Turbulence Boundary Conditions Calculator
Setting the right turbulence values at your CFD inlets can be the difference between a simulation that captures real flow physics and one that gives misleading results. This tool helps you estimate k, ε, ω, and Spalart-Allmaras ν̃ from turbulence intensity and flow conditions — with built-in guidance for pipe flows, fluid presets, and a correct Newton-solved SA model that avoids the common ν̃ ≈ ν_t approximation error.
Turbulence Boundary Conditions Calculator
Estimate inlet turbulence properties for your CFD simulation. Get k, ε, ω, and ν̃ from flow conditions.
TI ≈ 0.16 · ReDh−1/8 (core/centerline value for fully developed flow)k = 1.5 · (U · TI)²ε = Cμ0.75 · k1.5 / ltω = k0.5 / (Cμ0.25 · lt)From TI and viscosity ratio (μt/μ):
k = 1.5 · (U · TI)²ε = Cμ · k² / νt where νt = (μt/μ) · νω = k / νtSpalart-Allmaras ν̃:
νt = ν̃ · fv1 where fv1 = χ³/(χ³ + cv1³), χ = ν̃/ν, cv1 = 7.1ν̃ is solved iteratively using Newton's method (not the common but inaccurate approximation ν̃ ≈ νt).
Constants:
Cμ = 0.09, cv1 = 7.1Notes:
• These formulas assume incompressible flow. For compressible flow (Mach > 0.3), consult your solver's documentation for density-weighted formulations.
• Some CFD codes (notably ANSYS Fluent, Phoenics, CFD-ACE) use a mixing-length based definition where lmix = Cμ0.25 · lt ≈ 0.547 · lt. This calculator uses the standard turbulence length scale as defined in OpenFOAM, STAR-CCM+, and CFD-Wiki.
Frequently Asked Questions
What turbulence intensity should I use for my CFD simulation?
It depends on your flow scenario. For external aerodynamics (cars, airfoils, buildings), use 1–5 %. For internal flows in pipes and ducts, 5–10 % is typical. For complex geometries like heat exchangers or turbomachinery, 10–20 %. For fully developed pipe flow, you can estimate TI from the Reynolds number using the formula TI ≈ 0.16 · Re−1/8 (this gives the core/centerline value).
Should I use "Intensity + Length Scale" or "Intensity + Viscosity Ratio"?
For internal flows where you know the geometry (pipe diameter, duct size), use Intensity + Length Scale with lt ≈ 0.07 · Dh. For external flows where a characteristic turbulence length is hard to define, use Intensity + Viscosity Ratio with μt/μ between 1 and 10 for free-stream conditions.
What is the difference between k-ε, k-ω SST, and Spalart-Allmaras?
k-ε models are robust for free-stream and wake flows but less accurate near walls. k-ω SST combines the best of k-ε and k-ω and is the most widely used general-purpose RANS model. Spalart-Allmaras is a one-equation model well suited for attached wall-bounded aerospace flows. For k-ε, specify k and ε at your inlet. For k-ω SST, specify k and ω. For Spalart-Allmaras, specify ν̃.
Why is ν̃ not simply equal to νt for Spalart-Allmaras?
The Spalart-Allmaras model defines νt = ν̃ · fv1, where fv1 is a damping function that approaches 1 only at high eddy viscosity ratios. At typical free-stream conditions (μt/μ = 1–10), fv1 can be significantly less than 1, making ν̃ considerably larger than νt. For example, at μt/μ = 1, ν̃/ν ≈ 4.6 — not 1. This calculator solves for ν̃ correctly using Newton's method.
How do I use these values in Simcenter STAR-CCM+?
In STAR-CCM+, set the turbulence specification at your inlet boundary condition. For k-ω SST, enter k and ω directly, or use the built-in intensity + length scale method. This calculator helps you understand what the resulting values will be and verify that your turbulence BCs are in a physically reasonable range. For guidance on optimal setup for your specific application, contact Volupe's application engineers.
How to Estimate Turbulence Inlet Boundary Conditions for CFD
Every RANS-based CFD simulation needs turbulence values at the inlets. Get them wrong, and you may see artificial turbulence decay, delayed or premature flow separation, or poor convergence. The tricky part is that the actual turbulence properties at your inlet are rarely known — you almost always need to estimate them from more intuitive quantities like turbulence intensity and a characteristic length scale.
This guide explains how to choose the right inputs and what to watch out for when using the calculator above.
Choosing Between Turbulence Intensity + Length Scale and Intensity + Viscosity Ratio
There are two common approaches for specifying turbulence at an inlet, and the right choice depends on your flow type.
Intensity + Length Scale works best when you have a well-defined geometry upstream of your inlet. Pipe flows, duct systems, and channel flows all have a clear hydraulic diameter that you can use to estimate the turbulence length scale. The relationship l_t ≈ 0.07 · D_h (based on the mixing-length convention) gives a reliable starting point for fully developed flow.
