Flow simulations with relevance to a centrifugal compressor and the eect of the inlet geometry

Flow simulations with relevance to a centrifugal compressor and the eect of the inlet geometry

Ander Eza 25/02/2015

Abstract

Turbocharging the internal combustion engine is one of the most ef- fective ways to reduce the fuel consumption and fulll the green house gas emissions requierements. Nevertheless, this techinque has some lim- itations that need to be addressed in order to improve the turbocharger performance. The range of use of the compressor is restricted by the surge line at low mass ow rates and the choke line at high mass ow rates. The compressor map gives valuable information of the compressor stable oper- ating points. However, due to the space constraints in an engine comparti- ment, complex pipes are needed to integrate all the components correctly leading to a dierence in the compressor preformance from measurments to in-situ congurations. Computational Fluid Dynamics is a powerful tool to predict compressor maps in a shorter time and less laborious way compared to experimental measurements and obtaining data in the whole domain.

The compressor map of a turbocharger compressor was calculated us- ing a steady-state RANS approach and the Moving Reference Frames tech- nique to handle the rotating parts of the machine, validating the method with experimental data. The ow eld from near optimal eciency points to near surge was assessed identifying a strong swirling backow at o- design conditions responsible for the eciency and pressure ratio drop.

The eect of a 90º bent pipe upstream the compressor inlet was stud- ied. Two counter-rotating vortices were observed to form after the bend and vanishing under the eect of the wheel rotation in evey case. It was shown that the ow structures introduced by the bend can be benecial at near surge condition, mitigating the rotating backow and improving the eciency and pressure ratio of the compressor at this particular case.

Acknowledgements

I would like to rstly thank Mihai for being my supervi- sor during these six months and for having accepted me as his student without knowing me beforehand. Also, his suggestions have made this work improve signicantly.

Special contribution have made some PhD students to this the- sis. I would like to thank Elias for his day-to-day support on the software and his numerous advices to present the data in the best way possible, Bernhard for his always valuable feedback and help throughout the project and Bertrand for providing me with nice information and showing a lot of interest.

I would like to thank CCGEx since this work has been done within the Compressor o-Design Operation - CoDOp Project and Borg Warner for the turbochager geometries.

In general, I would like to thank the entire turbocharging group from which I have learned a lot and KTH Mechanics for pro- viding me with the resources to make this thesis happen.

Contents

1 Introduction 5

1.1 Turbocharging . . . . 5

1.1.1 Historical Perspective . . . . 5

1.1.2 Mechanism . . . . 5

1.2 Integration with the Internal Combustion Engine . . . . 7

1.3 Compressor maps . . . . 8

2 Background & Motivation 10 2.1 Compressor performance & Compressor maps . . . 10

2.2 Compressor ow phenomena . . . 11

2.3 Upstream manifold eects . . . 12

2.4 Motivation . . . 13

3 Turbulence & Turbulence Modeling 15 3.1 Basic concepts . . . 15

3.2 Assessment of compressor ows . . . 16

3.2.1 Computational Fluid Dynamics vs. Experimental Measurements . . . 16

3.2.2 The necessity for robust tools . . . 16

3.2.3 The wall region . . . 18

3.3 Limitations With Turbulence Modeling . . . 20

4 Numerical Methodology 21 4.1 Governing Flow Equations . . . 21

4.2 Numerics . . . 21

4.3 Motion . . . 22

4.3.1 Moving Reference Frames vs. Sliding Mesh . . . 22

4.3.2 Interfaces . . . 23

4.4 Boundary Conditions . . . 24

4.4.1 Inlet boundary condition . . . 24

4.4.2 Outlet boundary condition . . . 24

4.4.3 The wall . . . 25

4.5 Solving Strategies . . . 25

5 Compressor Flow: the set-up 27 5.1 Geometry & Computational Domain . . . 27

5.1.1 Straight Inlet case . . . 27

5.1.2 Curved Inlet case . . . 30

5.2 Cases Investigated & Operating Conditions . . . 32

5.3 Grid Resolution Eect . . . 33

6 Results 34 6.1 Performance Parameters . . . 34

6.2 Flow Assessment . . . 36

6.3 Bent pipe eects . . . 47

7 Conclusions 59

8 Future Work 60

1 Introduction

1.1 Turbocharging

1.1.1 Historical Perspective

Turbocharging has its immediate backgroud in supercharging -mechanically driven- when in 1885 Gottlieb Daimler used for the rst time a gear-driven pump to force air into an internal combustion engine. Ten years later, the Swiss engineer Alfred Büchi patented the rst turbocharger consisted of a compressor device driven by exhaust gases to force air into an engine and increase the power.

Nonetheless, the devolpment of these machines was not fully accomplished until 20 years later.

During the World War I, a French engineer called Auguste Rateau succeeded in powering French aircrafts with turbocharged Renault engines. In 1918, an engineer called Sanford Alexander Moss from General Electric managed to im- plement a turbocharger in an aircraft engine mitigating the power loss frequently encountered in internal combustion engines. In the 1920s, ships and locomotives started equipping turbocharged Diesel engines and during the World Warr II, many planes mainly from the U.S. carried turbocharged engines.

The rst car that mounted a turbocharger on its engine was developed by General Motors back in 1962. The turbocharger was manufactured by Garret.

Although the power was increased, the reliability was pretty low. In 1973, BMW introduced a turbocharged engine in one of its cars, but was retired due to the large turbo lag. In 1974, under the oil crisis, Porsche started producing the 911 Turbo. The Porsche 911 is still available today with a turbocharged engine. In 1977, Saab also introduced a turbocharged engine in one of its models. Since 1978, the production and use of turbochargers in the automotive industry has been rising.

