# Flow Phenomena Within a Compressor Cascade

**Published:**
**Last Edited:**

**Disclaimer:** This essay has been submitted by a student. This is not an example of the work written by our professional essay writers. You can view samples of our professional work here.

Any opinions, findings, conclusions or recommendations expressed in this material are those of the authors and do not necessarily reflect the views of UK Essays.

Paolo __Mastellone__

**\section{Aim of the investigation}**

The scope of the assignment is to study and assess the flow phenomena within a compressor cascade employing controlled diffusion blades through a computational fluid dynamic simulation. The results of the simulation are subsequently compared to the experimental data obtained from the simulated cascade. The quality and the discrepancies are discussed in order to demonstrate the understanding of the theory and the application computational tools.

**\section{Experimental data}**

The simulation is based on the experimental work done by Hobson et al.\cite{rif1} that studied the effect of the Reynolds number on the performances of a second generation controlled-diffusion stator-blades in cascade. The three Reynolds numbers evaluated were 6.__4E5__, 3.__8E5__ and 2.__1E5__. This work was carried out in order to analyse a more representative Reynolds number of flight conditions and to create a test case for computational fluid dynamic models of turbulence and transition.

The experimental cascade is made of 10 __67B__ stator blades with an aspect ratio of 1.996 and the solidity of 0.835. The __tecnique__ used for the experimental measurement is the laser Doler __velocimetry__ (__LDV__) with a seed material of 1$\mu $m oil mist particles.

The experimental data and e cascade geometric parameters are shown in the figures below.

The Reynolds number used for the simulation is 6.__4E5__, which gives an inlet velocity of:

$$

where is the kinematic viscosity and $L$ is the blade chord.

**\section{Mesh}**

The software used for the mesh generation is ANSYS ICEM. The mesh has a critical importance and consequences on simulation and results, a well-constructed mesh eliminates problem of instabilities, absence of convergence and increase the opportunity to achieve the right solution \cite{rif4}. There are key aspects to take into account, the mesh must capture the geometric details and the physics of the problem.\\

The discretization is made for one representative flow passage introducing periodic boundary conditions. The fluid domain thickness is half of the blade spacing in order to use properly the periodic boundary conditions: the fluid quantities at the top and the bottom of the domain will be the same, in order to represents the periodicity of the cascade. The inlet and the outlet distances from the blade are respectively 2.5 and 3 times the blade chord so that their position doesn't have an influence on the results and the flow is fully developed at this stations. In order to get low numerical diffusion the mesh must be aligned with the flow direction\cite{rif2}, consequently to have the same geomety of the simulation the blade is staggered of $\ang{16.3}$ and the inlet grid inclination is $\ang{38}$ while the outlet one is $\ang{5.5}$. The mesh is a structured type made of quadrilateral elements, because they can be fitted to flow direction and are quite tolerant of skew and stretching\cite{rif2}. To adapt the mesh at the profile

an O-grid type made of 9 blocks is used.

**\subsection{First node position}**

One major parameters for the mesh sizing is the non dimensional distance $y^+=\frac{u^+y}{\nu}$. This parameter must be chosen as a function of the type of boundary layer treatment. The use of a "wall function" consents to bridge the explicit resolution of the near wall region, which is described by the dimensionless parameters $u^+$ and $y^+$. The turbulent boundary layer is subdivided into the "viscous sub-layer" for $y^+<5$Â and the "log-law layer" for $20 \leq y^+ \leq 500$. To employ the "wall function" the first node must be placed outside the first layer, typically between 20 and 30 \cite{rif4}. Two turbulent model have been used for comparison purposes: the K-$\omega$ SST and the k-$\varepsilon$ __RNG__. For the k-$\omega$ SST a near wall treatment has been chosen and hence a $y^+=1$, which resulted in first node distance of 0.004 mm.

With the K-$\epsilon$ __RNG__ model a standard wall function has been adopted and choosing $y^+=25$ the first node distance is 0.1 mm.

**\subsection{Grid independence study}**

The number of nodes required for a 2D simulation with resolved boundary layers is around 20000 while is around 10000 nodes if a wall function is used \cite{rif2}. The grid adopted for the K-$\omega$ SST has 20128 nodes. The mesh for the K-$\varepsilon$ __RNG__ model, which uses a wall function, has 14488 nodes. The two meshes have been chosen between three types with increasing resolution: a coarse, an intermediate and a finer one. The __Cd__ and Cl values obtained from the three meshes are displayed in the table below for the two different turbulent models used for the simulation: k-$\omega$ SST and k-$\varepsilon$ __RNG__.

