stable problem
I calculate a steady flow field around a cascade with my time dependent NS code in which BL algebraic model was employed.I found the residual only decreased two orders,and the maximum residual position near trailing edge where a pairs of vortex located. the aerodynamic parameters varied periodically.But most of the researchers point out that residuals can decreased five or more order.I confused!! I hope you answer,thank you.

Re: stable problem
(1). This is because you are using time dependent formulation. (2). The time dependent formulation does not guarantee to give a steadystate solution. (3). On the other hand, the steadystate formulation will provide a steadystate solution. (4). In your case, if you modify the trailing edge geometry to a sharp one, the oscillation should reduce. But then, you are solving a different problem. It really depends on what you are after in the simulation. (5). In my steadystate calculation, I normally set the normalized residuals to 1.0E08, and stop the calculation when the residuals drop below 1.0E06. The right approach should be the monitoring of the flow variable itself VS time or iteration number. So, if your flow variable near the trailing edge is oscillating in time, then the flow is transient flow. (6). The situation is rather complex, because the solution could be real, or artificial due to the mesh, time step, turbulence model, etc. In other words, what you are getting is typical. It takes a great deal of experience to know whether it is useful or not, right or wrong.

Re: stable problem
You've probably got periodic vortex shedding from the trailing edge. One ugly trick to reduce this problem is to mesh the trailing edge with a coarse mesh. This often adds enough numerical dissipation in this region to damp out these oscillations. If you're only intereseted in pressure distributions etc. on the blade then this approach is usally okay. If you are interested in wake profiles and detailed lossed then this is not a good approach.

Re: stable problem
(1). Your email received. Thank you. (2). You did not mention the Mach number and the blade condiguration, so, it is difficult to know exactly the problem areas. (3). It does make a big difference whether you are using a pressure based method or a density based method. For density based methods, at low mach number, there is always oscillations in the solution. For this type of method, you can try to increase the artificial viscosity parameters to smooth out the oscillations. (4). For the pressure based method, you can use smaller underrelaxation parameters to reduce the oscillation. (5). The mesh used is also important to the convergence of the solution. You can improve the mesh density distribution, the mesh smoothness, and skewness. It is likely that in some areas you don't have enough mesh points. (5). Then, there comes the treatmnet of the boundary conditions. It can also affect the oscillation of the numerical calculations. (6). I think, what you need to do is to isolate the problem first. So, a simple cascade with zero or small flow turning could be used as a test case first. (7). The simplest way to check the convergence of the solution is to print the flow variable up to 4 decimal points vs time step (or iteration number) and observe the change in value until all the decimal points are identical. So, for single precision variable, you should run the calculation until 6 digits are identical between time steps. (8). If you don't know the slow convergence area, then the contour should be used, until two contour plots are identical between two test time steps. (9). So, try a stepbystep aproach to see whether you can learn something in the process.

All times are GMT 4. The time now is 08:35. 