多孔介质在fluent中的操作方法 网络上传版本

经过痛苦的一段经历，终于将局部问题真相大白，为了使保位同仁不再经过我之痛苦，现在将本人多孔介质经验公布如下，希望各位能加精：1。

Gambit中划分网格之后，定义需要做为多孔介质的区域为fluid,与缺省的fluid分别开来，再定义其名称，我习惯将名称定义为porous;2。

在fluent中定义边界条件define-boundary condition-porous(刚定义的名称)，将其设置边界条件为fluid,点击set按钮即弹出与fluid边界条件一样的对话框，选中porous zone与laminar复选框,再点击porous zone标签即出现一个带有滚动条的界面；3。

porous zone设置方法：1）定义矢量：二维定义一个矢量，第二个矢量方向不用定义，是与第一个矢量方向正交的；三维定义二个矢量，第三个矢量方向不用定义，是与第一、二个矢量方向正交的；（如何知道矢量的方向：打开grid图，看看X,Y,Z的方向，如果是X向，矢量为1,0,0,同理Y向为0,1,0，Z向为0,0,1,如果所需要的方向与坐标轴正向相反，则定义矢量为负）圆锥坐标与球坐标请参考fluent帮助。

2）定义粘性阻力1/a与内部阻力C2：请参看本人上一篇博文“终于搞清fluent中多孔粘性阻力与内部阻力的计算方法”，此处不赘述；3）如果了定义粘性阻力1/a与内部阻力C2,就不用定义C1与C0，因为这是两种不同的定义方法，C1与C0只在幂率模型中出现，该处保持默认就行了；4）定义孔隙率porousity，默认值1表示全开放，此值按实验测值填写即可。