A grid independence study and mesh quality analysis have been effectuated for both the meshes of the two different models, and satisfactory results were achieved. In the assignment just the mesh analysis of the K-$\omega$ SST model with $y^+=1$ has been reported.\\

The difference between the values of Cl and __Cd__ of the intermediate and the fine mesh are negligible, hence the results don't rely upon the mesh resolution __anymore__ and a further increase of the nodes is ineffective. Consequently the intermediate mesh has been adopted in both cases since the results are mesh-independent.

The quality of the mesh can be analysed through specific tools available in the software. The overall quality level is acceptable, above 0.85 over 1, even if there are some parts that can be improved. Indeed the skewness at the top due to the curved flow profile and near the trailing edges should be reduced. The region not interested by the wake and the upper and lower parts have been left intentionally coarse since there is not presence of steep gradient in these regions (see figure 10).

The quite high aspect ratio in the zones in front and behind the blade can be tolerated because it hasn't a great influence since the mesh is parallel to the flow.

The outcomes are displayed below.

**\section{Simulation}**

The software used for the simulation is __ANSYS__ FLUENT with double precision and four processors enabled for the calculations. The problem has to be properly set up through subsequent steps.

**\subsection{Solution **__setup__**}**

In this section the inputs for the simulation must be implemented. The mesh has to be scaled to the proper geometric dimensions (mm) and afterwards has to be checked to find eventual errors. The solver is a pressure-based type and the simulation is 2D planar. The turbulent model used and compared are the K-$\varepsilon$ RNG with a standard wall function and the K-$\omega$ Shear Stress Transport both with default model constants. The methods use two separate transport equations for the turbulent velocity and length scale which are independently determined \cite{rif5}. The first model is characterised by robustness,economy and reasonable accuracy. The __RNG__ formulation contains some refinements

which make the model more accurate and reliable for a wider class of flows than the standard K-$\varepsilon$ model \cite{rif5}.

It is semi-empirical and based on the transport equations for the turbulence kinetic energy ($K$) and its dissipation rate ($\varepsilon$) \cite{rif5}. The limit of this model is the assumption of complete turbulent flow, which is not the case in consideration.\\

The second model is also empirical but is based on the specific dissipation rate ($\omega$). The K-$\omega$ SST is an improvement of the standard K-$\omega$ and it is more reliable and accurate for adverse pressure gradient flows because it includes the transport effects for the eddy viscosity \cite{rif5}. This model should capture more accurately the flow behaviour because of the adverse pressure gradient on the suction side of the blade.

The fluid used is air, the specific heat and the thermal conductivity are kept constant as well as the density and the viscosity. Indeed the Reynolds and hence the velocity field are low and the problem can be considered incompressible, as a consequence the energy equation is not necessary.\\

The boundary conditions for the blade profile, the outlet and the lateral edges have been set to wall, pressure outlet and periodic respectively.\\

For the inlet boundary condition the "velocity-inlet" has been selected, through the "magnitude and direction method", the main velocity from the Reynold number is 73.56 m/s and the components are $x=cos(38\degree)=0.78801$ and $y=sin(38\degree)=0.61566$.

For the turbulence definition the "intensity and length scale" method is used since there are no informations about the value of $K$, $\omega$ and $\varepsilon$ but just about the inlet turbulence.

The value of the turbulence intensity is determined by the formula:

$$

The turbulent length scale, from the Fluent manual, is:

$$

which is an approximate relationship based on the fact that in fully-developed duct flows, $\ell$ is restricted by the size of the duct since the turbulent eddies cannot be larger than the duct \cite{rif5}.

**\subsection{Calculation parameters}**

In this step the parameters to achieve the solution are decided. The calculation has been split into two parts: in the first one the solution method has a "simple" scheme with a "first order Upwind" spatial __discretization__; the second one has a "coupled" scheme and is "second order Upwind". In the first part a first-order accuracy result is achieved and is used as the input for second part of the calculation.\\

The monitors are enabled to assess the convergence of the calculation. For the residuals the convergence criterion has been set to __1E__-6 for continuity, x-velocity, y-velocity, energy, k and $\omega$. Other two monitors for Cl and __Cd__ have been added to appraise the convergence. For __Cd__ the vector components are x = 0.78801 and y = 0.61566 although for Cl are x = -0.61566 and y = 0.78801. Their their value must be asymptotic when the solution converges. The last parameter used to check the convergence is the net value of mass flow flux inside the domain, which must be zero. To initialize the solution an hybrid method is used, afterwards the calculation can be run.

