Acta Polytechnica


doi:10.14311/APP.2016.56.0062
Acta Polytechnica 56(1):62–66, 2016 © Czech Technical University in Prague, 2016

available online at http://ojs.cvut.cz/ojs/index.php/ap

COMPARISON OF AXIAL FAN ROTOR EXPERIMENTAL
DATA WITH CFD SIMULATION

Aleš Prachař

Aerospace Research and Test Establishment, Beranových 130, 199 05 Praha–Letňany, Czech Republic
correspondence: prachar@vzlu.cz

Abstract. Data obtained from an experimental simulation on a new test rig for axial fans are
compared to a CFD simulation. The Edge solver is used and the development needed for the simulation
(boundary conditions, free stream consistency) is described. Adequate agreement between the measured
and calculated data is observed.

Keywords: axial fan; CFD; Edge software; boundary conditions.

AMS Mathematics Subject Classification: 65N08, 76M12.

1. Introduction
Axial flow fans are used in many applications ranging
from cooling of the computer CPU’s to the propulsion
of wind tunnels or cooling towers of the power plants,
to emphasize extreme scales.

For better understanding of the flow phenomena it
is usual and today almost inevitable to include CFD
into the design and testing. It is, however, necessary
to develop sufficiently accurate computational tools
and validate them extensively.
A test rig for axial fans has been designed and

constructed in recent years. Compared to the previous
state it allows automatic flow regulation and data
acquisition. From the point of view of the CFD user
it serves as a valuable source of validation data for
computational methods.
The Edge CFD solver package [1] has been used

so far mainly for external aerodynamics problems
with encouraging results [2]. Since the solver includes
many of the ingredients needed to solve problems in
rotating domains (turbomachinery), it was decided
to test its ability to deal with this kind of problems.
Several updates, corrections and generalizations of
the existing code had to be developed for the required
functionality.
This paper starts with a brief description of the

experimental device and the data obtained. However,
the main part is dedicated to the development of
the Edge flow solver and to a comparison with the
experimental data.

2. Experimental set-up and
measured data

A test rig for the axial fans, see Fig. 1, has been
designed. Since the electric motor has been placed
upstream of the fan rotor and the shaft is relatively
short to prevent problems with vibrations, the inlet
channel has been designed to change the direction
of the incoming air from radial (centripetal) to axial.

The shaft is fitted with dynamometer to measure
torque.

The hub and the shroud (casing) are fixed together
by the struts which are placed upstream (airfoil shape)
and downstream of the rotor. The diameter of the
shroud at the rotor position is 630 mm and the hub
to shroud diameter ratio is 0.55.

To vary the volume flow rate by aerodynamic resis-
tance, the adjustable choking element is mounted at
the outflow area.

The properties of the flow (total and static pressure,
velocity vector) are measured at the planes approxi-
mately 130 mm upstream and downstream of the fan
rotor by a pair of 5-hole pitot–static probes (see Fig. 1)
traversing along the radial direction. The test rig has
a constant cross section between those two planes.
The measured quantities, obtained as functions of

radial coordinate, were later utilized to calculate inte-
gral values (volume flow rate, average total or static
pressure).

3. CFD Simulation
For the CFD simulation the Edge software, see [3],
which is a compressible flow solver for unstructured
grids with arbitrary elements was used. Edge is based
on the node–centred finite volume formulation of the
Euler or the Navier–Stokes equations in two or three
dimensions using dual grids.

3.1. Solver description
The solver has been used in its parallel version uti-
lizing convergence acceleration techniques like multi–
grid, low speed preconditioning [4], implicit residual
smoothing and local time stepping.

The flow equations formulated in a reference frame
rotating around an arbitrary axis Ω with an angular
velocity |Ω| are written with the aid of the Einstein
summation convention as

∂U

∂t
+
∂Fi
∂xi

+
∂Gi
∂xi

= S. (1)

62

http://dx.doi.org/10.14311/APP.2016.56.0062
http://ojs.cvut.cz/ojs/index.php/ap


vol. 56 no. 1/2016 Axial Fan CFD Simulation

Figure 1. Test stand scheme. A pair of 5-hole pitot-static probes is placed upstream and downstream of the fan
rotor.

