The presented research demonstrates the results of a series of numerical simulations of gas flow through a single-stage centrifugal compressor with a vaneless diffuser. Numerical results were validated with experiments consisting of eight regimes with different mass flow rates. The steady-state and unsteady simulations were done in ANSYS FLUENT 13.0 and NUMECA FINE/TURBO 8.9.1 for one-period geometry due to periodicity of the problem. First-order discretization is insufficient due to strong dissipation effects. Results obtained with second-order discretization agree with the experiments for the steady-state case in the region of high mass flow rates. In the area of low mass flow rates, nonstationary effects significantly influence the flow leading stationary model to poor prediction. Therefore, the unsteady simulations were performed in the region of low mass flow rates. Results of calculation were compared with experimental data. The numerical simulation method in this paper can be used to predict compressor performance.
Detailed experimental and numerical research of flow structures in centrifugal compressors began in the last century. Nonstationary effects were experimentally observed and described in detail in [
Eckardt (1976) [
Compressor Design Department of Saint Petersburg Polytechnical University has a special test stand for gas compressors. This stand allows the measurement of different instantaneous and mean parameters, such as pressure, velocity, and temperature. The basic characteristic of gas compressors is the pressure characteristic that shows the dependence of the gas pressure ratio from mass flow rate for a given rotational speed.
The compressor under research is a laboratory low-pressure centrifugal compressor with a vaneless diffuser. It was designed for very low total pressure ratios (
Up to now, there were a small number of papers, known to authors, devoted to numerical simulation of the centrifugal compressor [
The objective of this work is a numerical simulation of the gas flow in the centrifugal compressor and validation of the obtained results against the physical experiment.
Experimental data and the geometry of a single-stage centrifugal compressor with a vaneless diffuser were provided by Compressor Design Department of Saint Petersburg State Polytechnical University. The experiments were carried out for eight regimes with different mass flow rates. Three different cross-sections of the compressor duct were examined during the experiments. These cross-sections are the inlet, diffuser inlet, and diffuser outlet (see Figure
Geometry of the centrifugal compressor.
Tables
Experimental data for regimes 1–4.
Regimes | 1 | 2 | 3 | 4 |
---|---|---|---|---|
|
294.6 | 294.8 | 294.8 | 294.9 |
|
0.629 | 0.553 | 0.495 | 0.434 |
|
101791 | 101778 | 101778 | 101778 |
|
1.047 | 1.053 | 1.060 | 1.066 |
|
1.045 | 1.051 | 1.056 | 1.061 |
Experimental data for regimes 5–8.
Regimes | 5 | 6 | 7 | 8 |
---|---|---|---|---|
|
295.0 | 295.0 | 295.1 | 295.2 |
|
0.312 | 0.266 | 0.116 | 0.105 |
|
101911 | 101765 | 101765 | 101765 |
|
1.073 | 1.076 | 1.076 | 1.075 |
|
1.068 | 1.069 | 1.068 | 1.067 |
The compressor contains 16 rotational blades. The rotating speed of the impeller is 6944 rpm. The diameter of the impeller is 275 mm (Figures
Geometry of the impeller.
Geometry of the blade.
Periodic boundary conditions are used when the flows across two opposite planes in a computational model are identical [
Wall boundaries can be either stationary or moving. The stationary boundary condition specifies a fixed wall, whereas the moving boundary condition (e.g., using a moving reference frame) can be used to specify the translational or rotational velocity of the wall or the velocity components [
The boundary conditions for the studied model are shown in Figure
Boundary conditions.
Steady-state simulations were done in NUMECA FINE/TURBO 8.9.1 using different available turbulence models and discretization schemes. The calculations were carried out on a single structured mesh with 700 000 control volumes. The mesh was constructed to fit the wall
Figures
Pressure characteristic at the diffuser inlet for different turbulence models using first-order upwind discretization.
Pressure characteristic at the diffuser outlet for different turbulence models using first-order upwind discretization.
The first-order turbulence models give out similar results of pressure characteristic. As could be noticed from the figure, the calculated pressure characteristics are plain even where nonstationary effects are strong (below 0.3 kg/s). Moreover, the obtained total pressure ratio is within predicted values in the region of high mass flows. It could result in high pressure losses due to dissipation effect of first-order schemes. Therefore, the first-order approximation is insufficient to reproduce the stationary characteristic of the low-pressure ratio compressor.
Figures
Pressure characteristic at the diffuser inlet for the Spalart-Allmaras turbulence model using second-order central discretization.
Pressure characteristic at the diffuser outlet for the Spalart-Allmaras turbulence model using second-order central discretization.
