fluent用LES算水翼边界层选择中心差分引起的震荡如何消除
-
感谢李老师的及时回复！目前情况是这样
- https://aip.scitation.org/doi/pdf/10.1063/1.5045795 文献引用的文献[23]提到了一种filter,但是并不清楚怎样应用到fluent
- 试过dynamic也会震荡，貌似跟模型无关，因为要算边界层还是主要用WALE
3.目前fluent自带的差分格式包括upwind, 2nd upwind, 3ord MUSCL, quick, bound cd 和cd都试了，只有cd能比较精确的算准边界层的速度剖面和脉动强度，检索到涉及定量分析边界层的文献比如槽道流动，平板流动，绝大多数也是用的中心差分，只是雷诺数都偏低。
震荡并不影响边界层平均速度和脉动与实验的对照，但是瞬时流场会有这样的锯齿形状，所以Q涡显示时会有一些非物理的碎涡出现，怎么都感觉会对后处理有影响。。
-
有试过二阶中心差分格式中耦合小部分一阶迎风格式吗，比如给个0.02%的一阶迎风格式，之前用fluent算3900的圆柱绕流，用纯二阶中心出现过数值振荡容易发散的情况，改成混合之后收敛性好很多，精度也还行，没有很明显的下降
-
@cccrrryyy 直接用TUI命令：
solve/set/numerics/
一直回车到1-st order to higher order blending factor: 1就是纯二阶，0.98就是耦合0.02的一阶迎风
感觉有点像TVD格式，也不是很懂，导师之前教我的操作，具体也不是太懂
-
感谢老铁的建议，我查了查好像没有这种现成的耦合操作，bounded cd可能是最像的，但是经过计算发现在边界层应该是全部切换成迎风格式了，没有部分耦合这种机制。
在国外cfd论坛上找到一个相似的情况，幸运的是那个人好像不关注边界层就改成迎风就没有震荡了，我看有个人的回答也解释了为什么除了中心差分都算不太准边界层。。
The choice of the scheme for LES should be based on the numerical diffusion it introduces. Ideally you should use linear（中心差分）, or cubic. You need good and prett uniform mesh anyways for LES, since you are assuming the filter operator and the differential operator are commutative, which is not true on non-uniform grids! The filtered schemes are a last resort scheme in my view, if you can't really do better with your mesh. Upwind and linearUpwind, but also limitedLinear and QUICK should be avoided because they are too dissipative.
可惜就是无法消除震荡
-
@李东岳 https://www.cfd-online.com/Forums/openfoam-solving/106700-dicretization-schemes-les-pitzdaily.html 李老师，这是钝体扰流那个原贴，里面好像发了几个算例文件，不过我Openfoam水平有限，您可以参考下帖子
-
试了下，把水的粘性增大了一百倍，也就是雷诺数降了100倍，震荡就没有了，但是边界层整个就加厚了几十倍。。难道高雷诺数下解析边界层是无解的吗
-
@李东岳 谢谢李老师
您有时间的话可以试试foam的中心差分格式，我用CFX和fluent都会有震荡。这是约450万的网格文件：https://cowtransfer.com/s/82c878e62de64d
介质为水，边界条件inlet 5m/s, outlet 静压45300 Pa，wall为滑移壁面，foilwall为无滑移壁面，symmetry面设为symmetry，LES模型用的WALE，时间步长用的5e-5 -
@gengchen 在 fluent用LES算水翼边界层选择中心差分引起的震荡如何消除 中说：
目前fluent自带的差分格式包括upwind, 2nd upwind, 3ord MUSCL, quick, bound cd 和cd都试了，只有cd能比较精确的算准边界层的速度剖面和脉动强度
Regarding this, do you have any plots?
-
李老师，可以先看下0.15弦长处的速度剖面，我是在这个位置插入一根沿z方向4mm线导出平均速度，x=0.0002m, y=-0.059182m, z=0.016964m到0.020964m，根据最大值无量纲化，图表附在文件里。velocity_profile_ldv_test_0.15C.zip
-
抱歉，李老师，那我直接把LDV的数据贴上吧，谢谢老师！
0.51874 0.02 0.54523 0.04 0.57821 0.06 0.60027 0.08 0.61619 0.1 0.63168 0.12 0.65259 0.16 0.67519 0.2 0.69035 0.24 0.71312 0.28 0.72578 0.32 0.75144 0.38 0.76757 0.42 0.78385 0.46 0.79825 0.5 0.81624 0.54 0.83174 0.58 0.86305 0.66 0.89698 0.74 0.9205 0.82 0.94188 0.9 0.96355 0.98 0.98842 1.14 0.99863 1.3 1.00000 1.46 0.99797 1.62 0.99706 1.78
-
- is it time-averaged U predicted by LES?
- What is the maxima? the Umax in this line or in the computational domain?
Your results look quite good. Is it predicted by linear scheme? How about the other schemes, e.g., limited schemes?
I am runing LES simulation, but it is very slow. I try to limit Co under 0.6. Since the global Umax is around 10 m/s, it indicates
Courant Number mean: 0.00518159 max: 0.59921 deltaT = 2.67779e-06 Time = 0.0168822 GAMG: Solving for p, Initial residual = 0.0474207, Final residual = 0.00156874, No Iterations 2 time step continuity errors : sum local = 3.90116e-10, global = -6.12223e-14, cumulative = 5.73243e-11 DICPCG: Solving for p, Initial residual = 0.0105353, Final residual = 9.99036e-07, No Iterations 608 time step continuity errors : sum local = 2.48515e-13, global = -3.59741e-15, cumulative = 5.73207e-11 ExecutionTime = 401.48 s ClockTime = 421 s fieldMinMax minMaxp write: min/max(mag(U)) = 0 10.5464 Courant Number mean: 0.0051816 max: 0.601813 deltaT = 2.61829e-06 Time = 0.0168848 GAMG: Solving for p, Initial residual = 0.0479045, Final residual = 0.00156265, No Iterations 2 time step continuity errors : sum local = 3.72593e-10, global = 2.37179e-14, cumulative = 5.73444e-11 DICPCG: Solving for p, Initial residual = 0.0102726, Final residual = 9.97099e-07, No Iterations 152 time step continuity errors : sum local = 2.38352e-13, global = 2.12724e-14, cumulative = 5.73657e-11 ExecutionTime = 402.54 s ClockTime = 423 s
11/45