Numerical Simulation of the Internal Flow Field of Test Chamber at High Altitude Environment

In order to further promote the digitalization extent of environmental test, ensure that the test chamber can more realistically simulate the actual environment, and improve the environmental adaptability of vehicle equipment in extreme environments, the three-dimensional CFD simulation method was used to calculate simulation test chamber of an armored vehicle in high-altitude environment in the form of low-speed return flow wind tunnel. There are movable suspension and flap in the entrance to the contraction section of the test chamber. The velocity field and temperature field were analyzed, the temperature distribution and heat transfer in the characteristic section of the test section under different flap deflection angles were compared and analyzed by selecting working conditions, and make the relationship among flow speed and flow rate and the temperature field of the test section clear.


Introduction
The armored vehicle equipment is highly dispersed in use areas, which carries out complex and diverse tasks, and faces the test of various extreme environmental conditions.Vehicle environmental adaptability is an important index to evaluate the advanced performance of armored vehicle equipment [1].At present the test evaluation method is the main method to assess the environmental adaptability of armored vehicles [2].
The wind tunnel laboratory is artificially generating and controlling the flow of airflow and gases, which is one of the most frequently used and effective tools for performing aerodynamic experiments.Domestic and foreign vehicle environmental simulation laboratory often use low-speed return flow wind tunnels as the main simulation tool [3,4].However, even in the laboratory, there are also shortcomings, such as long test cycles, high costs.Due to the development of computer science, the development of various industrial software programs for CFD, numerical simulation of vehicle environmental test has become the key direction of environmental adaptability research [5].
This paper build a geometric model based on a simulation test chamber in a high-altitude environment, commercial CFD software Ansys Fluent was used for simulation calculation, the characteristics of its flow field and temperature field under specific working conditions were analysed, which provides references for values that are difficult to measure in actual tests, and gives predictions on the effect of the contraction section on the test section.
Motion equation: Energy equation: In the above equation (1)(2)(3),  is the density, , ,  is the velocity component of the fluid in x, y and z direction, respectively;  ,  ,  is the component of the mass force of unit mass fluid in three directions, respectively; , etc. are the components of the fluid internal stress tensor;  ℎ ,    is the effective heat transfer coefficient,  is the heat transfer coefficient of turbulence, according to the turbulence model,  is the component diffusion flow, and  ℎ is the generalized source term.

Heat Exchanger Model
The circulation duct of test chamber is equipped with a large tube-fin heat exchanger to simulate the working condition of low-temperature environment.The heat exchange model in Fluent is used to simulate the heat transfer in the test chamber.The heat exchange model divides the radiator core area into various macrocells, and calculates the heat fluid inlet temperature and heat loss of each macrocells.thesum of heat loss of all macrocells is the total heat exchange of the radiator.The heat exchange of each macrocell in the NTU model is min , , ( )

Porous Media Model
The tube-fin radiator is allocated for the plateau environment simulation chamber, the number of fins is large and its thickness is thin, therefore, if the actual geometric structure of the radiator core is used when modeling, it will generate vast grids,when carrying out grid division in the ICEM module, which is almost impossible to realize calculation.Therefore, in order to reduce the calculation difficulty and better reflect changes in velocity and pressure after the fluid passes through the heat exchanger, during the simulation, the porous media model is used to deal with the pressure loss when cooling air pass through the radiator core, and carry out reasonable simplification of the radiator core.In essence, the porous medium model is a momentum source term attached to the standard fluid momentum equation, this momentum source term consists of viscous loss term and internal loss term, whose mathematical expression is 3 3 In the above equation, i S is the source term of the momentum equation, v is the velocity, and D and C are the predetermined matrices.
In order to obtain the viscous coefficient and inertial term coefficient in Eq.( 5) as simulation input terms, the flow velocity-pressure drop test data are substituted into Ergun's equation for fitting.The expression of Ergun's equation is as follows.
In the equation, p L  is the pressure gradient, A is the dimensionless coefficient of viscosity term, B is the dimensionless coefficient of inertia term, A and B are empirical coefficients,  is the material porosity, and p d is the particle diameter.
The porous step is the one-dimensional simplification of the porous media model, which is used to characterize the downstream vortex-fragmenting net and shutter in contraction section in this model.The mathematical expressions is as follows:  is the laminar flow viscosity,  is the medium permeability, 2 C is the pressure mutation coefficient, v is the velocity perpendicular to the porous step surface, and m  is the medium thickness.

Fan Boundary Model
In order to reduce calculation and improve simulation efficiency, the Fan boundary model is used for the simulation of the main shaft flow fan.This is a model of lumped parameter, according to the characteristic of input fan P-Q, a plane is used to replace the complex fan model.
The mutation of pressure after the air flow passes through the plane is defined as the following function: p  is the pressure mutation, and the right side of the equation is a polynomial with perpendicular to the velocity of the Fan surface.

Model Simplification and Building
According to the actual geometric structure and size of the test chamber, the three-dimensional model was built, ignoring the airtight door, transition room, observation window, dynamometer, monitoring device and other components that have a small impact on the flow field of the computational domain, the computational domain shown in Fig. 1.