完了，其他设置与普通k-e或RSM相同。

总结一下，与君共享!Tutorial 7. Modeling Flow Through Porous MediaIntroductionMany industrial applications involve the modeling of flow through porous media, such as filters, catalyst beds, and packing. This tutorial illustrates how to set up and solve a problem involving gas flow through porous media.The industrial problem solved here involves gas flow through a catalytic converter. Catalytic converters are commonly used to purify emissions from gasoline and diesel engines by converting environmentally hazardous exhaust emissions to acceptable substances.Examples of such emissions include carbon monoxide (CO), nitrogen oxides (NOx), and unburned hydrocarbon fuels. These exhaust gas emissions are forced through a substrate, which is a ceramic structure coated with a metal catalyst such as platinum or palladium.The nature of the exhaust gas flow is a very important factor in determining the performance of the catalytic converter. Of particular importance is the pressure gradient and velocity distribution through the substrate. Hence CFD analysis is used to design efficient catalytic converters: by modeling the exhaust gas flow, the pressure drop and the uniformity of flow through the substrate can be determined. In this tutorial, FLUENT is used to model the flow of nitrogen gas through a catalytic converter geometry, so that the flow field structure may be analyzed.This tutorial demonstrates how to do the following:_ Set up a porous zone for the substrate with appropriate resistances._ Calculate a solution for gas flow through the catalytic converter using the pressure based solver. _ Plot pressure and velocity distribution on specified planes of the geometry._ Determine the pressure drop through the substrate and the degree of non-uniformity of flow through cross sections of the geometry using X-Y plots and numerical reports.Problem DescriptionThe catalytic converter modeled here is shown in Figure 7.1. The nitrogen flows in through the inlet with a uniform velocity of 22.6 m/s, passes through a ceramic monolith substrate with square shaped channels, and then exits through the outlet.While the flow in the inlet and outlet sections is turbulent, the flow through the substrate is laminar and is characterized by inertial and viscous loss coefficients in the flow (X) direction. The substrate is impermeable in other directions, which is modeled using loss coefficients whose values are three orders of magnitude higher than in the X direction.Setup and SolutionStep 1: Grid1. Read the mesh file (catalytic converter.msh).File /Read /Case...2. Check the grid. Grid /CheckFLUENT will perform various checks on the mesh and report the progress in the console. Make sure that the minimum volume reported is a positive number.3. Scale the grid.Grid! Scale...(a) Select mm from the Grid Was Created In drop-down list.(b) Click the Change Length Units button. All dimensions will now be shown in millimeters.(c) Click Scale and close the Scale Grid panel.4. Display the mesh. Display /Grid...(a) Make sure that inlet, outlet, substrate-wall, and wall are selected in the Surfaces selection list.(b) Click Display.(c) Rotate the view and zoom in to get the display shown in Figure 7.2.(d) Close the Grid Display panel.The hex mesh on the geometry contains a total of 34,580 cells.Step 2: Models1. Retain the default solver settings. Define /Models /Solver...2. Select the standard k-ε turbulence model. Define/ Models /Viscous...Step 3: Materials1. Add nitrogen to the list of fluid materials by copying it from the Fluent Database for materials.Define /Materials...(a) Click the Fluent Database... button to open the Fluent Database Materials panel.i. Select nitrogen (n2) from the list of Fluent Fluid Materials.ii. Click Copy to copy the information for nitrogen to your list of fluid materials. iii. Close the Fluent Database Materials panel.(b) Close the Materials panel.Step 4: Boundary Conditions. Define /Boundary Conditions...1. Set the boundary conditions for the fluid (fluid).(a) Select nitrogen from the Material Name drop-down list.(b) Click OK to close the Fluid panel.2. Set the boundary conditions for the substrate (substrate).(a) Select nitrogen from the Material Name drop-down list.(b) Enable the Porous Zone option to activate the porous zone model.(c) Enable the Laminar Zone option to solve the flow in the porous zone without turbulence.(d) Click the Porous Zone tab.i. Make sure that the principal direction vectors are set as shown in Table7.1. Use the scroll bar to access the fields that are not initially visible in the panel.ii. Enter the values in Table 7.2 for the Viscous Resistance and Inertial Resistance. Scroll down to access the fields that are not initially visible in the panel.(e) Click OK to close the Fluid panel.3. Set the velocity and turbulence boundary conditions at the inlet (inlet).(a) Enter 22.6 m/s for the Velocity Magnitude.(b) Select Intensity and Hydraulic Diameter from the Specification Method dropdown list in the Turbulence group box.(c) Retain the default value of 10% for the Turbulent Intensity.(d) Enter 42 mm for the Hydraulic Diameter.(e) Click OK to close the Velocity Inlet panel.4. Set the boundary conditions at the outlet (outlet).(a) Retain the default setting of 0 for Gauge Pressure.(b) Select Intensity and Hydraulic Diameter from the Specification Method dropdown list in the Turbulence group box.(c) Enter 5% for the Backflow Turbulent Intensity.(d) Enter 42 mm for the Backflow Hydraulic Diameter.(e) Click OK to close the Pressure Outlet panel.5. Retain the default boundary conditions for the walls (substrate-wall and wall) and close the Boundary Conditions panel.Step 5: Solution1. Set the solution parameters. Solve /Controls /Solution...(a) Retain the default settings for Under-Relaxation Factors.(b) Select Second Order Upwind from the Momentum drop-down list in the Discretization group box.(c) Click OK to close the Solution Controls panel.2. Enable the plotting of residuals during the calculation. Solve/Monitors /Residual...(a) Enable Plot in the Options group box.(b) Click OK to close the Residual Monitors panel.3. Enable the plotting of the mass flow rate at the outlet.Solve / Monitors /Surface...(a) Set the Surface Monitors to 1.(b) Enable the Plot and Write options for monitor-1, and click the Define... button to open the Define Surface Monitor panel.i. Select Mass Flow Rate from the Report Type drop-down list.ii. Select outlet from the Surfaces selection list.iii. Click OK to close the Define Surface Monitors panel.(c) Click OK to close the Surface Monitors panel.4. Initialize the solution from the inlet. Solve /Initialize /Initialize...(a) Select inlet from the Compute From drop-down list.(b) Click Init and close the Solution Initialization panel.5. Save the case file (catalytic converter.cas). File /Write /Case...6. Run the calculation by requesting 100 iterations. Solve /Iterate...(a) Enter 100 for the Number of Iterations.(b) Click Iterate.The FLUENT calculation will converge in approximately 70 iterations. By this point the mass flow rate monitor has attended out, as seen in Figure 7.3.(c) Close the Iterate panel.7. Save the case and data files (catalytic converter.cas and catalytic converter.dat).File /Write /Case & Data...Note: If you choose a file name that already exists in the current folder, FLUENTwill prompt you for confirmation to overwrite the file.Step 6: Post-processing1. Create a surface passing through the centerline for post-processing purposes.Surface/Iso-Surface...(a) Select Grid... and Y-Coordinate from the Surface of Constant drop-down lists.(b) Click Compute to calculate the Min and Max values.(c) Retain the default value of 0 for the Iso-Values.(d) Enter y=0 for the New Surface Name.(e) Click Create.2. Create cross-sectional surfaces at locations on either side of the substrate, as well as at its center.Surface /Iso-Surface...(a) Select Grid... and X-Coordinate from the Surface of Constant drop-down lists.(b) Click Compute to calculate the Min and Max values.(c) Enter 95 for Iso-Values.(d) Enter x=95 for the New Surface Name.(e) Click Create.(f) In a similar manner, create surfaces named x=130 and x=165 with Iso-Values of 130 and 165, respectively. Close the Iso-Surface panel after all the surfaces have been created.3. Create a line surface for the centerline of the porous media.Surface /Line/Rake...(a) Enter the coordinates of the line under End Points, using the starting coordinate of (95, 0, 0) and an ending coordinate of (165, 0, 0), as shown.(b) Enter porous-cl for the New Surface Name.(c) Click Create to create the surface.(d) Close the Line/Rake Surface panel.4. Display the two wall zones (substrate-wall and wall). Display /Grid...(a) Disable the Edges option.(b) Enable the Faces option.(c) Deselect inlet and outlet in the list under Surfaces, and make sure that only substrate-wall and wall are selected.(d) Click Display and close the Grid Display panel.(e) Rotate the view and zoom so that the display is similar to Figure 7.2.5. Set the lighting for the display. Display /Options...(a) Enable the Lights On option in the Lighting Attributes group box.(b) Retain the default selection of Gourand in the Lighting drop-down list.(c) Click Apply and close the Display Options panel.6. Set the transparency parameter for the wall zones (substrate-wall and wall).Display/Scene...(a) Select substrate-wall and wall in the Names selection list.(b) Click the Display... button under Geometry Attributes to open the Display Properties panel.i. Set the Transparency slider to 70.ii. Click Apply and close the Display Properties panel.(c) Click Apply and then close the Scene Description panel.7. Display velocity vectors on the y=0 surface.Display /Vectors...(a) Enable the Draw Grid option. The Grid Display panel will open.i. Make sure that substrate-wall and wall are selected in the list under Surfaces.ii. Click Display and close the Display Grid panel.(b) Enter 5 for the Scale.(c) Set Skip to 1.(d) Select y=0 from the Surfaces selection list.(e) Click Display and close the Vectors panel.The flow pattern shows that the flow enters the catalytic converter as a jet, with recirculation on either side of the jet. As it passes through the porous substrate, it decelerates and straightens out, and exhibits a more uniform velocity distribution.This allows the metal catalyst present in the substrate to be more effective.Figure 7.4: Velocity Vectors on the y=0 Plane8. Display filled contours of static pressure on the y=0 plane.Display /Contours...(a) Enable the Filled option.(b) Enable the Draw Grid option to open the Display Grid panel.i. Make sure that substrate-wall and wall are selected in the list under Surfaces.ii. Click Display and close the Display Grid panel.(c) Make sure that Pressure... and Static Pressure are selected from the Contours of drop-down lists.(d) Select y=0 from the Surfaces selection list.(e) Click Display and close the Contours panel.Figure 7.5: Contours of the Static Pressure on the y=0 planeThe pressure changes rapidly in the middle section, where the fluid velocity changes as it passes through the porous substrate. The pressure drop can be high, due to the inertial and viscous resistance of the porous media. Determining this pressure drop is a goal of CFD analysis. In the next step, you will learn how to plot the pressure drop along the centerline of the substrate.9. Plot the static pressure across the line surface porous-cl.Plot /XY Plot...(a) Make sure that the Pressure... and Static Pressure are selected from the Y Axis Function drop-down lists.(b) Select porous-cl from the Surfaces selection list.(c) Click Plot and close the Solution XY Plot panel.Figure 7.6: Plot of the Static Pressure on the porous-cl Line SurfaceIn Figure 7.6, the pressure drop across the porous substrate can be seen to be roughly 300 Pa.10. Display filled contours of the velocity in the X direction on the x=95, x=130 and x=165 surfaces.Display /Contours...(a) Disable the Global Range option.(b) Select Velocity... and X Velocity from the Contours of drop-down lists.(c) Select x=130, x=165, and x=95 from the Surfaces selection list, and deselect y=0.(d) Click Display and close the Contours panel.The velocity profile becomes more uniform as the fluid passes through the porous media. The velocity is very high at the center (the area in red) just before the nitrogen enters the substrate and then decreases as it passes through and exits the substrate. The area in green, which corresponds to a moderate velocity, increases in extent.Figure 7.7: Contours of the X Velocity on the x=95, x=130, and x=165 Surfaces11. Use numerical reports to determine the average, minimum, and maximum of the velocity distribution before and after the porous substrate.Report /Surface Integrals...(a) Select Mass-Weighted Average from the Report Type drop-down list.(b) Select Velocity and X Velocity from the Field Variable drop-down lists.(c) Select x=165 and x=95 from the Surfaces selection list.(d) Click Compute.(e) Select Facet Minimum from the Report Type drop-down list and click Compute again.(f) Select Facet Maximum from the Report Type drop-down list and click Compute again.(g) Close the Surface Integrals panel.The numerical report of average, maximum and minimum velocity can be seen in the main FLUENT console, as shown in the following example:The spread between the average, maximum, and minimum values for X velocity gives the degree to which the velocity distribution is non-uniform. You can also use these numbers to calculate the velocity ratio (i.e., the maximum velocity divided by the mean velocity) and the space velocity (i.e., the product of the mean velocity and the substrate length).Custom field functions and UDFs can be also used to calculate more complex measures ofnon-uniformity, such as the standard deviation and the gamma uniformity index.SummaryIn this tutorial, you learned how to set up and solve a problem involving gas flow through porous media in FLUENT. You also learned how to perform appropriate post-processing to investigate the flow field, determine the pressure drop across the porous media and non-uniformity of the velocity distribution as the fluid goes through the porous media.Further ImprovementsThis tutorial guides you through the steps to reach an initial solution. You may be able to obtain a more accurate solution by using an appropriate higher-order discretization scheme and by adapting the grid. Grid adaption can also ensure that the solution is independent of the grid. These steps aredemonstrated in Tutorial 1.。

