Time step for Low pressure turbine simulation
Hello every one,
I am solving flow on low pressure turbine profile T106A using pressure based coupled solver. I saw a paper (J of Turbomachinery) on the same profile where author had used finitie difference LES (Explicit solver) code to solve the flow. Here he had enforced CFL <=0.2. Now I would like to ask should I enforce same CFL condition in my simulation which is Implicit solver. Presently time steps I am studying are 0.001, 0.0001 and 0.00001 which are giving me maximum cell cournt number 100, 17 and 1.3 respectively. My questions are: 1. What time step I should take? Which parameter I should observe? 2. How much time I should run simulation? 3. What should be convergence criteria for each time step? Currently I have set it as 0.05 in relative convergence criteria. More details in next post. 
1. Coupled pressure based solver is used.
2. 2nd order implicit time formulation is used 3. 2nd order schemes for all varaibles including turbulence parameters. 4. Mesh size is 70,000 nodes with highly resolved boundary layer. As per laminar and turbulent calculations for Re = 91000 the boundary layer thickness is 3.2 and 7.8 for laminar and turbulent flows. There are 110 nodes in normal direction and first cell was placed at 0.01 mm height to ensure Y+<1 every where. Expansion rate is 1.03 5. The aft portion of suction side is resolved with more than 120 nodes streamwise where flow is transitional. 6. Size functions were used to mesh efficiently in important regions. It has also helped to reduce the mesh size by using bigger cells in unimportant areas. 7. BOCO: Velocity inlet and pressure outlet. Translational periodicity was enforced. Turbulence parameters were specified at inlet in terms of turbulence intensity and length scale. 8. Turbulence model is KtKlomega model 9. Solution converged between 1012 iterations. PS: We have already simulated this case with 1e3 and results were satisfactory as we have applied passive devices to control separation so unsteadiness was almost removed http://img59.imageshack.us/img59/7094/t106a.png http://img854.imageshack.us/img854/4372/t106a2.png http://img255.imageshack.us/img255/4576/t106a3.png http://img836.imageshack.us/img836/4576/t106a3.png http://img33.imageshack.us/img33/4418/t106a4.png 
update
Solution is being converged within 89 iterations for time step size of 5e05

What is the motivation for doing a transient simulation here?
Which transient effects are to be captured? BTW: Why are you using a tet mesh here? 
Hi Far,
I would completely agree with the remarks from flotus1. Your questions were: 1. What time step I should take? Which parameter I should observe? Answer. I would run this test case first as a 2D Steady state RANS case. Then if you observe any unsteady features (may be in the Journal publication you have), go for unsteady computation (2D vs 3D). But one should always take into account, that is it really necessary to spent time on these computationally expensive simulations. 2. How much time I should run simulation? 3. What should be convergence criteria for each time step? Currently I have set it as 0.05 in relative convergence criteria. Answer: Well this totally depends upon what kind of a flow you are doing, in Ansys Fluent you can use the monitoring of the variable in unsteady regions (if it exists). Obviously you need to check the convergence of the solution by monitoring the local convergence within each timestep.  Some tips and further replies related to your current mesh and simulation strategy: It would be better if you use a fully structured mesh or proper hybrid mesh for such configuration. Because your mesh looks very weak in the wake region which is very important for such flow to account for the losses and rapidly changing strong gradients. Have a look at your mesh interface between quad to triangular region. Try to reduce the triangle cell smaller here to avoid large jump in cells. Explicit formulation restricts the CFL condition to CFL~1 and the LES solver used the CFL~0.2 in order to resolve the turbulent scales properly on the turbulent energy spectrum. Using the larger CFL might lead to inefficient resolution of the turbulent scales (additionally it depends also on chosen timestep + grid resolution). In an implicit formulaiton, you can increase the CFL number to larger values depending on the solution. Also try to compare your results against the experiment and LES if available. I hope this helps and regards. 
Quote:
Motivation behind using transient simulation is unsteady nature of flow. There are three separation bubble formed at the suction side towards trailing edge and they roll up into vortex and convected towards outlet at some rate, therefore flow is not steady. http://img547.imageshack.us/img547/4262/t106a5.png Quote:
I have more than 15 Journal papers to compare my results in general and four to five papers on this particular geometry including LES and experimental results. Also I am searching DNS results. I think Hexa mesh is not required for RANS simulation. I may consider it when I will be conducting LES simulation. Moreover quality is more controlled and mesh is not propagated into the inlet, out and periodic boundaries as I also need very fine mesh in streamwise direction. So instead of 70K nodes I may end up with 200,000 nodes. It will not be possible to complete research in reasonable time. With current mesh and time step size of 1e4, simulation takes 2436 hours to complete, so you can estimate the time required for the too fine mesh. Quote:
Another question, pressure based solver uses explicit or implicit formulation? 
Ok. I found that segregated solver uses implicit formulation. But no idea about the new pressure based coupled solver. Logically it should be same. I dont know why they have not provided explicit formulation for unsteady flows!!! See attached pdf for details and some paragraphs are quoted below...
Quote:
Quote:
Quote:

