Development of a Validated CFD Model for the 

Mixing Behavior of Parallel Triple-Channel Flows

Amir Dajani, SURF Student

Undergraduate Student in Bioengineering

George Mason University
Certain commercial equipment, instruments, or materials are identified in 

this study in order to specify the experimental procedure adequately. Such 

identification is not intended to imply recommendation or endorsement by 

the National Institute of Standards and Technology, nor is it intended to 

imply that the materials or equipment identified are necessarily the best 

available for the purpose.

Disclaimer

2
Amir Dajani

• Rising Senior at George Mason University

• Bioengineering Major

• Concentration in Imaging

• Minor in Computational Data Sciences

Introduction

3
• NIST Neutron Source (NNS) • Looking to replace existing 

reactor (NBSR)

• Three regions of interest to us: • Inlet Region • 3 Legs • Separation-Mix-Separatio

n

• Active Height (rectangular 

channels) • Core • Fuel Plates

• Outlet Region • Cycles back

Nuclear Reactor

4

Ref [2,3]
Problem Area

5

Ref [2,3]
•Problem: May have uneven flow 

distribution into fuel plates

•Insufficient or over-cooling of fuel plates

•Previous work showed differences of >30% 

in velocity prediction based on turbulence 

model variation only.

•Needs experimental validation of the 

mixing phenomenon!

NNS Inlet Region (from previous study)

6

Mixing Region

My work’s motivation!!

Ref [2,3]
• Experiment measured velocity distributions in the 

triple-channel mixing phenomenon.

• Inlet velocity was measured at a shift from the 

actual inlet (origin).

• Shift is “~ 1.25 hydraulics diameters” from 

the inlet

• This work also investigates 0.7D from the 

inlet as a shift

3-channel mixing experiment (Literature)

7

0.7D 1.25D

Ref [1]
• Using OpenFOAM code (v10) for simulations

• Developed mesh in OpenFOAM

• BlockMesh utility used

• Objectives

• Compare different turbulence models

• Produce contour and line plots of flows 

behavior

• Compare CFD results to literature

• Serves as validation of CFD model

Project Summary

8

Goal:

Develop Computational Fluid Dynamics (CFD) model of the experiment (literature)
• Predict and model physical fluid flow

• Attempts to model the Navier-Stokes 

equations

• Reynolds-Averaged Navier Stokes 

(RANS) turbulence models are used in 

this work!

• Model different types of flow

• Laminar, Turbulent, incompressible, 

compressible, etc.

• Assess presence of turbulence

• Software: OpenFOAM

Computational Fluid Dynamics (CFD)

9

∂Ui

∂t + Uj

∂Ui

∂xj

Gas Pedal

= −

ด

∂P

∂xi

Steering

Wheel

+ ν

∂

2Ui

∂xj∂xi

Brakes

Navier-Stokes Equation
• RANS resolves larger Eddies only

• Not exact solutions

• Captures up to Energy containing range

• Good for practical applications

• Most computationally efficient

• LES resolves both larger and smaller Eddy’s to a 

certain extent

• Captures up to Inertial subrange

• DNS captures everything in simulation up to 

Viscous range

• There are multiple RANS models, and this study 

will investigate 4 of them.

Reynolds-Averaged Navier Stokes (RANS)

10
• RANS models used in this project

1. k-ε (2-eqn model)

2. k-ω (2-eqn model)

3. Spalart-Allmaras (1-eqn model, models νttransport)

4. k-ω SST (shear stress transport) (2.5-eqn model)

Models

11

k = turbulent kinetic energy

ε = k dissipation rate

ω = k specific dissipation rate

νt = turbulent viscosity

Turbulent kinetic energy (k) transport equation

∂k

∂t + Uj

∂k

∂xj

= − uiuj

∂ Ui

∂xj

− ε +

∂

∂xj

ν +

νt

σk

∂k

∂xj

Dissipation rate (ε) transport equation

∂ε

∂t + Uj

∂ε

∂xj

= −Cε1

ε

k

uiuj

∂ Ui

∂xj

− Cε2

ε

2

k

+

∂

∂xj

ν +

νt

σε

∂ε

∂xj

νt = Cμ

k

2

ε

Cμ Cε1 Cε2 σk σε

0. 09 1. 44 1. 92 1. 0 1. 3

k-ε

Transport eqns.

As an example
Geometry

12

Recall the shifts!!!

Note our coordinates (origin behind the shifts)!

