1、OR-05-1 0-4 CFD Simulation of Heat Transfer in Compact Brazed Plate Heat Exchangers O. Pelletier Member ASHRAE F. Strmer A. Carlson ABSTRACT Thispaperprovides the result of an investigation about the possibili of simulating heat transfer in compact brazedplate heat exchangers (CBE) usinga commercial
2、 CFDsoftware. The simulations are performed using CFD software FLUENT 6.1 and a volume geometry corresponding to the channel in between two corrugatedplates. Two different plate geometries are simulated and referred to as models CBE5a and C3E5b. The focus of the investigation is to try to reproduce
3、with reason- able accuracy the experimentally measured differences between the two models. First, the paper presents the governing equations and the solving method used in CFD as well as considerations about the mesh generation. Then, three geometries are simulated in total, starting with a simplifi
4、ed volume geometry formed between two flatplates. Thesejrst simulations provide an idea of the necessary settings for the more complicated simulations on the two volume geometries made between two corrugated plates. The k-o SST turbulence model is used. The Reynolds number is about 3500. A tetrahedr
5、al mesh, includinga bound- ay layer made of two rows of cells, is used. Two different boundary conditions for the heat transfer on the walls arestud- ied. The heatflux and the wall temperature are alternatively held constant. The results of the simulations are discussedfor two differ- ent volume geo
6、metries made of corrugated plates. The best accuracy in the difference between the two corrugated models is obtained when a constant heatflux boundary condition is used. According to laboratory tests, the heat transfer charac- teristic of model CBE5b is 7.6% higher than that of model CBE5a. The simu
7、lations show a difference of 4.2%. It is not possible to get better accuracy when using a constant wall temperature boundary condition. Finally, simulations for test- ing the mesh dependency show that a coarse mesh leads to an even better estimation of the difference in heat transfer between both vo
8、lume geometry models. INTRODUCTION Computational fluid dynamics (CFD) is a tool used to simulate fluid flow and heat transfer. It makes it possible to build models of existing products and virtual ones for design analysis and improvements in terms of heat transfer and pres- sure drop. It predicts th
9、e performance of a given design illus- trated by pictures and data. Most CFD software offer a graphical interface that allows for studying, testing, and more quickly analyzing local behaviors and their interactions. This is something that sometimes is hard to obtain on physical prototypes. The insig
10、ht gained through this process helps to understand how to optimize a design. Different geometrical parameters of a design can be modified and tested under differ- ent sets of boundary conditions until an optimal result is reached. The foresight it gives allows for answering many questions before man
11、ufacturing real prototypes. Also, the use of CFD would hopefully lead to better product design in a shorter time or allow for more design cycles within a given period of time. In both cases, the work efficiency is increased and the new product development cycle is accelerated. Compact brazed plate h
12、eat exchangers (CBE) are made of corrugated plates placed on top of each other, as shown in Figure 1. Channels are formed between plates and alterna- tively filled by two different working media. In this type of heat exchanger, the plates are vacuum brazed together, which makes the package strong so
13、 that it can sustain high pressures. O. Pelletier is manager and E Strmer is an R&D engineer in the Department of Heat Transfer Research, SWEP International AB, Landsk- rona, Sweden. A. Carlson was a graduate student in the Divison of Heat Transfer, Lund Institute of Technology, Lund, Sweden. 846 02
14、005 ASHRAE. se?- - The corrugation makes both fluids flow very near to each other without physically mixing them. Moreover, the fluid flow is highly turbulent, which gives high heat transfer characteris- tics. The energy equation states that the rate of change of energy is equal to the sum of the ra
15、te of heat addition to a fluid Particle and the rate of work done on it (first law of thermo- dynamics). It yields (Sundn 2002): Today, CFD is used primarily for fluid flow simulations because the quantitative results from heat transfer simulations in plate heat exchangers have not been satisfactory
16、. The purpose of this study is to investigate the possibility of using CFD to simulate the heat transfer characteristics of two differ- ent compact brazed plate heat exchangers and to reproduce with reasonable accuracy the experimentally measured differ- ences. Accurate absolute values are therefore
17、 of minor inter- est. The CFD software Fluent, version 6.1, is used and simulations are carried out on a Linux cluster consisting of four computers connected in parallel. Each computer is made of double Intel Pentium 1-GHz processor and 1-GB of memory. When using the k-o SST turbulence model, the cl