1.1.2 Mechanism

A turbocharger basically consists of a centrifugal compressor and a radial turbine installed on the same shaft. The compressor is driven by the turbine which converts the energy from the hot exhaust gases into mechanical energy. Hence, the energy from the gases is used and not wasted. As we can see in Figure 1, the air is taken from the ambient and carried to the compressor. Once it has interacted with the compressor it is made go through an intercooler and then to the cylinders of the engine. After the combustion, the hot gases are driven to the turbine where the energy is extracted to move the compressor.

In this thesis we will be focusing on the compressor side of a turbocharger for the automobile industry. In general, centrifugal compressors are used in a wide range of applications. They are used in industrial gas turbines, usually in more than one stage; in oil reneries or natural gas processing to move the product from one place to another; in air conditioning systems or in the auto- motive industry for example. They are composed of the inlet, the impeller, the diuser and the volute. The ow enters the compressor axially and interacts

Figure 1: Turbocharger. Source: mr-engineer.com

with the impeller where the kinetic energy of the uid is increased. After that the ow continues through the diuser where the kinetic energy is transformed into potential energy increasing the static pressure. The angular momentum is conserved inside the difusser, the velocity of the ow decreases as the uid advances radially converting the kinetic energy or dynamic pressure into static pressure according to Bernoulli's uid dynamic principle (1.1). The volute is responsible for collecting the ow and delivering it to the following components.

The dierent components of the centrifugal compressor can be seen in Figure 2.

P +1

2ρv²+ ρgh = constant (1.1)

Figure 2: Centrifugal Compressor

1.2 Integration with the Internal Combustion Engine

Nowadays the use of turbochargers in the automobile industry is a widely spread technique. It is known that around 32 million turbochargers were sold worlwide in 2014. The estimations say that this industry will be increasing by a rate of 9% per annum for the next ve years reaching 49 million sales by 2019. In

ve years time, 43% of annual new-vehicle production will carry turbochargers.

Therefore, the increasing demand of this industry makes very attractive to study and reasearch turbochargers in order to improve the current technology as far as possible.

The reason for the global use of turbochargers lies on the fact that by tur- bocharging the internal combustion engine the air density inside the cilinders can be increased making it possible to add more fuel and get more power in each combustion. This leads to a specic power improvement and therefore, the engine can be downsized, meaning that fuel consumption is reduced and less pollutant gases are emitted fulling the continous increasing demand for reducing green house gas emissions. Moreover the friction losses decrease given the smaller size, thus improving the overall eciency. However, there are also some limitations concerning the turbocharging technique.

The turbocharger lag is a delay of the turbocharger response against changes in load which occurs because it takes some time until the mechanical devices overcome the inertial forces. This is what a driver feels when driving a tur- bocharged diesel engine car and suddenly pushes the throttle, the response is not immediate. On the contrary, when driving a naturally aspirated gasoline car the response to throttle is faster.

Another drawback we should consider relates to the margins of operation of the turbocharger compressor both at low mass ow rates and at high mass ow rates, this is surge and choke. The choke arises when working at high mass ow rates and may lead to the appearance of sonic waves, reducing the eciency and in the end, blocking the passage. The surge, on the contrary, appears when the compressor is operating at low mass ow rates. In the compressor difusser the ow encounters an adverse pressure gradient since the pressure increases in the streamwise direction. Adverse pressure gradients are typically responsible for ow instabilities such as stall and recirculation. At low mass ow rates the inertial forces of the ow may have diculties in overcoming the advese pressure gradient leading to stall or even periodic instabilities such as rotating stall and

nally surge. The stationary stall is a phenomenon typically caused by the incidence angle increase and characterized by the ow separation on the suction side of the blade, originating vibrations and a performance drop. If strong enough, the bubble can make the inow deviate towards the neighbouring blade passage -aecting the incidence of the blade- propagating the instability and forming the rotating stall. The rotating stall is not xed and rotate in the compressor system at some fraction of the impeller speed. This phenomenon can eventually develop into surge. Surge makes the entire system unstable and the ow entering the compressor breaks down periodically with periods of strong backow. It can be identied by a disturbing noise and a violent ow

process. It can be either mild or deep, where the previous occurs with the natural fequency of the compression system whereas deep surge is characterized by a low frequency emptying and relling process. Surge has to be avoided since it can seriously damage or even destroy the compressor. These margins denitely limit the range of operation of the compressor and we should be able to predict those points in order for the turbocharger not to work beyond them.

The correct integration between the components inside an internal combus- tion engine is important and the additional space required to install the tur- bocharger makes the limitation of space in the engine an issue to bear in mind.

A lot of pipes and bends are required ot overcome the space constraints in the engine compartiment as it can be seen in Figure 3, where an in-situ conguration of a turbocharger is shown. Especially at the compressor inlet, where twisted pipes are needed in order to carry the air from outside the vehicle up to inlet nozzle. The question is if these complex geometries can aect the peformance of the turbochager. In order to have a better understanding of the entire system, a study of the ow inside these bendt pipes should be carried out.

Figure 3: In-Situ Turbocharger. From KTH Mechanics lab

1.3 Compressor maps

Compressor maps give valuable information of the compressor performance un- der dierent conditions. Basically all stable conditions under which the tur- bocharger compressor can operate are shown in these maps and this is very im- portant to predict the respones of the compressor at dierent situations. They are usually measured on test rig experiments. On the y-axis the pressure ratio is presented against the corrected mass or volumetric ow on the x-axis. As it has been said, the surge line limits the operation of the compressor at low mass

ow rates and the choke line at high mass ow rates as it can be seen in Figure 4.

