CFD Analysis Of A Wind Turbine Blade: A Simple Breakdown

ByMina Al-Rawi

What Is CFD Analysis?
(Computational Fluid Dynamics)

In engineering, we use different methods to study how an object and its environment interact, and the effects of that interaction.
For wind turbines, the main analyses are CFD, FEA, and FSI:

  • FEA (Finite Element Analysis) simulates how solids respond to forces, loads, or heat. It shows stress, strain, and deformation. Imagine pressing a sponge and seeing it compress.
  • FSI (Fluid-Structure Interaction) combines CFD and FEA. It shows how fluids and solids affect each other. Imagine a flag waving in the wind. The wind moves the flag, and the flag changes the airflow.
Vibrant splash of sea water captured at sunrise, showcasing dynamic motion and vivid colors.

Together, these methods help engineers understand fluid behavior, structural response, and their interaction in a single simulation.

The tutorials linked in this article show a CFD analysis of the wind blade’s aerodynamic performance. This CFD analysis predicts the forces, torque, and power the blade can generate under the specified wind conditions and rotation. Wind speed = 6 m/s.

How To Do CFD Analysis, Step-By-Step?

1. Blade Geometry Preparation

  • Download the blade CAD file and clean it to remove gaps or unnecessary details.
  • Make sure the geometry is watertight and correctly oriented relative to the wind.

2. CFD Platform Setup

  • Use a CFD tool like ANSYS, SimScale or CONSELF, which allows setup, solving, and post-processing.

3. Computational Domain

  • Create a fluid domain around the blade extending several blade lengths. 
  • Set boundary conditions for wind inlet, outlet pressure, blade walls, and far-field or symmetry sides.

4. Mesh Generation

  • Discretize the fluid domain with a mesh, using finer cells near the blade surface to capture boundary layers and coarser cells away from the blade. 
  • Check mesh quality metrics before solving.

5. Physical Models and Solver Setup

  • Select turbulence models (k-ω SST or k-ε), set air properties, and configure blade rotation. 
  • Choose steady-state or transient solver depending on analysis type.

6. Boundary and Initial Conditions

  • Apply wind velocity at the inlet, outlet pressure at the exit, and no-slip conditions on blade surfaces. 
  • For rotating blades, set up a rotating reference frame or sliding mesh.

7. Simulation Run

  • Start the solver and monitor residuals and aerodynamic forces. 
  • Make sure there is convergence of lift, drag, and torque values.

8. Post-Processing, Validation & Iteration

  • Visualize flow patterns, velocity, and pressure fields. 
  • Compute aerodynamic forces, torque, and power, and examine flow separation or tip vortices.
  • Check results against analytical models, experimental data, or mesh refinements. 
  • Refine geometry or solver settings to optimize performance and accuracy.

CFD Analysis Of Wind Turbine Blade – Tutorial Breakdown:

Geometry Setup
Of Wind Turbine Blade

Software: ANSYS Workbench & SpaceClaim

  1. Import Geometry
    • In Component Systems, right-click Geometry → Import Geometry.
    • Select your wind blade 3D model file.
  2. Edit Geometry in SpaceClaim
    • Right-click Geometry → Edit Geometry in SpaceClaim.
  3. Rotate Blade Axis Vertically
    • Select Move → Body, choose the blade body.
    • Set anchor at the origin.
    • Rotate 90° to align the blade axis with the Y direction (vertical).
  4. Orient Blade Pitch (XZ Plane / Chord Line)
    • Switch to Body Mode, select the top face of the blade.
    • Create a sketch on the top face.
    • Draw the chord line (leading edge to trailing edge).
    • Create the XY plane to measure the angle.
    • Measure the angle between chord line and XY plane (example: 1.06°).
    • Rotate the blade clockwise by the measured angle to neutral pitch.
  5. Delete Temporary Sketch and Plane
    • Remove the chord line sketch and the XY plane to declutter the workspace.
  6. Set Blade Pitch Angle
    • Move → select blade body → anchor at origin.
    • Rotate 4° clockwise (or desired pitch).
  7. Translate Blade for Hub Clearance
    • Move the blade along the Y-axis 40 mm from the origin (no rotation needed).
  8. Save Project
    • In Workbench: File → Save As → choose location.
    • Save as .wbpj (project folder) or .wbpz (archived, shareable version).
    • Ensure “Import Files” is checked to include the blade geometry in the project folder.

