evaluation of the simulated flow
The flow through the grille, intercooler, radiator and the combination of a cowl and fan and finally the engine compartment is important with respect to cooling system performance of a truck. All the before mentioned components influence the air flow profile through the radiator and a sound understanding of the basic flow phenomena, pressure losses and opportunities for modifications is needed in order to be able to optimise the flow quality.
Today computational fluid dynamics (CFD) can be used as a major design tool for this purpose. However, detailed experimental measurements are still needed as a validation of the used numerical and physical models, grids and assumed boundary conditions. In this paper the major results of the comparison between numerical simulations and experimental data are presented. The cooling system of this project has been stepwise extended from a simple grille-radiator combination to the complete engine compartment, including the effects of a rotating fan. Fan modelling will be discussed in detail because it determines the quality of the simulation results.
Various measurement techniques were used: Laser-Doppler Anemometer (LDA) measurements behind the grille and in the cowl; microprobes in the main radiator; a 5-hole pressure probe behind the fan and finally simple pressure manometers. The data obtained from the experiments on special test-rigs will be compared with the numerical simulations of the following Front-End configurations:
It will be shown that the results of the numerical simulations are reliable. The employed rotating fan model even correctly predicts off-design conditions. Therefore complex 3D numerical simulations of the complete cooling system are feasible even under extreme conditions.
Both experimental measurement methods and numerical models are not error-free, especially when used in exceptional conditions. Discrepancies between numerical results and experimental data will be discussed and the sources of error will be indicated.
Finally, the results gained in this project will be used as input for cooling system layout computer programs.
Current European heavy trucks show an increase in engine power with an accompanying increase in heat rejection. These high-powered engines are more and more encapsulated in order to meet stricter by-pass noise levels. Due to the encapsulation the cooling airflow through the engine compartment is disturbed. Therefore an advanced in-depth study was initiated of the cooling system performance of a heavy truck. The goal was to develop tools, which enable the optimisation of the flow through the cooling system early in the design. One of the tools is a combination of computational fluid dynamics (CFD) and dedicated heat transfer simulation software as is described in the accompanying paper "Prediction of cooling airflow and cooling system performance" . Because CFD plays an important role in this tool-set it was necessary to perform an extensive validation program.
The airflow through the engine compartment goes through the following components: grille, intercooler and radiator, a cowl and fan, around the engine and leaves the compartment through various openings. Every component has an influence on the flow through the main radiator; some of them direct others through an alteration of the fan characteristics. As the flow and the interactions are complex and the use of CFD is relatively new, every relation has to be studied, measured and simulated separately. The experimental programme of the Front-End was carried out on a suitably modified radiator test facility (see Fig. 1), which was capable of dealing with large truck radiators. Basic studies of the fan were done on a special test rig at the University of Hannover.
Figure 1: The modified radiator test facility showing the grille, cowl/fan, dummy engine and the first part of the tunnel (intercooler and radiator are not drawn).
The basic series of Front-End tests were carried out on a radiator test facility, which was able to deal with the large pressure drops of a truck cooling system. The instrumentation and additions to the test rig are shown in Fig. 2. On this facility the following flow rate measurements were carried out:
Figure 2: Experimental set-up of the radiator test facility.
The measurements with a bell mouth were necessary in order to isolate the characteristics of the intercooler and radiator from possible non-uniform upstream flow. Microprobes were installed in the radiator and calibrated in measurement 3. From measurements 1 to 5 the following two pressure loss relationships were found:
in which a and b are the coefficients which describe the pressure loss Dp (over the thickness of the matrix Dx) as a function of the mean velocity V through the system:
This radiator formula is used in all the simulations to model the effect of the radiator and intercooler. As it is relatively useless to make a numerical model of any of the first six measurements, the first CFD study was done for measurement 7. Models were made of:
Followed by additional models of:
5. An axisymmetric fan model and a cowl (resembling model 3).
This concludes the Front-End series. Later on Model 7 formed the basis of the encapsulation studies:
8. A model of the engine compartment replaces the test
facility after the fan.