Figure 4: Compressor Map

The choke line is typically dened by the condition when the eciency drops below a certain value and the surge line has several denitions according to dif- ferent people but for example, it is sometimes measured by the static tempera- ture at the inlet, increasing when the hot backow comes from the impeller and difusser to the inlet pipe. The corrected speedlines can be observed going from the surge line to the choke line and represent constant rotation of the shaft for dierent mass ow rates. The iso-eciency lines show those points of the com- pressor performance when the eciency of the machine is the same, typically two of them for each speedinle and eciency value, one closer to surge from the highest eciency point and one closer to choke. The highest eciency line is composed of those points where the eciency is maximum for each speedline.

During extreme engine acceleration the operating condition of the compres- sor moves almost vertically towards the surge line and this has to be carefully studied so that the compressor does not operate under instabilities that could damage the device. During upshifting the accleration line is smoother and step by step. At the moment the clutch is pushed we move towards lower mass

ow rates at the same speedline and after that, when the throttle is pushed the operating point moves to a higher speedline and higher mass ow rates.

2 Background & Motivation

2.1 Compressor performance & Compressor maps

Predicting compressor maps experimentally is an important step to have an overall vision of the compressor performance. The data is usually obtained from specic compressor gas stands. Typically on a test rig, the rotation of the shaft is maintained by means of the turbine air ow and the compressor mass

ow is handled by opening or closing a back a pressure valve. The characteris- tics of the compressor are obtained from the measurements of the compressor inlet and outlet stagnation temperature, inlet and outle static pressure and the mass ow rate. The atmospheric pressure is also required since the pressures are measured relative to the atmospheric pressure. In some cases the humidity is also measured to accout for its eects. The accuracy of the facility is re- ally important and sometimes it can be a great challenge to map properly all the points. Some studies analyzing the uncertainty when obtaining compressor maps have been carried out (Guillou et al., 2013). It was shown that pressure ratios were not very sensitive to uncertainties but mass ow rates could be espe- cially near surge conditions. Nonetheless the temperature measurements were observed to highly aect the eciency, for instance through the heat transfer from the turbine to the compressor making complicated to sometimes compare two maps from dierent test rigs.

In order to study the operating range of a turbocharger compressor fre- quently used in diesel engines, the map was obtained experimentally on a spe- cic turbocharger test rig emphasizing at low mass ow rates (Gancedo et al., 2012). The process was carried out by maintaining the speed of the shaft and closing the pressure valve, as mentioned earlier, from full opening -choke- to the appearance of instabilites -surge- for each speedline. Each operating point was measured when the outlet temperature did not change any more. Small dif- ferences were found comparing the map with that provided by the compressor manufacturer probably due to the fact that the manufactuer measured total-to- total pressure ratios while static-to-total values were calculated this time. Even though maps represent the compressor stable conditions, the steady compressor map from a turbocharger was measured experimentally -in a specic facility- and was also extended beyond the stable points for a small automotive com- pressor showing the pressure ratios at negative mass ow rates (Galindo et al., 2008).

The performance of a small automotive turbocharger compressor from design conditions to near surge points was studied using steady-state Reynolds Aver- aged Navier-Stokes (RANS) approach and unsteady RANS method comparing the results with experimental data (Després et al., 2013). The compressor map was plotted near surge condition showing a better agreement between the un- steady solver and the experiments. At some points URANS solution did not converge however, highlighting the necessity for a dierent tool to capture the unsteadiness.

A comparison between RANS and the more complex Large Eddy Simulations

(LES) method was completed for a centrifugal compressor near surge and under stable operating conditions (Sundström et al., 2014). The more computational expensive sliding mesh technique was used to handle the wheel rotation. It was found that at o design conditions RANS simulations diered from experimental measurements while LES showed a much better behaviour when comparing the results on a compressor map. Nonetheless, RANS approach produced good agreement with experimental data at highest eciency points and the time to reach the solution was considerably faster so it was concluded that this could be the best method when evaluating compressor maps where several points have to be calculated.

2.2 Compressor ow phenomena

One of the most characteristic and important ow phenomenon inside centrifugal compressors is surge. Several discussions regarding the precursos of surge have been carried out. The physics and behaviour of stall, rotating stall and surge have been widely explained (Japikse, 1981). Surge phenomenon does not have a specic denition and it is hard to say when it has entirely developed. In order to dene the surge limit, an installation was created to measure and detect the surge phenomenon (Galindo et al., 2006). A frequency based criterion was used to predict surge condition and it was found that the most representative variable was the pressure downstream of the compressor. The volume after the compressor and before the engine was discoverd to be highly related to surge.

The ow eld of a turbocharger compressor was studied near surge condition using a URANS approach and was observed a strong shroud separation from the diuser to upstream of the impeller at lower mass ow rates and a reverse velocity at the blade tip clearances which could be potential precursors of surge phenomenon (Després et al., 2013). The ow eld was assessed at design and o design conditions using a more complex Large Eddy Simulation (LES) tech- nique (Jyothishkumar et al., 2010). At design points, the ow showed a uniform behaviour and the pressure distribution was homogeneus, no separation or back-

ow was observed. On the contrary, near surge point, unsteadiness was found given the uctuations in the pressure and velocity elds and severe backow occurred in the diuser and through the impeller with high-swirl ow.

