Abstract
In this study, centrifugal compressor performance was predicted using CFD. Three-dimensional time-averaged impeller and volute simulations were performed using a Navier-Stokes code. The presented performance prediction method has been divided into three phases. Firstly, the impeller was calculated with a vaneless diffuser. That gives inlet boundary conditions for the volute analysis and the pressure ratio at the diffuser exit. Next, the volute analysis was performed and a static pressure recovery coefficient obtained. Finally, that result was combined with the pressure ratio prediction from the impeller analysis, and the overall compressor performance thus obtained.
INTRODUCTION
Scroll-type volutes, typically used in industrial centrifugal compressors, are used to collect the flow from a vaned or vaneless diffuser, and to guide the flow to the downstream pipeline. The volute geometry is usually fixed or stiff and the area is designed according to a certain rotational speed and mass flow rate, i.e., the design point of the compressor. The aim is to get a constant flow in that point, which means also a constant static pressure distribution in the circumferential direction. At off-design conditions the flow behaves differently and, as a result, there are circumferential pressure distortions in the volute, which reflect upstream into the diffuser and the impeller.
INTRODUCTION
Experimental, theoretical, and numerical results concerning centrifugal compressor volutes have been published by many authors, including works by Stiefel (1972) and Ayder et al. (1991 Ayder et al. ( ,1993 Ayder et al. ( ,1994 . Recently, Hagelstein et al. (1997) have investigated both constant-area and scroll-type volutes experimentally. They noticed, that pressure distortions are associated with both configurations.
INTRODUCTION
The development of computers will gradually render the simultaneous three-dimensional time-accurate analyses of the impeller and volute possible. However, according to Hillewaert and Van den Braembussche (1998) , some simplifying assumptions are still needed. Sorokes et al. (1998) have used a method where the impeller and the volute analyses were made separately, and they were able to solve the non-uniform circumferential static pressure distributions in the volute. The separate analysis reduces the need for a large computational capacity compared to simultaneous simulation. On that basis, that kind of independent simulation might also be a practical alternative for analysing compressor performance, which is the topic of this paper.
INTRODUCTION
The results of a centrifugal compressor CFI) analysis without volute modelling were published recently by one of the current authors, Pitklinen (1997) . The volute was taken into account approximatively using a constant static pressure recovery factor. This paper shows how the overall compressor performance estimation can be modified by using an independent volute analysis. With this method, the impeller is firstly calculated with a vaneless diffuser thus giving inlet boundary conditions for the volute analysis. After that, a static pressure recovery coefficient of the volute is obtained from a separate analysis. Combining the coefficient with the pressure ratio prediction from the impeller analysis, the overall compressor performance is obtained.
IMPELLER GEOMETRY
A schematic cross-sectional view of the impeller and parallel-wall-type vaneless diffuser with the volute boundaries is shown in Fig. 1 . The impeller has seven full and seven splitter blades with a 30 degree bacicsweep at the trailing edge. The diameter ratio of the vaneless diffuser is 1.9. The impeller is unshrouded, but in this analysis the tip clearance was assumed to be zero. The modelling of the clearance will be added to the analysis in forthcoming studies. The compressor impeller and vaneless diffuser were each calculated independently in order to get physically correct boundary conditions for the volute analysis. For simplicity, only one blade passage between two adjacent full blades was modelled. In addition to the impeller, corresponding sectors of the non-rotating space before and after the impeller, i.e., the co-annular inlet duct and the vaneless diffuser, were modelled. The structured multi-block grids used in this study were generated using IGG software by Numeca. The surface grid of the impeller and vaneless diffuser is shown in Fig. 2 . The impeller passage was modelled using 64 streamwise cells, 32 blade-to-blade cells on either side of the splitter blade, and 32 cells in the hub-to-shroud direction. The total number of the cells in the impeller grid was approximately 300 000.
VOLUTE GEOMETRY
The computational domain of the volute geometry, as shown in Fig.3 , includes the vaneless diffuser which leads the flow to the volute, the non-axisymmetrical scroll part which goes around the diffuser, and the exit cone which leads the flow to the pipeline. The computational space was discretized using approximately 550 000 cells, which should capture enough of the physical aspects of the flow field.