fluent多孔板处理方法
Fluent多孔板处理方法是指在Fluent软件中使用多孔板模型进行流体处理的技术。

多孔板是一种被广泛应用于过滤、分离和增加传质过程的设备，它具有各种孔隙形状和尺寸。

在使用Fluent进行多孔板处理时，首先需要建立一个合适的几何模型，包括多孔板的尺寸和流体领域的设置。

然后，根据实际情况选择适当的物理模型和边界条件。

在多孔板模型中，主要涉及两个关键参数：流体流动速度和多孔介质的阻力系数。

流体流动速度可以通过设置入口边界条件来实现，常用的边界条件有速度入口和压力出口。

多孔介质的阻力系数可以通过实验或经验公式获得，并在模型中进行设置。

在处理过程中，还需要考虑多孔板的材料特性，如孔隙率、孔隙形状和孔隙分布。

这些参数将直接影响到流体在多孔介质中的传递和分布过程。

Fluent提供了多种求解器来模拟多孔板处理过程，其中包括具有多孔效应的流体流动模型。

通过使用这些求解器，可以获得多孔板内部的流体速度分布、压力分布和质量传递情况。

总之，Fluent多孔板处理方法是利用Fluent软件模拟多孔板内部流体流动和传质过程的一种技术。

通过合理设置模型参数、边界条件和材料特性，可以准确地模拟和分析多孔板系统中的流体行为，为工程设计和优化提供有效的参考依据。

FLUENT多孔介质数值模拟设置多孔介质条件多孔介质模型可以应用于很多问题，如通过充满介质的流动、通过过滤纸、穿孔圆盘、流量分配器以及管道堆的流动。

当你使用这一模型时，你就定义了一个具有多孔介质的单元区域，而且流动的压力损失由多孔介质的动量方程中所输入的内容来决定。

通过介质的热传导问题也可以得到描述，它服从介质和流体流动之间的热平衡假设，具体内容可以参考多孔介质中能量方程的处理一节。

多孔介质的一维化简模型，被称为多孔跳跃，可用于模拟具有已知速度/压降特征的薄膜。

多孔跳跃模型应用于表面区域而不是单元区域，并且在尽可能的情况下被使用（而不是完全的多孔介质模型），这是因为它具有更好的鲁棒性，并具有更好的收敛性。

详细内容请参阅多孔跳跃边界条件。

多孔介质模型的限制如下面各节所述，多孔介质模型结合模型区域所具有的阻力的经验公式被定义为“多孔”。

事实上多孔介质不过是在动量方程中具有了附加的动量损失而已。

因此，下面模型的限制就可以很容易的理解了。

流体通过介质时不会加速，因为事实上出现的体积的阻塞并没有在模型中出现。

这对于过渡流是有很大的影响的，因为它意味着FLUENT不会正确的描述通过介质的过渡时间。

多孔介质对于湍流的影响只是近似的。

详细内容可以参阅湍流多孔介质的处理一节。

多孔介质的动量方程多孔介质的动量方程具有附加的动量源项。

源项由两部分组成，一部分是粘性损失项 (Darcy)，另一个是内部损失项：其中S_i是i向(x, y, or z)动量源项，D和C是规定的矩阵。

在多孔介质单元中，动量损失对于压力梯度有贡献，压降和流体速度（或速度方阵）成比例。

对于简单的均匀多孔介质：其中a是渗透性，C_2时内部阻力因子，简单的指定D和C分别为对角阵1/a 和C_2其它项为零。

FLUENT还允许模拟的源项为速度的幂率：其中C_0和C_1为自定义经验系数。

注意：在幂律模型中，压降是各向同性的，C_0的单位为国际标准单位。

多孔介质的Darcy定律通过多孔介质的层流流动中，压降和速度成比例，常数C_2可以考虑为零。

FLUENT多孔介质数值模拟设置C=对于不同D/t的不同雷诺数范围被列成不同的表的系数A_p=圆盘的面积（固体和洞)如果你选择在多孔介质中模拟热传导，你必须指定多孔介质中的材料以及多孔性。