18、us- ter can solve a mesh with a maximum of about 3 million cells. GOVERNING EQUATIONS AND NUMERICAL METHOD The governing equations of a fluid flow represent math- ematical statements of the conservation laws of physics. The continuity equation states that the mass of a fluid is conserved. For incomp
19、ressible steady-state flow, the continuity equation is (Versteeg 1995): The momentum equation, or Navier-Stokes equation, states that the rate of change of momentum equals the sum of the forces on a fluid particle. For incompressible fluid flow the Navier-Stokes equation is (Versteeg and Malalaseker
20、a 1995): With these equations, it is possible to obtain velocity, pressure, and temperature fields. The commonly used method to solve the governing equa- tions when working with CFD is the finite volume method (FVM), which integrates and conserves the fluid properties over a small control volume. Th
21、e general equation of conser- vation of a fluid property, here without time dependence, is (Mller 2003): where is an arbitrary fluid property. The governing equations cannot be solved analytically for complex geometries (White 1999). It is therefore necessary to solve them at a discrete number ofpoi
22、nts, which forms a mesh, The accuracy of the solution is highly dependent on the quality of the mesh. This is very critical in some regions, such as close to walls. MESH GENERATION The volume geometries are imported in Fluents pre- processor called Gambit, where the mesh is generated. The mesh forme
23、d to solve the governing equations at discrete points can be classified into different types, such as structured, unstructured, and hybrid, a mix of both. The structured mesh is made of two-dimensional quadri- lateral elements, as shown in Figure 2 (left), or three-dimen- sional hexahedral elements.
24、 All interior nodes have an equal number of adjacent elements. This type makes the mesh gener- ation appropriate for simple geometries, while it is difficult ASHRAE Transactions: Symposia a47 Figure 3 Uniform mesh in the core flow with boundary layers at the walls. and more time consuming for comple
25、x ones. The solvers for structured mesh need less computer memory and are often faster and more accurate than the best solvers for unstructured mesh. The unstructured mesh is made of two-dimensional triangle elements, as shown in Figure 2 (right), or three- dimensional tetrahedral elements. This typ
26、e makes it easy for mesh generation for more complex geometries. Solvers for such mesh require, however, longer execution time and more computer memory. The hybrid mesh uses the best of both the structured and the unstructured mesh. A structured mesh is preferable in the near-wall region where the g
27、radients are high, while unstructured mesh is used in the core flow. The good quality of the mesh has a direct impact on the stability of the simulation and its convergence. When creating the mesh, typical guidelines are that the mesh shall be made up of small cells where the gradients of the flow p
28、arameter are expected to be large, while larger cells are used where gradi- ents are small. As an example, the flow evolves rapidly over a small distance in a region with high gradients. In order to take into account and resolve these changes, a fine mesh is needed. In Fluents pre-processor Gambit,
29、a boundary layer consisting of a few rows with gradually growing cells can be made at the wall (Figure 3), while a more uniform mesh is used in the core flow. Another feature of Gambit is the so-called size function. This enables the user to control the size of the cells on specific surfaces (Figure
30、 4), which is of special interest for resolving the mesh at the walls and is very appropriate in complex geom- etries when using an unstructured mesh. The drawback of such a solution is the very large number of cells it necessitates. The so-called mesh adaptation is another way to enhance the mesh r
31、esolution in the region close to the walls. This can be done in Fluent, where the mesh can be adapted to the geometry as well as to the flow properties and the temperature fields. The attributes associated with mesh quality are node point distribution, smoothness, and skewness. A high node point den
32、sity in some regions is required in order to resolve property variations with good accuracy. Examples of such regions are boundary layers, shear layer, shock wave, and mixing zones (Fluent 2003). A mesh that is too coarse leads to loss of a lot of important information. The smoothness attribute tell
33、s how fast the cells grow from one row to another. A typical guideline is a value lower than 1.2 in growth rate (Carlson and Glaumann Figure 4 Mesh with size function. U 73 m 4m Figure 5 A simplijied volume geometry in between two flat plates. 2004), while the width by height aspect ratio of the cel
