Prediction of Vane Pump Performance Using CFD

The vane pump is a positive displacement pump, which can be used for both fixed and variable flow by varying the eccentricity of the design.

The main components (refer Fig.1) of the pump are cam ring, rotor, vanes inside the radial slots of rotor and vane ring to keep the vanes in contact with cam ring in order to provide low slip and high volumetric efficiency. The cam ring center line and rotor axis are offset to each other to creating an eccentricity between them. This eccentricity causes increasing and decreasing volume between them, when the rotor is rotating inside the cam. The vanes are assembled in radial slots of rotor, which are sliding in and out as the rotor rotates inside the cam. The regions between vanes are called as chambers. When rotor rotates in its direction from inlet port, volume increases in the chamber next to inlet port creating a suction pressure which causes the fluid to flow from inlet port to chamber. As rotor rotates further, the volume changes in the subsequent chambers and finally fluid is displaced by the decreasing volume to outlet port.

The eccentricity is the key parameter in determining the volumetric displacement of the pump. In variable flow design, based on the flow requirement cam ring is adjusted to vary the eccentricity either manually or in reaction to the hydraulic pressure.

Various types of vane pumps are used in automotive for engine lubrication and fuel supply. Although it has advantages over gear pumps like quiet, smooth operation with small pressure ripples, it is more expensive and time consuming to develop the pump. Hence CFD plays a significant role in its design and development and greatly reduces testing cost and time.

Computational Fluid Dynamics (CFD) is used in vane pump to simulate 3-Dimensional transient flow with heat transfer to predict pressure in the chambers, velocity vectors of flow fields, temperatures, etc. and validate the pump performance parameters with test results. CFD also accounts for leakage and cavitation effects.

The following is the methodology established to simulate the flow analysis of vane pump:

Fluid Volume Extraction and Simplification

As the scope of this analysis is to study the dynamics of fluid flow, fluid path (i.e. Domain enclosed by wetted surfaces) is extracted from the given 3D CAD model. The extracted fluid domain is classified into rotating and stationary zones based on its functionality. Different zones of fluid path is simplified, cleaned and checked for sharp angles, slivers, holes etc. Geometry Simplification and cleanup is done to avoid the meshing complexities without affecting the physics of the flow.

Grid generation

The rotating fluid domain between rotor and cam ring is discretized with structured hexahedral elements (refer Fig.2) using mapped scheme to facilitate the dynamic motion of the mesh. Meshing is done with at most care to improve the quality of the elements, to avoid solution divergence issue while solving. In order to capture the physical reality of the flow characteristics, proper mesh density is maintained in the fluid chambers enclosed between rotor and cam ring considering the aspect ratio. Maintaining the aspect ratio with optimum cell size and cell count in the small clearance (micron range) provided between rotor and cam ring is a challenge. The decrease in cell size correspondingly decreases the time step size which leads to increase in computational time and cost. The stationary fluid ports are discretized with unstructured tetrahedral elements (refer Fig.3) of good quality.

For geometry simplification and mesh generation, Ansys Design modeler (DM) and Ansys Mesher (AM) are used.

Boundary conditions

Since the atmospheric pressure is acting on the oil in the sump, pressure at the inlet is considered as atmospheric. The back pressure is assigned at the outlet of the pump for the rated pump speed.

Solving Methodology

For solving, we use the pressure based transient solver provided by Ansys Fluent to capture the periodic behavior of flow parameters. The flow is considered as incompressible. To model the high level of turbulence created inside the pump, the k-ε model with standard wall function is used. Sliding interfaces are created between the rotating chambers and stationary ports to get the continuous flow field data between these two domains. PISO (Pressure Implicit with splitting of operators) pressure velocity coupling scheme is used for faster convergence and stable transient flow calculations. First order implicit scheme is applied for spatial and temporal discretization.

The flow requirements are specified at both inlet and outlet boundaries for the corresponding rotor speed and the solution is solved with a minimum convergence criteria of 0.001.

In order to find the priming time or to study the cavitation effects, Multiphase modeling can also be included.

Dynamic mesh motion

To simulate the time‐varying vane motions, the dynamic mesh capability of Ansys Fluent was used. The following two motions are defined to solve vane pump simulation:

  • Rotation of the pump rotor and vanes.
  • Sliding motion of the vanes in the radial slots of the rotor.

User defined function is used for defining these rigid dynamic motion of fluid chambers and also for smoothing the deformed mesh each time step in order to maintain the overall mesh quality. The motions are assigned to the respective walls of the pump core (shown in Fig. 2). The node displacement in the moving mesh is calculated as the function of eccentricity, pump speed and time step size.

Results and Discussion

The important performance parameters like flow rate, pressure head and volumetric efficiency are extracted from the analysis results and validated with the experimental data.

The pressure and velocity field (refer Fig.4 & 5) at various positions of rotor are visualized and animated. For ‘n’ number of vanes, ‘n’ cycles of delivery takes place for each revolution of the pump. The periodic delivery of the pump and the pressure built up inside fluid chambers (refer Fig.6 & 7) causing the discharge can be plotted for the degree of rotation. The details of the pressure pulsation acting on the rotor and vanes show a significant role in the design of vane pumps as these pulses causes the component stress and shorten its life. By locating the recirculation zones in the ports and other flow phenomena, we can arrive at change in the design.

Leakages are also accounted in CFD simulation which depends on various clearances provided and the oil temperature. In the case of high back pressures, the vane tip leakage (refer Fig.8) and leakage due to other clearances show a significant reduction in the flow rate. Hence thin gaps between vanes and the cam walls as well as other clearances are modeled depending upon the complexity. Since CFD model represents a rigid model, leakages due to deformation of housing, cover and cam at high pressure cannot be captured.


CFD is used extensively in development and validation of various vane pump designs. CFD Analysis drastically reduces the overall time, cost and effort associated with testing and validate the designs in conceptual and development stages.

CFD predicts the performance and efficiencies of various vane pump designs, such as peak pressure acting on chambers are within design limits, flow discharge at the outlet is at designated value for rated speeds. CFD prediction shows that, the location of peak pressure is observed at the same position in same chamber for various speeds and pressure outlet conditions. This confirms the correctness & robustness of vane pump design. Overall CFD Prediction of vane pump parameters are 90% matching with the experimental data.