Applications of different turbulence models in simulations of a large annular volute-type pump with the diffuser

It's necessary to choose a good turbulence model for the reliable numerical simulation of the pump in hydraulic optimization. In this paper, the four widely used turbulence models are selected and compared in three dimensional steady numerical simulations for a large annular volute-type pump with the diffuser. The pump performance is verified by the experiments in an open test rig. The results show that the SST turbulence model gets closer values to the experiment in predicting head. The trend of the pressure distribution at design condition for the four models on pressure side is very similar, which first increases and then decreases along the streamline. There are a minimum at 0.05 and a maximum at 0.8 of the length of the streamline, due to the existence of vortices. The predicted pressure distribution on the suction side is more similar. With the increase of flow rate, the flow field in the impeller becomes more uniform, and the number as well as the size of the vortices decrease. Secondary flow is observed in the volute and three vortices are found near the upside of the volute.


Introduction
Pumps play an important role in transmitting the energy and substance in almost every field. Many researchers have done a lot of research in many aspects from experiments and simulation. With the development of computer, the CFD(Computational Fluid Dynamic)is more widely used and has achieved a lot of success. Ji et al. [1] proposed many procedures of to optimize the diffuser to improve the efficiency by CFD. Kong et al. [2] designed a thermal shock loop to test heat shock resistance and operation stability of residual heat removal pump, which could really simulate practical working conditions of nuclear power plant. Teng et al. [3] analyzed the heating status of bearing body based on heat transfer theory and the relations between recycled water flow and its outlet temperature. Liu et al. [4] obtained the fluid-structure coupling force based on the fluid-structure coupling analysis. The rotor modal was calculated by means of the model function of ANSYS considering pre-stress or not.
But there are not many studies on the turbulence models used in the simulation of the annular volute-type pump. In some literatures the applicability of different models of volute-type centrifugal pump has been discussed. Feng et al. [5] investigated the unsteady flow in a radial pump by utilizing six different models, and compared the numerical results with LDV and PIV results. It was found that turbulence model didn't exert significant influence on the pressure field. At off-design condition, the SST and DES turbulence model predicted successfully the "two-channel" stall phenomenon in the impeller detected by the measurements. Zhang et al. [6] examined applicability of the standard k-ε model, the RNG k-ε model and the Realizable k-ε model in the simulation of centrifugal pump. It was confirmed that all the three models are suitable for the numerical simulation of the internal flow of a centrifugal pump, but the Realizable k-ε model has the best agreement with the experimental results．Zhang et al. [7] also simulated the flow in a low specific speed pump impeller under off-design conditions with k-ε and SST models. It was assumed that using standard k-ε and SST could simulate the flow in a low specific speed pump impeller under off-design condition accurately，but there were some errors compared with PIV measurements and LES results of the flow field in the impeller.
Choosing an appropriate turbulence model for the annular volute-type pump is a big challenge. Most of pumps above were small, so in this paper, a larger pump is chosen. Four common turbulence models are selected to simulate the flow in the pump, based on which a direct comparison of the results predicted by different models could be made. The obtained numerical results are compared with the experiment results. This paper is aimed to offer a reference about the turbulence model applicability of the annular volute-type pump.

Pump model
A commercial single-stage, single-suction, annular volute-type pump with diffuser is selected as the simulation model. The pump has five backswept blades, followed by seven straight radial vanes. The design parameters of the pump are shown in table 1.

Computational domains and meshes
The computational domains consist of seven parts suction, impeller, ring, diffuser, volute, and front and back chambers, as shown in figure 1. Considering the back-flow at inlet and outlet, a long straight pipe with the five times the diameter of the inlet and outlet is added respectively, in order to save calculation time and improve the calculation accuracy.  independence analysis is shown in figure 2. It can be seen that when the mesh number is less than 5.2 million, the head changes greatly. But when it is larger than this mesh number, the heads almost remain unchanged. So considering the accuracy and economy, the 5.2 million mesh number is chosen for the future research. For the whole domains, the Y plus is less than 200.