A ported shroud centrifugal compressor was analysed using LES for an op- erational point close to surge (Hellström et al., 2012). A highly unsteady ow

eld with reversed ow in the inlet region, wheel and difusser was observed. The volute tongue, where the ow separates depending on the pressure gradient, was found to be very related to the unsteadiness. The ported shroud has demon- strated to extend the range of operation of turbocharger compressors at low mass ow rates. The ow inside a ported shroud compressor was studied exper- imentally using a Particle Imaging Velocimetry (PIV) method (Guillou et al., 2010). Dynamic pressures at the inlet and outlet of the compressor were mea- sured showing a clear distinction between stable and unstable conditions. The

ow patterns during a whole surge cylce were followed, identifying a recircula- tion zone at the exit of the ported shroud due to the interaction with the inow.

Three dierent regimes of operation were identied experimentally in a ported shroud centrifugal compressor (Gancedo et al., 2012): stable condition, mild surge and deep surge. All these regimes were characterized by their pressure oscillation and and specic frequencies. The comparison between a centrifugal compressor with and withoug ported shroud at near surge and near optimal eciency point was carried out numerically using Large Eddy Simulation and the sliding mesh approach to handle the rotation of the wheel (Semlitsch et al., 2014). At near optimial eciency point the two congurations -with and without ported shroud- showed similar performance parameters but a recircu- lating ow was observed for the ported shroud case. At o-design conditions the ported shroud setup made the compressor eciency drop but the ow uc- tuations were reduced due to the recirculation of the unsteady ow through the ported shroud.

2.3 Upstream manifold eects

Inlet distortions on the performance and surge margin of a centrifugal compres- sor were studied experimentally (Ariga et al., 1983). The inlet ow distortion was separated into radial distortion and circumferential distortion where the for- mer can be divided into hub and tip distortion. It was observed that pressure ratios in the compressor with distorted inlet ow fell in the order of circumfer- ential, hub and tip distortions. Inlet circumferential distortion remained at the impeller exit and radial distortion almost disappeared.

The space limitation in the compartiment of an IC engine sometimes requires the inlet pipe to bend 90º so that the whole engine is integrated correctly. The inlet ow is distorted right before interacting with the impeller forming an asym- metric ow eld and aecting the compressor performance. Curved ducts are known to create a pressure gradient between the inner and the outer parts of the duct leading to the appearence of a secondary ow and two counter-rotating vortices (Kim et al., 2001). Non-uniform ow angle at the leading edges and non-uniform pressure distribution in the blade passages were observed experi- mentally leading to eciency degradation. A vaned inlet setup was simulated numerically and the counter-rotating vortices found in the vaneless setup dis- appeared with the vaned inlet approach.

Steady-state simulations were carried out with three dierent inlet geome- tries -a 90º vanless bent pipe with a nozzle, a 90º vaned bent pipe with a nozzle and a straight pipe with a nozzle- to study their eect on the compres- sor performance (Engeda et al., 2003). It was shown that the vaned bent pipe improved the the stage eciency by 3% compared with the vanless case due to the improved secondary ow eect.

A device consisting of a radial inlet and centripetal vanes was developed in order to overcome the space limitations of a turbocharger and to improve the surge margin (Galindo et al., 2006). It was found that a pre-whirl ow spinning in the opposite direction to the compressor rotation increased the surge margin. It basically moved the surge line towards the left extending the range of operation of the compressor.

The eect of a nozzle upstream the compressor was studied experimentally (Desantes et al., 2013). It was found that the eect of the nozzle shifted the surge line towards lower mass ow rates. The compessor map was obtained in a turbocharger test bench for both congurations with and without the inlet nozzle. The nozzle losses were found to be negligible and when comparing both compressor maps the surge line of the inlet nozzle case was seen to move to the left.

2.4 Motivation

Having a better understanding of how the compressor behaves quantitatively under dierent conditions is a valuable information to predict its performance.

As it has been stated, the compressor map provides a lot of information about the operation of the compressor under stable conditions. The rst purpose then, is to calculate the compressor map of a turbocharger to have a clear vision of which are the limits of operation, this is the surge line at low mass ow rates and the choke line at high mass ow rates since overpassing those limits can damage the turbocharger. Several points are going to be calculated by means of RANS numerical simulations at three dierent speeds: the lowest speedline, an intermediate speedline and the highest speedline to have wide vision of the compressor performance at dierent speeds.

Once we have identied the stable conditions on the compressor map the question is: what is making the compressor unstable beyond the surge or choke line? Analyzing the compressor ow eld qualitatively can be a good practice to recognize those ow structures that are causing the instabilities. The idea is to compare the ow eld between near optimal eciency points and near surge points to identify whatever is changing as we move towards lower mass ow rates on the same speedline. But it is important to make a comparison between speedlines as well, since the conditions will not be the same as we increase the speed of the shaft.

It has also been said that the limitation in space is an issue of relevance.

The increasing demand of turbochargers in the automotive industry and the necessity of extra space in the engine compartiment to couple properly the tur- bocharger to the engine makes the study of this integration really interesting.

Since the compressor maps are usually measured with straight inlet geometries they may vary when the compressor is placed in-situ. The correct integration of the turbocharger with the internal combustion engine tipycally introduces complex pipes to connect the air between dierent components. Sometimes a 90º bent pipe is required at the compressor inlet to overcome the packaging constraints. So a question that quickly comes up is: is the compressor aected by the distortion of the upstream geometry? Both a quantitatively and a qual- itatively study need to be performed to rstly nd out whether the compressor map is aected by the inlet geometry and secondly to analyze what structures the bent pipe could be introducing in our set-up.