要定义多孔介质的材料，向下拉流体面板中阻力输入底下的滚动条，然后在多孔热传导的固体材料下拉列表中选中适当的固体。

另一个处理收敛性差的要领是临时取消多孔介质模型（在流体面板中关闭多孔区域）然后获取一个不受多孔区域影响的初始流场。

取消多孔区域后，FLUEＮT会将多孔区域处理为流体区域并按响应的流体区域来计算。

一旦获取了初始解，或者计算很容易收敛，你就可以激活多孔模型继续计算包罗多孔区域的流场（对于大阻力多孔介质不保举使用该要领）。

这些变量会在后处理面板的变量选择下拉菜谱制定类别中出现。

然后在多孔热传导下设定多孔性。

多孔性f是多孔介质中流体的体积分数（即介质的开放体积分数）。

多孔性用于介质中的热传导预测，处理要领请参阅多孔介质能量方程的处理一节。

它还对介质中的反应源项和体力的计算有影响。

这个源项和介质中流体的体积成比例。

如果你想要模拟完全开放的介质（固体介质没有影响），你应该设定多孔性为1.0。

当多孔性为1.0时，介质的固体部门对于热传导和（或）热源项/反应源项没有影响。

注意：多孔性永远不会影响介质中的流体速率，这已经在多孔介质的动量方程一节中介绍了。

不管你将多孔性设定为何值，，FLUEＮT所预测的速率都是介质中的外貌速率。

对于多孔介质动量源项（多孔介质动量方程中的方程5），如果你使用幂律模型近似，你只要在流体面板的幂律模型中输入系数C_0和C_1就可以了。

如果C_0或C_1为非零值，解算器会忽略面板中除了多孔介质幂律模型之外的所有输入。

定义源项一般说来，在模拟多孔介质时，你可以使用标准的解算步骤以及解参数的设置。

然而你会发现如果多孔区域在流动方向上压降至关大（比如：渗透性a很低或者内部因数C_2很大）的话，解的收敛速率就会变慢。

7.19.6 User Inputs for Porous MediaWhen you are modeling a porous region, the only additional inputs for the problem setup are as follows. Optional inputs are indicated as such.1. Define the porous zone.2. Define the porous velocity formulation. (optional)3. Identify the fluid material flowing through the porous medium.4. Enable reactions for the porous zone, if appropriate, and select the reaction mechanism.5. Enable the Relative Velocity Resistance Formulation. By default, this option is already enabled and takes the moving porous media into consideration (as described in Section 7.19.6).6. Set the viscous resistance coefficients ( in Equation7.19-1,or in Equation 7.19-2) and the inertial resistance coefficients ( in Equation 7.19-1, or in Equation 7.19-2), and define the direction vectors for which they apply. Alternatively, specify the coefficients for the power-law model.7. Specify the porosity of the porous medium.8. Select the material contained in the porous medium (required only for models that include heat transfer). Note that the specific heat capacity, , for the selected material in the porous zone can only be entered as a constant value.9. Set the volumetric heat generation rate in the solid portion of the porous medium (or any other sources, such as mass or momentum). (optional) 10. Set any fixed values for solution variables in the fluid region (optional).11. Suppress the turbulent viscosity in the porous region, if appropriate.12. Specify the rotation axis and/or zone motion, if relevant.Methods for determining the resistance coefficients and/or permeability are presented below. If you choose to use the power-law approximation of the porous-media momentum source term, you will enter thecoefficients and in Equation 7.19-3 instead of the resistance coefficients and flow direction.You will set all parameters for the porous medium inthe Fluid panel (Figure 7.19.1), which is opened from the Boundary Conditions panel (as described in Section 7.1.4).Figure 7.19.1: The Fluid Panel for a Porous Zone Defining the Porous ZoneAs mentioned in Section 7.1, a porous zone is modeled as a special type of fluid zone. To indicate that the fluid zone is a porous region, enablethe Porous Zone option in the Fluid panel. The panel will expand to show the porous media inputs (as shown in Figure 7.19.1).Defining the Porous Velocity FormulationThe Solver panel contains a Porous Formulation region where you can instruct FLUENT to use either a superficial or physical velocity in the porous medium simulation. By default, the velocity is set to SuperficialVelocity. For details about using the Physical Velocity formulation, see Section 7.19.7.Defining the Fluid Passing Through the Porous MediumTo define the fluid that passes through the porous medium, select the appropriate fluid in the Material Name drop-down list in the Fluid panel. If you want to check or modify the properties of the selected material, you can click Edit... to open the Material panel; this panel contains just the properties of the selected material, not the full contents of thestandard Materials panel.If you are modeling species transport or multiphase flow,the Material Name list will not appear in the Fluid panel. Forspecies calculations, the mixture material for all fluid/porous zones will be the material you specified in the SpeciesModel panel. For multiphase flows, the materials are specified when you define the phases, as described in Section 23.10.3.Enabling Reactions in a Porous ZoneIf you are modeling species transport with reactions, you can enable reactions in a porous zone by turning on the Reaction option inthe Fluid panel and selecting a mechanism in the ReactionMechanism drop-down list.If your mechanism contains wall surface reactions, you will also need to specify a value for the Surface-to-Volume Ratio. This value is the surface area of the pore walls per unit volume ( ), and can be thought of as a measure of catalyst loading. With this value, FLUENT can calculate the total surface area on which the reaction takes place in each cell bymultiplying by the volume of the cell. See Section 14.1.4 for detailsabout defining reaction mechanisms. See Section 14.2for details about wall surface reactions.Including the Relative Velocity Resistance FormulationPrior to FLUENT 6.3, cases with moving reference frames used the absolute velocities in the source calculations for inertial and viscous resistance. This approach has been enhanced so that relative velocities are used for the porous source calculations (Section 7.19.2). Using the Relative Velocity Resistance Formulation option (turned on by default) allows you to better predict the source terms for cases involving moving meshes or moving reference frames (MRF). This option works well in cases withnon-moving and moving porous media. Note that FLUENT will use the appropriate velocities (relative or absolute), depending on your case setup. Defining the Viscous and Inertial Resistance CoefficientsThe viscous and inertial resistance coefficients are both defined in the same manner. The basic approach for defining the coefficients using a Cartesian coordinate system is to define one direction vector in 2D or two direction vectors in 3D, and then specify the viscous and/or inertial resistance coefficients in each direction. In 2D, the second direction, which is not explicitly defined, is normal to the plane defined by the specified direction vector and the direction vector. In 3D, the third direction is normal to the plane defined by the two specified direction vectors. For a 3D problem, the second direction must be normal to the first. If you fail to specify two normal directions, the solver will ensure that they are normal by ignoring any component of the second direction that is in the first direction. You should therefore be certain that the first direction is correctly specified. You can also define the viscous and/or inertial resistance coefficients in each direction using a user-defined function (UDF). The user-defined options become available in the corresponding drop-down list when the UDF has been created and loaded into FLUENT. Note that the coefficients defined in the UDF must utilize the DEFINE_PROFILE macro. For moreinformation on creating and using user-defined function, see the separate UDF Manual.If you are modeling axisymmetric swirling flows, you can specify an additional direction component for the viscous and/or inertial resistance coefficients. This direction component is always tangential to the other two specified directions. This option is available for both density-based and pressure-based solvers.In 3D, it is also possible to define the coefficients using a conical (or cylindrical) coordinate system, as described below.Note that the viscous and inertial resistance coefficients aregenerally based on the superficial velocity of the fluid in the porous media.The procedure for defining resistance coefficients is as follows:1. Define the direction vectors.To use a Cartesian coordinate system, simply specify the Direction-1 Vector and, for 3D, the Direction-2 Vector. The unspecifieddirection will be determined as described above. These directionvectors correspond to the principle axes of the porous media.For some problems in which the principal axes of the porous mediumare not aligned with the coordinate axes of the domain, you may notknow a priori the direction vectors of the porous medium. In suchcases, the plane tool in 3D (or the line tool in 2D) can help you todetermine these direction vectors.(a) "Snap'' the plane tool (or the line tool) onto the boundary of theporous region. (Follow the instructions inSection 27.6.1 or 27.5.1 for initializing the tool to a position on anexisting surface.)(b) Rotate the axes of the tool appropriately until they are alignedwith the porous medium.(c) Once the axes are aligned, click on the Update From PlaneTool or Update From Line Tool button inthe Fluid panel. FLUENT will automatically set the Direction-1Vector to the direction of the red arrow of the tool, and (in 3D)the Direction-2 Vector to the direction of the green arrow.To use a conical coordinate system (e.g., for an annular, conical filter element), follow the steps below. This option is available only in 3D cases.(a) Turn on the Conical option.(b) Specify the Cone Axis Vector and Point on Cone Axis. Thecone axis is specified as being in the direction of the Cone AxisVector (unit vector), and passing through the Point on Cone Axis.The cone axis may or may not pass through the origin of thecoordinate system.(c) Set the Cone Half Angle (the angle between the cone's axis andits surface, shown in Figure 7.19.2). To use a cylindrical coordinate system, set the Cone Half Angle to 0.Figure 7.19.2: Cone Half AngleFor some problems in which the axis of the conical filter element is not aligned with the coordinate axes of the domain, you may notknow a priori the direction vector of the cone axis and coordinates ofa point on the cone axis. In such cases, the plane tool can help you todetermine the cone axis vector and point coordinates. One method is as follows:(a) Select a boundary zone of the conical filter element that isnormal to the cone axis vector in the drop-down list next to the Snap to Zone button.(b) Click on the Snap to Zone button. FLUENT will automatically"snap'' the plane tool onto the boundary. It will also set the Cone Axis Vector and the Point on Cone Axis. (Note that you will still have to set the Cone Half Angle yourself.)An alternate method is as follows:(a) "Snap'' the plane tool onto the boundary of the porous region.(Follow the instructions in Section 27.6.1 for initializing the tool to a position on an existing surface.)(b) Rotate and translate the axes of the tool appropriately until thered arrow of the tool is pointing in the direction of the cone axisvector and the origin of the tool is on the cone axis.(c) Once the axes and origin of the tool are aligned, click onthe Update From Plane Tool button inthe Fluid panel. FLUENT will automatically set the Cone AxisVector and the Point on Cone Axis. (Note that you will still have toset the Cone Half Angle yourself.)2. Under Viscous Resistance, specify the viscous resistancecoefficient in each direction.Under Inertial Resistance, specify the inertial resistance coefficient in each direction. (You will need to scroll down with the scroll bar to view these inputs.)For porous media cases containing highly anisotropic inertial resistances, enable Alternative Formulation under Inertial Resistance.The Alternative Formulation option provides better stability to the calculation when your porous medium is anisotropic. The pressure loss through the medium depends on the magnitude of the velocity vector ofthe i th component in the medium. Using the formulation ofEquation 7.19-6 yields the expression below:(7.19-10) Whether or not you use the Alternative Formulation option depends on how well you can fit your experimentally determined pressure drop data to the FLUENT model. For example, if the flow through the medium is aligned with the grid in your FLUENT model, then it will not make a difference whether or not you use the formulation.For more infomation about simulations involving highly anisotropic porous media, see Section 7.19.8.Note that the alternative formulation is compatible only with the pressure-based solver.If you are using the Conical specification method, Direction-1 is the cone axis direction, Direction-2 is the normal to the cone surface (radial ( )direction for a cylinder), and Direction-3 is the circumferential ( ) direction.In 3D there are three possible categories of coefficients, and in 2D there are two:∙In the isotropic case, the resistance coefficients in all directions are the same (e.g., a sponge). For an isotropic case, you must explicitlyset the resistance coefficients in each direction to the same value.