如何在fluent中设置多相流.doc

3 设置一般的多相流问题（Setting Up a General Multiphase Problem）3.1使用一般多相流模型的步骤（Steps for Using the General Multiphase Models）设置和求解一般多相流问题的步骤的要点如下，各个子部分详细的讲述在随后的章节中。记住这里给出的仅是与一般多相流计算相关的步骤。有关你使用的其它模型和相关的多相流模型的输入的详细信息，将在这些模型中合适的部分给出。1) 选中你想要使用的多相流模型（VOF, mixture, or Eulerian）并指定相数。Define Models Multiphase.2) 从材料库中复制描述每相的材料。Define Materials.如果你使用的材料在库中没有，应创建一种新材料。!如果你的模型中含有微粒（granular）相，你必须在fluid materials category中为它创建新材料（not the solid materials category.）3) 定义相，指定相间的相互作用（interaction）(例如，使用欧拉模型时的drag functions)Define Phases.4) (仅对欧拉模型)如果流动是紊流，定义多相紊流模型。Define Models Viscous.5) 如果体积力存在，turn on gravity and specify the gravitational acceleration.Define Operating Conditions.6) 指定边界条件，包括第二相体积份额在流动边界和壁面上的接触角。Define Boundary Conditions.7) 设置模拟具体的解参数Solve Controls Solution.8) 初始化解和为第二相设定初始体积份额。Solve Initialize Patch.9) 计算求解和检查结果*欧拉多相流模拟的附加指南（Additional Guidelines for Eulerian Multiphase Simulations）一旦你决定了欧拉多相流模型适合你的问题，你应当考虑求解你的多相流问题的需求计算能力。要求的计算能力很强的依赖于所求解的输运方程的个数和耦合程度。对欧拉多相流模型，有大数量的高度耦合的输运方程，计算的耗费将很高，在设置你的问题前，尽可能减少问题的statement到最简化的可能形式。在你开始第一次求解尝试，取而代之尽力去求解多相流动的所有的复杂方面，你可以以简单近似地开始并且知道问题定义的最终形式。简化多相流问题的一些建议列举如下：1 使用六面体或四边形网格（而不用四面体或三角形网格）。2 减少相的数目。你会发现即使简单的近似也会给你的问题提供有用的信息。3.2选用多相流模型并指定相数（Enabling the Multiphase Model and Specifying the Number of Phases）为了选VOF, mixture, Eulerian多相流模型，在Multiphase Model panel下选Volume of Fluid, Mixture, or Eulerian as the Model。Define Models Multiphase.如果你选的欧拉模型，输入如下： number of phases：为了给多相流计算指定相数，在Number of Phases下输入合适的值。你最多可以指定20相。 (optional) cavitation effects：包含气穴影响（Including Cavitation Effects）对混合的欧拉模型计算，包含气穴影响是可能的。为了选气穴模型，在Multiphase Model panel中Interphase Mass Transfer下打开Cavitation。由于气穴影响，接下来你应指定在使用传质计算时的两个参数。这些参数的指定应当于调查下的流动特征参数相一致：Reynolds number and cavitation number。在Multiphase Model panel中Cavitation Parameters下面，设置Vaporization Pressure（PV）和Bubble Number Density（）。的默认值是10000，由Kubota et al推荐。默认的PV值是2367.8，环境温度下水的汽化压力。3.3定义相概述（Overview of Defining the Phases）为了定义相（包括它们的材料属性）和相间的相互作用（例如，欧拉模型中的曳力函数），你将使用Phases panel (Figure1). Define Phases. Figure 1: The Phases Panel这个面板中Phase下的每一项两类之一，如在Type列表中所示：primary-phase指出了所选项是主相，secondary-phase指出所选项是第二相。指定相之间的相互作用，点击Interaction. button.。3.3.1 Defining the Primary Phase 定义主相！通常，你可以你喜欢的任何方式指定主相和第二相。考虑你的选择如何影响问题的设置是一种很好的主意，特别是在复杂的问题中。例如，对区域一部分中的一相，如果你计划patch其初始体积份额为1，指定这个相为第二相更方便。同样，如果一相是可压缩的，为了提高解的稳定性，建议你指定它为主相。！记住，只能有一相是可压缩的。确定你没有选择可压缩材料（也就是对密度使用可压缩理想气体定律的材料）为多于一相的。1) Select phase-1 in the Phase list.2) Click Set., and the Primary Phase panel (Figure 2) will open.Figure 2: The Primary Phase Panel3) In the Primary Phase panel, enter a Name for the phase.4) Specify which material the phase contains by choosing the appropriate material in the Phase Material drop-down list.5) Define the material properties for the Phase Material. Click Edit., and the Material panel will open. In the Material panel, check the properties, and modify them if necessary. ! If you make changes to the properties, remember to click Change before closing the Material panel.6) Click OK in the Primary Phase panel.3.3.2 Defining a Non-Granular Secondary Phase定义非颗粒（即液体或气体）第二相1) Select the phase (e.g., phase-2) in the Phase list.2) Click Set., and the Secondary Phase panel (Figure 3) will open.Figure 3: The Secondary Phase Panel for a Non-Granular Phase3) In the Secondary Phase panel, enter a Name for the phase.4) Specify which material the phase contains by choosing the appropriate material in the Phase