VOLUTE GEOMETRY
The cross-sectional shape of the volute used was the combination of a rectangle and a semicircle resulting in an overhungtype volute where the bottom or back surface was flat and the top surface had a circular shape. The generation of the H-type grid used in this study can be done manually in several days, but the problem is the grid clustering near the walls. The more complicated butterfly-type grid with several cross-sectional sub-blocks, used, e.g., by Flathers (1996) , would give much better resolution near the walls.
VOLUTE GEOMETRY
The region around the volute tongue illustrated in Fig. 4 is a difficult location for structural grid generation. In that case, the tongue area was modelled by using a special block which had a singular (or zero area) wall. The drawback of this modelling technique is the local discontinuities of the grid cell sizes. In the computational model, the region around the volute tongue and also the shape of the exit-cone differ somewhat from the actual measured geometry because accurate surface data was not available when the modelling was done.
VOLUTE GEOMETRY
The circumferential variation of the cross-sectional area nondimensionalized by the diffuser outlet area is shown in Fig.  5 . The origin of the circumferential position is shown in Fig. 4 . In addition, the mean radius nondimensionalized by the diffuser exit radius is shown in Fig. 5 . 
MEASURED DATA
The compressor was measured in Laboratory of Fluid Mechanics at Lappeeru-anta University of Technology. The compressor had originally been designed for a vacuum application. However in this study, the measurements were carried out at both vacuum and normal conditions. Only the normal (or overpressure) operation is discussed in this paper.
MEASURED DATA
The compressor was measured at several speeds which cor- respond to a total pressure ratio up to 1.8 and a mass flow range from 0.2 to 3.6 kg/s. Three measured points on each constantspeed line represent a design condition, and the minimum and maximum stable flow conditions, i.e. near-stall and near-choke operations. The map in Fig. 6 is shown at the reference conditions 101 kPa and 288 K. It should be noted that even the highest speed is lower than the corresponding design speed of the compressor at under vacuum operation. This was due to limitations of the laboratory power supply. Circumferential static pressure distributions were measured with five static pressure taps on the volute top surface. The pressure distributions were recorded at all the measured points OD the compressor map. Qualitatively, they all show the same trend, i.e., at the lowest mass flow rate the pressure tends to rise, and at highest mass flow rate it decreases in the circumferential direction. The distributions are shown in Fig. 7 and it can be seen that they mimic similar trends that other authors have presented with scroll-type centrifugal compressor volutes.
NUMERICAL METHOD
The CFD analysis was performed using the flow solver FIN-FLO developed at Helsinki University of Technology, Siikonen et al. (1990) . The flow simulation was based on the solution of the Reynolds-averaged Navier-Stokes equations (RANS). The impeller calculations were performed in a coordinate system which rotates around the rotational axis of the compressor, Siikonen and Pan (1992) .
NUMERICAL METHOD
In this study, the algebraic turbulence model by Baldwin and Lomax (1978) has been applied. The basic assumption is that the turbulent viscosity coefficient depends only on the instantaneous local variables. Despite the simplicity of the model, it has been used succesfully in many kinds of turbomachinery simulations. The solution method is based on an implicit LUfactorization. In order to accelerate the convergence, the multigrid method by Jameson (1986) was used. With this kind of simulation, two or three multigrid levels are typically used. Another convergence-related parameter is a locally defined non-dimensional time step, or CFL number. It should be chosen to be as large as possible in order to reduce computational time.
NUMERICAL METHOD
All the results shown in this paper represent steady (or timeaveraged) solutions. Second-order upwind-biased discretization in all directions was used for the convection terms. The viscous fluxes were centrally differenced.
IMPELLER ANALYSIS
The boundary conditions for the impeller analysis were given using the mass flow rate, and the total temperature at the inlet, and only the static pressure at the outlet. The location of the inlet boundary was some distance before the impeller, and the outlet location was at the exit of the vaneless diffuser. The inflow velocity profile was constant, and the flow angle was assumed to be zero. Also, the outlet pressure was assumed to be uniform. The value of the outlet pressure along with the given mass flow rate and the rotating speed determines the pressure ratio of the impeller at the operating point in question.
IMPELLER ANALYSIS
The CFD-predicted total-to-total and total-to-static pressure ratios at the vaneless diffuser exit are shown in Fig. 8 with the measured total-to-total stage pressure ratio. The results are presented only for the highest measured speed. The region between the calculated curves shown in Fig. 8 depicts the dynamic pressure variation at the diffuser exit. Comparison to the stage pressure ratio indicates how the pressure should behave in the volute. It should be noted that the impeller was modelled without tip clearance, which could have some effect for the pmdiction.
