Three-Dimensional Primary Design of a 3kW Class Electronically Commutated Motor Fan Impeller

3.1 Fan selection

A specific speed is used to categorize the type of fan to be used for a certain application. With design specifications, specific speed is calculated using eq. (1) [9], which has a value of 1.75. Generally, when a specific speed (N_s) is in the range of 1.0 < N_s < 1.8, the type of fan will be a mixed-flow fan [9]. Additionally, using specific diameter (D_s= 2.2) as a basis in eq. (2) [9] and the correlation between D_s- N_s in eq. (3) [9], derived from the Cordier diagram for high-efficiency turbo machines, ensured that this fan will not only operate at this best efficiency point (BEP) but will also meet performance requirements of flow rate (Q), and total pressure difference (ΔPt). The impeller is designed in CFturbo software (Version 2022 R2.2).

N is rotation speed (rad/s), Q is flow rate (m³/sec), ΔPt is the total pressure difference (Pa), ρ is the density of air (kg/m³), and D is the impeller diameter (m).

In Table 1, the known specifications are outlined which helped us to assess and plan the impeller design process. These specifications provided a baseline for designing an aerodynamically efficient impeller. The design specifications serve as critical physical and operational constraints that define the operating requirements and performance targets of the intended fan. By starting with these predefined specifications, the design process focuses on achieving an impeller that operates efficiently at the target conditions. These parameters are essential because they directly influence the aerodynamic and mechanical design of the impeller. The specification values form the foundation for achieving design objectives such as aerodynamic efficiency & energy consumption.

Table 1

Design specifications of the EC fan model

Using these design specifications, optimum values of head, flow and, power coefficients (ψ, φ, ᶓ) are calculated. Head coefficient is ratio of pressure produced by fan (ΔPt) to dynamic pressure of blade's peripheral velocity (ρ/2)*u² [11]. It helps in evaluating the efficiency of the fan to convert mechanical energy into kinetic energy. Formula for head coefficient is given [9].

Using this formula pressure coefficient is determined. Then by rearranging, peripheral velocity at impeller outlet (u²) is calculated.

Flow coefficient is a dimensionless parameter used to characterize the performance of fans [9]. The flow coefficient normalizes the flow rate based on parameters like fan speed and size. Q is in m³/sec.

Then eq. (5) is rearranged to find out impeller tip diameter. D= 0. 355m is a value obtained from eq. (5). This indicates, at this diameter, the impeller efficiently meets the demand of required flow rate.

Power coefficient is also another important factor in fan design. It relates the actual power required by fan to the theoretical power available in the fluid. It is derived from empirical data. The power coefficient normalizes the fan power with respect to flow conditions and geometry. It is given below [9].

In eq. (6), ᶓis the symbol of power coefficient, P is input power in Watts, ρ is the density of air, N is rotation speed in rad/s. D is the impeller diameter (m).

Fan efficiency is ratio of product of head and flow coefficients divided by the power coefficient [9]. To maximize efficiency best combination of these coefficients is obtained.

In this fan, the impeller design is backward-curved blades (BC). According to the Euler equation (eq. 8), the pressure head is developed by blades [11].

Eq. (9) shows that as β₂ is increased, the absolute velocity at exit c₂ is also increased. A bigger c₂ value resulted in a higher c_u2 value, which caused an increase in pressure head. The value of c_u2 can be calculated from velocity triangle using above formula [13]. The vector sum of peripheral velocity (u) and relative velocity (W) is absolute velocity (C), these vectors construct two triangles. Using these triangles shown in Fig. 1, entry and exit angles β₁, and β₂ are determined respectively.

Fig. 1

Inlet and Outlet Velocity Triangles

The values of velocity components are taken from CFturbo software. However, these values can also be computed using theoretical formulas as well.

From velocity triangles two equations (eq. 10, 12) are formed which compute entry and exit angles β₁, β₂.

In eq. (10) C_m1 is meridional component of absolute velocity in (m/s) and W_u1 is circumferential component of relative velocity in (m/s) at leading edge of blade. The value of β₁ from eq. (10) is 47.7°. In eq. (11) C_m2 is meridional component of absolute velocity in (m/s) and m_u2 is circumferential component of relative velocity in (m/s) at trailing edge. Cu² is a circumferential component of absolute velocity. ^*β₂ is angle of reduced flow. The value of ^*β₂ from eq. (12) is 32°. To calculate β₂, consideration of slip factor is necessary because the direction of relative flow W₂ at impeller outlet does not exactly follow the blade surface and, flow gets deflected and reduced. This is called slip velocity. The slip is estimated using an empirical model. The angle of flow deflection should be 10°∼14° to restrict the high turbulence losses. In this impeller, the deviation angle is 13.7°so exit β₂ is 45.7° which is sum of angle ^*β₂ and deviation angle.