∙When (in 3D) the coefficients in two directions are the same and those in the third direction are different or (in 2D) the coefficients inthe two directions are different, you must be careful to specify thecoefficients properly for each direction. For example, if you had aporous region consisting of cylindrical straws with small holes inthem positioned parallel to the flow direction, the flow would passeasily through the straws, but the flow in the other two directions(through the small holes) would be very little. If you had a plane offlat plates perpendicular to the flow direction, the flow would notpass through them at all; it would instead move in the other twodirections.∙In 3D the third possible case is one in which all three coefficients are different. For example, if the porous region consisted of a plane ofirregularly-spaced objects (e.g., pins), the movement of flow between the blockages would be different in each direction. You wouldtherefore need to specify different coefficients in each direction. Methods for deriving viscous and inertial loss coefficients are described in the sections that follow.Deriving Porous Media Inputs Based on Superficial Velocity, Using a Known Pressure LossWhen you use the porous media model, you must keep in mind that the porous cells in FLUENT are 100% open, and that the values that you specify for and/or must be based on this assumption. Suppose, however, that you know how the pressure drop varies with the velocity through the actual device, which is only partially open to flow. The following exercise is designed to show you how to compute a valuefor which is appropriate for the FLUENT model.Consider a perforated plate which has 25% area open to flow. The pressure drop through the plate is known to be 0.5 times the dynamic head in the plate. The loss factor, , defined as(7.19-11)is therefore 0.5, based on the actual fluid velocity in the plate, i.e., the velocity through the 25% open area. To compute an appropriate valuefor , note that in the FLUENT model:1. The velocity through the perforated plate assumes that the plate is 100% open.2. The loss coefficient must be converted into dynamic head loss per unit length of the porous region.Noting item 1, the first step is to compute an adjusted loss factor, , which would be based on the velocity of a 100% open area:(7.19-12) or, noting that for the same flow rate, ,(7.19-13)The adjusted loss factor has a value of 8. Noting item 2, you must now convert this into a loss coefficient per unit thickness of the perforated plate. Assume that the plate has a thickness of 1.0 mm (10 m). The inertial loss factor would then be(7.19-14)Note that, for anisotropic media, this information must be computed for each of the 2 (or 3) coordinate directions.Using the Ergun Equation to Derive Porous Media Inputs for a Packed BedAs a second example, consider the modeling of a packed bed. In turbulent flows, packed beds are modeled using both a permeability and an inertial loss coefficient. One technique for deriving the appropriate constants involves the use of the Ergun equation [ 98], a semi-empirical correlation applicable over a wide range of Reynolds numbers and for many types of packing:(7.19-15)When modeling laminar flow through a packed bed, the second term in the above equation may be dropped, resulting in the Blake-Kozenyequation [ 98]:(7.19-16) In these equations, is the viscosity, is the mean particlediameter, is the bed depth, and is the void fraction, defined as the volume of voids divided by the volume of the packed bed region. Comparing Equations 7.19-4 and 7.19-6 with 7.19-15, the permeability and inertial loss coefficient in each component direction may be identified as(7.19-17) and(7.19-18) Using an Empirical Equation to Derive Porous Media Inputs for Turbulent Flow Through a Perforated PlateAs a third example we will take the equation of Van Winkle et al. [ 279, 339] and show how porous media inputs can be calculated for pressure loss through a perforated plate with square-edged holes.The expression, which is claimed by the authors to apply for turbulent flow through square-edged holes on an equilateral triangular spacing, is(7.19-19) where= mass flow rate through the plate= the free area or total area of the holes= the area of the plate (solid and holes)= a coefficient that has been tabulated for various Reynolds-numberrangesand for various= the ratio of hole diameter to plate thicknessfor and for the coefficient takes a value of approximately 0.98, where the Reynolds number is based on hole diameter and velocity in the holes.Rearranging Equation 7.19-19, making use of the relationship(7.19-20)and dividing by the plate thickness, , we obtain(7.19-21)where is the superficial velocity (not the velocity in the holes). Comparing with Equation 7.19-6 it is seen that, for the direction normal to the plate, the constant can be calculated from(7.19-22)Using Tabulated Data to Derive Porous Media Inputs for Laminar Flow Through a Fibrous MatConsider the problem of laminar flow through a mat or filter pad which is made up of randomly-oriented fibers of glass wool. As an alternative to the Blake-Kozeny equation (Equation 7.19-16) we might choose to employ tabulated experimental data. Such data is available for many types offiber [ 158].fraction of dimensionless permeability of glass woolwhere and is the fiber diameter. , for use inEquation 7.19-4, is easily computed for a given fiber diameter and volume fraction.Deriving the Porous Coefficients Based on Experimental Pressure and Velocity DataExperimental data that is available in the form of pressure drop against velocity through the porous component, can be extrapolated to determine the coefficients for the porous media. To effect a pressure drop across a porous medium of thickness, , the coefficients of the porous media are determined in the manner described below.If the experimental data is:then an curve can be plotted to create a trendline through these points yielding the following equationwhere is the pressure drop and is the velocity.Note that a simplified version of the momentum equation, relating the pressure drop to the source term, can be expressed as(7.19-24)or(7.19-25)Hence, comparing Equation 7.19-23 to Equation 7.19-2, yields the following curve coefficients:(7.19-26)with kg/m , and a porous media thickness, , assumed to be 1m in this example, the inertial resistance factor, .Likewise,with , the viscous inertial resistancefactor,.Note that this same technique can be applied to the porous jump boundary condition. Similar to the case of the porous media, you have to take into account the thickness of the medium . Your experimental data can be plotted in ancurve, yielding an equation that is equivalent to Equation 7.22-1. From there, you can determine the permeability and the pressure jumpcoefficient.Using the Power-Law ModelIf you choose to use the power-law approximation of the porous-media momentum source term (Equation 7.19-3), the only inputs required are the coefficients and . Under Power Law Model in the Fluid panel, enter the values for C0 and C1. Note that the power-law model can be used in conjunction with the Darcy and inertia models. C0 must be in SI units, consistent with the value of C1.Defining PorosityTo define the porosity, scroll down below the resistance inputs in the Fluid panel, and set the Porosity under Fluid Porosity .You can also define the porosity using a user-defined function (UDF). The user-defined option becomes available in the corresponding drop-down list when the UDF has been created and loaded into FLUENT. Note that the porosity defined in the UDF must utilize the DEFINE_PROFILE macro. For more information on creating and using user-defined function, see the separate UDF Manual.The porosity, , is the volume fraction of fluid within the porous region (i.e., the open volume fraction of the medium). The porosity is used in the prediction of heat transfer in the medium, as described in Section 7.19.3, and in the time-derivative term in the scalar transport equations for unsteady flow, as described in Section 7.19.5. It also impacts the calculation of reaction source terms and body forces in the medium. These sources will be proportional to the fluid volume in the medium. If you want to represent the medium as completely open (no effect of the solid medium), you should set the porosity equal to 1.0 (the default). When the porosity is equal to 1.0, the solid portion of the medium will have no impact on heat transfer or thermal/reaction source terms in the medium.Defining the Porous MaterialIf you choose to model heat transfer in the porous medium, you must specify the material contained in the porous medium.To define the material contained in the porous medium, scroll down below the resistance inputs in the Fluid panel, and select the appropriate solid in the Solid Material Name drop-down list under Fluid Porosity. If you want to check or modify the properties of the selected material, you canclick Edit... to open the Material panel; this panel contains just the properties of the selected material, not the full contents of thestandard Materials panel. In the Material panel, you can define thenon-isotropic thermal conductivity of the porous material using auser-defined function (UDF). The user-defined option becomes available in the corresponding drop-down list when the UDF has been created and loaded into FLUENT. Note that the non-isotropic thermal conductivity defined in the UDF must utilize the DEFINE_PROPERTY macro. For more information on creating and using user-defined function, see the separate UDF Manual.Defining SourcesIf you want to include effects of the heat generated by the porous medium in the energy equation, enable the Source Terms option and set anon-zero Energy source. The solver will compute the heat generated by the porous region by multiplying this value by the total volume of the cells comprising the porous zone. You may also define sources of mass, momentum, turbulence, species, or other scalar quantities, as described in Section 7.28.Defining Fixed ValuesIf you want to fix the value of one or more variables in the fluid region of the zone, rather than computing them during the calculation, you can do so by enabling the Fixed Values option. See Section 7.27 for details. Suppressing the Turbulent Viscosity in the Porous RegionAs discussed in Section 7.19.4, turbulence will be computed in the porous region just as in the bulk fluid flow. If you are using one of the turbulence models (with the exception of the Large Eddy Simulation (LES) Model), and you want the turbulence generation to be zero in the porous zone, turn on the Laminar Zone option in the Fluid panel. Refer to Section 7.17.1 for more information about suppressing turbulence generation.Specifying the Rotation Axis and Defining Zone MotionInputs for the rotation axis and zone motion are the same as for a standard fluid zone. See Section 7.17.1 for details.。