Figure 3: An impression of one of the largest models.
It was clear from the beginning that models, or parts thereof, should be reused as often as possible. Especially the model of the grille was made at the very beginning of the project and it was not changed at any moment. This concept has also the advantage that relative changes or trends can not be attributed to different geometrical representations of the domain in front of the cooling system, the grille and both the intercooler and radiator. The sizes of the models were:
Table 1: Sizes of the used meshes.
Because one of the objectives was to study the influence of the grille the models could not start at or near the grille. Therefore the room of the radiator test facility was modelled as well. Air enters the domain at the sides of the cooling system mock-up and has to move to the front and then enters the cooling system through the grille and other openings in the front. This has been kept unchanged throughout the complete project.
All simulations were performed using the RNG variant of the k-e turbulence model. Wherever possible a second order differencing scheme was used; in the beginning the linear upwind scheme, later the gamma scheme was used which is essentially a variant of the central difference scheme. For a complete discussion on the effects of differencing schemes on the accuracy of the solution the reader is referred to .
The project originally included the development and validation of a comparatively crude fan model, which should have enabled the reproduction and prediction of the flow through the fan and engine compartment. Experimental data was available for the validation of the model.
A very popular way to incorporate ventilators in a CFD model is using so called body forces. The option of including body force terms is straightforward in the Finite Volume Method. The basic conservation equation for a variable f is of the form (see for example ):
with the four parts describing the rate of change, the convection, the diffusion and finally the source or body force term Sf. For the momentum equations the source term is split showing the pressure force term dp/dxi explicitly. In order to demonstrate the role of the source term, consider the one dimensional incompressible steady flow through a tube with constant cross section and only an axial velocity component; the viscous stresses will be neglected. The momentum equation for the axial velocity component w then reduces to:
Note that because of the continuity equation (mass conservation) the velocity w is in this special case constant and hence the first term vanishes also. If Sw equals zero then the pressure remains constant. If it is positive then the static pressure, and the energy of the flow, rises over the length where Sw is non-zero. This is the basic concept of body forces, which can be easily extended into three dimensions.
Different kinds of fan models can be built depending on the number of source terms and the extent of the active region:
In  a method was developed especially for truck fans, which is based on successive calculation of flow properties and velocity components at four axial locations. Local flow directions and properties just behind the leading edge of the fan are calculated from the geometry of the fan, and an estimation of the radial distribution of the axial velocity at the inlet. The losses, which occur between the leading and trailing edge of the fan blade, are governed by a single loss factor. The trailing edge area and the far field conditions are calculated using thermodynamic relations and also an assumption of the radial distribution of the axial velocity component. Empirical data must be provided for the parameters of both the blade leading and trailing edges. Finally several correction parameters are introduced to account for various efficiencies and distributions, and they are valuable parameters in the reproduction of the experiments.
Once the local velocities are available from the above-mentioned procedure, then it is possible to reproduce the local forces, which must have acted upon the flow. Star-CD augmented with specially developed user subroutines reads these forces at the start of the simulation. A deficiency of this model is that the forces are calculated based on an assumed velocity distribution at the inlet of the fan, and they are imposed disregarding the actual flow conditions at this point, which are usually less favourable. However, modifying the fan model was not considered to be useful.
This fan model has been extensively tested on simple and complex geometries. One of the major problems encountered was that parameter sets of two geometrically very similar fans could differ substantially. In other cases the model was not able to reproduce the measured flow characteristics of a fan at all. It is therefore certainly not a tool to predict the performance of new unknown configurations. After a while the use of a body force fan model was abandoned completely.