Material drop-down list.5) Define the material properties for the Phase Material, following the same procedure you used to set the material properties for the primary phase.6) In the Secondary Phase panel, specify the Diameter of the bubbles or droplets of this phase. You can specify a constant value, or use a user-defined function. See the separate UDF Manual for details about user-defined functions.7) Click OK in the Secondary Phase panel.3.3.3 Defining a Granular Secondary Phase 定义颗粒第二相1) Select the phase (e.g., phase-2) in the Phase list.2) Click Set., and the Secondary Phase panel (Figure4) will open.3) In the Secondary Phase panel, enter a Name for the phase.4) Specify which material the phase contains by choosing the appropriate material in the Phase Material drop-down list.5) Define the material properties for the Phase Material, following the same procedure you used to set the material properties for the primary phase. For a granular phase (which must be placed in the fluid materials category).! You need to specify only the density; you can ignore the values for the other properties, since they will not be used.In the Secondary Phase panel. 6) Enable theGranularoption.7) (optional) Enable thePacked Bedoption if you want to freeze the velocity field for the granular phase. ! Note that when you select the packed bed option for a phase, you should also use the fixed velocity option with a value of zero for all velocity components for all interior cell zones for that phase.8) Specify theGranular Temperature Model. Choose either the defaultPhase Propertyoption or thePartial Differential Equationoption. Figure 4: The Secondary Phase Panel for a Granular Phase9) In theSecondary Phasedialog box, specify the following properties of the particles of this phase: Diameterspecifies the diameter of the particles. You can selectconstantin the drop-down list and specify a constant value, or selectuser-definedto use a user-defined function. Granular Viscosityspecifies the kinetic part of the granular viscosity of the particles (s,kin). You can select constant(the default) in the drop-down list and specify a constant value, selectsyamlal-obriento compute the value, selectgidaspowto compute the value, or selectuser-definedto use a user-defined function. Granular Bulk Viscosityspecifies the solids bulk viscosity (q). You can selectconstant(the default) in the drop-down list and specify a constant value, selectlun-et-alto compute the value, or selectuser-definedto use a user-defined function. Frictional Viscosityspecifies a shear viscosity based on the viscous-plastic flow (s,fr). By default, the frictional viscosity is neglected, as indicated by the default selection ofnonein the drop-down list. If you want to include the frictional viscosity, you can selectconstantand specify a constant value, selectschaefferto compute the value, selectjohnson-et-alto compute the value, or selectuser-definedto use a user-defined function. Angle of Internal Frictionspecifies a constant value for the angle used in Schaeffers expression for frictional viscosity. This parameter is relevant only if you have selectedschaefferoruser-definedfor theFrictional Viscosity. Frictional Pressurespecifies the pressure gradient term, Pfriction, in the granular-phase momentum equation. Choosenoneto exclude frictional pressure from your calculation,johnson-et-al,syamlal-obrien,based-ktgf where the