It needs to be highlighted that this work is part of a bigger project involving several studies on both the centrifgual compressor and the turbine of a tur-

bocharger. There will be people covering unsteady simulations, more suitable to predict the ow eld at o desing conditions. So this thesis is thought to be a rst step of a deeper study mainly carried out by PhD students.

3 Turbulence & Turbulence Modeling

3.1 Basic concepts

Almost every uid ow in real life is turbulent. Of course, uid ows inside internal combustion engines are turbulent because of the complex geometries.

Usually when dealing with turbulence, we divide the variables in one mean, time-averaged part ¯u and other uctuating part u⁰, then the variable can be written asu = ¯u + u⁰. The uctating part is irregular and has to be described by statistical methods. Turbulence is deterministic and governed by Navier- Stokes equations. We can identify turbulent ows by a number of characterisctic properties that all turbulent ows show in some way or another.

They are three dimensional, irregular and chaotic. Dierent scales can be found in a turbulent ow ranging from those similar to the ow geometry to smaller scales. Small eddies are universal and have an isotropic behaviour.

They are dissipated by the viscous forces into heat. The larger eddies transfer the energy to smaller eddies, which in turn, transfer the energy to the smallest eddies. And eventually viscous forces dissipate the smallets eddies into internal energy. The Reynolds number, which represents the ratio of inertial forces to viscous forces, plays a major role when identifying turbulence (3.1). It is a key parameter to characterize the transition forom laminar to turbulent regime. For instance, when the ow in a pipe reaches certain Reynolds number, it is said to have become turbulent.

Re = ρ U l

µ (3.1)

being ρ the density, U the characteristic velocity, l a characteristic length and µ the dynamic viscosity of the uid.

Turbulent ows are also diusive, meaning that they tend to spread into the available space. They are also dissipative in the way that large eddies extract energy from the mean ow and transfer it to smaller eddies which transfer it again to the smallest eddies until viscous forces dissipate it into heat. This is sometimes called the cascade process.

In this thesis the uid considered will be the air. The air is treated as ideal gas and the properties can be seen in Table 1

Property Law Value

Dynamic Viscosity Sutherland's Law µ = µref(_T^T

ref)^32Tref_{T +S}^+S [P a · s]

Molecular Weight Constant 28.9664 [_kmol^kg ]

Specic Heat Constant 1003.62 [_{kg K}^J ]

Thermal Conductivity Sutherland's Law κ = κ_ref(_T^T

ref)^32Tref_{T +S}^+S [_{m K}^W ]

Turbulent Prandtl Number Constant 0.9 [-]

Table 1: Air properties

In Sutherland's law for the dynamic viscosity µref has a value of 1.716 · 10⁵[P a · s], Tref is 273.15 [K] and S is the Sutherland constat and has a value of 111.0 [K]. In Sutherland's law for the thermal conductivity κref has a value of 0.02614 [W/m k], Tref is 273.15 [K] and S is the Sutherland constant and has a value of 194.0 [K].

3.2 Assessment of compressor ows

3.2.1 Computational Fluid Dynamics vs. Experimental Measure- ments

One way to study the performance of the compressor and analyze the ow eld is by means of computational uid dynamics (CFD). CFD is a powerful tool used to predict uid ow, heat transfer, mass transfer or similar issues by solving the mathematical equations that govern these phenomena using a numerical proccess. This approach has been used in the aerospace industry for a while in order to simulate the aerodynamics of planes or the interaction between the turbomachinery and the uid ow inside jet engines for example. Lately its use has spread into internal combustion engines as well becoming a quite popular tool to assess the ow eld through the complex geometries that these engines present.

CFD has some advantages over experimental measurements. Firstable, time and cost reduction of new setups is an issue since physical experiments can sometimes be really expensive and laborious to carry out. Moreover, CFD allows us to study complex or large systems, for instance centrifugal compressors, where measurements are sometimes hard to reach because of the space constraints.

Another benet is the level of detail of the results and the ability to simulate almost all real conditions where experiments sometimes nd it dicult, for example hypersonic conditions. Whereas experimental measurements points are placed at limited locations in our study eld, CFD obtains data from the entire ow eld of our setup and permits to idealize conditions having a good control over the physics of the problem. Having expressed some advantages, it has to be taken into account that CFD cannot replace measurements anyway.

To validate our numerical model it will always be needed some experimental data to compare with so both techniques complement each other. A CFD study approach has been carried out in this thesis.

3.2.2 The necessity for robust tools

Within numerical simulations there are several ways to deal with turbulence.

Usually, CFD is a trado between computational cost and solution accuracy. Di- rect Numerical Simulations (DNS) resolve the entire range of turbulent scales.

It is the most accurate approach to numerical simulations but it requires so much computational power that, even nowadays, few simple geometry cases can be calculated using this technique and a lot of computational eort is required.

Large Eddy Simulation (LES) is a more aordable turbulence approach even

though it still requires powerful computers. With LES a space lter is applied to the Navier-Stokes equations to keep the larger scales. So the larger eddies are resolved and the smaller eddies (those smaller than the size of the grid) are modeled according to a sub-grid scales (SGS) model. The simplest turbu- lence simulation is the Reynolds Averaged Navier-Stokes equations. With this approach the entire turbulent scales range is modeled. It basically assumes an isotropic and universal behaviour of the turbulent scales. This is the method mainly used in the industry and will continue to be in the future because it is a fast techinque that gives reasonable good results for engineering purposes. As it is the faster technique, it has been chosen to deal with the turbulence because of the fact that several points on dierent speedlines will be calculated as it is going to be shown later.

