CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Time step for Low pressure turbine simulation (https://www.cfd-online.com/Forums/fluent/115089-time-step-low-pressure-turbine-simulation.html)

 Far March 23, 2013 12:23

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.

 Far March 23, 2013 13:00

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 un-important 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 Kt-Kl-omega model

9. Solution converged between 10-12 iterations.

PS: We have already simulated this case with 1e-3 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

 Far March 23, 2013 13:03

update

Solution is being converged within 8-9 iterations for time step size of 5e-05

 flotus1 March 23, 2013 16:40

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?

 taxalian March 23, 2013 17:43

Hi Far,
I would completely agree with the remarks from flotus1.

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.

 Far March 24, 2013 02:12

Quote:
 Originally Posted by flotus1 (Post 415910) 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?
It is hybrid mesh.

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:
 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. Also try to compare your results against the experiment and LES if available. I hope this helps and regards.
As I am interested in separation behaviour and its interaction with upstream disturbances therefore I am not interested in losses in wake. Nonetheless, I am going to incorporate that wake resolution (done) so that I have another parameter to correlate (loss coefficient in this case).

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 stream-wise 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 1e-4, simulation takes 24-36 hours to complete, so you can estimate the time required for the too fine mesh.

Quote:
 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.
Thats good information. Otherwise my understanding was that CFL ~ 1 for all simulation including DNS and LES. How much larger values I can use for time step in Implicit formulation? What should be deciding parameter?

Another question, pressure based solver uses explicit or implicit formulation?

 Far March 24, 2013 02:49

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:
 In the segregated solution method each discrete governing equation is linearized implicitly with respect to that equation's dependent variable. This will result in a system of linear equations with one equation for each cell in the domain.
Quote:
 In the coupled solution method you have a choice of using either an implicit or explicit linearization of the governing equations. This choice applies only to the coupled set of governing equations. Governing equa-tions for additional scalars that are solved segregated from the coupled set, such as for turbulence, radiation, etc., are linearized and solved im-plicitly using the same procedures as in the segregated solution method. Regardless of whether you choose the implicit or explicit scheme, the solution procedure shown in Figure 22.1.2 is followed.
Quote:
 There is no explicit option for the segregated solver.
http://gendocs.ru/docs/19/18603/conv_22/file22.pdf

 flotus1 March 24, 2013 04:28

Quote:
 Originally Posted by Far (Post 415953) It is hybrid mesh. 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.
To me it rather looked like a usual tet mesh with a high number of automatically generated prism layers. Keep in mind that the total number of cells is not the only parameter that affects simulation time.
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:
 Originally Posted by taxalian (Post 415960) I would still insist upon doing one steady state simulation (SST k-w 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.
Totally agree on that

 taxalian March 24, 2013 04:31

Hi Far,

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 k-w 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.

 Far March 24, 2013 11:50

A
Quote:
 s 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.
Except with restriction on time step size in explicit formulation. But explicit option is not available in Fluent for pressure based solvers.

Quote:
 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.
Yes it is. Yes I do know the transition location and in our previous results that matched with experimental data. This time I want to find out more results and with more visualization.

Quote:
 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.
It is walters Kl-kt-w model and is based on physics unlike SST gamma theta model which uses correlations. In fact in our previous work we used SST gamma theta model.

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:
 I would still insist upon doing one steady state simulation (SST k-w 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.
I tried but no luck in getting converged solution as results were changing from iteration to iteration. Otherwise this would have made my life easier.
Do you still recommend using SST (fully turbulent) model for mesh independence study keeping in view above discussion

Quote:
 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.
Not possible as I am using Gambit and it wraps boundary layer around all surfaces and it would not good idea to use hanging nodes in this kind of simulation.

 Far March 24, 2013 12:00

Quote:
 I would still insist upon doing one steady state simulation (SST k-w 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.
How can I justify my meshes with fully turbulent SST model for the transition flow?

I can recall a paper in which same geometry was solved using K-omega and K-epsilon model and that had not accounted transition effects.

Edit : will update with results from fully turbulent SST simulation.

Time averaged Cp plot from kl-kt-omega model:

http://imageshack.us/a/img802/7523/t106a7.png

 taxalian March 24, 2013 13:05

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.

 Far March 24, 2013 14:00

Quote:
 Originally Posted by taxalian (Post 416030) 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).
You mean to say to have mesh independence study based on fully turbulent SST model. How can I justify to use this mesh with transition model?

 Far March 24, 2013 14:11

SST fully turbulent results

 taxalian March 24, 2013 15:57

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.

 Far March 25, 2013 00:36

Please have a look on video clip which clearly shows why flow is unsteady:

 Far March 26, 2013 08:06

wake-seperation interaction

Here is the video clip showing interaction of upstream wakes with separation and subsequent transition of laminar to turbulent flow and reattachment.

 Far April 1, 2013 05:20

SST - Steady state - Better mesh

I realized that mesh is not good to resolve flow in wake and quality is poor at hexa-tetra 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.