frictional pressure is defined by the kinetic theory. The solids pressure tends to a large value near the packing limit, depending on the model selected for the radial distribution function. You must hook a user-defined function when selecting theuser-definedoption. Frictional Modulusis defined aswithG0, which is thederivedoption. You can also specify auser-definedfunction for the frictional modulus. Friction Packing Limitspecifies a threshold volume fraction（开始体积分数） at which the frictional regime becomes dominant. It is assumed that for a maximum packing limit of 0.6, the frictional regime starts at a volume fraction of about 0.5. This is only a general rule of thumb as there may be other factors involved. Granular Conductivityspecifies the solids granular conductivity (ks). You can selectsyamlal-obriento compute the value, selectgidaspowto compute the value, or selectuser-definedto use a user-defined function. ! Note, however, thatANSYS FLUENTcurrently uses an algebraic relation for the granular temperature. This has been obtained by neglecting convection and diffusion in the transport equation. Granular Temperaturespecifies temperaturefor the solids phase and is proportional to the kinetic energy of the random motion of the particles. Choose either thealgebraic, theconstant, oruser-definedoption. Solids Pressurespecifies the pressure gradient term, Ps, in the granular-phase momentum equation. Choose either thelun-et-al, thesyamlal-obrien, thema-ahmadi,none, or auser-definedoption. Radial Distributionspecifies a correction factor that modifies the probability of collisions between grains when the solid granular phase becomes dense. Choose either thelun-et-al, thesyamlal-obrien, thema-ahmadi, thearastoopour, or auser-definedoption. Elasticity Modulusis defined aswith. Packing Limitspecifies the maximum volume fraction for the granular phase (s,max). For mono dispersed spheres, the packing limit is about 0.63, which is the default value inANSYS FLUENT. In poly dispersed cases, however, smaller spheres can fill the small gaps between larger spheres, so you may need to increase the maximum packing limit.10) ClickOKin theSecondary Phasedialog box.3.3.4 Defining the Interfacial Area ConcentrationTo define the interfacial area concentration on the secondary phase in the Eulerian model, perform the following steps:1) Select the phase (e.g.,phase-2) in thePhaseslist.2) ClickEdit.to open theSecondary Phasedialog box.3) In theSecondary Phasedialog box, enter aNamefor the phase.4) Specify which material the phase contains by choosing the appropriate material in thePhase Materialdrop-down list.5) Define the material properties for thePhase Material.6) Enable theInterfacial Area Concentrationoption. Make sure theGranularoption is disabled for theInterfacial Area Concentrationoption to be visible in the interface.7) In theSecondary Phasedialog box, specify the following properties of the particles of this phase: Diameterspecifies the diameter of the particles or bubbles. You can selectconstantin the drop-down list and specify a constant value, or selectuser-definedto use a user-defined function. See the separateUDF Manualfor details about user-defined functions. TheDiameterrecommended setting issauter-mean, allowing for the effects of the interfacial area concentration values to be considered for mass, momentum and heat transfer across the interface between phases. Packing