If we decompose the velocity in a time-averaged part and a uctuating part as in (3.2)

u = ¯u + u⁰ (3.2)

and insert it in the Navier-Stokes equations we can get to the Reynolds Aver- aged Navier-Stokes equations (based on Reynolds 1895). It is enough to say that on the right-hand side of the equations, due to their non-linearity, a new term appears −ρu⁰iu⁰_jthat is called the Reynolds stress tensor. It correlates uc- tuating velocities and is a new stress term driven by turbulence. As this term is unknown we must model it in order to close the mathematical equation system.

The Boussinesq assumption (3.3) claims that the stresses are proportional to the rate of deformation and gives a reasonable approximation

−ρu⁰_iu⁰_j= µ_t(∂ui

∂x_j +∂uj

∂x_i) −2

3ρkδ_ij (3.3)

where µtis the dynamic turbulent or eddy viscosity and k = ¹₂(u⁰²+v⁰²+w⁰²) is the turbulent kinetic energy per unit of mass.

One has to take into account the fact that this decompostion works only if our problem is incompressible. When the problem is compressible Favre averaging (3.4) approach needs to used instead, the instantaneous velocity can be writen as

u =u + ub ⁰⁰ (3.4)

wherebu = ^ρu_ρ is the Favre averaged velocity and u⁰⁰represents the turbulent velocity uctuations including the eects of density uctuations.

The most popular turbulence models are the two-equation models, being the k − and the k − ω the most representative ones. The k − ω model was rst introduced and described by Wilcox. He stated the advantages of his model over the k −  model demonstrating that the performance for boundary layers under adverse pressure gradients was improved and that it can be applied to the entire boundary layer without any changes. However, one main disadvantage of this model is that the boundary layer is sensitive to the ω parameter in the free stream. This leads to a highly sensitivity to inlet boundary conditions for

internal ows, something that does not happen in the k −  model. Menter addressed this problem by realizing that if a damped cross-diusion derivative term is added to the ω transport equation the k −ω model behaved pretty much in the same way as the k −  model. He basically proposed a blending function that would include the suggested term far from walls but not near the wall region which is the same as using thek −  model far from wall and the k − ω model near the wall. As a consequence, the main problem of the original k − ω model from Wilcox was xed. In addition, the denition of the turbulent viscosity is modied to account for the transport of the turbulent shear stress and the constants in the equations are dierent. This is called the SST (Shear-Stress Transport) model. It has been demonstrated to perform much better for ows under adverse pressure gradient and to predict separation in a more reasonable way than any other two-equation turbulence models. The k − ω SST model by Menter is going te be briey described described since it is the model used in this thesis. The Reynolds stress tensor is modelled through the Bousinessq eddy viscosity assumption. The two additional transport equations are one for the turbulent kinetic energy k (3.5)and one for the specic dissipation rate ω = _k^ (3.6), where  is the turbulent dissipation

∂

∂t(ρk) + ∂

∂xj

(ρu_jk) = P − β^∗ρωk + ∂

∂xj

[(µ + σ_kµ_t)∂k

∂xj

] (3.5)

∂

∂t(ρω)+ ∂

∂xj

(ρujω) = γ νt

P −βρω²+ ∂

∂xj

[(µ+σωµt)∂ω

∂xj

]+2(1−F1)ρσω2

ω

∂k

∂xj

∂ω

∂xj

(3.6) and the turbulent viscosity is calculated from the following expression

µt= ρCµ

k²

 (3.7)

where Cµ is a constant.

3.2.3 The wall region

The region near the wall needs to be specically treated because lots of things happen in short distances. This issue becomes even more important when we deal with complex geometries, such as the inside of a centrifugal compressor.

According to gure 5, that there are three main regions near the wall boundary.

The region adjacent to the wall is called the viscous sublayer (y⁺ < 5) where the viscous forces become more important. The following region as we separate from the wall is called the buer layer, which connects the viscous sublayer with the logarithmic region. The next region is called the logarithmic region and goes from y⁺∼ 30up to the mean ow y⁺∼ 200.

The dimensionless value of y⁺can be calculated from y⁺=^yu_ν^τ, where y can be computed from the distance between the wall and the center of rst cell next to wall, ν is the kinematic viscosity and uτ is the friction velocity uτ =q_τ

w

ρ , where the wall shear stress is calculated from the formula

τw= µ∂u

∂y |y=0 (3.8)

The velocity is zero at the wall and increases in the y direction. The dimen- sionless value of u⁺can be calculated from u⁺= _u^u

τ.

In computational uid dynamics there are two options regarding the wall region, one is to resolve the whole boundary layer. To do this, the height of the cell center next to the wall should be so y⁺ < 1. One has to take into account that resolving the wall region requires an extra computational eort and sometimes it is just better no to do so. The second option is to use wall functions. This way is sometimes preferred, time is saved because instead of resolving the wall it is assumed that that the ow behaves like a fully developed turbulent boundary layer. The height of the cell center next to the wall should be set so it lies on the logaritmic region, this is y⁺> 30.

The outline of the boundary layer for a turbulent ow near the wall region is shown in gure 5. The velocity prole follows a linear behaviour in the viscous sublayer u⁺ = y⁺. In the logarithmic region, however, the velocity prole follows a logarithmic law

u⁺= 1

κln y⁺+ C⁺ (3.9)

Figure 5: The log-law near the wall. Source: www.arc.vt.edu

The wall region in the commercial software Star-CCM+ is handled with the All y+Wall Treatment which is basically a mixed approach between using wall functions and resolving the wall. The variable y+is computed and depending on its value, the solver resolves the boundary layer or it is modeled. When it is small -typically less than 1- the solver resolves the wall and when it falls in the logarithmic region -typically more than 30- wall functions are used. The grid near the wall was intended to be in such way that wall functions were activated in order to save computational cost.