IMPELLER ANALYSIS
The pressure ratio of the compressor has been previously predicted by a CFD model of the impeller and varteless diffuser using a constant pressure recovery coefficient for volute, Pitkanen (1997) . The pressure coefficient is a measure of the static pressure changes with respect to dynamic pressure and it was defined as c p,, 35 = (p5 -/33)/ (pip -p3), where the subscript 5 represent the outlet of the exit cone, and 3 the vaneless diffuser exit, see Fig. 9 . In this study, the pressure recovery was studied by modelling the vaneless diffuser together with the volute.
VOLUTE ANALYSES General
The separate analyses of the compressor impeller and of the volute obviously 'filters' out all the interaction which really occurs between these components. But a simulation of that phenomenon, would necessitate the simultaneous analysis of the impeller and the volute. The results and lessons learned from this study may be utilized later when more sophisticated methods are developed. 
Boundary conditions
The inflow boundary conditions for the volute analysis were given at the vaneless diffuser inlet, i.e., the diffuser component was modelled a second time. The mass flow rate, the flow angle and the total temperature were taken from the impeller analysis by averaging the flow quantities on the constant grid plane at the impeller exit. The flow angle was defined at the impeller exit by defining firstly the radial and circumferential velocity components individually on either side of the splitter trailing edge and then taking the mean value of the components across the spitter. The total temperature boundary condition for volute was taken from the vaneless diffuser exit from the impeller analysis. Because of the single-passage impeller analysis and the averaging, the inflow conditions for the volute analysis were assumed to be constant in the hub-to-shroud direction and also uniform circumferentially. These assumptions were also used by Sorokes (1998). In reality, the hub-to-shroud and circumferential distributions are not so ideal.
Boundary conditions
A uniform static pressure was given at the volute exit. This outlet pressure was chosen according to the measured exit pressure of the compressor, and also in order to match the pressure at the common plane between the impeller and the vaneless diffuser in both the separate analyses. The locations of the boundary conditions are shown in Fig. 9 . 
Convergence history
The typical convergence history is shown in terms of mass flow rates in Fig. 10 . These histories represent simulations where the runs have been re-started from previous solutions obtained with a coarser grid.
Convergence history
All three mass flow rates show quite different convergence characteristics. At the design point, the flow is, naturally, most stable and the solution can be obtained in approximately 1000 iterations. Also, at the lowest mass flow rate, i.e., at near-stall operation, the convergence is good despite some oscillation occuring. The flow solver seems to need about three times more iterations in that case compared to at the design point. The highest mass flow convergence is interesting as some aperiodic, relatively small amplitude fluctuation, remains in the solution. This indicates some time dependent nature of the flow which the steady-state solver is probably not able to capture exactly. 
NEAR-CHOKE

Results
The primary goal of this study was to estimate the static pressure recovery of the volute at different operating points. There were basically two possible ways to combine the results of the impeller and the volute analyses in order to get the overall performance prediction. The first approach was that the pressure ratio was taken across the impeller and vaneless diffuser combination from the impeller analysis, and only the volute pressure recovery coefficient was added from the volute analysis. The second approach would have been that the impeller pressure ratio was defined firstly, and then the pressure recovery of the diffuservolute combination added to it. The first approach was adopted hem.
Results
The CFD-predicted pressure recovery coefficients are shown in Fig. 11 . The coefficient cpn5 = (ps -p3)/(p03 -p3) shows the variation of the pressure in the volute, and the factor c 5 = (Ps -P2)/(PG2 -P2) includes also the pressure recovery in the vaneless diffuser. The static and total pressures were taken from constant grid surfaces as mass-averaged values from locations 2, 3, and 5 shown in Fig. 9 . In addition, the total pressure loss coefficient of the volute defined as 0235 = (p03 -pos)/(p03 -P3) is shown in Fig. 11 . The variation of the coefficients show the same trends as those observed, e.g., by Ayder (1993) .
Results
The volute pressure recovery coefficient Cp r3s at the nearstall point is positive, the design point value is approximately zero, and at the biggest mass flow rate the coefficient is clearly negative. The pressure recovery of the diffuser-volute combination, cns , is always positive, because of the static pressure rise in the vaneless diffuser. The loss coefficient, w35, increases with the mass flow rate.