Limitspecifies the maximum volume fraction for the particle/bubble phase. Growth Rateallows you to specify the particle growth rate (m/s). You can selectnone,constant, oruser-definedfrom the drop-down list. If you selectconstant, specify a value in the adjacent field. If you have a user-defined function (UDF) that you want to use to model the growth rate, you can choose theuser-definedoption and specify the appropriate UDF. Coalescence Kernal and Breakage Kernelallows you to specify the coalescence and breakage kernels. You can selectnone,constant,hibiki-ishii,ishii-kim, oruser-defined. In addition to specifying thehibiki-ishiiandishii-kimas the coalescence and breakage kernels, you can also tune the properties of these two models by using the/define/phases/iac-expert/hibiki-ishii-modeland/define/phases/iac-expert/ishii-kim-modeltext commands.For the Hibiki-Ishii model, you can specify the following parameters: Coefficient Gamma_c, Coefficient K_c, Coefficient Gamma_b, Coefficient K_b, alpha_maxFor the Ishii-Kim model, you can specify the following parameters: Coefficient Crc, Coefficient Cwe, Coefficient C, Coefficient Cti, alpha_max3.3.5 Defining the Interaction Between Phases对颗粒和非颗粒流动，你必须指定在动量交换系数的计算中使用的曳力函数。对颗粒流，你也必须指定颗粒碰撞的归还系数（restitution coefficients）。为颗粒和非颗粒流动包含可选的升力和虚拟质量力（下面描述）也是可能的。为指定这些参数，click Interaction. to open the Phase Interaction panel (Figure 5).1) Specifying the Drag Function FLUENT允许你为一对相指定曳力函数，步骤如下：a) Click the Drag tab to display the Drag Function inputs.b) 对每一对相，从下面相应的列表中选择合适的曳力函数。（1） Select schiller-naumann to use the fluid-fluid drag function. The Schiller and Naumann model is the default method, and it is acceptable for general use in all fluid-fluid multiphase calculations.（2） Select morsi-alexander to use the fluid-fluid drag function. The Morsi and Alexander model is the most complete, adjusting the function definition frequently over a large range of Reynolds numbers, but calculations with this model may be less stable than with the other models.（3） Select symmetric to use the fluid-fluid drag function described. The symmetric model is recommended for flows in which the secondary (dispersed) phase in one region of the domain becomes the primary (continuous) phase in another. For example, if air is injected into the bottom of a container filled halfway with water, the air is the dispersed phase in the bottom half of the container; in the top half of the container, the air is the continuous phase.（4） Select wen-yu to use the fluid-solid drag function. The Wen and Yu model is applicable for dilute phase flows, in which the total secondary phase volume fraction is significantly lower than that of the primary phase.（5） Select gidaspow to use the fluid-solid drag function. The Gidaspow model is recommended for dense fluidized beds.（6） Select syamlal-obrien to use the fluid-solid drag function. The Syamlal-OBrien model is recommended for use in conjunction with the Syamlal-OBrien model for granular viscosity.（7） Select syamlal-obrien-symmetric to use the solid-solid drag function. The symmetric Syamlal-OBrien model is appropriate for a pair of solid phases.（8） Select constant to specify a constant value for the drag function, and then specify the value in the text field.（9） Select user-defined to use a user-defined function for the drag function (see the separate UDF Manual for details).