3.3 Limitations With Turbulence Modeling

As it has been said previously RANS will be used to model the turbulence with a steady-state approach. So it is a good idea to rst describe the limitations that this model introduces. Steady-state simulations mean that the time is not taken into accout; this is, the case is simulated until it reaches a stationary solution. The time-dependant terms in the equations are forced to converge to zero. So it can be inferred that one of the main drawbacks of this procedure is that transiet eects are not captured. For instance, surge will be impossible to predict since it is characterized by a low frequency time dependant unsteady

ow. Likwise, the possible precursor of surge will not be captured either given their natural unsteadiness. As stated earlier, DNS and LES have the capabil- ity to resolve larger eddies but not RANS since the turbulence is assumed to behave isotropically and all scales are modeled the same way. Hence, wakes or strong separation are not expected to be captured correctly with this technique.

Moreover, one has to think that RANS are based on physicals models. The solution will be inuenced by the accuracy of those models meaning that we will inevitably incur in some modeling errors. The solution will only be able to be as good as the physical model. Despite these limitations, RANS approach has proven to behave pretty good for near optimal eciency conditions and will still be very used in the industry for its quick results. Given the number of cases that are going to be run in this thesis, RANS use is justied.

4 Numerical Methodology

4.1 Governing Flow Equations

For a uid ow the governing equations are called the Navier-Stokes (NS) equa- tions: conservation of mass (4.1), momentum (4.2) and energy (4.3)

∂ρ

∂t + ∂

∂x_j(ρuj) = 0 (4.1)

∂

∂t(ρui) + ∂

∂xj

(ρuiuj) = −∂p

∂xi

+∂σij

∂xj (4.2)

∂

∂t(ρE) + ∂

∂xj

(ρujE) = − ∂

∂xj

(puj) + ∂

∂xj

(σijui) − ∂qj

∂xj (4.3)

p = ρRT (4.4)

along with the equation of state (4.4), whereρ stands for density, p is the pressure, R the gas constant, T the temperature,t is the time, x the coordinate system, subscripts i, j, k are the component indexes,σij is the viscous stress tensor, E = e + ¹₂u_iu_i is the total energy, e the internal energy that can be written as e = cvT and qj the heat ux which is modeled by Fourier's law (4.5)

qj= −κ∂T

∂x_j (4.5)

where κ = κ(T ) is the heat conductivity.

The viscous stress tensor models the part of the stress at one point that is accounted for by the strain rate according to equation (4.6)

σij = µ(∂ui

∂x_j +∂uj

∂x_i −2 3δij

∂uk

∂x_k) (4.6)

where µ is the dynamic viscosity and δij is the Kronecker delta and has a value of 0 whenever i 6= j and a value of 1 whenever i = j.

4.2 Numerics

The Navier-Stokes equations are non-linear so except some few simple cases which can be resolved analytically, the proper way to treat them is numerically.

There are dierent discretization methods to solve problems numerically; these are, the nite dierence, the nite element and the nite volume method. In this thesis the commercial CFD software Star-CCM+ has been used which is based on the nite volume method. In the nite volume method the computational domain is divided into a large number of small control volumes forming the grid. The continuum transport equations are discretized and applied to every control volume composing the grid. Hence, a set of linear algebraic equations

are achieved and this system of equations are solved with an algebraic multigrid solver.

By default, Star-CCM+ uses a second-order upwind numerical scheme to solve the convection term in RANS equations. The convective term at a face of a cell is computed from (4.7)

[φρ(v · a − G)]_f =m^·_fφ_f (4.7) where φf is the scalar value andm^·f is the mass ow rate at the face and G is the grid ux which is calculated from Gf = vg· af, being vg the grid velocity and af the face area. The way we compute the value of φf at the face of a cell is very important for the stability and accuracy of the numerical scheme. For the second-order upwind numerical scheme, the convective ux is calculated in the following way:

m·fφf = ( _·

mfφf,0

m·_fφ_f,1

f orm^·f ≥ 0

f orm^·_f < 0 (4.8) where φf,0 and φf,1 are interpolated from the values of the cells on either side of the the current cell as follows:

φf,0= φ0+ s0(∇φ)r,0

φf,1= φ1+ s1(∇φ)r,1 (4.9) where (∇φ)r,0and (∇φ)r,1are the limited reconstruction gradients in cells 0 and 1 which are computed from the Hybrid Gauss-LSQ gradient method which uses the hybrid Gauss/weighted LSQ method for all variables. The values of s₀and s1 are calculated from

s₀= x_f− x₀

s₁= x_f− x₁ (4.10)

The advantage of this scheme over the rst-order is that the accuracy is one order of magnitude better. However, in some situations the reduced numerical dissipation can bring a poorer convergence than the rst-order scheme but in general, a second-order scheme is preferred.

4.3 Motion

4.3.1 Moving Reference Frames vs. Sliding Mesh

In turbomachinery the rotating elements need to be modeled somehow. For example, in centrifugal compressor the impeller rotates at certain speed whereas the casing and volute do not move at all. In CFD there are dierent ways of simulating the rotational movement and the two most important techniques are the sliding mesh and the moving reference frames.