1、输出grid图形2、选择surface---plane,打开plane surface面板3、通过确定三个点来确定平面位置。

单击slect point，出现提示，不点选cancel.在grid 图形的多孔介质区域任意位置右键点选3个点。

4、回到plane surface面板，勾选plane tool，则在grid图形的多孔介质区域出现一个平面。

若出现的平面与我们的预期相差比较大的话，可以单击reset points,可以获得一个特殊位置的平面。

5、打开多孔介质的控制面板，选择porous zone标签，点击update from plane tool按钮，获得方向矢量1，和方向矢量2的原始值，并与左下角的坐标系统比较，确定我们大概的旋转方向。

6、对比grid图形左下角的坐标系统，红线和红色箭头代表的是方向矢量1，绿线和绿色箭头代表的是方向矢量2应该使红线和X正方向平行，绿线和Y正方向平行。

具体的操作应该是：一：先单击白线的蓝色箭头，固定了该方向在旋转过程中不变，可以保证在旋转的过程比较有规律，然后右键点选白线的红色箭头旋转红线的红色箭头到X的正轴；二: 接下来应该是单击白线的红色箭头，固定该方向不变，单击白线的蓝色箭头，旋转绿线的绿色箭头指向Y的正轴。

（所以多孔介质区域我们一般是设置在坐标系统里面，轴线等与坐标系统无非直角角度关系）。

把平面移动到图形外有利于旋转，比较清楚。

平面法线方向的移动是用鼠标右键单击平面阴影部分并拖动，横向移动则需按下shift并进行如上操作。

7、旋转到适当的位置后（鼠标右键拖动箭头），再次点击update from plane tool按钮，获得方向矢量1，和方向矢量2。

得到的数值很可能不是整数，这个时候我们可以把他简化为整数。

例如：0.9123可以简化为1，0.01245可以简化为0，以此类推。

多孔介质-Fluent模拟7.19多孔介质边界条件多孔介质模型适用的范围非常广泛，包括填充床，过滤纸，多孔板，流量分配器，还有管群，管束系统。

当使用这个模型的时候，多孔介质将运用于网格区域，流场中的压降将由输入的条件有关，见Section 7.19.2.同样也可以计算热传导，基于介质和流场热量守恒的假设，见Section 7.19.3.通过一个薄膜后的已知速度/压力降低特性可以简化为一维多孔介质模型，简称为“多孔跳跃”。

多孔跳跃模型被运用于一个面区域而不是网格区域，而且也可以代替完全多孔介质模型在任何可能的时候，因为它更加稳定而且能够很好地收敛。

见Section 7.22.7.19.1 多孔介质模型的限制和假设多孔介质模型就是在定义为多孔介质的区域结合了一个根据经验假设为主的流动阻力。

本质上，多孔介质模型仅仅是在动量方程上叠加了一个动量源项。

这种情况下，以下模型方面的假设和限制就可以很容易得到:, 因为没有表示多孔介质区域的实际存在的体，所以fluent默认是计算基于连续性方程的虚假速度。

做为一个做精确的选项，你可以适用fluent中的真是速度，见section7.19.7。

, 多孔介质对湍流流场的影响，是近似的，见7.19.4。

, 当在移动坐标系中使用多孔介质模型的时候，fluent既有相对坐标系也可以使用绝对坐标系，当激活相对速度阻力方程。

这将得到更精确的源项。

相关信息见section7.19.5和7.19.6。

, 当需要定义比热容的时候，必须是常数。

7.19.2 多孔介质模型动量方程多孔介质模型的动量方程是在标准动量方程的后面加上动量方程源项。

源项包含两个部分:粘性损失项(达西公式项，方程7.19-1右边第一项)，和惯性损失项(方程7.19-1右边第二项)(7.19-1)式中，si是i(x，y，z)动量方程的源项，是速度大小，D和C是矩阵。

动量源项对多孔介质区域的压力梯度有影响，生成一个与速度大小(速度平方)成正比的压降。

Tutorial 7. Modeling Flow Through Porous Media IntroductionMany industrial applications involve the modeling of ow through porous media, such as _lters, catalyst beds, and packing. This tutorial illustrates how to set up and solve a problem involving gas ow through porous media.The industrial problem solved here involves gas ow through a catalytic converter. Catalytic converters are commonly used to purify emissions from gasoline and diesel engines by converting environmentally hazardous exhaust emissions to acceptable substances.Examples of such emissions include carbon monoxide (CO), nitrogen oxides (NOx), and unburned hydrocarbon fuels. These exhaust gas emissions are forced through a substrate, which is a ceramic structure coated with a metal catalyst such as platinum or palladium.The nature of the exhaust gas ow is a very important factor in determining the performance of the catalytic converter. Of particular importance is the pressure gradient and velocity distribution through the substrate. Hence CFD analysis is used to designe_cient catalytic converters: by modeling the exhaust gas ow, the pressure drop andthe uniformity of ow through the substrate can be determined. In this tutorial, FLUENTis used to model the ow of nitrogen gas through a catalytic converter geometry, so that the ow _eld structure maybe analyzed.This tutorial demonstrates how to do the following:_ Set up a porous zone for the substrate with appropriate resistances._ Calculate a solution for gas ow through the catalytic converter using the pressurebased solver._ Plot pressure and velocity distribution on speci_ed planes of the geometry._ Determine the pressure drop through the substrate and the degree of non-uniformityof ow through cross sections of the geometry using X-Y plots and numerical reports.许多工业应用都涉及通过多孔介质（如过滤器，催化剂床和填料）的流动模型。

