This paper compares experimental static pressure measurement with CFD simulation in a centrifugal compressor at 12 points through the diffuser. Three mass flow rates are selected, each for three operating speeds giving nine total operating conditions. The results show that the CFD model generally slightly underpredicts the static pressure value as compared to the experimental results. The discrepancy between experimental and numerical results ranges between -8% and +6% and is fairly consistent for a given operating condition, except for close to the blade trailing edge where the pressure variation is less regular and where the pressure is increasing most rapidly with radial position. In the consistent region, where the pressure gradient is low, the discrepancy is around two percent or less for simulations close to the design operating point. Away from the design operating point the errors increase up to approximately 5%. The simulation results were also used to investigate the effect of the position (from the blade trailing edge) of the impeller-diffuser interface (a characteristic of the frozen rotor simulation approach). Here an optimal position for the interface was found to be 2% of the blade radius. This value gave improved agreement with the experimental result in the initial region of the diffuser up to a distance of approximately 10% of the radius. At greater distances the position of the interface became less important. The results also highlighted a change in the pressure along the spanwise direction close to the tips. A dip in the pressure, which was observed in the experimental results, was only observed in the simulations close to the shroud. Close to the hub the simulation results recorded a small local peak. The simulation approach was then applied to further study the flow characteristics by examining the full-field velocity and pressure contours in the impeller and diffuser regions to identify changes due to the different operating conditions.
Centrifugal compressors are widely used in a range of applications including refrigeration and air conditioning, power generation, aeronautics, turbochargers, and the oil and gas industry; and their design is an important factor in the performance and efficiency of the systems in which they are incorporated. Thus the simulation of centrifugal compressors is becoming increasingly important and has been applied to investigate a range of phenomena such as noise generation [
In recent years, one of the major trends in centrifugal compressor research has been at off-design operating conditions. Both the widening of operating range and the efficiency at off-design operations have been extensively studied in recent years, as the efficiency requirements for different systems have been increasing. As the off-design operations is more important than previously and CFD is commonly used in different stages in the compressor design, the CFD accuracy at off-design conditions also becomes more important.
Out of the accumulation of a body of work, a number of common approaches have resulted in terms of CFD model settings with regard to turbulence models [
Another important consideration when modelling centrifugal compressors is simulating the interface between the rotating impeller region and the stationary inlet and diffuser. When performing a steady state simulation, the impeller region is simulated in a rotating frame of reference and the other regions are simulated in a stationary frame of reference. At the interface there are two approaches: the mixing plane, where quantities are averaged circumferentially at the interface, and the frozen rotor method, where pressure and velocity are transferred directly across the interface, with the circumferential velocity adjusted by the local blade speed [
The current body of literature for the purposes of CFD model validation, to the best of the author’s knowledge, focuses only on the inlet and outlet characteristics of the flow, namely, static pressure or a quantity derived from it, such as in [
Here we consider a CFD model validated against experimental pressure measurements at 12 points along the diffuser. The experimental and CFD details are set out in Sections
The test compressor is located in Laboratory of Fluid Dynamics, at Lappeenranta University of Technology, Finland. The compressor test facility is closed-loop, and the test compressor is a high-speed centrifugal compressor, controlled with active magnetic bearings. The impeller has nine full and nine splitter blades. The compressor is equipped with a parallel wall vaneless diffuser and a volute. The main design parameters are listed in Table
The main design parameters.
Mass flow [kg/s] | 1.8 |
Specific speed | 0.70 |
Rotational speed [1/s] | 461 |
Impeller outlet radius [mm] | 271 |
Diffuser outlet radius [mm] | 542 |
| |
Blade backsweep at the impeller outlet [°] | 40 |
Blade height at the impeller exit [mm] | 12.2 |
Diffuser height [mm] | 10.3 |
Number of full and splitter blades | 9 + 9 |
Process instrumentation chart.
Air is taken from a settling tank, through an inlet valve. The flowrate, pressure, and temperature are measured before and after the compressor. After the outlet measurements, the airflow is cooled in a heat exchanger with water and transferred back into the tank through a control valve. The performance measurement setup and calculations comply with ISO 5389. The measured design operating point performance and uncertainties are shown in Table
Design operating point performance.
Parameter | Value | Relative error [%] |
---|---|---|
Total-to-total efficiency [%] | 79.8 | |
Total-to-total pressure ratio [-] | 2.36 | |
Mass flow [kg/s] | 1.79 | |
Static pressures in the vaneless diffuser were measured at 12 different radial locations. The pressure taps were situated opposite to the volute tongue. Nine first pressure taps are on the shroud side, and the last three are on the hub side because of the volute. The pressure tap placement is shown in Figure
Pressure tap locations.
location | | location | |
---|---|---|---|
1 | 1.01 | 7 | 1.50 |
2 | 1.07 | 8 | 1.59 |
3 | 1.13 | 9 | 1.69 |
4 | 1.20 | 10 | 1.80 |
5 | 1.30 | 11 | 1.90 |
6 | 1.40 | 12 | 1.95 |
Pressure tap placement.