Results
When the pressure recovery coefficient Cpr 35 is combined to the pressure ratios shown in Fig. 8 , a CFD-predicted stage performance can be obtained, Fig. 12 . The method is simply based on the pressure coefficient definition, which can be written like p5 = c 5 (p0 -p3) + p3. The Cpris coefficient of the volute has now been calculated using the volute model, and all the other factors on the right-hand side are known from the impeller analysis. Thus, a new overall pressure ratio can be defined from Ps/Poi. It should be noted that the dynamic pressure at the compressor exit is assumed to be negligible. It can be seen from Fig.  12 that, qualitatively, the overall agreement is good between the calculated and measured data. The underprediction of the pressure ratio at the biggest mass flow rate could be corrected by adding the dynamic pressure to the static pressure p5.
Results
The isentropic efficiency of the compressor stage can be calculated using the pressure ratio shown in Fig. 13 and the temperature rise from the impeller analysis. The comparison between the measured and calculated efficiency referred to the maximum measured efficiency is shown in Fig. 13 . The good agreement proves that the method presented here can be used for the stage performance prediction of the compressor.
Results
The CFD-predicted circumferential surface pressure van- ation in the volute is compared to the measured one in Fig. 14. In addition, the shroud pressure distributions at the diffuser inlet are shown. The general agreement is satisfactory at all operating points. However, the rate of change of the measured pressure in the circumferential direction is consistently less negative than the CFD-predicted rate. This might indicate that the volute inlet boundary conditions (or flow angles) obtained from the impeller analysis were not exactly correct. In addition, the calculated pressure levels are slightly higher which can be explained with the larger blockage of the model compared to the measured one, because the shapes of the modelled tongue and the exit-cone were not exactly like the measured geometry. At the lowest mass flow rate, the measured pressure is lower than the corresponding CFD-predicted pressure at small angles near the tongue. This can be explained by the flow angle being slightly too small at the inlet, when measured from the radial direction, as the pressure rise is very sensitive to the diffuser inlet flow angle. If the angle were increased by a few degrees, an exact prediction would be obtained in terms of circumferential pressure. The shroud pressure distribution at the diffuser inlet is almost constant. At the design point, the agreement is quite good between the measured and the predicted data. Also, the measured and calculated pressures tend to decrease slightly along the volute. The diffuser inlet pressure also shows little variation. For the case of the highest mass flow rate, the calculation tends to overpredict the pressure most noticeably. The diffuser inlet pressure distortion is also strongest at this point.
Results
Generally speaking, the method for specifying the boundary conditions for the volute has to be verified more thoroughly. For that, more detailed experimental data for the compressor will be needed. Also the geometry modelling techniques have to be developed further.
Results
The swirling flow inside the volute has been visualized using velocity vector projections on some cross-sections of the scrollpart, see Fig. 15 . The strong main vortex, where the flow is rotating clockwise in the main flow direction, is clearly visible. The opposite secondary vortex near the corner is also present at this near-stall operation point. Fig. 15 shows the region around the circumferential position of 90 degrees. In a further study, this CFD method could be used to reduce the volute losses. This rectangular-semicircular cross-sectional volute shape would be replaced by a new one without any sharp corners.
CONCLUSIONS
A three-dimensional Navier-Stokes flow solver has been used in this centrifugal compressor performance analysis. The impeller and the volute components have been modelled separately instead of simultaneously which would require massive computational resources.
CONCLUSIONS
The impeller analysis was performed by modelling only one blade passage and the corresponding sector of the vaneless diffuser. The flow angle and total temperature were taken from the impeller exit in order to get consistent boundary conditions for the volute analysis.
CONCLUSIONS
The overall compressor performance prediction was based on the following: a) Total-to-static and total-to-total pressure ratio were obtained from the analysis of the impeller and of the vaneless diffuser at design and off-design conditions b) The volute was analyzed separately with the vaneless diffuser in order to obtain the static pressure recovery coefficient variation c) The combination of these two results represents the overall compressor performance
CONCLUSIONS
The CFD-predicted overall pressure ratio and efficiency were compared with the measured ones, and the resulting agreement was good. The comparison of the measured and the calculated circumferential pressure distributions shows that the volute geometry has to be modelled more accurately especially near the tongue region.

{'paper_id': '54492351', 'title': 'CFD Analysis of a Centrifugal Compressor Impeller and Volute', 's2_url': 'https://api.semanticscholar.org/CorpusID:54492351', 'source': 'S2ORC'}