Fig. 1 computational domain of high-altitude test chamber
In the figure, ① is the axial flow fan; ② is the vortex-fragmenting net, play a rectifying role in the downstream flow field of the fan; ③ is the large tube fin heat exchanger; ④ ⑨ are guide plate; ⑤ is the suspension and flap of contraction section, ⑥ is the shutter, ⑤ ⑥ are the idling system, suspension can mechanically displace, flap can rotate around the axis at a certain angle.At that time, the shutter is opened to adjust the wind speed of the test section without changing the speed of the fan, that is, to ensure the maximum flow rate.The structure of the contraction section under idling condition is shown in Fig. 2. ( 7) is the nozzle of contraction section, which can adjust length to adapt to different vehicles.The slide and expansion joint is ignored here to make sure the number of grids can be calculated; (8) is the test section and the test vehicle, in order to control the number of grid and calculation feasibility, the heat transfer definition is only made for the vehicle surface.

Grid Division
The computational domain of the four cases: no idle speed, idle suspension is retracted, and the flap rotate by 10°, 20°, and 30°, are divided by ICEM CFD, respectively, theay are called as case0, case1, case2, and case3 below, respectively.The hybrid grid is generated after partitioning the computational domain, since Fluent requires the heat exchanger area to be wedge grid or positive hexahedral grid, therefore, the structured grid is generated in the heat exchanger region and the unstructured grid dominated by tetrahedral grid in the other areas.In order to reduce the number of grids and shorten the calculation time, the walls such as guide plate and contraction section are treated without thickness.The narrower parts are filled with grids of several layers to make the grids finer.The total number of grid cells is about 25 million, 26.6 million, 26.6 million, and 26.6 million, respectively, and grid quality is good.

Other Initial Conditions
In order to better reflect the environmental test process of vehicle, the air is assumed to be an ideal gas in the solution setup, the Realizable k-ε model is used as the turbulence model, this model can better describe the turbulent flow of high Reynolds number and is suitable for the case when the turbulent flow is more fully developed.
In order to simulate the flow distribution in the test chamber, typical test conditions are selected.For the axial flow fan, the polynomial fitted according to its P-Q curve is entered in Fluent, and its maximum flow condition is selected.For damped surfaces/bodies such as heat exchanger, vortex-fragmenting net and shutter, the correlation coefficients are obtained according to Equation (5) (6).For tank wall surfaces, the experimental data and the results of the 1D heat flow simulation of the lumped parameter method are combined [6], conduct nonlinear least square fitting on it, and set it to the type I boundary condition.The temperature distribution of the vehicle armor surface is fixed.The relevant boundary conditions are shown in the following table.

Overall Analysis of Flow Field Velocity
Flow velocity distribution of Case0 in the high-altitude test chamber is shown in Fig. 3, it can be seen that due to the long length of the rear fairing, there is an obvious flow stratification downstream: the low velocity area appears in the center of the air duct.After passing through the diffusion section of the tunnel, the flow inhomogeneity begins to enhance, and after passing through the vortex-fragmenting network, the flow separation phenomenon is weakened, and velocity turns to be relatively stable, the fluid can enter the downstream heat exchanger more uniformly in the radial section, it suggests that this device can effectively suppress the velocity variation amplitude in the section and improve the flow field quality.After that, under the interference of the guide plate and the corner of the tunnel, the velocity decays and the flow inhomogeneity has been strengthened further, especially when passing through the guide plate, there is return flow vortex, which has a obvious impact on the flow field of chamber, resulting in up high and down low flow velocity distribution in the diffusion section.But under the contraction section afterwards, the flow gradually gather and flow velocity increase, after flow through the outlet of the contraction section, the flow velocity has been stabilized at about 25m/s and there is no obvious flow stratification phenomenon, it suggests that the air duct structure can simulate a uniform and controllable flow field; affected by the vehicle body, the flow form has changed significantly after passing through the vehicle, small-scale encircling flow is formed in the rear of the vehicle.Finally, when passing through the constriction section, the velocity increases again, thus completing the flow cycle of the whole test chamber.

Fig. 3 velocity cloud image of the axial plane of the test chamber
The flow capacity, flow field stability and uniformity, and turbulence of the wind tunnel are important performance indexes of the wind tunnel [7], the CFD simulation results of the test chamber for several key cross-sectional flow velocity area fractional mean values are compared with the design specifications.and the results are shown below.