The static pressures were measured at nine different operating points. The nine points were at three different rotational speeds, three points at each speed line. The nine operating points are shown on the compressor operating map in Figure
Operating points at which the static pressures were measured.
point | | | |
---|---|---|---|
1 | 461 | 1.98 | 2.28 |
2 | 461 | 1.80 | 2.36 |
3 | 461 | 1.44 | 2.48 |
| |||
4 | 364 | 1.46 | 1.81 |
5 | 364 | 1.33 | 1.72 |
6 | 364 | 1.06 | 1.76 |
| |||
7 | 323 | 1.24 | 1.54 |
8 | 323 | 1.13 | 1.57 |
9 | 323 | 0.90 | 1.61 |
Compressor operating map and the operating points at which the static pressures were measured.
Once the desired operating point had been set, the compressor was let to run until all the temperatures had settled to a steady value. Once steady state had been achieved, the static pressures were recorded. Five pressure values were recorded for each location, and once the results were processed, the five values were averaged to give a single pressure for each location at each operating point. Figure
Measurement uncertainty for each static pressure measurement.
Simulations were carried out using commercial CFD software ANSYS CFX version 17.1 in steady state.
Following [
Domain partition.
Total temperature and pressure were applied as inlet conditions with values of 96 kPa
The combination of a total pressure and temperature inlet with a mass flow rate outlet is the approach favoured for stability [
Following [
The computational grid was generated in ANSYS Turbogrid and a convergence study is shown in Figure
Mesh convergence.
Simulation grid.
The final mesh was the densest of those considered and consisted of approximately 2.2 million elements. The global size factor used was 1.75 and the near wall element size specification method was y+ with a Reynolds number of 7x106 to give a target y+ value of 0.5. The passage spanwise blade distribution method selected was proportional with a factor set to 1. Convergence was deemed sufficient when the RMS value of all the residuals reached O(10−5). Following Celik et al. [
A comparison of the experimental and simulated (area averaged) pressure ratios is presented in Figure
Comparison of experimental and simulated pressure ratios.
Away from the tips (r/r2 > 1.2) the differences remain somewhat constant. In this region the CFD results consistently underestimate the pressure ratio (ranging from virtually no underestimation to approximately 6%) with respect to the experimental data. It is interesting to note that these differences are smallest, 2% or less, at the design speed and mass flow rate (461 Hz and 1.8 kg/s) or close to them (461 Hz and 1.98 kg/s). Further from the design operating point the errors are larger in the range of 2% to just over 5%. This can be seen in Figure
Variation in the average error for r/r2 < 1.2 with the deviation from the design point.
In the region closer to the tips (r/r2 < 1.2) the difference varies more and the maximum differences (+6% and -8%) occur. This is to be expected due to the more rapid and less uniform variation in the pressure ratio is in this region. It is also interesting to note that in the inner region the differences are either positive (CFD overestimating the pressure ratio) or less negative (CFD underestimating the presser ratio by less) than in the outer region.
Other than this there is no clear trend in the data. For example, although the lowest mass flow rates flows all show the maximum difference of approximately -6% in the outer region for the higher speeds, this behavior is not replicated by 323 Hz results. This suggest that other than the results being more accurate close to the design point as described above, there is no systematic error featuring in either set of results.
In Figure
When comparing experimental and numerical results there is often an ambiguity as to where in the computational domain the inlet to outlet pressure line is taken in a spanwise sense. The experimental setup used had the first nine pressure taps placed into the diffuser shroud and as such represents a physical value b/b2 of close to unity. Figure
Pressure distribution at different spanwise positions at 461 Hz for a mass flow rate of 1.8 kg/s.
A key and interesting feature of the results is the initial drop in pressure immediately downstream of the impeller. This can be explained by the pinched diffuser with the pinch as r/r2 = 1.02, as indicated in Figure
Details of the pinched diffuser.
Physically speaking the interface between the impeller and the diffuser occurs at r/r2 = 1. However, for modelling and meshing reasons the interface is typically placed a small distance downstream, for example, 1.025 in [
Domain interface position pressure distribution at a spanwise distance of 0.9, 461 Hz, and 1.8 kg/s mass flow rate.
