fluent模拟是否一定要收敛

fluent模拟是否一定要收敛

当然；
收敛一般情况会以残差曲线为标准；
我们使用Fluent,就是为了求连续方程,动量方程（N-S方程）以及能量守恒方程；
在求解这三个微分方程时,都是采用迭代方法进行迭代.对于同一个节点的同一个物理值,第N次迭代的结果是c1,第N+1次迭代的结果是c2,那该点同一个物理值的残值就可以定义为c2-c1.
当然这个残差越小越好,没有一定的标准,但一般会要求小于10-3,即可认为收敛；
或监测一个面的速度（或者是压力等参数）基本上不随着计算时间的推移而变化,就认为基本达到收敛；
建议了解有限体积的计算过程,Fluent的计算过程,多看看计算流体力学书；

不收敛的话，那求解的结果是什么，谁也不知道
当然收敛的标准没有明文规定

说需要收敛的都是没做过实际工作的人，鄙视。。
不一定要收敛，因为收敛的标准是人为给出的，而收敛性和网格质量，计算模型，控制方程的复杂程度都有关系。
对于复杂模型，如果计算到最后收敛曲线在小范围震荡，而计算结果也大致正确，那么这个结果就是可用的。但是注意只是可用，由于收敛精度较低，所以计算结果和实际解存在一定的偏差。但是一般来说，这个偏差是可以接受的。...

全部展开

说需要收敛的都是没做过实际工作的人，鄙视。。
不一定要收敛，因为收敛的标准是人为给出的，而收敛性和网格质量，计算模型，控制方程的复杂程度都有关系。
对于复杂模型，如果计算到最后收敛曲线在小范围震荡，而计算结果也大致正确，那么这个结果就是可用的。但是注意只是可用，由于收敛精度较低，所以计算结果和实际解存在一定的偏差。但是一般来说，这个偏差是可以接受的。

收起

There's a few things that could be going on.
One possible answer is that your model is converged (that's always the happiest answer, isn't it?). The residuals you are looking at are normalized bas...

全部展开

There's a few things that could be going on.
One possible answer is that your model is converged (that's always the happiest answer, isn't it?). The residuals you are looking at are normalized based on the residuals of the first iteration. So if your initial guess is pretty accurate, then your first residuals will be small, and all of your following residuals will be small as well, but since they are normalized according to that first small value, they look large. This typically shows up in the continuity and momentum residuals, and sometimes even in the x, y, and z velocity residuals (at least in the coupled solver). One thing you should be doing with your model is monitoring other factors besides your residuals. If you're looking for the pressure distribution, then define a few points along your airfoil and monitor the pressure at these points. You should also monitor at least the lift of your airfoil. You can find these monitors under solve->monitors. Judge convergence by when these have leveled off. While your model is solving, you will probably have to go in and clear the data in the monitors or adjust the scale of the axis to get a better idea of when they've truly leveled off. That can all be done in the windows where you defined the monitors.
Another possibility is that your model isn't converged (the less happy of the answers). If that's the case, then there's lots of possible reasons. One common one is the use of the Coupled Solver in low speed flows. Since the coupled solver is a density based solver, it can get hung up in incompressible flow regimes. Typically, I only use the coupled solver for flows over Mach 0.7, but I've used the segregated solver from Mach 0.05 up to Mach 1.2 (paying CAREFUL attention to the mesh where shocks form). Another possible problem is that its an unsteady problem. If you've stalled, you could be shedding vortices at some frequency. The SA turb model does alright with small separation regions, but a large separation region (say behind a shock at some angle of attack) can cause it to fall apart. It was originally designed for 2D airfoils without any separation. They've modified it some to try and make it work in 3D, and to try and help it handle separation, but I still haven't had much luck with it. There could also be some issues with your mesh. Pay attention to your y+ values and the rules concerning them.
Either way, you really should be monitoring more than the residuals to judge convergence. I've seen it a lot here, where someone will call a model converged because the residuals dropped below 1e-03, but when I've taken the model and continued with the iterations, I've seen a dramatic change in the forces. I've also seen it where someone will be 8 or 9 thousand iterations in trying to get the residuals to drop, but the forces have been steady.
Hope this helps, and good luck,
Jason

收起