The efficiency of centrifugal fan depends on higher pressure rise (ρgH) that is achieved by optimized blade shape. The efficiency is given [9].

In a backward curv ed shape, the blades are swept radially resembling a circular arc [10]. The radius of curvature R of circular arc blade is computed using the formula given below [11]. Here r₁ and r₂ are radii of circles formed at leading and trailing edges.

The number of blades for this mixed-flow impeller is 9 blades. Many fan handbooks recommend between 8 to 12 blades is a good selection [10]. The number of blades is computed using this empirical formula given by Pfleirderer [14].

In eq (16) d₂ is impeller diameter, d₁ is inlet diameter at entry. 6.5 is an empirical constant (K_z). An increase in the number of blades resulted in a narrow passage between the blades which provided better guidance to the air stream. However, it caused resistance to flow due to blade blockage, but this resistance is not too high. To mitigate flow resistance blade thickness is kept lowest to ensure smooth airflow. Thinner blades aided in reducing friction losses and flow turbulence. Careful attention is given to the exit angle β₂. The angle β₂ is very crucial for proper guidance of air through flow channel [13]. Typically, the β₂ angle value for BC blades is between 35° to 50° [10]. In this fan, the β₂ angle is kept at 45°to ensure air direction is diagonal. Increasing the number of blades and high β₂ caused a high boost in fan pressure. Blade span is another important feature in this impeller design. In this impeller, the blade span is longer (9 spans) so it helped to increase the surface area available for interaction with the flow of air.

3.2 Preliminary design procedure

To design an impeller three parameters are required to be defined. These are flow rate, total pressure difference and rotational speed, their values are put in the global setup in CFturbo [15]. Also, the rotation direction of the impeller is set.

Table 2

Impeller blade specifications

The next step is to define the Impeller material which is stainless steel (density 7,750 kg/ m³).

Then Impeller main dimensions are defined. These dimensions depend on approximation functions that are based on experimental data. Euler equation of turbo-machinery is the basis to compute these dimensions and these are automatically calculated by software. The dimensions are given in Table 3.

Table 3

Impeller main dimensions

In the next step, the meridional contour is sketched. The shape of shroud is kept tapered. The hub and shroud are represented by 4th-order Bezier curves. The outlet is designed to be diagonal. The second stage is specifying material to the hub and shroud. When the impeller design is completed these material parts and blade solid are connected to make a single solid impeller. The third stage is defining the secondary flow path e.g., diffuser. Since for this design, no diffuser is required, that's why no secondary flow path is defined [16].

In the final stage, the shape of leading and trailing edges is defined. The leading edge is rounded and elliptical while the trailing edge is abrupt and straight. This is because, at the trailing edge, the requirement is to reduce blade blockage in flow passage to ensure smooth airflow. In Fig. 2 it can be seen that the blade passage is reducing along the blade radius. This is as per need, to guide the air stream in the required direction.

Fig. 2

Blade Passage Area

Finally, a 3D impeller geometry is obtained (Fig. 3).

Fig. 3

3D Model of Fan

4.1 CFD setup

The traditional method of experimental study of fans is often complex, time-consuming, and expensive, making it less appealing. The advancement of numerical investigation, especially the use of computational fluid dynamics (CFD), has emerged as an effective technique to analyze the internal flow characteristics of fans. CFX 2021 R1 is used for the numerical analysis [17]. The fan analyzed in this study is an ECM plenum fan, which basically does not include a casing or housing as part of its design. Plenum fans are specifically designed to operate without any of these additional flow path components, relying instead on the surrounding plenum for airflow distribution. Therefore, the computational analysis was restricted to the impeller domain only. Moreover, the analysis presented in this work was based solely on CFD simulations, which were performed with great care to ensure accuracy through proper mesh refinement, selection of appropriate boundary condition and turbulence modeling. In future studies, this work will be extended to include experimental test results to validate the numerical results.

The 3D model from CFturbo is imported into the ANSYS design modeler. In the design modeler, by combining hub, shroud, inlet, and outlet curves on the ZX plane, the flow path is generated. Then the flow path was used to generate export points for fan geometry. The export points generated three curves namely hub, shroud, and blade. Then these curves are used in BladeGen.