**\section{Results}**

**\subsection{Convergence}**

The convergence has been reached after 479 iterations for the k-$\omega$ SST and after 410 for the k-$\varepsilon$ __RNG__.

From the reports the mass flow flux can be evaluated, the difference between the inlet and the outlet is in the order of __1E__-7 in both cases. According to this outcomes the convergence has been verified and the validation of the simulation results with the experimental study can be performed.

**\subsection{Post processing}**

The post processing of the results is useful to understand the validity of the simulation.\\

From the velocity contours the acceleration of the fluid on the suction side and the deceleration on the pressure side is captured. The pressure contours show the depression on the suction side and an overpressure on the pressure side. The stagnation point on the leading edge is highlighted by pressure and the velocity contours: the velocity is zero and the pressure reach the stagnation value. The separation of the fluid can be seen from the reverse velocity region on the rear part of the __airfoil__. The two methods made different predictions for the separation phenomenon. Indeed the velocity and the turbulence contours as well as the velocity __pathlines__ show a less intense separation region and a smaller recirculation zone for the k-$\varepsilon$ __RNG__ model.

**\subsubsection{K-$\omega$ SST}**

**\subsubsection{**__Cp__** distribution}**

The __Cp__ distribution is compared to the experimental one. The values from the paper have been extrapolated and inserted in a Matlab graph to give a better comparison. The __Cp__ coefficient is defined by:

$$ Cp = \frac{p-p_{\infty}}{1/2\rho_{\infty} V_{\infty}^2}$$

where the value of $\rho_{\infty}$ and $p_{\infty}$ are extracted from the Fluent reports in terms of mass-weighted average:

The abscissa values from Fluent data has been normalised with the chord length in order to obtain the same type of graph. In the experiment for the low and the intermediate Reynold numbers there was a separation bubble between approximately 50 and 65\% of the chord for Re=3.8E5 and between 45 and 70\% for Re=2.1E5, while it was absent for the highest Reynolds number. The absence of the separation bubble is captures from both the models since the Cp coefficient rises continuously after the point of minimum pressure. The separation at about 80\% of the chord is highlighted by flat trend of the Cp \cite{rif6} by both models .

On the pressure side the trends are very similar to the experiment. On the suction side a difference is observed after the 40\% of the chord. Both the simulation results are shifted, a possible explanation

could be the presence of __3D__ effects and secondary flows which are not captured by the __2D__ simulations.

In the subsequent sections only one passage has been taken into account for the comparison with the results of Hobson et al.\cite{rif1}. The stations 7,8,9 and 13 have been used for the observations (see figure 4). Station 7,8 and 9 have been taken perpendicular to the profile as showed in the paper.

**\subsubsection{Wake profile}**

The wake profile presents the velocity distribution behind the blade leading edge, the measurement has been made at station 13 that is 20\% of the chord downstream the leading edge.

The data from the simulation were exported from Fluent and plotted on Matlab, the abscissa is normalised with the blade spacing S. Both the models highlight a profile similar to the experiment even if the wake wideness is underestimated. Anyway the obtained trends appear to be quite accurate.

**\subsubsection{Turbulence intensity}**

The turbulence intensity profiles exhibit a trend similar to the paper. The figures has been divided by $\sqrt{2}$ because of the different definition of turbulence intensity and the values on the abscissa have been normalised with the blade space S. The simulations captured the double-peaked distribution due to the boundary layer separation. The peaks are in correspondence of the maximum velocity gradient in the wake profile (see figure 27), likewise the experimental data. The outcomes ofÂ K-$\omega$ SST are more similar to the paper trend. The underestimation of the wake amplitude is consistent with the previous graph.