Figure 2. Primary (dotted) and dual grid (solid), the vectors representing facets (blue) and faces (red).

The definition of unknowns U, convective fluxes Fi
and the source term S is given by

U =




ρ
ρu1
ρu2
ρu3
ρEr


 , Fi =




ρwi
ρu1wi + δi1p
ρu2wi + δi2p
ρu3wi + δi3p
(ρEr + p)wi


 ,

S =


 0ρΩ ×u

0


 , (2)

where u denotes the absolute velocity vector and w
stands for the relative velocity. The exact form of
the viscous fluxes Gi is omitted here for brevity. Let
us note that the total energy in the energy equation
contains contribution from the rotation

Er = E −u · (Ω ×r). (3)

Since the grid movement (rotation) is included in the
governing equations, they can be solved in a steady
state manner.

For our simulation various k–ω models of turbulence
have been tested, and the low Reynolds number model
[5] has been used for the presented results.
In the Finite volume method, (1) is solved in the

integral form

d

dt

∫
V
U +

∫
∂V

(Fi + Gi) ·n =
∫

V
S. (4)

For the convective fluxes the second order central
scheme with the Jameson–Schmidt–Turkel type artifi-
cial dissipation term has been used.

The data structure for the finite volume flux cal-
culations is edge–based and the reduced scheme is
used, i.e., the normals representing the facets between
two adjacent dual cells are summed into a single one,
which is kept in the data structure, see Fig. 2. Hence,
only one flux evaluation between two adjacent cells is
needed.

It was noted by Raichle [6] that discretization error
is introduced if the grid velocity Ω × r at the cell
face is averaged from the cell centres. He proposed a
formulation assuring exact integration and, hence, free
stream consistency for rotating flows. The scheme,
still based on reduced formulation, was implemented.

The only additional requirement is that along with
the computed normals, representing the cell faces, ad-
ditional vector for each face has to be stored in the
data structure. For a typical case we observed in-
creased memory demands for up to 10–15% compared
to the inexact reduced scheme. Increase in the CPU
time is negligible.

3.2. Boundary conditions
For internal aerodynamics it is usually natural to
use the pair of boundary conditions prescribing total
quantities (total pressure, total temperature and flow
direction) at the inlet and the static pressure at the
outlet from the computational domain. We consider
the inlet boundary condition adequate for our case.

However, the exit static pressure is influenced by the
performance of the rotor at various volume flow rates.
If we inspect the dependence of the exit static pressure
on the volume flow rate, see Fig. 3, we find that the
static pressure alone does not uniquely determine the
flow regime. We prescribe the average of boundary

63



Aleš Prachař Acta Polytechnica

Figure 3. Outlet static pressure (relative) and corre-
sponding kL parameter for a typical case.

pressure p̃b according to

p̃b = pref +
1
2
kLρ̃ũ

2
ax, (5)

where pref denotes reference pressure and kL is a free
parameter. The calculation was carried out for a range
of kL’s to cover various flow regimes.
Moreover, since the flow exhibits large circumfer-

ential (peripheral) velocities as a consequence of the
absence of stator blades, the outlet boundary condi-
tion is implemented to satisfy the radial equilibrium
condition which we assume at the outlet and which is
considered in a simple form, cf. [7],

dpb
dr

=
ρu2θ
r
. (6)

Finally, pb is updated to vary along the radial coordi-
nate taking into account both (5) and (6).
Another type of boundary used in our simulation

is a solid wall. However, we need to distinguish be-
tween boundaries steady with respect to the fixed
coordinates (e.g., casing) where u = 0 is prescribed,
and boundaries moving with the reference frame (e.g.,
rotor blade) with w = 0. In Edge, weak formulations
for these boundary conditions are used, [8].

Since no information about the turbulence level was
known, the inlet turbulence intensity was set to 1%
of the inlet velocity and the freestream viscosity ratio
(turbulent to dynamic viscosity) was set to the default
value equal to 1.