Flow Domain Setup

Software: ANSYS Workbench & SpaceClaim

  1. Measure Blade Length
    • Use Measure Tool: click origin → top of blade.
    • Record blade length (example: 305 mm).
  2. Create Sketch for Flow Domain Cross-Section
    • Create a sketch plane on XY plane.
    • Draw one-third circle (120° arc):
      • Radius = 2.5 × blade length (example: 750 mm).
      • Arc angled 30° from horizontal.
  3. Complete the Arc
    • Draw second reference line.
    • Use 3-point arc tool to connect ends.
    • Confirm radius and 120° arc coverage.
  4. Pull Surface to Form Enclosure
    • Pull towards inlet (negative Z) 2.5 × blade length (e.g., 750 mm).
    • Pull towards outlet (positive Z) 5 × blade length (e.g., 1500 mm).
    • Pull options: No merge (keep blade separate).
  5. Combine Blade with Enclosure
    • Use Combine tool:
      • Target: solid enclosure.
      • Tool: blade.
      • Option: deselect “keep cutter”.
    • Result:
      • Blade wall solid – represents blade geometry.
      • Flow domain – volume around blade.
  6. Suppress Blade for Flow Domain View
    • Right-click Suppress for Physics on blade.
    • Use section view to verify cavity where blade sits.
  7. Create Name Selections for Faces
    • Outlet: downstream face.
    • Inlet top: top surface of inlet.
    • Inlet: main inlet surface.
    • Periodic boundaries:
      • Leading face → Periodic1.
      • Rotating face → Periodic2.
    • Blade wall: select entire blade (box selection).
  8. Finalize & Save Project
    • Ensure all name selections are correctly assigned.
    • Go to File → Save in Workbench.

Mesh Setup

Software: ANSYS Fluent & Mesher

  1. Insert Fluent Meshing System
    • In Component Systems, drag Fluent with Fluid Meshing.
    • Transfer the geometry into Fluent Mesher.
  2. Open Fluent Mesher
    • Double-click Mesh → Start.
    • Select Double Precision and number of cores available.
  3. Set Display Defaults
    • Display → Mouse Buttons → Workbench Defaults.
    • Close display menu.
  4. Import & Update Geometry
    • Click Import Geometry → Update.
    • Confirm units (e.g., millimeters).
  5. Add Local Sizing for Blade
    • Select Blade Wall → Add Local Sizing.
    • Leave other defaults.
  6. Create Surface Mesh
    • Enable Curvature and Proximity under size functions.
    • Click Create Surface Mesh.
    • Optional: Use clipping planes to inspect mesh quality, especially trailing edge.
  7. Describe Geometry
    • Set Geometry Type: fluid regions only, no voids.
    • Answer “No” for remaining questions.
    • Click Update.
  8. Set Periodic Boundaries
    • Right-click Describe Geometry → Insert Next Test Task → Setup Periodic Boundaries.
    • Select Periodic1 (P1) and Periodic2 (P2).
    • Update boundaries.
  9. Update Regions
    • Set Blade Wall to Dead (not part of fluid domain).
    • Keep Flow Domain as Fluid.
    • Update regions.
  10. Add Boundary Layers
    • Enable Boundary Layers → Yes.
    • Click Add Boundary Layers.
  11. Create Volume Mesh
    • Click Create Volume Mesh.
    • Observe mesh: coarse far from blade, fine near blade for good resolution.
  12. Save Project
    • Return to Workbench → File → Save.