多孔介质在fluent中的操作方法网络上传版本预览说明:预览图片所展示的格式为文档的源格式展示,下载源文件没有水印,内容可编辑和复制如何在Fluent中实现多孔介质双能量方程(LNTE)How to use Non-equilibrium Thermal equation (LNTE) model forPorous media in Fluent Software●请参照本人发表的文章：●Please refer to the following papers：1)Wang Fu–Qiang*，Shuai Yong*，Wang Zhi–Q iang，Leng Yu，Tan He–Ping.Thermal and chemical reaction performance analyses of steam methane reforming in porous media solar thermochemical reactor，International Journal of Hydrogen Energy，39(2)：718-730，2014关键词：Porous, Solar, Hydrogen, Methane, Reforming, P1 approximation, radiative heat transfer2)Wang Fu–Qiang*，Shuai Yong*，Tan He–Ping，Zhang Xiao-Feng，MaoQian-Jun，Heat transfer analyses of porous media receiver with multi–dish collector by coupling MCRT and FVM method，Solar Energy，93：158–168，2013关键词：Solar, Porous, dish concentrator, Receiver, Monte Carlo3)Wang Fu–Qiang*，Shuai Yong*，T an He–Ping，Yu Chun–Liang，ThermalPerformance Analysis of Porous Media Receiver with Concentrated Solar Irradiation，International Journal of Heatand Mass Transfer，62：247–254，2013关键词：Solar, Porous, dish concentrator, Receiver, Monte Carlo一、说明1、模型此例基于稳态、层流、对称模型。

