjacent regions is the practical limit

  • Cover the full wake — for bluff bodies, the wake zone should extend at least 3× body length downstream

Domain Sizing#

  • Too small is worse than too large — boundary effects contaminate the solution

  • External flow: Minimum 1.5× upstream, 3× downstream, 1.5× sides

  • Internal flow: Ensure adequate inlet development length (10× hydraulic diameter)

  • When in doubt, go larger — the extra cells are cheap compared to a wrong solution

Simulation#

Solver Type#

Use the density-based solver (the default) for all standard CFD applications. It runs significantly faster on GPU hardware than the pressure-based solver and produces equivalent accuracy for incompressible flows via low-Mach preconditioning. Reserve the pressure-based solver only for cases that specifically require an incompressible formulation.

Turbulence Model Selection#

Situation

Recommended Model

First analysis / general purpose

k-ω SST

Industrial pipe/duct flow

k-ε

Quick preliminary study

Spalart-Allmaras

Strong swirl or rotation

RSM

Unsteady/acoustic analysis

LES

Convergence#

  • Monitor residuals — density residual should decrease monotonically to at least 1e-5

  • Check integrated quantities — Cd, Cl, pressure drop should plateau before you declare convergence

  • Residuals alone are not sufficient — a simulation can have low residuals but wrong results if the setup is incorrect

  • Run enough iterations — 500 minimum for RANS, 1000+ for complex geometries

  • Use CFL ramping for difficult starting conditions — let the solver build up gradually

Common Pitfalls#

Pitfall

Consequence

Prevention

Forgetting moving ground for vehicle aero

Unrealistic ground boundary layer

Set ground as moving wall at freestream speed

Wrong turbulence intensity at inlet

Incorrect turbulence levels in domain

Use 1% for external, 5% for internal

CFL too high at startup

Immediate divergence

Enable CFL ramping; start at CFL 0.5

Coarse mesh near features of interest

Inaccurate local flow

Add refinement zones at correct AMR level

Ignoring mesh quality warnings

Poor convergence or wrong results

Inspect flagged cut-cells before simulating

Using pressure-based solver for large meshes

Slow GPU performance

Switch to density-based solver

Post-Processing#

Validate Your Results#

  • Compare with known data — use published Cd values, analytical solutions, or experimental data where available

  • Check mass conservation — inlet and outlet mass flow rates should match within 0.1%

  • Look for non-physical artifacts — negative pressures in unexpected places, symmetric flow that should be asymmetric, etc.

  • Verify force coefficients — are they in the expected range for your geometry type?

Effective Visualization#

  • Start with surface coloring — pressure on the body shows the overall flow structure

  • Use slice planes — mid-span/centerline cuts reveal internal flow patterns

  • Add streamlines sparingly — too many streamlines create visual clutter

  • Set color ranges manually — auto-scaling can hide important features

Workflow Efficiency#

Use the AI Assistant#

The AI Assistant saves time by:

  • Automating geometry analysis and repair recommendations

  • Suggesting appropriate mesh settings and AMR levels for your application

  • Auto-detecting boundary conditions from surface names

  • Interpreting quality reports and results

Save Time with Symmetry#

If your geometry and flow are symmetric:

  • Use a symmetry plane to mesh only half the domain

  • This halves cell count and compute cost

  • Results are mirrored automatically in visualization

Iterate Systematically#

For design optimization:

  1. Establish a baseline configuration

  2. Change one parameter at a time

  3. Use the same mesh settings for fair comparison

  4. Record all results in a structured format

Contents