34、ls should not exceed 5. The last attribute is the skewness of the cells. Quadrilateral meshes with orthogonal vertex angles and triangular meshes with angles close to 60 degree are optimal (Fluent 2003). The skewness of a face or a cell with a value of O indicates a best case equiangular cell, while
35、 a value of 1 indi- cates a completely degenerated cell. Values of skewness lower than 0.7 for a face or cell mesh and lower than 0.95 for a volume mesh are recommended (Fluent 2003). The consequence of representing the fluid flow equations in discretized form is that numerical diffusion might appea
36、r (Patankar 1980). Numerical difision arises when a first order differential scheme is used, for example, the upwind scheme. The order itself also plays a large role in the stability of the solution. A higher order scheme gives a more accurate result, but it is often unstable. The solution easily st
37、arts to oscillate and convergence is not obtained (Fluent 2003). When possi- ble, the use of a second-order differencing scheme reduces the numerical diffusion. Refining the mesh decreases the trunca- tion error term and thereby the numerical diffusion. If possi- ble, the mesh should be aligned with
38、 the flow. This is, however, not possible for an unstructured mesh. SIMPLIFIED MODEL In order to get an idea of how the different settings in Fluent affect the result of fluid flow and heat transfer simula- tions, an initial study is carried out on a simplified geometry, as shown in Figure 5. The vo
39、lume geometry is formed between two flat plates, which makes it easier to create a desirable mesh. The plates have the same dimensions as the corrugated 848 ASHRAE Transactions: Symposia Table 1. Turbulence Settings plate model CBE5a. The inlet and outlet ports are positioned at the same location as
40、 that of the corrugated plate. The main objective of the study is to examine how the order of approx- imation and the turbulence models affect the results. Water is used as the working media, and its thermody- namic properties are taken at the inlet temperature of 293 K and kept constant during the
41、simulations. The pressure drop through the volume geometry, from the inlet to the outlet port, is set to 5 kPa by setting constant pressure boundaries. This setting leads to a Reynolds number of about 5000, which is of the same magnitude as that from laboratory tests. Reynolds number is defined as R
42、e=-=- udh 2m v WP where the hydraulic diameter is defined as which is appropriate since the width of the volume geometry between two plates is much larger than its thickness. The width of the volume geometry is 73 mm and its thickness is 4 mm (Figure 5). The heat flux at the walls is kept constant t
43、o 130 kW/m2, which leads to a temperature increase of about 7 K along the volume geometry. This rather small temperature increase allows for a rather good accuracy in spite of the assumption of constant fluid properties. The focus is on investigating two turbulence models, i.e., the so-called k-E an
44、d k-o models. The different ways to treat the near wall region with the k-E model are investigated. In total, seven simulations with different settings are performed, as shown in Table 1. Because the turbulence models need specific mesh reso- lution close to the walls, two different meshes are creat
45、ed. The k-E model uses a coarse uniform mesh together with standard and non-equilibrium wall functions and a fine mesh with boundary layer cells in the case ofthe enhanced wall treatment function. The k-o model uses a fine mesh with boundary layer cells as well, shown in Figure 6. I Mm Figure 6 Coar
46、se mesh with tetraedals (lej) andjne mesh with prism (right). This preliminary study shows significant differences in results depending on the turbulence models. The k-E model predicts a higher mass flow than the k-o model, which is expected since the k-E model is known to underestimate the fiiction
47、 factor (Carlson and Glaumann 2004). The improved submodels have, however, minor impact on the mass flow prediction, while the differences are more evident on heat transfer prediction. The wall functions used with the k-E model are of higher importance. The so-called enhanced wall treat- ment functi
48、on with the k-& model leads to a mass flow predic- tion close to that of the k-o model. In these cases both models use a fine mesh. Finally, both k-o models led to the same results and the heat transfer prediction is slightly higher than that ofthe k-E models. Even if the k-E model is commonly used
49、in the industry, it is most likely that the k-o model is a better choice and would give the most accurate solutions (Pope 2000). The k-o model is therefore used later on when simu- lating heat transfer and fluid flow in volume geometries made of corrugated plates. A first order scheme is usually used for all the transport equations. It is, however, desirable to use a second order scheme (Fluent 2003). Nevertheless, a first order scheme is used for the transport equations of the turbulence properties in order to avoid solution unstability often related to schemes of higher order.