In the moving reference frames approach a new rotating coordinate system is applied to an entire region simulating motion but the mesh is actually not

moving. Instead, the Coriolis and centrifugal forces are added to the momentum equations (4.11) so even though the position of the cell vertices do not change the rotation is modeled. The moving reference frame technique is normally used in steady-state simulations. In a centrifugal compressor geometry the moving reference frame is usually applied to the impeller region whereas the rest of the compressor remains static. Some parts such as the shroud, however, are not rotating so the source terms are actually activated only in the regions where rotation exists. An important drawback of this method is that the ow eld that the stationary elements see depends on the relative position of these elements.

It is actually a very limited technique because it is very unrealistic that the impeller remains stationary. However, the computational cost is very aordable and it is the only way to succeed in running and calculating several points on the compressor map.

∂

∂t(ρurel) + ∇(ρurelurel) + ρ(2w × urel+ w × w × rrel) = −∇p + ∇σ (4.11) The sliding mesh, on the other hand, allows the adjacent cells to slide relative to one another. The sliding interface is updated every time step and the cells do not have a correspondant on the other side of the interface but the connectivity changes every time. In spite of being far more realistic than the moving reference frames technique it is much more expensive and is generally used when running transient simulations.

In this thesis the Moving Reference Frames method has been used to handle the rotation of the wheel.

4.3.2 Interfaces

Interfaces can be divided into direct and indirect interfaces. Direct interfaces di- rectly join the two boundaries that compose the interface by creating an explicit connection between cells. The two boundaries are merged during the meshing process to guarantee a conformal mesh across the interface. An example would be the in-place interface that has been used for some cases in this thesis. In this interface, there is no physical separation between the boundaries that conforms the interface and mass, momentum and energy are transferred directly from cell to cell.

Indirect interfaces, however, make an association between the faces of the boundaries. An example of this is the mixing plane interface, which tries to mitigate the disadvantage of the inuence of the relative position that the mov- ing reference frame brings. This interface averages circumferentially the ow conditions on both sides making the ow circumferentially uniform and thus giving rise to a single radial prole. The eect of this approach is similar to the idea of increasing the number of blades which would lead to a much more uniform ow. If we take a look at a fast rotating impeller outlet we would see a circumferentially homogenous ow and this is what the mixing plane is basi- cally trying to imitate. However, we have to be careful when using the mixing

plane interface because, for instance, wake eects cannot be predicted given the circumferential averaging that is done.

For the simulations run along this project, a mixing plane approach has been selected to treat the interfaces between moving and stationary regions.

4.4 Boundary Conditions

In CFD, boundary conditions are of vital importance to have a good denition of our case. Having a good control on our boundary conditions will make possible to obtain a good solution for our problem. Star-CCM+ provides the possibility to set dierent boundary conditions for the inlet and the outlet of the set-up.

Free stream, mass ow inlet, overset mesh, pressure outlet, stagnation inlet, symmetry plane, velocity inlet and wall are available.

4.4.1 Inlet boundary condition

Typically for the inlet, a velocity inlet, stagnation inlet, mass ow inlet or free stream boundary conditions can be applied. The free stream is a non- reective boundary condition frequently used when studying the acoustics. For the stagnation inlet boundary condition a total pressure needs to be specied.

A mass ow inlet has been chosen in this project since the mass ow is the known variable -from the turbocharger manufacturer data- we are imposing to calculate every case. Additionally, with this boundary condition, a supersonic static pressure can be dened in case the inow is supersonic -not our case-.

The total temperature, turbulence intensity and turbulent viscosity ratio can also be modied but they were remained as default.

4.4.2 Outlet boundary condition

For the outlet boundary condition, a pressure outlet is often specied. In this project, the outlet static pressure has been imposed. The pressure ratio -both total-to-total and total-to-static- of the compressor is known from the data recieved from the manufacturer. To get to know the outlet static pressure the inlet total pressure has to be calculated. Knowing the inlet velocity through the mass ow rate the inlet total pressure can be computed.

v1= m

ρ_∞A (4.12)

wherem^ is the mass ow rate, ρ∞is the ambient density and A is the area of the inlet pipe.

P01= P_∞+1

2ρ_∞v²₁ (4.13)

where P∞is the atomspheric pressure.

P2= P01πt−s (4.14)

where πt−sis the total to static pressure ratio provided by the manufacturer.

4.4.3 The wall

Together with the inlet and outlet boundary conditions the wall closes our com- putational domain. The whole compressor casing including the inlet pipe and the volute have been set as wall boundary conditions. The walls have been treated adiabatically since we were not interested in the heat transfer phe- nomenon. A non-slip wall condition has been specied, this is, the velocity of the uid is zero on the walls.

4.5 Solving Strategies

Star-CCM+ provides two dierent solving strategies. The Segregated Flow model is based on the SIMPLE algorithm and a Rhie-and-Chow type pressure- velocity coupling. It solves the equations sequentially and it uses a predictor- corrector approach to link both the momentum and continuity equations. It is normally used in constant-density ows, for instance in low-velocitiy ows which can be treated as incompressibles. It is denitely not appropriate to handle high Mach number scenarios and shock waves.

The Coupled Flow model is a fully compressible density based solver. It solves the equations of mass, momentum and energy simultaneously. One of the advantages of this approach over the Segregated Flow model is its ability for solivng compressible ows and its robustness for calcuating ows where source terms dominate, such as rotation. However, the convergence is usually slower and harder tho achieve. For steady state simulations the Coupled solver replaces the time-derivative for a pseudo-transient term and the solution advances in pseudo-time to take this term to zero making the convergence achievement the best way possible.

On the lowest speedlines the Segregated Flow solver was used in some cases while a Coupled Flow technique was used for the highest speedlines where highly compressible ow is expected.

Figure 6: SIMPLE algorithm. Source: An introduction to CFD [28]