The conclusion could be that the second-order central discretization scheme conforms to the pressure characteristic shape much better than first-order upwind schemes. In addition, the pressure ratio does not conform to the experimental results in the region of high mass flows. Due to ignoring of hub and shroud leakages, the observed deviation of the pressure ratio was to be expected. In the region of low mass flow rates, nonstationary effects are dominant and steady-state simulations are not capable of capturing them.
Figures
Flows paths at mass flow 0.4 kg/s, first-order upwind and second-order central discretization.
Flows paths at mass flow 0.3 kg/s, first-order upwind and second-order central discretization.
Flows paths at mass flow 0.2 kg/s, first-order upwind and second-order central discretization.
Flows paths at mass flow 0.175 kg/s, first-order upwind and second-order central discretization.
The large vortex structure starts to form when the flow rate falls below 0.4 kg/s only if the second-order scheme is used. First-order schemes do not predict any vortex structures until the flow rate falls below 0.2 kg/s, but even then predicted structures are not very large. This could be attributed to strong numerical dissipation effects that are present when using first-order schemes. The stalling regime is very strong when using second-order central schemes. Due to strong influence of unsteady effects on mean flow parameters, unsteady simulations are needed to be carried out for accurate capturing of these effects.
Steady-state and unsteady simulations were done in ANSYS FLUENT 13.0 using the realizable
Figures
Pressure characteristic at the diffuser inlet for the stationary case in the diffuser inlet.
Pressure characteristic at the diffuser outlet for the stationary case in the diffuser outlet.
It is clear from the pressure characteristic that computed pressure ratio values are slightly over experimental curve. This could be attributed to neglecting the influence of hub and shroud leakages. The shape of the numerical characteristic is in a good agreement with the shape of the experimental characteristic.
All nonstationary effects were observed in the experiments in the regimes with small mass flow rates. Therefore, only the first three regimes in the unsteady simulations were omitted.
Unsteady calculations were done in a transient formulation with first-order time discretization. 20 and 100 time steps for one period for the coarse and refined mesh were chosen, respectively. Thus, the time step for the coarse mesh was equal to
The pressure characteristics for the unsteady case are shown in Figures
Pressure characteristic at the diffuser inlet for the unsteady case in the diffuser inlet.
Pressure characteristic at the diffuser outlet for the unsteady case in the diffuser outlet.
As can be clearly seen from the figures, the unsteady pressure characteristics are very similar to stationary pressure characteristics.
To provide accurate results, the dependence of mass flow rate in the inlet on the mesh size was investigated (Figure
Mesh sensitivity analysis.
Table
Results of mass flow rate in the inlet for unsteady simulations.
|
|
ErrCM |
|
ErrRM |
---|---|---|---|---|
0.4338 | 0.4678 | 7.32 | 0.4434 | 3.15 |
0.3123 | 0.3443 | 9.29 | 0.3264 | 4.32 |
0.2661 | 0.3169 | 16.03 | 0.2983 | 10.79 |
0.1158 | 0.2618 | 55.57 | 0.2248 | 48.49 |
Unfortunately, no vortex structures are present and no rotating stall is reproduced for this case. The possible meaning is that the unsteady calculations do not cover nonstationary effects. It could be attributed to one-period geometry or the turbulence model. Further study of this phenomenon is necessary.
Numerical results of executed calculations show strong dependence on the order of discretization. First-order discretization schemes are unacceptable because they do not reproduce large scale vortex structures due to numerical dissipation effects. Second-order schemes are capable of reproducing these structures.
Numerical results agree with the experiments for regimes with high mass flow rates. In the regimes with low mass flow rates, formation of large nonstationary vortex structure (rotating stall) leads to the inability of stationary models to accurately reproduce flow physics. However, these effects have not been reproduced in unsteady simulations in ANSYS FLUENT 13.0. A possible reason for this is that one-period geometry is incapable of reproducing these nonstationary effects.
Steady-state calculations of a one-period model are required to be done for different turbulence models with second-order discretization schemes and on more refined meshes. Also, unsteady flow simulations for 360-degree geometry should be carried out.
Since the experimental measurements exist for the modelled compressors, it was possible to carry out the verification and validation of user software. The agreement between the results obtained by numerical modelling and by experiments is satisfactory, which enables complete replacement of the time-consuming experimental investigations by much rapid numerical simulations.
The represented numerical modelling of flow in centrifugal compressor makes it possible to carry out the optimisation of basic part of compressor (e.g., impeller) with the aim of improving the efficiency of machinery.
The authors declare that there is no conflict of interests regarding the publication of this paper.
The work has been carried out at the Department of Mathematics and Physics, Lappeenranta University of Technology, and Department of Applied Mathematics, Saint Petersburg State Polytechnical University. The experimental results have been obtained by the test stand for gas compressors at the Compressor Design Department, Saint Petersburg State Polytechnical University.