Oscillating Residuals (with picture)
Hi guys,
iam doing a wind flow velocity analysis around a building as a project for college (>external flow). As I said in the title, i have an issue with oscillating residuals. I meshed the system with tets and generated 10 boundary layers around the building. Number of elements is about 1.8 *10^6. I made the enveloping body as big as described in the ANSYS tutorials. As Inlet andOutlet I used velocity inlet and pressure outlet. The turbulence model is a kepsilon with realizable and enhanced wall treatment. The wind velocity at the inlet is 8 m/s. furhtermore, I defined SIMPLE and everything alse as secondorder. Y+ is about 200. I didnt change any of the URF's. There are no mesh warnings, if I check the mesh in the solver. solver is pressurebased and I defined steady state. thats how it looks after 5000 iterations: http://img5.imageshack.us/img5/3867/continuity.png Uploaded with ImageShack.us any ideas how to solve this problem? thank you! :) regards 
Some things you can try:

Hey flotus1, thanks for your answer.I will try that for sure.
But I have two questions about your suggestions: 1. Why would you deactivate the realizable option? I thought it generates more accurate results than the other options. 2. Could you explain how I can check the turbulence values at the inlet in a more detailed way? thank you : ) regards 
The realizable option may produce better approximations of the flow in some cases.
But if the solution doesnt converge with this option, then in my opinion the standard kepsilon formulation still is better. We experienced similar convergence problems for the external flow around blunt bodies with the realizable option. The komega SST model might also be an alternative worth trying. Since you get warnings about the turbulent viscosity ratio limited in many cells, you should make sure that you didnt set unreasonably high values at the inlet. Yet it is more probable that the warning comes from cells in the wake region of the building. 
if you can provide us with some picture of your mesh ...

Thanks for your answers. I will upload some pictures of my mesh wehn Im at home.
regards 
Hi again,
I gave it another try with the recommended options (realizable off, reduced URFs (momentum from 0.7 to 0.6 and pressure from 0.3 to 0.2), started with frist order then switched to second order when it converged, ) Result is looking way better than before, but there are still some jumps in the residuals. Another problem is the area weighted average velocity. It is oscillating very much. Any Ideas what I could do to obtain good results? Picture: http://img839.imageshack.us/img839/7928/continuity2.png Uploaded with ImageShack.us thank you! PS:Sorry for not uploading a picture of the mesh. I will do that today evening. 
Good progress. But need the picture of your setup.
comments # Area weg. avg velocity @ which location ? # how about the overall mesh distribution # mesh distribution in wake region (where the velocity gradients are more) # for extenal flow one equation (spalart allmaras) model is preferred , but i'm not sure check in fluent recommendation. # how close the BCs and object (buliding) 
Since you could afford 5000 Iterations in the first run, you can decrease the URFs further (0.7 to 0.6 doesnt make much difference).
I recommend 0.30.2 for momentum and 0.1 for pressure. Additionally, you should use a first order upwind scheme for the momentum discretization. If the solution converges, you can still switch to second order from this initialization. 
Quote:
Quote:
It may help to use first order scheme and kepsilon model untill you see some stability. Both of these induce a muchneeded diffusion to stabilise the turbulent instabilities in the initial part of solution. Once you see some stability, you can switch to second order. Also, you can explore the blended factor and choose the order of accuracy for momentum between 1 and 2(say 1.5). This should help in smooth convergence. Also, try FMG initialisation, to see if it helps. Additionally, it is a thumbrule to keep the addition of URFs for pressure and momentum as 1 for SIMPLE based schemes. But this is not always possible every time, as perhaps is the case here. 
Quote:
When I reduce the URFs, i reduce both pressure and momentum simultaneously and never got into trouble because they didnt add to 1. Quote:
Quote:

Quote:
Navigate to solve > set > numerics Keep entering till you get to: "1storder to higherorder blending factor [min=0.0  max=1.0]: " Here you can specify the factor. 0 means first order. 1 means second order. 0.5 means 1.5 etc. Use of blending factor will make convective fluxes more diffusive, inducing some stability. But make sure in original setting, you have specified discretization as second order. OJ 
what I recommend before all, check you mesh. make sure that you have enough fine mesh. check for the skewness. If you have low quality, you will not have a converge solution. Moreover, big size variation, you will have fluctuation in the residuals.

All times are GMT 4. The time now is 05:30. 