The applicability of fan models based on body forces should be restricted to cases were only a crude effect is sufficient and details are unimportant. In the case of a truck the fan is of the same size as the engine compartment and therefore plays a very dominant role and local details can become very important.
|3.2. Rotating frames
Instead of using a model in which the effects of the fan blades are caught empirically, it is also possible to include the fan explicitly. For a numerical model three methods are conceivable:
In all three cases the momentum conservation equations in the rotating areas are augmented by centrifugal and Coriolis terms (as source terms).
The first option only applies to cases that are axisymmetrical. The effect of stationary walls is taken into account by letting them rotate in the opposite direction. After introducing cyclic symmetry planes one can even model just one fan blade. The resulting models are very economical with respect to computer resources.
The second option is the most demanding with respect to computer resources and coding. As soon as some part of a model is rotating or moving, the analysis is by definition transient. Even for a code which employs implicit time integration the mean and maximum Courant numbers are restricted to of the order one and ten respectively. Especially the area near the tip of a large fast rotating fan where very high velocities exist and small cells are needed (e.g. tip clearance and vortices) is dominating the very small times steps which are needed. This restricts the applicability of this method for an engine compartment simulation. This method also poses restrictions on how the rotating mesh is connected to the stationary parts.
The last option is in a way an extension of the first method although now only a part of the model rotates, for example a cylindrical core rotating in a stationary enclosure. The classic example is the flow in a stirring tank with baffles mounted at the exterior walls. When an engine fan is considered, a cylindrical domain around the fan is defined relative to a rotating frame of reference. In order to match the rotating and non-rotating domains correctly with respect to numerical accuracy, cell distribution and domain boundaries need to be planned carefully. In general this method only requires modest extra computer resources.
The last method is thus indeed a very attractive method for an engine fan. However it has the disadvantage that the resulting solution is physically not completely correct. Immediately behind the fan are fast fluctuating flow areas, which are coupled to the passing of the blades and the time it took since the air left the trailing edge. Using a rotating frame of reference the solution is "frozen" for a particular fan position. The flow field behind the fan corresponds to this position but the time history is lost. Further downstream this effect vanishes rapidly. The most attractive feature is that no additional empirical models are needed.
|3.3. Rotating fan tests
The rotating reference frame model was extensively tested. First using a simple rotating axisymmetric model but the main series of tests were performed on a model based the University of Hannover fan test facility. The basic test facility consists of a pipe with screens to regulate the loading of the fan, a diffusor to the intercooler and radiator, cowl and finally the same dummy engine block that was used on the radiator test facility mentioned earlier. Examples of both models are shown in Fig. 4.
Figure 4: Two types of fan test models. Left: Axisymmetric model.
The velocity vectors behind the rotating fan were measured using a Schiltknecht 5-hole pressure probe, which has been calibrated in stationary flow conditions. The probe is said to be aligned to the flow when the pressures of the two holes at the sides are equal. The remaining three pressures are then used to find the direction and the flow speed. Shown in Fig. 5 is a typical validation result at a distance of 130 mm behind the trailing edge of the fan.
Figure 5: Comparison of measured and simulated velocity profiles.
The following remarks can be made on the results in Fig. 5:
The result presented here is a typical result; other comparisons were sometimes of less and sometimes of better quality and, remarkably, the velocity component in error was not always the same.
Note that the flow conditions behind the fan are strongly fluctuating and in principle not suited for this probe. Using potential flow theory it is possible to study the effects of the unsteady flow on the probe measurements. The static pressure p at a tangential position q of a sphere is (see Fig. 6):
Figure 6: Measurement positions of a 5-hole probe.
Assuming that the flow is aligned to the plane of the probe holes 1-2-3 (which means that p4 = p5) the angle q follows from the pressure differences Dp31 = p3 - p1 and Dp24 = p2 - p4:
The fraction k1234 can be calculated analytically but will be calibrated for a real probe. Once the angle q is known the velocity follows from:
Again the factor k24 can be calculated and calibrated. The velocity U is extracted from Eqn. (7) by
The static pressure upstream of the probe is found by
in which k2 is another calibration factor. Combining Eqns. (9) and (8) yields:
If the flow direction fluctuates with a = am sin(wt) around the main axis then after some algebra integrating the pressures as function of amplitude q and am one finds:
Table 2: Measurement errors as a function of amplitude am.