经过痛苦的一段经历;终于将局部问题真相大白;为了使保位同仁不再经过我之痛苦;现在将本人多孔介质经验公布如下;希望各位能加精：1..Gambit中划分网格之后;定义需要做为多孔介质的区域为fluid;与缺省的fluid分别开来;再定义其名称;我习惯将名称定义为porous;2..在fluent中定义边界条件define-boundary condition-porous刚定义的名称;将其设置边界条件为fluid;点击set按钮即弹出与fluid边界条件一样的对话框;选中porous zone 与laminar复选框;再点击porous zone标签即出现一个带有滚动条的界面；3..porous zone设置方法：1定义矢量：二维定义一个矢量;第二个矢量方向不用定义;是与第一个矢量方向正交的；三维定义二个矢量;第三个矢量方向不用定义;是与第一、二个矢量方向正交的；如何知道矢量的方向：打开grid图;看看X;Y;Z的方向;如果是X向;矢量为1;0;0;同理Y 向为0;1;0;Z向为0;0;1;如果所需要的方向与坐标轴正向相反;则定义矢量为负圆锥坐标与球坐标请参考fluent帮助..2定义粘性阻力1/a与内部阻力C2：请参看本人上一篇博文“终于搞清fluent中多孔粘性阻力与内部阻力的计算方法”;此处不赘述；3如果了定义粘性阻力1/a与内部阻力C2;就不用定义C1与C0;因为这是两种不同的定义方法;C1与C0只在幂率模型中出现;该处保持默认就行了；4定义孔隙率porousity;默认值1表示全开放;此值按实验测值填写即可..完了;其他设置与普通k-e或RSM相同..总结一下;与君共享Tutorial 7. Modeling Flow Through Porous MediaIntroductionMany industrial applications involve the modeling of flow through porous media; such as filters; catalyst beds; and packing. This tutorial illustrates how to set up and solve a problem involving gas flow through porous media.The industrial problem solved here involves gas flow through a catalytic converter. Catalytic converters are commonly used to purify emissions from gasoline and diesel engines by converting environmentally hazardous exhaust emissions to acceptable substances.Examples of such emissions include carbon monoxide CO; nitrogen oxides NOx; and unburned hydrocarbon fuels. These exhaust gas emissions are forced through a substrate; which is a ceramic structure coated with a metal catalyst such as platinum or palladium.The nature of the exhaust gas flow is a very important factor in determining the performance of the catalytic converter. Of particular importance is the pressure gradient and velocity distribution through the substrate. Hence CFD analysis is used to design efficient catalytic converters: by modeling the exhaust gas flow; the pressure drop and the uniformity of flow through the substrate can be determined. In this tutorial; FLUENT is used to model the flow of nitrogen gas through a catalytic converter geometry; so that the flow field structure may be analyzed.This tutorial demonstrates how to do the following:_ Set up a porous zone for the substrate with appropriate resistances._ Calculate a solution for gas flow through the catalytic converter using the pressure based solver. _ Plot pressure and velocity distribution on specified planes of the geometry._ Determine the pressure drop through the substrate and the degree of non-uniformity of flow through cross sections of the geometry using X-Y plots and numerical reports.Problem DescriptionThe catalytic converter modeled here is shown in Figure 7.1. The nitrogen flows in through the inlet with a uniform velocity of 22.6 m/s; passes through a ceramic monolith substrate with square shaped channels; and then exits through the outlet.While the flow in the inlet and outlet sections is turbulent; the flow through the substrate is laminar and is characterized by inertial and viscous loss coefficients in the flow X direction. The substrate is impermeable in other directions; which is modeled using loss coefficients whose values are three orders of magnitude higher than in the X direction.Setup and SolutionStep 1: Grid1. Read the mesh file catalytic converter.msh.File /Read /Case...2. Check the grid. Grid /CheckFLUENT will perform various checks on the mesh and report the progress in the console. Make sure that the minimum volume reported is a positive number.3. Scale the grid.Grid Scale...a Select mm from the Grid Was Created In drop-down list.b Click the Change Length Units button. All dimensions will now be shown in millimeters.c Click Scale and close the Scale Grid panel.4. Display the mesh. Display /Grid...a Make sure that inlet; outlet; substrate-wall; and wall are selected in the Surfaces selection list.b Click Display.c Rotate the view and zoom in to get the display shown in Figure 7.2.d Close the Grid Display panel.The hex mesh on the geometry contains a total of 34;580 cells.Step 2: Models1. Retain the default solver settings. Define /Models /Solver...2. Select the standard k-ε turbulence model. Define/ Models /Viscous...Step 3: Materials1. Add nitrogen to the list of fluid materials by copying it from the Fluent Database for materials.Define /Materials...a Click the Fluent Database... button to open the Fluent Database Materials panel.i. Select nitrogen n2 from the list of Fluent Fluid Materials.ii. Click Copy to copy the information for nitrogen to your list of fluid materials. iii. Close the Fluent Database Materials panel.b Close the Materials panel.Step 4: Boundary Conditions. Define /Boundary Conditions...1. Set the boundary conditions for the fluid fluid.a Select nitrogen from the Material Name drop-down list.b Click OK to close the Fluid panel.2. Set the boundary conditions for the substrate substrate.a Select nitrogen from the Material Name drop-down list.b Enable the Porous Zone option to activate the porous zone model.c Enable the Laminar Zone option to solve the flow in the porous zone without turbulence.d Click the Porous Zone tab.i. Make sure that the principal direction vectors are set as shown in Table7.1. Use the scroll bar to access the fields that are not initially visible in the panel.ii. Enter the values in Table 7.2 for the Viscous Resistance and Inertial Resistance. Scroll down to access the fields that are not initially visible in the panel.e Click OK to close the Fluid panel.3. Set the velocity and turbulence boundary conditions at the inlet inlet.a Enter 22.6 m/s for the Velocity Magnitude.b Select Intensity and Hydraulic Diameter from the Specification Method dropdown list in the Turbulence group box.c Retain the default value of 10% for the Turbulent Intensity.d Enter 42 mm for the Hydraulic Diameter.e Click OK to close the Velocity Inlet panel.4. Set the boundary conditions at the outlet outlet.a Retain the default setting of 0 for Gauge Pressure.b Select Intensity and Hydraulic Diameter from the Specification Method dropdown list in the Turbulence group box.c Enter 5% for the Backflow Turbulent Intensity.d Enter 42 mm for the Backflow Hydraulic Diameter.e Click OK to close the Pressure Outlet panel.5. Retain the default boundary conditions for the walls substrate-wall and wall and close the Boundary Conditions panel.Step 5: Solution1. Set the solution parameters. Solve /Controls /Solution...a Retain the default settings for Under-Relaxation Factors.b Select Second Order Upwind from the Momentum drop-down list in the Discretization group box.c Click OK to close the Solution Controls panel.2. Enable the plotting of residuals during the calculation. Solve/Monitors /Residual...a Enable Plot in the Options group box.b Click OK to close the Residual Monitors panel.3. Enable the plotting of the mass flow rate at the outlet.Solve / Monitors /Surface...a Set the Surface Monitors to 1.b Enable the Plot and Write options for monitor-1; and click the Define... button to open the Define Surface Monitor panel.i. Select Mass Flow Rate from the Report Type drop-down list.ii. Select outlet from the Surfaces selection list.iii. Click OK to close the Define Surface Monitors panel.c Click OK to close the Surface Monitors panel.4. Initialize the solution from the inlet. Solve /Initialize /Initialize...a Select inlet from the Compute From drop-down list.b Click Init and close the Solution Initialization panel.5. Save the case file catalytic converter.cas. File /Write /Case...6. Run the calculation by requesting 100 iterations. Solve /Iterate...a Enter 100 for the Number of Iterations.b Click Iterate.The FLUENT calculation will converge in approximately 70 iterations. By this point the mass flow rate monitor has attended out; as seen in Figure 7.3.c Close the Iterate panel.7. Save the case and data files catalytic converter.cas and catalytic converter.dat.File /Write /Case & Data...Note: If you choose a file name that already exists in the current folder; FLUENTwill prompt you for confirmation to overwrite the file.Step 6: Post-processing1. Create a surface passing through the centerline for post-processing purposes.Surface/Iso-Surface...a Select Grid... and Y-Coordinate from the Surface of Constant drop-down lists.b Click Compute to calculate the Min and Max values.c Retain the default value of 0 for the Iso-Values.d Enter y=0 for the New Surface Name.e Click Create.2. Create cross-sectional surfaces at locations on either side of the substrate; as well as at its center.Surface /Iso-Surface...a Select Grid... and X-Coordinate from the Surface of Constant drop-down lists.b Click Compute to calculate the Min and Max values.c Enter 95 for Iso-Values.d Enter x=95 for the New Surface Name.e Click Create.f In a similar manner; create surfaces named x=130 and x=165 with Iso-Values of 130 and 165; respectively. Close the Iso-Surface panel after all the surfaces have been created.3. Create a line surface for the centerline of the porous media.Surface /Line/Rake...a Enter the coordinates of the line under End Points; using the starting coordinate of 95; 0; 0 and an ending coordinate of 165; 0; 0; as shown.b Enter porous-cl for the New Surface Name.c Click Create to create the surface.d Close the Line/Rake Surface panel.4. Display the two wall zones substrate-wall and wall. Display /Grid...a Disable the Edges option.b Enable the Faces option.c Deselect inlet and outlet in the list under Surfaces; and make sure that only substrate-wall and wall are selected.d Click Display and close the Grid Display panel.e Rotate the view and zoom so that the display is similar to Figure 7.2.5. Set the lighting for the display. Display /Options...a Enable the Lights On option in the Lighting Attributes group box.b Retain the default selection of Gourand in the Lighting drop-down list.c Click Apply and close the Display Options panel.6. Set the transparency parameter for the wall zones substrate-wall and wall.Display/Scene...a Select substrate-wall and wall in the Names selection list.b Click the Display... button under Geometry Attributes to open the Display Properties panel.i. Set the Transparency slider to 70.ii. Click Apply and close the Display Properties panel.c Click Apply and then close the Scene Description panel.7. Display velocity vectors on the y=0 surface.Display /Vectors...a Enable the Draw Grid option. The Grid Display panel will open.i. Make sure that substrate-wall and wall are selected in the list under Surfaces.ii. Click Display and close the Display Grid panel.b Enter 5 for the Scale.c Set Skip to 1.d Select y=0 from the Surfaces selection list.e Click Display and close the Vectors panel.The flow pattern shows that the flow enters the catalytic converter as a jet; with recirculation on either side of the jet. As it passes through the porous substrate; it decelerates and straightens out; and exhibits a more uniform velocity distribution.This allows the metal catalyst present in the substrate to be more effective.Figure 7.4: Velocity Vectors on the y=0 Plane8. Display filled contours of static pressure on the y=0 plane.Display /Contours...a Enable the Filled option.b Enable the Draw Grid option to open the Display Grid panel.i. Make sure that substrate-wall and wall are selected in the list under Surfaces.ii. Click Display and close the Display Grid panel.c Make sure that Pressure... and Static Pressure are selected from the Contours of drop-down lists.d Select y=0 from the Surfaces selection list.e Click Display and close the Contours panel.Figure 7.5: Contours of the Static Pressure on the y=0 planeThe pressure changes rapidly in the middle section; where the fluid velocity changes as it passes through the porous substrate. The pressure drop can be high; due to the inertial and viscous resistance of the porous media. Determining this pressure drop is a goal of CFD analysis. In the next step; you will learn how to plot the pressure drop along the centerline of the substrate.9. Plot the static pressure across the line surface porous-cl.Plot /XY Plot...a Make sure that the Pressure... and Static Pressure are selected from the Y Axis Function drop-down lists.b Select porous-cl from the Surfaces selection list.c Click Plot and close the Solution XY Plot panel.Figure 7.6: Plot of the Static Pressure on the porous-cl Line SurfaceIn Figure 7.6; the pressure drop across the porous substrate can be seen to be roughly 300 Pa.10. Display filled contours of the velocity in the X direction on the x=95; x=130 and x=165 surfaces.Display /Contours...a Disable the Global Range option.b Select Velocity... and X Velocity from the Contours of drop-down lists.c Select x=130; x=165; and x=95 from the Surfaces selection list; and deselect y=0.d Click Display and close the Contours panel.The velocity profile becomes more uniform as the fluid passes through the porous media. The velocity is very high at the center the area in red just before the nitrogen enters the substrate and then decreases as it passes through and exits the substrate. The area in green; which corresponds to a moderate velocity; increases in extent.Figure 7.7: Contours of the X Velocity on the x=95; x=130; and x=165 Surfaces11. Use numerical reports to determine the average; minimum; and maximum of the velocity distribution before and after the porous substrate.Report /Surface Integrals...a Select Mass-Weighted Average from the Report Type drop-down list.b Select Velocity and X Velocity from the Field Variable drop-down lists.c Select x=165 and x=95 from the Surfaces selection list.d Click Compute.e Select Facet Minimum from the Report Type drop-down list and click Compute again.f Select Facet Maximum from the Report Type drop-down list and click Compute again.g Close the Surface Integrals panel.The numerical report of average; maximum and minimum velocity can be seen in the main FLUENT console; as shown in the following example:The spread between the average; maximum; and minimum values for X velocity gives the degree to which the velocity distribution is non-uniform. You can also use these numbers to calculate the velocity ratio i.e.; the maximum velocity divided by the mean velocity and the space velocity i.e.; the product of the mean velocity and the substrate length.Custom field functions and UDFs can be also used to calculate more complex measures ofnon-uniformity; such as the standard deviation and the gamma uniformity index.SummaryIn this tutorial; you learned how to set up and solve a problem involving gas flow through porous media in FLUENT. You also learned how to perform appropriate post-processing to investigate the flow field; determine the pressure drop across the porous media and non-uniformity of the velocity distribution as the fluid goes through the porous media.Further ImprovementsThis tutorial guides you through the steps to reach an initial solution. You may be able to obtain a more accurate solution by using an appropriate higher-order discretization scheme and by adapting the grid. Grid adaption can also ensure that the solution is independent of the grid. These steps aredemonstrated in Tutorial 1.。