3.3. CFD Geometry
For the CFD calculation the model was simplified con-
siderably. First, the struts were removed and only the
rotor blades were preserved. This makes the problem
rotationally periodic. Only one rotor blade was mod-
elled and the rotation periodic boundary condition

Figure 4. Layout of the CFD simulation.

was applied. The CFD geometry models the constant
cross–section part of the test rig, prolonged upstream
and downstream.
A hybrid (tetrahedral and hexahedral elements)

computational grid was used as a primary grid with
approximately 2.3 million nodes. The layout of the
simulation and of the planes where the flow properties
were evaluated is indicated in Fig. 4. The structured
hexahedral blocks were placed upstream and down-
stream of the rotor. The structured block with O-grid
topology was used around the rotor blade with 100
points on each side of the blade surface, 35 points in
the normal direction and 120 radial grid points. The
boundary layer was fully resolved around the solid
walls and in the tip gap to keep the parameter y+
below 1. The cell expansion ratio from the wall was
kept close to 1.2. The rest of the space between the
blade O-grid block and the periodic boundaries was
filled with tetrahedral elements.

4. Comparison of experiment data
with CFD results

To match the experimental data the flow field obtained
from the CFD simulation was evaluated at the planes
upstream and downstream of the rotor. The volume
flow rates, average of static and total pressure are the
basic data which together with torque at the rotor
blades are used to calculate integral values.

The experimental data were obtained for three set-
tings of blade angle (25°, 35° and 45°), constant an-
gular velocity (|Ω| = 394 rad/s, ut = 124 m/s) and for
a range of choking element settings from fully open
to and beyond the blade stall. The non-dimensional
pressure and flow coefficients are used for comparison,
see Fig. 5. The notation is similar to [9].

We observe satisfactory agreement of experimental
and CFD data. Let us note that the computation
was performed for several settings of the solver. The
choice of turbulence model had a notable effect on
the prediction of the blade stall. In our cases the low
Reynolds numbers k–ω turbulence model [5] gave the
best results in terms of capturing the blade stall. The
cases in the stall region for the given blade settings
are averaged values since oscillatory behaviour was

64



vol. 56 no. 1/2016 Axial Fan CFD Simulation

Figure 5. Axial fan performance in non–dimensional
parameters for various blade angles. Full line denotes
the experiment, dashed lines with triangles represent
CFD calculation.

observed. In this case the unsteady solution could be
used to improve accuracy.
Extensive validation of the turbulence models is

necessary for the class of problems considered in this
paper since testing of their implementation in Edge
was done mainly for external flows. Various other
simplifications and idealizations can also cause dif-
ferences, e.g., tip clearance height estimate, which is
never perfectly uniform in the experiment, the effect
of struts, etc.

The (relative) isentropic efficiency for the considered
cases is shown in Fig. 6.
We can also consider the agreement of the data

acceptable. The slightly higher efficiency for higher
volume flow rates (especially for the blade setting
of 35°) can be partly explained by the turbulence
modelling. The flow is considered fully turbulent
in CFD, however, turbulent transition could cause
improvement.

5. Conclusion
The main result of this paper is that it is possible
to use the Edge software, a code primarily designed
for external aerodynamics, for the problem under
consideration. Various enhancements were necessary
for appropriate functionality. However, the changes
to the code were compatible with the solver structure.
An acceptable agreement between the measured

and calculated data was observed. Local quantities
could be compared in the next step.
Future research will focus on the rotor–stator con-

figuration and the modelling of the interface between
the blade rows.

List of symbols
A Flow area (cross–section) [m2]

Figure 6. Relative efficiency for three blade settings.
Full line denotes the experiment, dashed lines with
triangles represent CFD calculation.