In this case the angle is measured correctly but the measured velocities are erroneous. However, the fluctuations are not regular and easily reach ±40º, which results in an error of 24% in the velocity U (immediately behind the fan near the shaft even ±180º). Another aspect is the long length of the tubes connecting the probe to the manometer, which results in some unknown damping of the signal.
Summarising, the flow velocity measurements contain a considerable inaccuracy. It is at least very reassuring that both the numerical and experimental data show the same qualitative tendencies that are of the same order of magnitude.
Apart from velocity measurements the numerical solutions were also compared with qualitative results of special balanced tufts, which were mounted on the fan blades. Basic flow features like regions of reversed flow were found to be in agreement.
The first configuration is made up of the grille, intercooler and radiator. The numerical solution is compared with microprobe data in Fig. 7. Here the numerical data has been mapped to the same measurement grid (needless to say that the actual used numerical mesh was considerably finer).
Figure 7: Comparison of grille, intercooler and radiator.
Now it is possible to calculate the average of the absolute deviations relative to the mean velocity:
Using Eqn. (11) both the microprobes and the numerical simulation resulted in i = 6.0%. The uneven distribution can be completely attributed to the grille only. The agreement is excellent. The same applies to the recorded pressure drop:
Table 3: Pressure loss over grille, intercooler and radiator for various flow rates Q.
In the next configuration a cowl is added. Using Eqn. (11) again results in i = 8.7% for the microprobes and i = 7.5% for the numerical simulation. It is currently agreed upon that something went locally slightly wrong during the measurement, as the addition of the cowl should not result in the irregular pattern, which can be observed in Fig. 8.
Figure 8: Comparison of grille, intercooler, radiator and cowl.
The pressure loss of this case is presented in Table 4:
Table 4: Pressure loss over grille, intercooler, radiator and cowl.
The numerical results of the two previous configurations were also compared with LDA measurements behind the grille. The comparison showed also good agreement, but is not presented here.
In contrast to the previous results, which are at normal operating conditions the results of the configuration with the rotating fan are shown for a highly loaded case. In Fig. 9 the numerical results of the flow through the radiator are compared with the microprobe data. The relative deviations are 25% experimentally and 35% numerically. Also shown is the result of the fan model which was based on body forces; the relative deviation for this case is only 7.9%. It is obvious that this model did not predict the very uneven distribution through the radiator.
Figure 9: Comparison of grille, intercooler, radiator, cowl and including a rotating fan.
The deviations are now larger compared to the cases without the rotating fan. The main difference is that due to the high loading a ring vortex appears in the cowl (at higher airflow rates the ring vortex disappears and the deviations decrease). This ring vortex can be very large and strong (see Fig. 10). As a result four stagnation areas are formed in the corners of the cowl. These stagnation zones can be so strong that even reversed flow can occur back to the front side of the radiator. In fact this is what happened also during the microprobe measurements. Due to the fact that the measurement system can not deal with negative velocities the measured velocity dropped down to zero (see the bottom left corners in Fig. 9, the deviation i is therefore in the order of 2% underestimated). From the numerical point of view the vortex stresses the capabilities at the interfaces of the rotating frame of reference. It seems that the predicted vortex is a bit too strong which accounts for the 10% increase in deviation i. The ring vortex is a phenomenon which has to be taken into account if very closed encapsulations are considered.
Figure 10: Streamlines of the ring vortex in the cowl.
No attempt is made here to compare the numerical and experimental pressure rises. In the experimental set-up four static pressure probes were mounted in the corners of the tunnel. Due to the strong swirl introduced by the fan in the tunnel the pressure gradients in the corners are high. Thus a small alteration of the flow leads to a significantly different recorded pressure.