Table 4

Number of elements in each grid section

Fig. 4

3D mesh of Single blade passage

4.2 Mesh generation

The precision of the computational solution depends heavily upon the mesh quality. The numerical solution of the flow field's partial differential equations requires computations at definite discrete points. The grid generation process involves the placement of these discrete points throughout the entire flow field. For the model fan, complete flow passages are taken into account during mesh generation. A Hexahedral-type mesh was generated on the 3D model of the fan using TurboGrid meshing software. The generated mesh of the mixed flow fan model is shown in Fig. 5. The y+ method was used to obtain a fine mesh for near-wall regions of the flow domain. For the entire flow domain, the distance from the wall to the first node is considered for the y+<2, based on the turbulence model of the current study. Unlike axial fans, the centrifugal fans often require computational domain extension. In the present research, the numerical analysis is performed on extended domains.

Fig. 5

Comparison of Single and Full passage

To achieve an optimal mesh, it is essential to assess mesh dependencies. The grid convergence index method (GCI) developed by Celik et al. [18] is used to verify mesh dependency. In the GCI method, three separate meshes are used to check the uncertainty caused by discretization errors. The extrapolations are performed with mesh refinement factor of 1.307 and 1.272. The efficiency and head are selected as the main variables and their values are normalized against those found from the fine mesh. As the number of elements increases, the values in Table 5 exhibit a pattern of monotonic convergence.

Table 5

Grid independence test

Celik et al. [18] recommended, that the main variables must have index values of less than 1% ensuring smaller error. Hence, the smaller values of the GCI_Fine and e²¹ show that the mesh is optimum and more refinement is not needed. Hence, the ideal mesh have 0.46M elements.

4.3 Boundary conditions

The steady-state analysis was carried out on both single-passage and full passage. The fluid domain is created by joining the fan components with interfaces. General Grid Interface (GGI) is used to transfer data at the linkage of domains. The rotating and stationary parts are coupled using the stage mixing plane interface for steady-state simulation. The stage mixing model transports the data by circumferential averaging at the boundary between the spinning and stationary domains [19]. Commonly known boundary conditions are employed for the CFD. The inlet is specified by the total pressure and the outlet is specified by mass flow rate. The no-slip boundary condition and automatic wall function are used on the walls of all domains. The working fluid air is set at 25°C. The impeller is set to be a rotating domain having an angular velocity of 3214 revolutions per minute and a reference pressure of 1 atm. The hub and shroud are also set to be rotating walls of the impeller. The inlet & outlet are set to be stationary domains. At the inlet, a turbulence intensity level of 5% is applied. The model was solved numerically for these operating conditions applied to inlet and outlet domains [19]. RANS equations were solved on the generated mesh with an SST turbulence model implemented on the mesh. The SST blended the k-ε and k-ω models to provide accurate flow predictions in near-wall and the flow stream.

4.4 Numerical procedure

A high-resolution central approach is employed to discretize the convection and diffusion terms. The turbulence numerics are of the first order. The flow regime is set to be subsonic type. Maximum 2000 iterations were set to reach convergence in solution. The root-mean-square (RMS) value of the residuals is used for the time-varying convergence standard, and the value is set at 10^-6. In the present work, the auto time scale is used with the timescale factor set to 5. Various expressions for calculating fan efficiency, input power, total pressure at the outlet, etc. are put in the output control and also set as monitor objects to evaluate fan performance based on their values [19].

5.1 Comparison of single passage & full passage

The single blade passage analysis method allowed to reduce computational cost and provide faster simulation time. The full passage analysis method provided a comprehensive view of the fan's performance by capturing the correct operating conditions with high accuracy. Overall, in this research, the single passage method is the preferred approach because of the efficient use of computational resources for early-stage design. Moreover, the CFD result obtained from full-passage method is not much different from single-passage so we concluded that single-passage method is enough at this stage. This study evaluated the fan performance based on specification data given by the fan manufacturer. The resulting values gained from CFD analysis are in good agreement with fan specification data. In Fig. 5 single blade and full blade passages are displayed. In Table 6, a comparison of single-blade passage and full-blade passage is shown [19].

