|
Question Regarding Turbulence Numerics
Hello, after being a Fluent user for the past 10 years I have made the jump to use CFX for the past 6 months since this is the software the company I now work for uses. I have found that all CFD models that are run here use only 1st order turbulence numerics. I was told that version 10 did not have a high resolution option and basically they haven't tried the high resolution and felt that the results would not change much if high resolution was used. We now use version 12. The CFD work we deal with the most is turbine blades. So, we do have a highly turbulent swirling flow. We use the SST option with automatic wall functions. My argument is that since most of the meshes are tets with prism layer that using high resolution is paramount to achieve a better accurate solution over 1st order turbulence. Unless, bear in mind convergence issues. I am having a very difficult time convincing senior and management engineers here to go forth and use high resolution. Any ideas? Also, are there any studies out there comparing CFX's 1st order and high resolution turbulence numerics and also if there are any CFX vs. Fluent turbulence comparisons? Thanks
|
I haven't ran many cases using high resolution turbulence, but those I have ran have shown little difference. Turbulence is a fairly diffusive process, so I can see that it's often not necessary to resolve sharp gradients. Also switching to high resolution may be insignificant considering some of the other approximations made in two-equation turbulence models. Still, I'd be interested to see any good comparisons.
|
I would have thought the way forward is obvious - run a test case with and without high order turbulence numerics and see if accuracy improves. That should make the case as to whether it is worth the effort better than any theoretical arguement.
Try asking CFX support for some papers looking at the high order numerics. |
It isn't that critical to use a very high-order scheme for the turbulent variables. These variables are very source term dominated and the accuracy of the convection scheme isn't very important. It is more important that the scheme behaves well and never creates unphysical oscillations that can trigger turbulence problems.
Many years ago I did a study comparing results for turbine blades using 1st and 2nd order schemes in Fluent. This was on structured hex meshes though. The study showed that most of the time it was okay to use first order schemes for k and epsilon. It might be more important on coarses tet meshes though, I do not know since I rarely use tets on blading simulations. For the non-turbulence variables having something better than first-order upwind is critical though, but I assume that you are well aware of that. If you are working on turbines and are worried about turbulence. Have you ever looked at, for example, eddy-viscosity ratios in the region just outside of the suction side after the suction peak and further down-stream between the wakes? Most two-equation models have a tendency to produce completely unphysical eddy-viscosity ratios there, especially if you run with fairly large (and realistic) inlet length-scales. That is something to show to your scepetic seniors/management if they think they know everything about turbulence modeling ;) |
Querry regarding Turbulence numeric
Hello everyone,
I need help. I would like to know about turbulence numeric term. What is its physical significance. In my project, When I use first order it show me smooth graph of K and epsilon in CFX solver. On the other hand, using hogh resolution leads to lot of variation in graph. Why it has happened. Kindly consider my request. Thanks Manpreet Singh manpreet_singh_er@yahoo.co.in |
High order differencing is resolving lots of smaller scale detail which the low order scheme damps out.
|
Do you think that switching to high resolution would have any efect on [Heat transfer coefficient] results, with t-bulk included ? I m doing a train brake rotor power disipation problem, and will definitly try it out in near future.
And is there a way that (steady state solver) would run first let say 100 iterations with (upwind) and than switch to (1st order). ...this is an (edit)... I have tried out high resolution but find it wery dificult to converge, should the mesh be finer for high order? |
You can change the advection settings either by doing a upwind run then using that as the initial condition to a higher resolution scheme, or use the edit run in progress option. The first can be scripted to do the change automatically.
|
| All times are GMT -4. The time now is 09:58. |