1 这个应该是湍流模型的选取与第一层网格高度之间不满足近壁处理关系而产生的问题，如果你没有使用壁面函数的话，第一层网格高度尽可能地小点儿，比如取为弦长的百万分之一左右；另外，边界条件中关于湍流量的设置不合理也会导致这个警告。

2 （不推荐）solve-controls-limits Maximum Turb. Viscosity Ratio 加多两个0，估计是一些单元的最大Turb. Viscosity Ratio超出了限定值

（）恕我直言，你的这个方法只是治标不治本，他这个问题多数是由于网格尺度太大引起的。也可能是边界条件上的湍流相关参数不合理导致的。[br][br][以下内容由 larky 在 2007年06月23日 00:00am 时添加] [br] 
调大限制值可能导致发散

3 这是一个办法，能够解决一部分问题，有一些问题无论你怎么调整都没有用，如果出现这种情况可以通过调整初始流场，找到合适的初始值大部分能够解决，其实如果只是一开始初现这个问题，可以不作调整，除非影响到收敛性

4 在别的论坛上看到的：
为了尽快收敛对异常的数值进行的限制，对最后收敛结果无影响
1）如果边界条件设置合理，一般来说会在收敛后自动消除。
2）为了加快收敛对异常的数值进行的限制（以引用2楼），是加快收敛的一种措施。
3）但是如果你的问题中流场变化很大，有可能在最有还会有。
4）如果网格不好会经常出现这种现象。
5）如果不想看见它总是报告而影响计算速度（写屏会降低计算速度），可以在下面把它关闭：
  solve->control->flow limit....具体记不住了，自己看看就知道了。

5 我也遇到这种情况,不过是在叠代求解的前一百多步,后面就没有了.因此我想是否是因为前面计算的误差大引起?而随着计算误差的减少,就消失了.如果是这样,就可以放心啦.

6 一般是边界上或是网格质量差的地方出现了奇点.由于是数值耗散,随着迭代次数越多,影响整个流场的范围越大,最终可能导致这个流场发散.
如果是网格质量差的地方出现,就只能重划网格了
如果是在边界上,一般是湍流相关参数设置不合理造成的,改成固定湍流比可能能解决

7  Why don't you try as follows (If you still have the same warning, please go to the next step. Usually, the initail flow condition used for the RSM run is obtained from the RNG k-e model result);

First step:
Solve - Controls - Solution -Default => iteration

Second Step:
Decrase "Under-relaxation factors" => iteration

Third Step:
Adaptation of cells : I usaually use y+ and velocity gradient conditions => iteration

Fourth Step: Regenerate mesh, goto step 1
If your solution stats to converge, you can increase under-relaxation factors.

If you have converged solutions, you can increase the order of the discretization parameters (for ex. 1st -> 2nd -> QUICK etc.)

8，  once i posted a big message on this issue, i am pasting that message again, you can read this:

{

well this is one common problem lot of people have asked about it before. i will try to summarize the approach i take to solve this problem.

first of all, the very basic cause of this warning is the wrong set up of boundary conditions. So if you are sure that nothing is wrong with the set up of the problem, you can follow the following things.

The origin of the problem lies in the fact that if the solver calculates the value of k and e or omega (in two equation models) wrongly, its very likely it will calculate turbulent viscosity wrongly and thus we get the warning. In the ideal condition, as the solution converges the warning should go away and we all live happily ever after. But generally this does not have so happy ending. The reason is mainly we have a case which is very large and convergence is already difficult and which is exacerbated by the wrong calculations of turbulent quantities. So what are the remedies for it.

The usual remedy is to switch to coupled solver, and work with it, and this usually solves the problem. But my personal thinking is that if the case is incompressible the coupled solver may not work well there. But yes this is one solution. The second solution which is far more stable is, and if you fail to get the solution from coupled solver too, switch to FAS, increase the number of pre post iterations, make the coarsening levels to 4, (4 is more than enough). And this converges almost every problem, but there are case where you might fail to get convergence.

Anyway if you are stuck with segregated solver (like me), what are the options.

First of all if we consider that the divergence is because of turbulence quantities, we may want to force the convergence on these quantities before we move to next iteration.

The way I do is this, I change the multigrid options for k, e to V cycle, make the pres sweeps to 1 post sweeps to 2, and chose Bicgstab as smoother. And let it run.

Sometimes I just want to first get the best approaximation of k,e for the flow field I have, for this I usually switch off the solver for momentum equations and just solve for k,e or k, omega till I get warning free turbulent field, then I switch on all the equations and go on to iterate further.

This approach works well, but it has one problem. if the mesh size is very large say around 3 million cells then even to first get the turbulent quantities to converge might take day or two. So what to do in this case.

Whenever I have to do calculations for the cases around 2-3 million cells, I make two meshes one very very coarse, with same boundary conditions as finer mesh (which is of course around 3 million cells). Now first I get converged solution on coarse mesh, which I can get in hour or two. Then go to file->interpolate, and write the data for corresponding zones, and then when you read the fine mesh read this initial guess from same file->interpolate->read.

And here switch off the momentum calculations do some calculations only for turbulent quantites, (if u get viscocity warning, it will soon go away, though I never got warning here since the solution is already converged), so after say 3-4 calculations switch on solver for all the quantities and go on to iterate, you will get converged solution.

(well on coarse grid you can use FAS to force convergence, its quite handy there).

Hope this will be useful.

}