CFD Setup

Software: ANSYS Fluent, Boundary Conditions & Solution

  1. Check Mesh
    • Click Mesh → Check for errors/warnings.
    • Click Report Mesh Size → Update (example: ~63,000 cells).
  2. Switch to Solution
    • Click Switch to Solution.
    • Confirm mesh check.
  3. Set Viscous Model
    • Go to Models → Viscous (SST k-omega).
    • Switch to GEKO model (if applicable).
  4. Check Materials
    • Under Materials → Fluid → Air, verify properties at standard temperature and pressure.
  5. Cell Zone Conditions
    • Select Flow Domain → Frame Motion.
    • Set rotation origin: (0,0,0).
    • Rotate about positive Z-axis.
    • Set rotational velocity: 98 rad/s.
  6. Boundary Conditions – Inlets
    • Select Inlet and Inlet Top.
    • Set Velocity Components: only Z-direction = 6 m/s.
  7. Boundary Conditions – Outlet
    • Select Outlet → Gauge Pressure = 0.
  8. Periodic and Wall Conditions
    • Ensure Periodic Faces are assigned correctly.
  9. Assign Blade Wall → Wall condition.

This sets up the CFD simulation with rotating frame, correct inlet velocity, outlet pressure, and proper wall/periodic boundaries, ready for solution.

CFD Solution

Software: ANSYS Fluent, Run & Monitor

  1. Set Residual Monitors
    • Go to Monitors → Residuals.
    • Set absolute criteria (0.001).
  2. Create Surface Report
    • Solution → Definitions → New → Surface Report → Integral.
    • Select Pressure (static) → Surface = Blade Wall.
    • Enable Report File and Report Plot.
  3. Initialize Solution
    • Go to Initialization → Standard Initialization → Compute from Inlet.
    • Click Initialize.
  4. Run Calculation
    • Go to Run Calculation.
    • Set Iterations = 1500.
    • Click Calculate.
    • Monitor residuals and pressure integral to check convergence.
  5. Verify Convergence
    • Confirm residuals drop below the threshold.
    • Ensure pressure integral stabilizes over time.
  6. Save Project
  7. Return to Workbench → File → Save.

This ensures the CFD solution converges properly, with a monitored integral of blade pressure and residuals, ready for post-processing.

CFD Post-Processing
& Power Calculation

Software: ANSYS Results

  1. Insert Results System
    • In Component Systems, drag in Results System.
    • Transfer the solution from Fluent → Results.
    • Double-click Results to open the post-processor.
  2. Create Pressure Contours on Blade Surface
    • New Contour → Name: Pressure1.
    • Domains: Blade Wall.
    • Variable: Pressure.
    • Set 100 contours.
    • Under Render → Turn off contour lines.
    • Zoom to inspect low/high pressure regions on the blade.
  3. Pressure Contours on Blade Cross-Section
    • Location → Plane → XZ Plane, adjust Y position as needed.
    • New Contour → Name: Pressure2.
    • Domains: XZ plane slice.
    • Variable: Pressure.
    • Range: Local.
    • Set 100 contours, no contour lines.
    • Click apply.
    • Adjust view along Y-axis to visualize flow over the cross-section.
  4. Calculate Torque & Power
    • Calculators → Function Calculator.
    • Function: Torque.
    • Location: Blade Wall.
    • Axis: Global Z (rotation axis).
    • Fluid: Air.
  5. Calculate Torque & Power. Formula is:
    P = T × ω × n =
    Power = Torque × Angular Velocity (98 rad/s) × Number of Blades (3)
    = 0.0407 x 98 x 3 = 11.97 W

    Note: The assumptions are a linear elastic blade, no losses, and constant angular velocity

This process allows you to visualize pressure distribution on the blade and calculate the generated power from the CFD results!

Conclusion

  • This example of a CFD analysis shows the importance of simulation in wind blade design. The CFD analysis reveals pressure distribution and identifies areas of high and low aerodynamic load.
  • This way, the CFD analysis allows us to estimate energy production accurately. With the use of CFD analysis, it is possible to optimize blade geometry, orientation, and pitch. In addition, it improves efficiency and performance, and reduces costly physical testing.
  • In conclusion, CFD acts as a virtual wind tunnel. CFD gives detailed insight into the interaction between the object (wind turbine blade) and fluid (air). This way, CFD provides insightful data, for informed design decisions about wind turbine blades.
A row of wind turbines on a sandy coastline under a clear blue sky, promoting renewable energy.

Leave a Reply

Your email address will not be published. Required fields are marked *