Four turbulence models
The eddy viscosity turbulence models are widely used, which can be divided into zero-equation and two-equation models. Two-equation model solves two additional transport equations making it offer a good compromise between numerical effort and computational accuracy [8]. Both the velocity and length scale are solved using separate transport equations. To simulate the annular volute-type pump, four types of two-equation turbulence models are selected to make a choice with steady simulation by using CFX 14.0.
The k-ε model introduces two new variables into the Reynolds averaged energy equation. The values of k and ε come directly from two different transport equations as follows: (b) RNG k-ε turbulence model Compared to k-ε model, RNG k-ε model is modified to account for the different scales of motion through changes to the production term [9]. The constant One of the advantages of the k-ω formulation is the near wall treatment for low-Reynolds number computations. It allows for smooth shift from a low-Reynolds number form to a wall function formulation. The transport equation for k and ω are as follows: The model constants are given by: accurate predictions of the onset and the amount of flow separation under adverse pressure gradients. It combines the advantages of the k-ε and k-ω model. The proper transport behavior can be obtained by a limiter to the formulation of the eddy-viscosity:

Steady simulation setup
In the simulation, the discretization in space is of high resolution accuracy, and the first-order backward Euler scheme is chosen for the time discretization. The Multiple Reference Frame is used, which means the impeller is in rotating frame while other parts in stationary frame. The interfaces between the rotating and the stationary domains are set to "Frozen Rotor": one is the interface between the inlet and impeller and the other is between the impeller and the diffuser. The inlet boundary condition is set to total pressure and the outlet is flow rate with no-slip wall for the rest walls. The own wall functions of the models are chosen for the simulation. The max iteration step is 300 and the convergence is considered to be 10 -5 .

Results and discussion
The accuracy of the simulation is weighed by the performance based on the steady simulation results. Then the flow characteristic pressure and velocity distributions in the flow passage components for different models and flow rates are compared.

Comparison between different models
Eight different kinds of mesh numbers are divided for the mesh independence analysis [10]. At last the 5.2 million mesh numbers is chosen for the steady simulation. The head is chosen as the criteria for weighing the simulation. Experimental data were collected at the laboratory for the model pump. The comparison of the delivery head curves obtained by numerical calculations and experiments for all conditions of nominal speed is shown in figure 3. The delivery head agrees with the experiments quite well at design and over-load conditions for the four models while at part-load conditions they differ greatly. The SST and k-ω models predict more accurately than the k-ε and RNG k-ε models.

Figure 3.
Head curves for four models. To compare in greater detail, the head and errors at five flow rates for different models are given in table 2 [11]. From table 2, it can be seen that the error is the least at designed condition, which is below 2.5%, reaching the least 0.48% for the SST model. Within 5.5%, the errors at over-load conditions increase as the condition is away from the designed one. The errors for SST and RNG k-ε models are smaller. At part-load conditions with errors within 8%, the SST and k-ω get smaller errors. So considering the head, SST model is better for simulating this pump. For the RNG k-ε model, the errors fluctuate more largely than other models. So it can be concluded that the RNG k-ε model is not suitable for simulating this large annual-volute pump. The SST modal gets a smaller error than the k-ε model at four conditions. The errors for the k-ω and k-ε models differ more at part-load conditions than at over-load conditions. It can be concluded that the computational values vary greatly at part-load conditions, so it is necessary to find a more suitable model.