Hydraulic diameter = D = 72.57 mm
• OpenFOAM software

• Geometry and mesh constructed in 

OpenFOAM with blockMesh utility

• Use VSCode IDE for code editing

• Specify vertices, dimensions, size, 

locations, etc. of blocks of the mesh

• View the geometry and mesh in 

ParaView

Geometry and Mesh

13
• Given in Literature:

• Hydraulic Diameter (D): 0.07257 m

• Inlet Velocity (Ub): ~8.3 m/s

• Average Temperature: 24.35 °C

• Turbulence Intensity (Ti): ~0.05

• Cμ: 0.09

• Derived Values:

• Viscosity: ν = −10. 9184 ∗ ln 24. 35 + 48. 48063 = 1.36 ∗ 10−5

kg

m∗s

• Turbulent Viscosity: νt = 15ν = 2.04 ∗ 10−4 kg

m∗s

• Turbulent Kinetic Energy (k): urms = Ti ∗ Ub = 0.415, k =

3

2

urms

2 = 0.2583

• Dissipation Rate: ε = Cμ ∗

k

2

νt

= 29.38

• Specific Dissipation Rate: ω =

ε

Cμ∗k

= 1.26 ∗ 103

Boundary Conditions

14

This is important!!!

(for normalization)
Refining Mesh

Velocity Convergence (U/Ub)

Top channel Middle channel Bottom channel

k-ε 0.0012 0.0034 0.0011

k-ω 0.0014 0.0075 0.0022

Spalart-Allmaras 0 0.0021 0.0001

k-ω SST 0.0008 0.0017 0.001

15

Inlet Velocity = Ub = 8.3 m/s

All meshes were convergent to within less than 1 cm/s
Convergent Mesh Metrics

k-ε k-ω SpalartAllmarask-ω SST

y

+ Min 0.881 0.125 ~7 0.122 

Max 88.5 42.728 ~31 31.744

Avg 10.312 6.342 ~19 3.782

Max 

Skewness 5.810e-13

Volume

Min 6.034e-11

Max 4.843e-10

Avg 5.292e-05

Face Area

Min 6.034e-08

Max 3.387e-06

Max Aspect 

Ratio 36.197

16
• Create Spanwise Velocity Distribution at each x/D 

location

• x/D location: 10.35, 10.67, 11, 14.25

• Plot results

• U/Ub vs y/D

• Compare with results of literature

• Do this process for each RANS model

• Plot all on the same plot

• Account for the horizontal shift

• Inlet profiles captured at 1.25 away from 

the origin (approximate value) in literature

• Shift of 1.25 and 0.7 conducted for this 

project

Spanwise Velocity Distribution

17

Exit of 

channels Mixing Downstream Development

Ref [1]
Reminder

18

Ref [2,3]
Contour Plot

19

x/D=10.35 10.67

11 14.25

Ref [1]
Contour Plots

20

k-ε

Spalart-Allmaras

k-ω

k-ω SST
Spanwise Velocity Distribution with shift of 1.25

1.25 Hydraulic Diameters from physical 

inlet of test section

Estimated shift

21
Spanwise Velocity Distribution with shift of 0.7

0.7 Hydraulic Diameters from physical 

inlet of test section

Estimated shift

22
• RANS seems appropriate for modeling the mixing behavior of 

Parallel Triple-Channel Flows

• Future use: Researchers, scientists, engineers

• 0.7 shift from origin displayed closer fit to data

• Best models: k-Epsilon and Spalart-Allmaras

Conclusion

23
Acknowledgements

Mentors: Abdullah Weiss, Anil Gurgen

NCNR SURF Directors: Susana Marujo Teixeira, Julie Borchers, 

Leland Harriger
[1] Weiss, Abdullah G., et al. "Flow regime and Reynolds number variation effects on 

the mixing behavior of parallel flows." Experimental Thermal and Fluid Science 134 

(2022): 110619.

[2] Weiss, Abdullah G., Joy S. Shen, and Anil Gurgen. "A Turbulence Model Sensitivity 

Analysis on the Hydraulic Behavior in the Inlet Plenum of the Proposed NIST Neutron 

Source Design." Proceedings of the 20th International Topical Meeting on Nuclear 

Reactor Thermal Hydraulics (NURETH-20).

[3] Shen, Joy, et al. "A Turbulence Model Sensitivity Analysis of Thermal-Hydraulic 

Properties on The Pre-Conceptual NIST Neutron Source Design." Proceedings of the 

International Conference on Nuclear Engineering. 2023.

References

25
Amir Omar Dajani

NIST Center for Neutron Research

George Mason University, Volgenau School of Engineering

26

Questions??