Quote:
The number of faces for example, which is much higher for tet meshes, aswell as the mesh quality, affect the simulation time. So if simulation time is an issue, I would always prefer hex. I agree with you that the flow is not steady. But turbulent flow never is. I must admit that I am not a fan of unsteady RANS methods for resolving vortex formation and advection in turbulent flows. One of the issues here is that the simulation is only 2D (and will always be kind of 2D with a RANS approach), which has proven to yield unphysical results for 3D turbulent flows. Quote:

Hi Far,
I am really glad with your detailed reply and your motivation to carry out such a simulation. As you already replied in your last post the difference b/w explicit vs implicit formulation, i don't need to elaborate that. Nevertheless their is no restriction on using the explicit/implicit formulation. Both should result in same result but different convergence behavior. Motivation behind using transient simulation is unsteady nature of flow. There are three separation bubble formed at the suction side towards trailing edge and they roll up into vortex and convected towards outlet at some rate, therefore flow is not steady. :) The flow you are trying to simulate seems to be a transition problem, do you know the transition locations? That would improve the accuracy and prediction of your results. The turbulence model you are trying to use, is this a transition model based on empirical formulation? If yes, then you should specify at least the turbulent intensity and other turbulent values exactly the same as used in the publication. I would still insist upon doing one steady state simulation (SST kw turbulence model) that is quite good in separated flows and performing a grid convergence study (coarse, medium and fine meshes respectively) i.e. a must approach in any kind of simulation. One last thing, seeing your last attached picture exhibiting the separation bubble, i would propose to increase the thickness of your boundary layer mesh (hex block) may be more only on the suction side of the airfoil. hope this helps and improve your understandings. 
A
Quote:
Quote:
Quote:
Any how, in both models turbulence intensity and turbulent length scale are important parameters and I am specifying them according to experiment and my results matches closely to that of experiments done at Cambridge university' Whittle lab. Quote:
Do you still recommend using SST (fully turbulent) model for mesh independence study keeping in view above discussion Quote:

Quote:
I can recall a paper in which same geometry was solved using Komega and Kepsilon model and that had not accounted transition effects. Edit : will update with results from fully turbulent SST simulation. Time averaged Cp plot from klktomega model: http://imageshack.us/a/img802/7523/t106a7.png 
Hi Far,
May be you could at least use some refined block with triangular cells in combination of sizing function to reduce the cell size in the transition region in Gambit. Yes i would still encourage you to do the mesh independence study as it is kind of normal practice. It would also support your result more if you want to publish your work later on (if its a research oriented study). Because at industrial level mostly the gird independence is not taken into account primarily. May be you can try running first your coarse grid with SST and then try to map the results onto your fine grid and continue with further running the fine grid SST computation. 
Quote:

SST fully turbulent results
Results with fully turbulent SST model:
http://img203.imageshack.us/img203/7913/t106a6.png http://imageshack.us/a/img213/7676/t106a8.png http://imageshack.us/a/img585/9412/t106a10.png http://imageshack.us/a/img822/2959/t106a9.png http://img40.imageshack.us/img40/7009/t106a11.png http://imageshack.us/a/img18/42/t106a13.png 
Hi Far,
I think this is quite justified the solution with SST looks good in full turbulent mode. You can try to do the grid independence study based on the full turbulent computations. Then use your grid independent mesh for your real computation case with the transition model. The mesh independent study is not dependent on the choice of your turbulence model or the flow. I would also monitor or at least report the cl, cd value for the different grids and then use the mesh that produces grid independent solution. Other than that you are on the right track :). good luck and regards. 
Please have a look on video clip which clearly shows why flow is unsteady:
http://www.youtube.com/watch?v=eQak7dWbXQA http://www.youtube.com/watch?v=Joc5hvnOfTM 
wakeseperation interaction
Here is the video clip showing interaction of upstream wakes with separation and subsequent transition of laminar to turbulent flow and reattachment.
http://www.youtube.com/watch?v=CvTbSVgbemk 
SST  Steady state  Better mesh
I realized that mesh is not good to resolve flow in wake and quality is poor at hexatetra interface which was also indicated by my fellows in this thread. Here is the new mesh and results with SST model in steady state mode.
Will run transition model today. http://imageshack.us/a/img341/9792/mesht.png http://imageshack.us/a/img585/2384/mesh2.png http://img255.imageshack.us/img255/9949/mesh3.png http://img545.imageshack.us/img545/7647/mesh4.png http://imageshack.us/a/img543/2344/l...returbine2.png http://imageshack.us/a/img14/3416/lo...returbine1.png 
All times are GMT 4. The time now is 17:25. 