Intensity + Viscosity Ratio is the better choice for external flows — flow around vehicles, airfoils, buildings, or any case where defining a meaningful length scale is difficult. The eddy viscosity ratio μ_t/μ directly describes how much the turbulent viscosity exceeds the molecular viscosity. For free-stream conditions far from walls, values between 1 and 10 are typical. For fully developed internal flows, values of 100 or more are common.
If you are unsure, start with the Intensity + Length Scale method for internal flows and the Intensity + Viscosity Ratio method for external flows.
Understanding Turbulence Length Scale Definitions
One source of confusion in CFD is that different solvers define the turbulence length scale differently. Three definitions are common in the literature and across commercial CFD codes:
Classical definition (Wilcox): l = C_μ · k^(3/2) / ε, where C_μ = 0.09. This is the smallest of the three and gives l_t ≈ 0.038 · D_h for fully developed pipe flow. Used in several academic references and the original Wilcox textbook on turbulence modeling.
Mixing-length definition: l = C_μ^(3/4) · k^(3/2) / ε. This is approximately 1.83× the classical definition and gives l_t ≈ 0.07 · D_h. Used by ANSYS Fluent, OpenFOAM, Simcenter STAR-CCM+, and most modern CFD codes. Our calculator uses this convention.
Dimensional definition: l = k^(3/2) / ε. This is approximately 11× the classical definition and gives l_t ≈ 0.42 · D_h. Used by ANSYS CFX.
The table below shows which definition each solver expects:
| Solver | Length scale convention | Pipe flow estimate |
|---|---|---|
| Simcenter STAR-CCM+ | Mixing-length | l_t ≈ 0.07 · D_h |
| OpenFOAM | Mixing-length | l_t ≈ 0.07 · D_h |
| ANSYS Fluent | Mixing-length | l_t ≈ 0.07 · D_h |
| ANSYS CFX | Dimensional | l_t ≈ 0.42 · D_h |
If you are using CFX, multiply the value from this calculator by approximately 6.1 (which is 1 / C_μ^0.75) to convert to the dimensional convention. For all other major solvers, the values from this calculator can be used directly.
Practical Guidance for Turbulence Intensity
Turbulence intensity I is defined as the ratio of velocity fluctuations to the mean flow velocity. Here are typical values for different flow scenarios:
Below 1 % — Very low turbulence. External flow around streamlined bodies (aircraft, submarines). High-quality wind tunnels with turbulence management screens can reach I < 0.05 %.
1 – 5 % — Low to medium. External flow around cars and buildings, moderate-quality wind tunnels, large ventilation ducts, low-Reynolds-number internal flows.
5 – 10 % — Medium to high. Fully developed pipe and duct flows, downstream of flow conditioning elements, HVAC systems.
10 – 20 % — High. Downstream of complex geometries, heat exchangers, turbomachinery stages (compressors, turbines), flows with strong recirculation.
For fully developed pipe flow, the turbulence intensity at the pipe center can be estimated from the empirical correlation I ≈ 0.16 · Re^(−1/8), where Re is the Reynolds number based on hydraulic diameter. The calculator above includes a built-in helper that computes this for you.
For turbomachinery applications, the turbulence length scale is commonly set to about 5 % of the channel height at the stage inlet. For grid-generated turbulence (e.g., downstream of screens or grids in wind tunnels), the length scale is typically close to the grid bar size.
A Note on the Spalart-Allmaras Model
The one-equation Spalart-Allmaras model is widely used in aerospace applications and requires only the modified kinematic viscosity ν̃ at the inlet. A common shortcut is to assume ν̃ ≈ ν_t, but this approximation is only valid at high eddy viscosity ratios where the damping function f_v1 approaches 1.
At typical free-stream conditions (μ_t/μ = 1–10), the error can be substantial. For example, at μ_t/μ = 1, the correct value of ν̃/ν is approximately 4.6, not 1. The calculator above solves for ν̃ correctly using Newton’s method on the full SA relation ν_t = ν̃ · f_v1(ν̃/ν).
For free-stream boundaries, the NASA Turbulence Modeling Resource recommends setting ν̃/ν directly between 3 and 5, regardless of calculated k/ε values. This provides a good balance between having enough eddy viscosity to prevent solver issues and not overpowering the boundary layer development.
References and Further Reading
The formulas in this calculator follow the conventions documented in the NASA Turbulence Modeling Resource, CFD-Wiki, and Frank M. White’s Viscous Fluid Flow. For solver-specific implementation details, consult the user documentation for your CFD code.
Looking for more CFD tools? Try our Y+ Calculator, Nusselt Number Calculator, or Heat Transfer Coefficient Correlations.
Training and mentoring for the products in the Simcenter Suit
Volupe offers training and mentoring for Simcenter products, including an introductory course for Simcenter STAR-CCM+ with basic CFD concepts. Videos on fluid dynamics and CFD are also available for users without a background in the field.