Numerical simulations and measurements on the radiator test facility showed also that the dummy engine block actually increases the efficiency of the fan. One of the explanations is that the engine disturbs the reversed flow near the fan shaft.
Another way to look at the numerical results is to seed a couple of hundred particles in the flow upstream the grille and to trace them through the complete cooling system. Once the streamlines are found it is possible to extract the corresponding static and total pressures along the streamlines and plot the results in the vehicle co- ordinate system. This method is better suited for the analysis of the pressures since it removes the potentially large influence of the ring vortex (with very low pressures in the core) from a method based on a mean pressure over a cowl section area.
In Fig. 11 the result of the static pressure relative to the external atmospheric pressure is shown (the pressures are normalised with respect to the mean values at the end of the tunnel of the radiator test facility). Upstream the grille the relative pressure is, of course, zero. Next, due to the accelerations of the flow through the openings in the grille the pressure drops a bit. This is followed by two pressure drops of the intercooler and radiator, respectively. In the cowl the influence of the ring vortex is already apparent before the pressure rise of the fan takes place. The most important aspect of this figure is the broad band at the end of the fan, which makes it difficult to define the "real mean" pressure rise. The first destruction of the pressure takes place around the dummy engine. Due to the highly swirling and slowly decaying flow within the tunnel the pressure converges to a final value. When an engine compartment is considered and the air leaves the compartment into the surrounding environment the pressure returns to the atmospheric value again (or relative to zero). Instead of the static pressure the total pressure is traced in Fig. 10. Basically the same characteristics of Fig. 9 are visible. However the huge total pressure rise is directly related to the high tangential velocities. As can be seen, quite a lot of the high dynamic pressure is almost immediately lost near the dummy engine. This, by the way, is also true for the engine compartment, which decreases the fan efficiency.
Figure 11: Static pressure levels
Figure 12: Total
Both Fig. 11 and 12 can be used to calculate the pressure losses of the various components, which can be fed into cooling system performance codes. Especially for the grill and radiators this is an easy task. However the definition of the pressure increase of the fan and the losses in the vicinity of the dummy engine are by nature of the physical complexity inexact.
It has been shown that complex three-dimensional CFD simulations of the flow through the Front-End of a truck a simplified engine compartment are possible under a variety of conditions. The accompanying validations have shown that the results are realistic even under exceptional conditions. This opens the door to the possibility to optimise the cooling system design early in the development. The next step is to incorporate heat transfer effects in the radiator and a tighter coupling of the CFD simulation with heat transfer models.
The comparison with experimental data was not always easy since both the used numerical and measurement techniques were not free of errors. However, the results are very satisfactory, the match is not always quantitatively correct but definitely qualitatively. The amount of error in the numerical simulations is estimated to be of typically in the order of 10%. Especially the comparisons with the 5-hole pressure probe have to be judged carefully.
The prominent role of the fan model has been discussed in detail. A fan model based on "body forces" is not usable for the conditions encountered in the engine compartment of a truck. Good results were achieved with a fan model based on "multiple rotating reference frames". This method has the advantages that no additional empirical parameters have to be introduced and is also attractive with respect to computer resources. Even the characteristics of a fan operating in off-design conditions were captured reasonably well.
Finally a method based on extracting pressure loss data from streamlines has been introduced. This method only takes into account the actual path of the airflow through the cooling system and thus automatically removes recirculation areas (in the cowl when present and behind the fan) from the analysis. However the actual performance of a fan in an enclosed space is still difficult to determine. Data gathered from this analysis can subsequently be fed into special heat transfer models.
This work is part of the project Technology for Low Noise Vehicles and has been supported by the Dutch Ministry of Housing, Physical Planning and Environment (VROM) for 50% of the project costs.
Please adress all enquiries
about this site to our webmaster.