Table 6

Comparison of single and full passage

5.2 Fan performance curves

The fan performance is analyzed on different flow rates and rotating speeds to assess the effect of speed variation on pressure rise and efficiency. Analyzing the behavior across a range of speeds helps identify optimal operating points and any potential aerodynamic inefficiencies. Changes in impeller rotating speed affect internal flow physics which helps to understand flow separation patterns, pressure contours, velocity streamlines, etc. Additionally, fan curves are generated at different rotational speeds which allow designers to determine the fan's capability across a wide range of operating conditions. This ensures that the impeller design not only meets the rated design point but also performs efficiently in off-design conditions. The fan model is simulated by changing the rotating speed of impeller and flow rate to observe how variation in speed and flow rate affect its performance.

Fig. 6, shows that compared to other rotating speeds, the highest value of fan outlet pressure is obtained at design point of 80 m³/min The curve showed a steeper drop in total pressure beyond 105 m³/min. This suggested increased aerodynamic losses which limited the pressure recovery as the flow rate increased. This decline in total pressure at high flow rates pointed towards a reduction in efficiency at these higher operating points.

Fig. 6

Outlet Pressure variation with Flow rate

Fig. 7 indicates that at lower RPMs, the optimal flow rate is between 45∼80 m³//min. At 3214 rpm, the pressure dropped significantly after 105 m³/min, which suggests the fan reached a flow rate beyond its design point where pressure generation becomes less efficient. This means operating this fan outside the optimal range will lead to higher energy consumption. The pressure drop could be mitigated by optimizing the blade angle.

Fig. 7

Static Pressure across Flow rates

It is shown in Fig. 8 that at 3214 rpm and 80 m³/min best efficiency point is obtained. At 3214 rpm, the efficiency slope is less steep, indicating a wider range of flow rates where the fan operates efficiently. Normally, when speed is increased the BEP moves to higher flow rate and higher-pressure conditions. The BEP shifting is validated by the affinity laws as given in eq. (17). Flow rate is directly proportional to speed so BEP shifts.

Fig. 8

Efficiency at different flow rates

The observed shift in BEP and changes in efficiency slopes are normal behaviors in fan performance. At high flow rates, beyond the BEP, the fan's efficiency declined. This is because the flow conditions become less optimal for energy transfer between the impeller and the fluid. The reasons for this trend are adverse pressure gradients at the blade surface and flow instabilities due to transient effects that are not fully captured in all of these CFD analyses as only the steady-state simulations are performed on different flow rates.

Another possible cause in efficiency fluctuations is flow separation at certain flow rates. As the flow separated from the blade, it caused sudden decrease in pressure recovery and increased the drag forces which led to efficiency losses. Moreover, at high flow rates shock losses at the impeller inlet and outlet become more dominant. Running at low operating speed condition add to this efficiency decline.

In Fig. 9, input power is plotted against different flow rates. For this fan, the required flow rate is 80 m³/min. The authenticity of the numerical analysis performed in this study is validated through this performance curve because at 80 m³/min the power as plotted on the curve is matching with required input power given in Table 1.

Fig. 9

Power over a range of flow rates

5.3 Impeller blade loading at different spans

Blade loading refers to the distribution of pressure along the blade surface. In Fig. 10 blade loading plots at different spans and rotating speeds are shown. In these plots, the Y-axis shows the pressure difference. The X-axis denotes the stream-wise position from the leading edge (0) to the trailing edge (1). The upper line represents the pressure side. The lower line characterizes the suction side of blade. On the suction side, a drop in pressure at the leading edge (between 0.0 ∼ 0.1) is common at all spans but the largest low-pressure zone is formed at 20% span. The reason is stronger blade curvature near hub which causes the air to accelerate rapidly at LE, resulting in higher suction effects (i.e. lower pressure). This low-pressure region is marked by the highest negative pressure value (-1700 Pa) in blade loading plot in Fig. 10 (a). The high negative pressure at the LE near hub indicates flow separation in this region. The 50% span in Fig. 10 (b) is intermediate in blade loading between 20% and 80% spans. On 50% span at 2040 rpm, between 0.2∼0.4 increase in pressure is much greater compared to 2720 rpm. The reason is less severe pressure gradient at low rpm which led to more attached flow over certain portions of blade. The better flow attachment resulted in unexpectedly higher local pressure between 0.2∼0.4. Fig.10 (c), shows that at 80% span, here the centrifugal forces are highest of all spans which resulted in more acceleration and streamlined flow. However, at 80% span on 3214 rpm, a large drop in pressure at trailing edge is observed. This is due to higher relative velocity of air at higher RPM at TE and energy losses due to turbulence, contributing to a sharp drop in static pressure at TE.