Flow field analysis
From figure 4(a), it can be seen that the trend of the pressure distribution at midspan on blade pressure side along the streamwise for four models is very similar, which first increases and then decreases along the streamwise. Streamwise=0 represents the leading edge of the blade while streamwise=1 represents the trailing edge of the blade. The pressure at inlet is close to 1 atm, a relatively large value. Then at about 0.05, there appears a minimum, where cavitation is likely to occur. The k-ω model predicts the largest pressure at inlet, while the others get similarly smaller values. As for the minimum point, the pressure for the RNG k-ω model is the least while that for the k-ω model is the largest. After 0.05, the pressure begins to be the same again, reaching the same at 0.2. But after 0.45, they develop in the reverse direction slowly. The pressure at impeller outlet decreases at first and then increases, which is influenced by the diffuser. The pressure for the four models at outlet differs from each other, being the largest for the RNG k-ω model and the least for the k-ω model, with a difference of 91608Pa. So the RNG k-ω model predicts the largest head.
(a)Pressure side (b)Suction side Figure 4. Pressure on blade pressure and suction side at midspan at Q=910m 3 /h. Figure 4(b) is the pressure distribution on the blade suction side along the streamwise. The pressure value is much less than that on the pressure side. It's positive at inlet but turns to the negative rapidly as result of the vacuum induced by impeller rotation. After the minimum point, the pressure begins to increase gradually because the impeller gives energy to the fluid. The pressures predicted by the four models show considerable variations from 0.15 to 0.6 along the streamwise, while at other parts they are almost the same. As shown above, pressure at part-load conditions is more complex. So the pressure at Q=120m 3 /h is shown in figure 5 for more details. It can be seen that the trend of pressure on the suction side is similar to that at Q=910 m 3 /h, but with higher values. But on the pressure side, the variation trend is not same as that at Q=910m 3 /h: there is no obvious pressure drop at 0.05; instead, it increases almost monotonically but with a slower rate. The pressures predicted by the four models are always different, particularly for the end part of the streamwise. There is a maximum at about 0.8 because vortices appear here. The vortices appear in sequence of the RNG k-ε, k-ω, k-ε and SST turbulence models. The RNG k-ε model has the largest peak value while the k-ε model gets the smallest.
(a)Pressure side (b)Suction side Figure 5. Pressure on both blade pressure and suction side at midspan at Q=120m 3 /h. Figure 6 is the pressure distribution on blade at midspan with the SST model at three different flow rates. The pressure on both sides differs greatly with the flow rate. The pressure on the pressure side at part-load condition has a great difference with the other two conditions, especially at the outlet. The pressure at outlet of the impeller is the largest at Q=120 m 3 /h, and is the smallest at Q=1475 m 3 /h. The pressure on suction side at the mid of the flow passage has a great decrease at Q=1475 m 3 /h, which is not as uniform as that at other conditions.
(a)Pressure side (b)Suction side Figure 6. Pressure on both blade pressure side and suction side at midspan with SST model at three flow rates. The velocity distribution can be seen in figure 7 with SST model at three flow rates. With the increase of flow rate, the flow field has a great variation, which becomes more uniform. At the same time, the number and size of the vortices decrease. At Q=120 m 3 /h, there are many vortices of different size in the flow passage. The vortices on the suction side in the middle of the passage are larger than those on the pressure side at the impeller outlet. The vortices distribute asymmetrically because of the outlet pipe. The streamline is smooth at Q=910 m 3 /h, but there are also small vortices on suction side at the inlet. The streamline is smoother in the passages away from the outlet pipe. At larger flow rate, the velocity becomes larger and more uniform with smaller vortices.  A cross-section with φ= 70° in the volute is chosen, which is defined in figure 8. The velocity distributions for different models are shown in figure 9. As a result of the centrifugal force, the secondary flow is developed for all the four models [12]. This volute is not asymmetrical, so three vortices are found in the upside of the volute. Two are near the opposite volute wall respectively, while the other is in the middle of the right angle. The locations of the vortices are slightly different for the k-ε, k-ω, and SST models. The RNG k-ε model fails to predict the vortex near the left wall and one more vortex is found in the downside of the volute.

Conclusions
(1) The SST turbulence model gets closer values to the experiment in predicting head.
(2) The trend of the pressure distribution at design condition for the four models on the pressure side is very similar, which first increases and then decreases along the streamline. There are a minimum at 0.05 and a maximum at 0.8, because of the existence of vortices. The predicted pressure distributions on the suction side by four models are more similar.
(3) With the increase of flow rate, the flow field in the impeller becomes more uniform. At the same time, the number and size of vortices decrease. (4) Secondary flow is observed in the volute. But as it is not asymmetrical, three vortices are found in the upside of the volute. (5) The locations of three vortices predicted by k-ε, k-ω, and SST models are almost the same while the RNG k-ε model fails to show one of the vortex.