Figure
Having verified the accuracy of the computational model throughout the diffuser domain, the full pressure and velocity fields are studied in more detail in the diffuser and impeller regions. This is shown in Figures
Static pressure and velocity magnitude contours at 461 Hz.
Static pressure (1.44 kg/s)
Velocity magnitude (1.44 kg/s)
Static pressure (1.8 kg/s)
Velocity magnitude (1.8 kg/s)
Static pressure (1.98 kg/s)
Velocity magnitude (1.98 kg/s)
Static pressure and velocity magnitude contours at 368 Hz.
Static pressure (1.06 kg/s)
Velocity magnitude (1.06 kg/s)
Static pressure (1.33 kg/s)
Velocity magnitude (1.33 kg/s)
Static pressure (1.46 kg/s)
Velocity magnitude (1.46 kg/s)
Static pressure and velocity magnitude contours at 322 Hz.
Static pressure (0.9 kg/s)
Velocity magnitude (0.9 kg/s)
Static pressure (1.13 kg/s)
Velocity magnitude (1.13 kg/s)
Static pressure (1.24 kg/s)
Velocity magnitude (1.24 kg/s)
The static pressure contours show that the pressure ratio decreases with mass flow rate and increases with rotational speed, as previously observed in Figure
When comparing the velocity magnitude contours a velocity jump across the frozen rotor interface can be observed. This view highlights the essential difference between the frozen rotor and mixing reference frame. Velocity “peaks” can be seen in the diffuser domain to be moving radially outwards and in the direction of rotation. If the diffuser were vanned this nonuniformity would be problematic; however as the diffuser is vaneless this is insignificant. In the impeller domain velocity contours show a “dead” spots of the Coriolis vortices, approximately 1/3 of the way through the impeller domain. These are present at each of the rotation speeds. At the moderate and higher mass flow rates these vortices are relatively small and positioned slightly closer to the pressure side of the blades. At the lowest mass flow rate, for each rotation speed, the regions are significantly larger. At 461 Hz the region extends up to the splitter blade and at the lower speeds it virtually encloses the lower third of the splitter blade.
Experimental and numerical approaches have been applied to analyse the performance of a centrifugal compressor.
In general, the CFD model showed good agreement with the experimental measurements throughout the diffuser region. A maximum difference of 8% was observed in one simulation in the region close to the tip (r/r2 < 1.2), where the pressure variation with radial position tends to be less regular and increases at its maximum rate. Outside this region the magnitude of the differences was less and approximately constant with radial distance. Generally, the CFD underpredicted the pressure ratio, except for a few points close to the blade tips for some simulations. In particular, it was observed that, in this outer region, the accuracy of the simulation results was particularly good close to the design point of the compressor where the difference between the experimental and the CFD results was less than 2%. Further from the design point the errors were larger but still less than approximately 5%. No systematic differences were noticed within the range of parameters considered, validating the use of the model.
Typically, when compressors are modelled with CFD for design or research purposes, only a single blade passage is modelled with the assumption of circumferential uniformity, and the volute is omitted, as was done here. The results indicate that the inaccuracy of the simulations increase the further from the design operating conditions the performance is predicted. As the off-design operations of compressors are becoming more important, the design engineers should bear this in mind. Works such as [
The conventional CFD practice of placing the diffuser domain interface as close to the blade tips as possible produces the most accurate results for regions close to the blade tips but under predicts the static pressure at the diffuser outlet. Conversely increasing the r/r2 position of the diffuser domain interface produces less accurate results near the blade tips but replicates the static pressure at the diffuser outlet more accurately. The variation in pressure in the spanwise direction through the diffuser was also considered. For r/r2 > 1.1 no significant variation was observed with the spanwise position; however, close to the impeller outlet a small but significant difference was observed. For spanwise positions greater than 0.5 a dip in the pressure was observed which was consistent with the experimental results (taken at the shroud with a spanwise position of approximately 1). This was not observed for spanwise positions of 0.5 or lower.
Contour plots were also presented which gave a detailed description of the velocity and pressure field through both the impeller and the diffuser region for the nine operating conditions considered.
Having validated a computational model more elaborate and detailed analysis can be undertaken with an increased degree of confidence, such as, for example, blade loading, flow contours, and examining the flow as it approaches surge and choke.
Experimental data collected at LUT was used.
The authors declare that there are no conflicts of interest regarding the publication of this paper.
Numerical computations were done on the Sciama High Performance Compute (HPC) cluster which is supported by the ICG, SEPNet, and the University of Portsmouth. Brett Dewar, Mike Creamer, Mariana Dotcheva, Jovana Radulovic, and James M. Buick wish to thank InnovateUK for financial support provided for this work through the KTP grant [KTP009973].