**\subsubsection{Outlet flow angle}**

The velocity flow angle distribution has considerable differences compared to the paper data. A likely explanation could be the limitation of the simulation that can capture only the __2D__ flow characteristics, while the significant flow angle is primarily caused by the secondary flows in the cascade which are typical __3D__ effects. This is supported by the fact that the trends predicted by the two models are very similar hence both

miss some flow characteristic that cannot be predicted by the __2D__ simulation.

The mass-averaged exit flow angle in the experiment was $\ang{9.25}$, the results from the fluent reports are showed below.

**\subsubsection{Velocity profiles}**

The velocity profiles, normalised with the inlet velocity and the blade chord, at station 7,8 and 9 have are presented.\\

At station 7 the curves are almost identical, the velocity evolves from zero in contact with the wall and then increases over the reference speed of 73.56 m/s.

At station 8 and 9 both the experimental and the K-$\omega$ SST present a reverse flow close to the wall, evidence of the separation. At station 8 and 9 the experimental reverse flow reaches 0.06 (7.6mm) and 0.1 (12.7 mm) of the blade chord that is in agreement with the results of the K-$\omega$ SST model. The K-$\varepsilon$ RNG fails to capture the reverse flow (only a negligible portion on at station 9). This is in accordance with the theory: the K-$\omega$ SST model has better performance in-handling non equilibrium boundary layer regions, like those close to separation \cite{rif4}.

**\subsubsection{Loss coefficient}**

According to \cite{rif3} the loss coefficient is defined by:

$$

The table below presents the values calculated for the two different models. The figures have been taken from the Fluent reports in term of mass-weight average. The loss coefficient found in the experiments is 0.029.

k-$\omega$ SSTÂ k-$\varepsilon$ __RNG__

Total pressure inlet $\bar{p}_{01}$ [Pa]& 2290 & 2209

Total pressure outlet $\bar{p}_{02}$ [Pa]& 2176 & 2103

Static pressure inlet $p_1$ [Pa]& -1048 & -1107

Loss coefficient $\omega$ & 0.034 & 0.031

The two coefficients are of the same order of magnitude to the one determined experimentally. The slightly difference could be explained by the different reference sections used for the mass-weight average in the experiment (upper and lower transverse slot for the experiment, see figure 1) since the inlet and the outlet have a different position. Moreover the lightly larger value obtained from the K-$\omega$ SST compared to the K-$\varepsilon$ __RNG__ is consistent with the greater separation, hence more dissipation of energy, predicted by the model.

**\section{Conclusions}**

In this assignment a __CFD__ simulation using __Icem__ and __Fuent__ software has been carried out and the results have been analysed with engineering judgement, in order to demonstrate the understanding of the theory and the tools.\\

The achievement of satisfying results is strictly related to successful implementation of every single steps of the simulation. The knowledge of the aerodynamics and the physics of the problem is paramount to set the mesh, the boundary conditions and the calculation.\\

Great attention has been taken on the mesh generation and it resulted to be the most challenging part since a lot of experience is needed to have good results. The key aspects taken into account are the they grid domain extension, the grid type, the alignment with the flow, aspect ratio and skewness. The choice of the wall treatment influences the first node position. To make a comparison between two turbulence models, for the K-$\omega$ SST has been used $y^+=1$ while for the K-$\varepsilon$ __RNG__ that uses a standard wall function $y^+=25$. When the mesh has an adequate quality is ready for the simulation.

The choice of the turbulence model and the boundary conditions depend on the problem studied and should represent the physic of the problem as precise as possible. Once the simulation has been run the control of the convergence is the necessary but not the sufficient condition to obtain exact outcomes. Indeed the calculation can converge to wrong results if the problem is not well posed. Some modifications have been made to the mesh in order to attain more precision and the calculation has been repeated several times, lots of experience is requested to reduce the number of attempts.\\

A qualitative and quantitative comparison with experimental results showed both accuracy and limitations of the simulation. Certainly the mesh can be improved, for example using more then nine blocks, to promote the skewness and the aspect ratio, particularly near the leading and the trailing edge. From the comparison between the K-$\omega$ SST and the K-$\varepsilon$ __RNG__ the limitations of the latter in the unstable boundary layer treatment have been highlighted.\\

The discrepancies observed can be addressed to the __3D__ effect not captured by the simulation and the limitations of the models adopted. The adoption on more sophisticated models such as the Transition SST (4 equations) and the Reynolds stress (5 equations) can improve the accuracy.

### Cite This Essay

To export a reference to this article please select a referencing stye below: