Fluent计算热耦合问题

2016-09-20 by:CAE仿真在线来源:互联网

问题:在设定边界条件的时候,固体和液体相接触的那个面如何设定?有人建议设为interface,但好象是用于滑移网格的,在计算的时候出错说明设为INTERFACE是错误的,那么应该怎么设定呢?

好象设置成WALL就可以了,没有什么特别的!
在fluent里面怎么设定WALL的性质呢?我又不知道它的实际温度?
耦合是不需要设置的interface是两边网格不是conform时才使用,又不是真真的边界条件,更不是你所要求的固液交界面。你既然设定完材料属性,固体和液体,还需要设置吗?
可以把整个管道设置为WALL的边界条件,WALL的厚度为管道壁的厚度,管道材料的属性如导热系数等可以自己在MATERIAL里定义,计算时只要知道传送介质的温度和管道外界的温度等边界条件,在管道WALL的边界条件选COUPLE,就可以耦合管道内外温度进行求解,最近正在采用这种办法进行计算。
我是用phoenics软件的,但是最近也是需要解决一些耦合的问题,我想请教一个问题:
管道WALL的边界条件选COUPLE是不是因为它的边界既有传送介质的温度边界,也有管道外界的温度边界的原因??
我认为如果上面的问题你的回答是肯定的话,你的这种做法根本行不通,主要原因在于传送介质的温度你根本没办法知道的,这就是耦合问题跟别的不同的地方所在!我用的是fluent,个人认为,其中的couple求解可能就是因为流动方向的温度分布事先并不知道,比如求解管壁内外的对流和管壁的导热传热,这时可能就要用到couple了,这种求解估计就是根据定义的边界条件,逐步迭代求解流动方向上各节点的温度分布的
不过fluent中的用couple的边界条件求解感觉有点太傻瓜化了,自己验证了好多case,结果总是不能令人完全信服,搞的问题太复杂了。看看陶教授的数值传热学后面一章的流固耦合问题
另外,如果你把"整个管道设置为WALL的边界条件"
你怎么在这个固体WALL来MAPPING MESH,又怎么可以算出这个固体WALL里面的温度梯度呢?
一点必须注意的就是:你的计算NODES只是在计算区域,不是在WALL.
耦合计算就是不需要设置,建体的时候用split将流体域和固体域分开,两者共面,分别设定成fluid和solid后,自动将两者的交界面定义成coupled边界条件,不需要再指定。wall可以指定厚度,一般我都是安实际尺寸画出网格作为计算域一部分进行计算。好像就是这样,没有他说得那么复杂。这种壁面可以不用设置的。网格当然在gambit里面建了,边界条件给定和计算当然在Fluent里面进行了。
其实关于TWO SIDE WALL的热边界条件设定问题,FLUENT里的UG写得很清楚,的确不需要再设置其他条件,WALL的厚度也是可以设置的,以下是FLUENT的UG里的描述:

Thermal Conditions for Two-Sided Walls
If the wall zone has a fluid or solid region on each side, it is called a``two-sided wall''. When you read a grid with this type of wall zone intoFLUENT, a ``shadow'' zone will automatically be created so that each side ofthe wall is a distinct wall zone. In the Wall panel, the shadow zone's namewill be shown in the Shadow Face Zone field. You can choose to specifydifferent thermal conditions on each zone, or to couple the two zones:
To couple the two sides of the wall, select the Coupled option under ThermalConditions. (This option will appear in the Wall panel only when the wall is atwo-sided wall.) No additional thermal boundary conditions are required,because the solver will calculate heat transfer directly from the solution inthe adjacent cells. You can, however, specify the material type, wallthickness, and heat generation rate for thin-wall thermal resistancecalculations, as described above. Note that the resistance parameters you setfor one side of the wall will automatically be assigned to its shadow wallzone. Specifying the heat generation rate inside the wall is useful if, forexample, you are modeling printed circuit boards where you know the electricalpower dissipated in the circuits but not the heat flux or walltemperature.
To uncouple the two sides of the wall and specify different thermal conditionson each one, choose Temperature or Heat Flux as the thermal condition type. (Convection and Radiation are not applicable for two-sided walls.) Therelationship between the wall and its shadow will be retained, so that you cancouple them again at a later time, if desired. You will need to set therelevant parameters for the selected thermal condition, as described above. Thetwo uncoupled walls can have different thicknesses, and are effectivelyinsulated from one another. If you specify a non-zero wall thickness for theuncoupled walls, the thermal boundary conditions you set will be specified on theouter sides of the two thin walls, as shown in Figure 6.13.3,where is the Temperature (or is the Heat Flux) specified on one wall and is theTemperature (or is the Heat Flux) specified on the other wall. and are thethermal conductivities of the uncoupled thin walls. Note that the gap betweenthe walls in Figure 6.13.3 is not part of the model; it is included in thefigure only to show where the thermal boundary condition for each uncoupledwall is applied.
虽然如此,但是FLUENT在处理流固耦合问题时,的确很弱,如果只关心流体的问题,可以用FLUENT算,如果流体和固体问题都很重要。个人觉得还是用ANSYS计算比较可行,个人观点。
至于INTERFACE边界条件,在FLUENT里只有采用滑移网格才能使用。

开放分享：优质有限元技术文章,助你自学成才