Fig. 10

Blade loading at different spans

It is clear from these blade loading charts that blade shape requires changes. This shows the optimization of leading and trailing edges of blade is necessary to mitigate adverse pressure effects.

5.4 Comparison of relative velocities on blade's trailing edge surface at different rotation speeds

The relative velocity is the velocity of air relative to moving blade. Fig. 11(a) showed relative velocity at 2040 rpm. The increase in relative velocity is not uniform across the blade surface. The maximum relative velocity is 35 m/s, noticed at mid-section, showing the flow is more attached to blade at this section. The low-velocity region near tip of TE is due to no-slip condition imposed on impeller surface at the wall. This condition led to zero relative velocity at the wall, meaning the air adheres to the wall surface and does not slip over it. The fluid velocity changed from zero to free-stream velocity while moving away from the wall, so owing to these viscous effects the velocity near to tip of TE is much lower than the velocity of bulk flow. In Fig. 11 (b) relative velocity at 2720 rpm is pres ented. As higher rpm caus ed an increase in kinetic energy of air, so here an obvious increase in relative velocity is observed. Fig. 11(c) presented relative velocity at 3214 rpm. The maximum relative velocity of 45 m/s is dominant at mid-section which indicated better flow attachment in this area and higher rpm resulted in efficient energy conversion.

Fig. 11

Relative velocities at different RPMs

5.5 Comparison of pressure distributions on blade surfaces for different rotational speeds

Fig. 12 (a) shows the pressure contour on the suction surface of the blade at 2040 rpm. The black lines are velocity streamlines. The colored contours represent pressure distribution on blade. At the leading edge, due to high flow velocity, the pressure dropped (marked by sea green). Moving along the suction side, at the mid-span, a region of higher pressure (green to yellow) is observed as flow stabilized here. At the trailing edge, the pressure rises to 1986 Pa, represented by red color. Fig. 12 (b) presented pressure contour on pressure side of blade. At the LE, the pressure is high due to attached flow. On the mid-span, the pressure reduced slightly, then increased afterward. As the flow approaches the trailing edge, the pressure increases, as shown by the orange color with a few red regions. The streamlines are relatively smooth. The streamline density near the TE is high, indicating a decelerating flow and pressure gradient.

Fig. 12

Pressure distribution at 2040 rpm (a) Suction side (b) Pressure side

Fig. 13 (a) represents suction side pressure at 2720 rpm. The pressure gradient at 2720 rpm compared to 2040 rpm is steeper. Due to adverse pressure gradient at leading edge, the boundary layer got separated causing a low pressure at LE. At higher rotational speed, the flow moves faster so the pressure rise is higher in contours of 2720 rpm, causing suction effect. At LE, due to stronger suction forces, the low-pressure region near the LE at 2720 rpm extends deeper as compared to 2040 rpm. The low-pressure region at LE depicts that flow separation occurred on the suction side at 2720 rpm. Moreover, the chaotic velocity streamlines indicate turbulent behavior of flow on the suction side. In Fig. 13 (b) the pressure side at 2720 rpm is shown. Here pressure dropped initially, then it increased at the end of mid-span and it continued to increase until the flow left the TE. Smooth streamlines indicate a uniform nature of flow at the pressure side.

Fig. 13

Pressure distribution at 2720 rpm (a) Suction side (b) Pressure side그림21

Fig. 14 (a) shows pressure distribution on the suction surface at 3214 rpm. As the flow entered the leading edge of the blade, it experienced an adverse pressure gradient near the hub section. This is due to the high blade curvature on the suction side. The flow underwent significant turning which led to a stronger suction effect and the air accelerated rapidly, causing a significant pressure drop Owing to this reason, a low-pressure region is formed near the hub which is highlighted as region (A) in Fig. 14 (a).

Fig. 14

Pressure distribution at 3214 rpm (a) Suction side (b) Pressure side

The same suction effect can also be validated through the blade loading plot at 20% span in Fig. 10 (a). Also in Fig. 14 (a), region (A) also highlighted flow stagnation as here the streamlines are not moving forward with the mainstream. In region (A) flow separation exists as both pressure and velocity are dropped. In the mid-chord region, the pressure increased marked by a green contour. Also at mid-chord, it is observed that the velocity streamlines are twisted, indicating flow deceleration. In accordance with Bernoulli's Principle, as the flow moved toward trailing edge, it slowed down substantially causing a considerable rise in pressure. The high pressure at TE is marked by an orange color. Compared to lower speeds, the centrifugal forces are stronger at 3214 rpm owing to higher speed. Because of this reason, the velocity streamlines are chaotic at trailing edge, indicating adverse pressure effects happening at trailing edge.