Mk Torque moment [N m]
p Fluid pressure [Pa]
p̃T Total pressure (ISO), p̃T = p̃ + 12 ρ̃(

Q
A

)2 [Pa]
Q Volume flow rate [m3 s−1]
r Radial coordinate [m]
u Absolute velocity vector [m s−1]
uax Axial component of velocity [m s−1]
uθ Peripheral component of velocity [m s−1]
ut Blade tip velocity [m s−1]
w Relative velocity vector, w = u− Ω ×r [m s−1]
δij Kronecker delta
η Isentropic efficiency η = Q∆p̃T/(Mk|Ω|)
ρ Fluid density [kg m−3]
ϕ Flow coefficient ϕ = Q/(Aut)
ψ Pressure coefficient ψ = 2∆p̃T/(ρ̃u2t )
Ω Rotation axis, angular velocity |Ω| [rad/s]
(̃ ) Average of the quantity across boundary
( )b Boundary value

Acknowledgements
This research was supported by The Ministry of Industry
and Trade of the Czech Republic for long-term strategic
development. Access to computing and storage facilities
owned by parties and projects contributing to the Na-
tional Grid Infrastructure MetaCentrum, provided under
the "Projects of Large Infrastructure for Research, Devel-
opment, and Innovations" programme (LM2010005), is
greatly appreciated.

References
[1] P. Eliasson. Edge, a Navier-Stokes solver for
unstructured grids. In Proceedings to Finite Volumes
for Complex Applications III., pp. 527–534. ISTE Ltd.,
London, 2002.

[2] P. Eliasson, S.-H. Peng, L. Tysell. Computations from
the fourth drag prediction workshop using the Edge

65



Aleš Prachař Acta Polytechnica

solver. Journal of Aircraft 50(5):1646–1655, 2013.
doi:10.2514/1.C032225.

[3] Edge theoretical formulation. Tech. Rep. 03-2870,
Swedish Defence Research Agency (FOI), 2007.

[4] A. Prachař. Local low speed preconditioning in
rotating reference frame. Applied Mathematical Sciences
9(5):209–218, 2015. doi:10.12988/ams.2015.411885.

[5] S.-H. Peng, L. Davidson, S. Holmberg. A modified
low-Reynolds-number k −ω model for recirculating
flows. ASME J Fluids Eng 119:867–875, 1997.
doi:10.1115/1.2819510.

[6] A. Raichle. Extension of the unstructured TAU-code
for rotating flows. In New Results in Numerical and
Experimental Fluid Mechanics V, vol. 92 of Notes on
Numerical Fluid Mechanics and Multidisciplinary
Design (NNFM), pp. 136–143. Springer Berlin
Heidelberg, 2006. doi:10.1007/978-3-540-33287-9_17.

[7] D. L. Tweedt, R. V. Chima, E. Turkel.
Preconditioning for numerical simulation of low mach
number three–dimensional viscous turbomachinery
flows. In Proceedings of 28th Fluid Dynamics
Conference. 1997. doi:10.2514/6.1997-1828.

[8] P. Eliasson, S. Eriksson, J. Nordström. The influence
of weak and strong solid wall boundary conditions on
the convergence to steady-state of the navier-stokes
equations. In Proceedings of 19th AIAA CFD
Conferenc. 2009. doi:10.2514/6.2009-3551.

[9] V. Cyrus, J. Cyrus, P. Wurst, P. Panek. Aerodynamic
performance of advanced axial flow fan for power
industry within its operational range. In Proceedings of
ASME Turbo Expo. 2014. doi:10.1115/GT2014-25339.

66

http://dx.doi.org/10.2514/1.C032225
http://dx.doi.org/10.12988/ams.2015.411885
http://dx.doi.org/10.1115/1.2819510
http://dx.doi.org/10.1007/978-3-540-33287-9_17
http://dx.doi.org/10.2514/6.1997-1828
http://dx.doi.org/10.2514/6.2009-3551
http://dx.doi.org/10.1115/GT2014-25339

	Acta Polytechnica 56(1):62–66, 2016
	1 Introduction
	2 Experimental set-up and measured data
	3 CFD Simulation
	3.1 Solver description
	3.2 Boundary conditions
	3.3 CFD Geometry

	4 Comparison of experiment data with CFD results
	5 Conclusion
	List of symbols
	Acknowledgements
	References