各位大侠们，关于用fluent模拟类似换热器的问题...

lala0910

大家好，小女子最近在模拟一个类似于管壳换热器的例子...如下图
，

图一

，水在水套中流动，下进上出，碳由上自下，进行热交换，达到碳的冷却。
而在fluent计算过程中，总是出现如下错误，
Error: divergence detected in AMG solver: pressure correction
Error Object: ()
我也将松弛因子改小了，还是出现这种错误。
刚开始做的时候，我只模拟二者的速度，是没有问题的，只要一加入换热问题，就死活不出结果，请高人指点啊。。。。。

Heidiadalheid

这个错误一般是由于网格质量差或者边界条件不合理造成的
如果是一开始就出现这样的错误，一般式边界条件造成的
如果是计算到一定步骤后出现这样的错误，这基本可以排除边界条件的原因。最大的可能是局部的网格不佳，你可以从调整压力松弛因子，跌代次数以及误差入手，当然根本办法还是从新构建更加合理的网格

以下是老外关于类似问题的回复，你可以参考一下。

I try to study the turbulence inside a vertical cylinder. In a first time, I take the case of steady flow. The air is introduced axially from below, deflected by means of a small conical deflector and thanks to the geometry of the chamber the air goes up into the cylinder. I take the ideal gas law, k-epsilon model, inlet and outlet pressure for boundary conditions. My problem is that I have directly the message "divergence detected in AMG solver : k when I want to iterate. I try a lot of solutions I have find in this forum without any result. Could anyone help me? Thanks in advance Check your hardware, especially RAM sockets. I have experience, that this could be initiated by some bad memory address sectors. I had a similar problem, but with pressure correction. I found that I had some highly skewed cells. Once I corrected the highly skewed cells by adapting the iso-values of cell skewness my case began to iterate. Perhaps this may be your problem. First initialize the solution and then go to contours grid and select equiangle skew and click compute to get you min and maxs. Having skewed cells of 0.9 or higher isn';t good, as in my case. Hope this helps I have check the skewed cells but it appears that in my case, this number is lower than 0.4 Is it to high? divergence in AMG solver Posted By: Steffen Date: Mon, 22 Nov 2004, 6:38 a.m. Hi. I have a simulation of a supersonic-valve running but the program shows me this message: divergence detected in AMG solver: temperature I tried to rise the limits for temperature and other solution limits but nothing has helped so far Does anyone what to do thanx Try to use more conservative Under-relaxation factor. I had the same problem with a wing in a transonic flight. According to me the segregated solver is not suitable for the conditions with high compressibility. Let me know if you succeed in using the segregated and how... I suggest using the coupled solver，Your problem will vanish... Hope to hear good news from you soon. Luca this will be something wrong with the either boundary condition or with model selection, generally if things are right fluent just converges fine without any warning or problem. in my opinion these are the signs that you are doing something wrong in settign up the case, look closely Hi, I have the same problem, and couldn't solve it by using the coupled solver. Is there any other possible way. I am simulating office room problem. It seems very simple but on every stage it is creating problems for me. I am going to try to change the underrelaxation. lets see what comes up. Thanks long ago, one of my friend was doing CFD analysis of a kitchen,, using coupled solver, and he faced the same problem, for some time he didn’t get the converged results. Finally when I looked at his mesh. It seemed the problem is with the mesh not with the solver settings. I suggested him to make mesh more finer, and viola it gave results in one run, without any problem. so moral of the story check your mesh. My mesh is quite fine, but I will try more finer mesh. Thanks then it shall converge ..anyway have you tried using segregated solver, how the results with that Error: Divergence detected in AMG solver? Posted By: frank Date: Sun, 16 Jan 2005, 3:58 p.m. What does mean and how do i fix it? I am runing a rosseland radiation model and it wont run past 1 iteration. Frank you are using the segregated solver, so you must reduce the under relaxation factor as you can. You could have a grid issue concerning high skewness. This can be checked by going to contours grid cell equiangle skew and select compute and check the min and max. You should be below .9. If over t5hen this could be your problem. It has happened to me a couple of times. thanks a million i will try this... frank AMG solver: k divergence? Posted By: Robert Date: Sun, 9 Mar 2003, 11:23 a.m. How do I remedy a divergence with this message. This is for scramjet combustion in 2D with injectors on both the top and bottom. Is there any way to look up error messages? reduce underalaxtion factor. I have tried reducing the underelaxation factors but the divergence persists. Any other suggestions? Perhaps in the AMG solver Menu? It looks like a problem with your boundary conditions, be sure they';re compatible with each other and consistent with the physics of what you';re trying to simulate, I think you';d better don';t touch anything in the AMG menu, unless you know exactly what you're doing, It is my opinion, if this could help.

Seventy721

看似很象CFD online里面的一篇，好像以前看过。

Seventy721

如果楼主只算速度没有问题，不妨先认真检验一下流速计算的结果是否符合实际情况。特别注意狭窄空间处、靠近管壁处、以及有较大曲率的表面处的网格质量。如果发现速度矢量有异常分布，比如垂直于管壁，或者边界层附近流速远远高于/低于应有的值，或者湍流强度过高，说明网格本身有问题。如果这些都正常，则可以考虑加上传热后更换一种压力离散算法。或者楼主读读fluent帮助25.4.1节，没准会有帮助。