On the pressure side of the blade in Fig. 14 (b), at the LE, the flow accelerated sharply as it moved over the blade surface. The streamlines are thick, which indicates a higher velocity at LE and relatively low pressure. The air pressure started to increase (yellow color) after flow decelerated due to blade twisting. Near trailing edge, the fluid slowed down which resulted in a pressure rise (red mark). From flow field behavior described in section 5.5, it is obvious that the blade shape can be optimized further to achieve maximum static pressure.

5.6 Pressure distribution through inlet to fan outlet

Fig. 15 represents pressure distribution from inlet to outlet. Pressure remains constant between stream-wise 0.0∼ 1.0 as flow is in inlet condition. As the fluid passed through the passage (1.0 to 2.0), we observed an increase in both static pressure (red line) and total pressure (green line). This increase is due to the energy imparted by the fan blades to the airflow, raising both the static and dynamic pressures. The fluid decelerated, converting kinetic energy into static pressure. The sudden jump in total pressure after location 2.0 involved multiple factors. At the impeller exit, the fluid has received the full work input from the blades, manifested as a sharp increase in total pressure. Also at 2.0, the transition from a rotating frame to a stationary frame occurred. Inside the impeller (rotating frame), the total pressure includes more static pressure with a little relative dynamic pressure. At impeller exit (stationary frame), total pressure also included the dynamic pressure due to wheel speed. This is attributed to a sudden increase in total pressure at 2.0. Towards outlet, the static pressure rises more rapidly, after stream-wise 2.0, down in the outlet section. This implies that most of the dynamic pressure has been converted to static pressure.

Fig. 15

Pressure distribution from inlet to fan outlet

5.7 Velocity vectors from inlet to fan outlet

Fig. 16 shows the velocity vectors through inlet section to outlet of fan. The flow accelerated at leading edge of the blade (yellow vectors) and then slowed down at mid-section of blade (green marks).

Fig. 16

Velocity vectors through inlet to fan outlet

It means the mid-section provided the static pressure rise. The same can be validated by looking at passage section in Fig. 15 at location 1.5, a rising red line indicating an increase in static pressure. There are many low-velocity vectors near shroud which shows that, due to steep shroud curvature, the phenomena of flow separation have occurred at shroud. Moreover, it is obvious from the velocity vectors that the flow is more accelerated in hub region, having yellow marks dominant in this section. Some velocity vectors are scattered at trailing edge, indicating adverse pressure gradient existed at trailing edge. After the trailing edge, when flow entered in outlet section. The flow area is increased, and the fluid decelerates which causes an adverse pressure gradient. In the near wall, a region named “S”, is a stagnation zone where flow velocity is reduced significantly which formed a re-circulation region. The “S” region has many vectors moving in a backward direction towards the impeller. The reversing flow reduced the overall momentum in the flow direction. As main flow interacted with re-circulation zones. This caused turbulent mixing losses, which resulted in energy dissipation in this stagnation zone. Due to these losses, pressure rise through the fan, and fan efficiency is reduced. The existing design needs optimization of the outlet section to provide a more gradual increase in the outlet area.

5.8 Comparison of meridional velocities on meridian surface at different rotational speeds

The meridional surface represents the shape of the impeller's hub, shroud, inlet and outlet. In Fig. 17, the meridional velocities are shown for different wheel speeds.

Fig.17

Meridional velocities

Fig. 17 (a) shows velocity distribution on meridional surface at 2040 rpm. A stagnation region is observed on shroud side due to weaker centrifugal force in this area. This caused an adverse pressure gradient in this region.

Fig. 17 (b) represents the meridional velocity at 2720 rpm. Similar flow stagnation is observed on shroud. But it is a little more pronounced as compared to stagnation observed at 2040 rpm.

Fig. 17 (c) presents the velocity distribution on meridional surface at 3214 rpm. The velocity distribution showed variation due to pressure gradient. At the shroud near the trailing edge, a stagnation zone is formed. This zone resulted in flow stagnation and caused energy losses. However, at 3214 rpm this stagnation region is smallest because at higher rpm the centrifugal forces are stronger which helps to push the air outward with greater momentum. Moreover, here the stagnation region is localized at shroud only and does not expand in other regions. The flow recovered from stagnation and the onward accelerated flow helped to induce pressure recovery on the fan outlet.