Fig. 4 comparison between the simulation value and design value of velocity of various sections
The analysis and comparison of results found that the velocity simulation value of the cross-section is basically consistent with the design value except for the large deviation of the velocity simulation value of the power section from the design value.Regarding the abnormal velocity of the power section, considering that the design value of the power section does not take into account the influence of the axial flow fan hub on the section, as a result, the relationship between flow and velocity is inconsistent with the reality.In general, the simulation value is larger than the design value, and it may be caused by not setting the wall resistance correctly in the simulation process or ignoring the simplification of some components.In addition, the velocity increases when passing through unpowered section and flat section, considering that the presence of turbulence on the statistical interface causes the calculation results of velocity vector to fluctuate.
The reasons for some deviations between CFD calculation and design result are complex.For the empirical design method, it is difficult to fully predict the actual situation of the wind tunnel flow field, such as whether flow separation occurs, the uniformity condition of the fan section flow, and these states have a great impact on the pressure loss and flow velocity distribution in the wind tunnel; in addition, the sections that require special design generally lack empirical formulas or complete theory to correspond with them, as a result, wind speed control is more difficult, such as the test section, test parts, and the wind speed changes of heat exchanger section.On the other hand, in this paper, the size of the base grid used for the calculating grid division is 10cm, the grid distribution is relatively dense at places where the unit flow changes dramatically, such as fans, near corners, or at sudden-change air duct in cross-sectional area, they can capture some turbulence with small flow fields relative to the whole computational domain scale, the numerical values reproduce the flow separation in the pipe, which still has a certain degree of confidence.However, due to the large scale and complex structure of the wind tunnel, the calculation accuracy still has room for improvement, and it is possible to capture more subtle flow field information.

Comparison Analysis of Inlet and Outlet Cross-section in Test Section
In order to further study the effect of the idling system on the flow and heat transfer in the test section, the temperature and velocity cloud image of the inlet and outlet sections of the test section are taken for the simulation results of case0, case1, case2 and case3, respectively, and the results are shown below.5), the highest temperature on the cross-section is about 267 K when the idling system is closed, while the highest temperature drops to about 256 K when the idling system is opened, and there is no significant change in the temperature with the further expansion of the flap opening.For Figure (6), it is clearly observed that as the flipping angle of the idling system flap increases, the measured velocity in the nozzle decreases and becomes unevenly distributed, while the overall velocity distribution in the section is more uniform.In Fig. (7), the temperature of outlet section of the test section decreases significantly after the idling system is opened, however, similar to the results in Fig. (5), the temperature characteristic distribution of outlet of the test section does not reflect the flipping angle of the idling system flap significantly, considering that excessive turbulence after fluid flows through the vehicle body.The velocity distribution of outlet section of the test section in Fig. (8) verifies this hypothesis: the velocity gradient on this side is huge and the distribution characteristics are more chaotic, and there is obviously strong turbulence.Combining the above analysis, whether the idling system open or not, it will have a significant impact on the heat dissipation of vehicle in the test section, while the effect on the velocity field distribution downstream of the vehicle is relatively small.With the increase of flipping angle of the idling system flap, the test section inlet flow changes significantly, while the temperature and velocity distribution of the outlet section of test section do not change significantly due to the turbulence through the vehicle body, and it is consistent with the heat transfer power calculation results of heat exchanger in Table 3.

Conclusion
This paper combines the target environment and relevant CFD theories of vehicle test, reasonably sets up the selected turbulence model, grid division method, boundary conditions and other simulation parameters, conducts fully functional numerical simulation of the whole simulated flow field, and obtains the calculation results of the idling system under four working conditions.The flow velocity distribution results of test chamber are analyzed, comparing the inlet and outlet velocity and temperature distribution of the test section from case0 to case3, the main conclusion are as follows: 1) The velocity distribution of various flow sections of the test chamber is basically consistent with the design velocity, thus ensuring the reliability of the simulation for different wind speed environments.
2) Due to the presence of the fan fairing and the vehicle test piece in downstream of the wind turbine section and the test section, there is strong turbulence, the turbulence downstream of the fan can be effectively suppressed by vortex-fragmenting net.
3) The idling system can significantly affect the inlet velocity distribution of test section, whether the idling system is opened or not, which significantly affects the velocity and temperature distribution of test section, the heat exchange of heat exchanger: when the idling system is opened, the air velocity of test section decreases and the highest temperature decreases.
4) When the idling system is opened, when the rotation angle of flap is greater than 10°, it can no longer have a significant effect on the outlet flow field and temperature field of the test section, and the heat exchange of heat exchanger.
Although this paper gives intuitive conclusions on some problems by CFD numerical simulation, there are still problems in the calculation such as the grid accuracy is not high enough, the boundary condition setting is not reasonable enough, and the resolution of the case variable setting is coarse, in the future, we can continue to deepen the research by improving the computing power of hardware and strengthening the combination of test and simulation.

Fig. 2
Fig. 2 flap and suspension of contraction section under idling condition

Fig. 5 Fig. 7
temperature cloud image of the inlet section in the test section case0 case1 case2 case3 Fig. 6 temperature cloud image of the inlet section in the test section FMIA-2023 Journal of Physics: Conference Series 2599 (2023) 012025 IOP Publishing doi:10.1088/1742-6596/2599/1temperaturecloud image of outlet section in the test section case0 case1 case2 case3 Fig. 8 temperature cloud image of outlet section in the test section As shown in Fig.(

Table 1 .
settings of relevant boundary conditions

Table 2 .
comparison of case0 simulation results and design velocity

Table 3 .
steady-state heat transfer power of heat exchanger