请教版主一个问题

mymailyh

1、在进行离心泵整 场 计算 时，边界条件rotor/stator如何设置，我将irsnew设为2，为
   什么在计算后的*.mf中记录number of blades=1？
   希望能给予详细指点啊。
2、我的边界条件是这样给的inlet：流量 outlet：静压 另外加了control backflow，但计算出的出口流量与进口流量相差20%。这是什么原因？
3、计算中用三重网格时，前两重收敛性很好，最后一层细网格总是发散，是不是网格的原因啊？

longwin

1：生成网格时在igg/autogrid设置边界条件，rotor出口和stator进口设成
ROT；叶片数与该参数无关，应该检查igg/autogrid或fine的设置
2：存在回流、叶片数不对、没有收敛等原因都会造成这一差异
3：和2一样，先解决1再讨论这个问题好一些

mymailyh

谢谢您 的解答，希望以后能多多向您请教!

redboy

将irsnew设为2干什么用呀？

kc

请问 mymailyh  longwin 两位
将Irsnew设为2干什么？什么时候才应该修改这个参数？

Batman

我的问题和mymailyh的第三个问题相同：(我计算的是向心透平的叶轮)
计算中用三重网格时，前两重收敛性很好，最后一层细网格总是发散，不知道是什么原因？
另外我发现，在计算向心透平叶轮时，如果进口给总压总温，就会出现这个问题，
但如果进口给流量，静温，计算结果却收敛很好！

belkang

First question in mymailyh: In EURANUS, the flow solver in Fine/Turbo, there are basically two methods to treat quasi-steady computation in multi-blade rows: Mixing plane and Frozen rotor.IRSNEW =1, means that the interface is FULL-NON-Macthed (FMG), IRSNEW= 2 means Frozen rotor method is used.  When IRSNEW=2, the whole rotor and/or stator has to be meshed. That is why the blades equal to 1.
Second question in mymailyh: Are you computing centrifugal impeller with volute? Is your ROT BC the interface between the impeller and the volute?
Please check if the flow path between these two part are well fitted in the meridional view.
In addition, is the computation fully converged? This error of mass was got from coarser mesh or fine mesh computation? Do you have more than one STRIPs in the interface (Fig.9.2.1-1)?
Third question in mymailyh: You have to realize that in the Full-MultiGrid computation which is only used for creating a better initial flow field, first order scheme is used. Hence the convergence is generally fast. After the Full-Multi-grid cycle is finished, second order scheme is used. So, the convergence problem could come from following different reasons:
1) Quality of the mesh.Please check the mesh quality from IGG. A better convergence and high accuracy may be got with Aspect Ratio <1000; Extension<3.
2) Operation point. You have to realize that different mesh level may give different working points even though the boundary condition is the same, and a converged solution can only be obtained in the machine working range. A suggestion is: if the mass flow is too low in the FMG cycle, or lower than what you expected, you should reduce the exit pressure.
3) In addition, computation with finer mesh will predict more detailed vortex or separation flow, which may also make the convergence difficult. Hence, you may reduce CFL when the finer mesh is computing.
Question in Batman: Please check if the two different inlet boundary conditions give the same computed working point. If it is different, you should then modifying values which make the divergence.
Hope my reply give you some help!

mymailyh

谢谢你的再次指点，我的这个问题在元旦后就解决了，问题来源于网格，泵转轮内的定常计算已通过，现在进行非定常计算。还望以后多多指教。