（10） If you want to temporarily ignore the interaction between two phases, select none.Figure 5: The Phase Interaction Panel for the Eulerian Model2) Specifying the Restitution Coefficients (Granular Flow Only)对颗粒流，你必须为颗粒间的碰撞指定归还系数（eIs and ess）。除了为每一对颗粒相之间的碰撞指定归还系数外，你也得为同相颗粒之间的碰撞指定归还系数。步骤如下： Click the Collisions tab to display the Restitution Coefficient inputs. For each pair of phases, specify a constant restitution coefficient. All restitution coefficients are equal to 0.9 by default. 3) Including the Lift Force对颗粒和非颗粒流，在第二相颗粒、液滴、或气泡中包含升力（Flift）的影响是可能的。这些升力作用于颗粒、液滴或气泡主要是由于主相流场中的速度梯度。在大多数情形下，升力与曳力相比是不重要的，因此没必要包含它，如果升力重要（也就是说，如果相很快分离），你可以包含这个影响。!注意对大颗粒，升力更重要，但是FLUENT模型假设粒子直径远小于粒子间距离。这样对接近充满的颗粒（closely packed particles）或者小颗粒，包含升力是不合适的。包含升力影响的步骤如下：a) Click the Lift tab to display the Lift Coefficient inputs.b) 对每一对相，从下面相应的列表中选择合适的指定方法。注意，既然作用于颗粒、液滴或气泡的升力主要是由于主相流场中的速度梯度，你不必为存在于两个第二相间的每对相指定升力系数；只对存在于第二相和主相之间的每对相指定升力系数。 Select none (the default) to ignore the effect of lift forces. Select constant to specify a constant lift coefficient, and then specify the value in the text field. Select user-defined to use a user-defined function for the lift coefficient (see the separate UDF Manual for details). 4) Including the Virtual Mass Force对颗粒和非颗粒流，当第二相相对于主相加速时包含存在的虚拟质量力（Fvm）是可能的。当第二相的密度远小于主相的密度时虚拟质量的影响是重要的（也就是对瞬态泡状柱流（transient bubble column）。包含虚拟质量力的影响，turn on the Virtual Mass option in the Phase Interaction panel.虚拟质量力的影响被包含在所有第二相内；使它仅为颗粒相是不可能的。5) Including Body Force(包含体积力) 在许多情况下，相的运动部分是由于重力的影响。为了包含这个体积力，应在Operating Conditions panel下选择Gravity并且指定Gravitational Acceleration.Define Operating Conditions. 对于VOF计算，你应当在Operating Conditions panel下选择Specified Operating Density,并且在Operating Density 下为最轻相设置密度。（这种排除了水力静压的积累，提高了round-off精度为动量平衡）。如果任何一相都是可压缩的，设置Operating Density为零。！对于涉及体积力的VOF 和mixture计算，建议你在Multiphase Model panel下为Body Force Formulation选择Implicit Body Force.这种处理通过解决压力梯度和动量方程中体积力的部分平衡提高了解的收敛。3.4 为Eulerian多相流计算选择紊流模型如果你使用Eulerian模型求解紊流，你必须在三种紊流模型中选择一种模型（在Viscous Model panel, Figure 6）。步骤如下：1 Select k-epsilon under Model.2 Select the desired k-epsilon Model and any other related parameters, as described for single-phase calculations.3 Under k-epsilon Multiphase Model, indicate the desired multiphase turbulence model: Select Mixture to use the mixture turbulence model. This is the default model. Select Dispersed to use the dispersed turbulence model. This model is applicable when there is clearly one primary continuous phase and the rest are dispersed dilute secondary phases. Select Per Phase to use a k- turbulence model for each phase. This model is appropriate when the turbulence transfer among the phases plays a dominant role*包含源项（Including Source Terms）默认情形，相间动量，、源项不包含在计算中。如果你想包含这些源项中的任一项，你可以使用multiphase-options command in the define/models/viscous/multiphase-turbulence/text menu。注意：包含这些项明显减慢收敛速度。如果你要寻找额外的精度，你应首先求的没有这些源项的解，接着包含上这些源项计算。大多数情形下这些源项可以忽略。Figure 6: The Viscous Model Panel for an Eulerian Multiphase Calculation3.5 设置边界条件多相流边界条件的设置在Boundary Conditions panel (Figure 7)中进行，但是设置多相流边界条件的步骤与单相流模型有些不同。你必须分别为各个相设置一些条件，而其他的条件是所有相（也就是mixture）所共享的，如下有详细的描述。3.5.1 Define Boundary Conditions. 混合相（mixture）和各个单相的边界条件Figure 7: The Boundary Conditions Panel如果你使用的是Eulerian模型，你必须为每一个区域类型指定的条件列举如下并总结在表1, 2, 3和4。注：具体的紊流参数取决于你使用的三个多相紊流模型，说明在表2-4中。 对于exhaust fan, outlet vent, or pressure outlet, 如果你使用层流模型或使用混合紊流模型（默认的多相紊流模型），没有条件为主相设置。对于每个第二相，你必须设置volume fraction为常数，型线或者UDF。如果相是颗粒的(granular),你也必须设置颗粒温度(g