当前位置:首页 >> 能源/化工 >>

FLUENT中百叶窗的模拟


Solution 1396 FLUENT 6 - how to use porous media to model louvers used in windows

Product Version No.

Fluent6 6.2.23

Problem:
Given the pressure loss vs

velocity characteristics for the louvers used for windows, how can one replace the louvers with porous media such that the presure drop matches AND the flow is turned? The velocity is the approaching velocity instead of velocity inside the louvers.

Resolution:
Since the flow is bended in louvers, care must be taken to ensure that the correct velocity and porous media length is used in the porous media coefficients calculation. The correct velocity is the velocity in the louvers not the approaching velocity, and the correct length is along the louver direction. The porous media directions have to be specified along the louver direction to bend the flow.

After the above, an additional udf is needed to bend the flow in the porous media without introducing additional loss. Otherwise, due to the bend, additional loss will be introduced and the pressure drop from porous media approach will be more than the data. The udf used is as follows:

/*********************** UDF to bend the flow without pressure increase **********************

This udf can bend the flow without pressure increase. This is used for certain porous media application. For example, one wants to replace the louvers with porous media. One can do the experiments or CFD to determine the pressure drop as a function of velocity. And then replace the louvers with porous model after calculating the porous media coefficients. This is the standard approach to use porous media. However, this approach gives problems if one wants to turn the flow due to the louvers. If so, the principle axis of the porous media will be inclined with the incoming flow. Care must be excised not to use the incoming velocity for the coefficients calculation. After that, the pressure drop in the flow will still be much larger than from the experiments. This is because the flow needs to be bended right at the inlet of the porous media. That bending is physical. The problem is that the pressure loss due to the bending of the flow is already considered in the porous media coeff. The bending in the CFD setup means that the bending is accouted for twice. To avoid this issue, a udf is needed right at the inlet of the porous media model to bend the flow without causing pressure drop. The way to achieve that is to make the cells at the inlet of porous media believe that the flow is inclinded. The momentum flux deficit at the inlet of the porous media

is calcuated based on that. The momentum flux is then converted to momentum source term and added to first layer of cells at the porour zone

How to use the udf:

- Set the case with porour media - Define two user defined memory - Provide the face zone ID of the interior face zone at the inlet of porous media - Provide the angle that needs to be bended. This has to be corresponding to the porous media principle axis. - Compile the udf - Hook the ADJUST udf and the momentum source.

Known limitation of the udf:

- The udf is hard coded for flow coming in x direction. So, only y momentum source is needed. For more general orientation, both x, y momentum source is needed for a 2d case.

Written by: Xiao Hu (xh@fluent.com) Last updated: 8/1/2006

*************************************************************************************/

#include "udf.h"

#define face_ID 1 #define ANGLE 30 /*degree*/

DEFINE_ADJUST(my_adjust,d) { Thread *tf; face_t f; Domain * domain; real area[2], vol, x_vel, density;

domain = Get_Domain(1); tf = Lookup_Thread(domain, face_ID);

begin_f_loop(f,tf) { F_AREA(area, f, tf); vol = C_VOLUME(F_C0(f,tf), THREAD_T0(tf)); x_vel = C_U(F_C1(f,tf), THREAD_T1(tf)); density = C_R(F_C1(f,tf), THREAD_T1(tf));

/* Momentum flux deficit calculation. It is divided by vol because flux needs to be converted to a source term. */

C_UDMI(F_C0(f,tf),

THREAD_T0(tf),

0)

=

density*x_vel*x_vel*tan(ANGLE*M_PI/180)*MAG(area)/vol;

C_UDMI(F_C0(f,tf), THREAD_T0(tf), 1) = 2*x_vel*density*tan(ANGLE*M_PI/180)*MAG(area)/vol;

} end_f_loop(f,tf)

}

DEFINE_SOURCE(ymom_source,c,t,dS,eqn) { dS[eqn] = C_UDMI(c,t,1);

return C_UDMI(c,t,0); }


相关文章:
FLUENT中百叶窗的模拟
FLUENT中百叶窗的模拟_能源/化工_工程科技_专业资料。本文介绍了如何使用FLUENT软件,编写用户自定义程序,模拟流体穿过百叶窗的流动。Solution...
fluent 传热模拟
FLUENT 在能量方程中忽略了粘性 生成热(各个耦合求解器总是包含有粘性生成热) ...半透明边界条件适合于诸如飞机上的玻璃窗的模拟。 DO 模型的漫射壁面边界条件 ...
第六章 FLUENT中的燃烧模拟
第六章 FLUENT中的燃烧模拟_工学_高等教育_教育专区。第六章 FLUENT中的燃烧模拟 第六章,FLUENT 中的燃烧模拟 6.1 燃烧模拟的重要性 ? ? 面向实际装置(如...
FLUENT喷雾模拟具体步骤
FLUENT喷雾模拟具体步骤_数学_自然科学_专业资料。用FLUENT进行喷雾器等涉及雾化的...面板中的Unsteady Parameters 属性框中激活了Unsteady Tracking 选项,在瞬态流动中...
fluent 模拟例子
fluent 模拟例子_工学_高等教育_教育专区。第一章 一维稳态导热的数值模拟一、模拟实验目的和内容本模拟实验的目的主要有 3 个: (1)学生初步了解并掌握 Fluent ...
FLUENT 6 计算模拟过程方法及步骤
FLUENT 12 模拟步骤 Problem Setup 读入网格:file read case 选择网格文件(后缀为。Mesh) 1 General 1)Mesh(网格) > Check(点击查看网格的大致情况,如有无负...
fluent的一个实例(波浪管道的内部流动模拟).
二、 周期性波浪管道模型的数值模拟 图 15 周期性网格 网格密度与完全管道网格相同。 在 fluent 中输入以下指令,创建周期性网格。 /grid> modify-zones /grid/...
FLUENT算例 (9)模拟燃烧
计算流体力学作业 FLUENT 模拟燃烧 组分传输与气体燃烧问题描述:长为 2m、直径为 0.45m 的圆筒形燃烧器结构如图 1 所示,燃烧筒壁上嵌有 三块厚为 0.0005 m...
Fluent 模拟中常见问题及解决办法,非常适合新手
Fluent 模拟中常见问题及解决办法,非常适合新手_计算机软件及应用_IT/计算机_专业资料。对于新手,总结的模拟中常见问题以及解决办法,值得一看 ...
Fluent数值模拟步骤
Fluent 数值模拟的主要步骤使用 Gambit 划分网格的工作: 首先建立几何模型,再进行网格划分,最后定义边界条件。 Gambit 中采用的单位是 mm,Fluent 默认的长度是 m。...
更多相关标签:
fluent中模拟空气流动 | 在fluent中空化模拟 | fluent可以中固流模拟 | fluent燃烧模拟实例 | fluent温度场模拟 | fluent模拟颗粒沉降 | fluent传热模拟实例 | fluent大涡模拟算例3d |