Turbulent Boundary condition, viscosity ratio and length scale
 

Hi everybody,

I am simulating a 2D inclined flat plate with an angle of attack of 70º. My domain goes 10H upstream (say H is the plate height, H=9.3 m), 20H downstream, 10H up and 10H down.

Velocity at the inlet is 10 m/s. I am using k-epsilon model with TI=10%. I have tried several values for the turbulence length scale (1m, 0.5m, 0.1m, 0.05m) but sooner or later I get turbulent viscosity ratio limited to 1e5 in several cells in the wake. Which should be the value of the turbulent length scale for this case? Also, TI decays too much at some distance from the inlet so I guess I have to use a higher inlet TI to get the appropriate value when the flow reaches the plate.

I’ve tried different approaches I’ve read in this forum like starting with sparlart-allmaras model and change to k-e later, using first order discretization for k and e, reducing TI for some iterations, etc. I always end with the TVR limited to 1e5.

I have also read that mesh quality can be the problem. Is there a relationship between cell size and turbulent length scale allowable?

I put pictures of the mesh, TVR and TI distribution for the 0.05m length scale case. Notice that the flow hasn't reached the outlet yet.


Any comments or help would be really appreciated. Thanks.

Hi Bollonga,

You say "sooner or later"... I guess you mean regarding to time steps, is that correct?
Do you run a time dependent simulation? What is your time step?

When your TI decays on the way to the plate it sounds like your discretization is too dissipative. Does the problem persist when you use higher order schemes?

Do you resolve the boundary layer or do you use wall functions?

Do you use a prism layer around the plate?

Can you upload the mesh?

Hi RodriguezFatz,

Yes, I'm solving a time-dependent problem. I have used several time steps: 0.001 s, 0.005 s, 0.01 s but the TVR is always limited. For all these time steps the solution has always converged with residuals of 1e-6.

I have tried:
PRESTO and Coupled schemes for pressure-velocity coupling.
Gauss-Green cell based and Least squares cell based for gradient discretization.
Second order for pressure discretization.
First order upwind scheme for k and e, and then changed to second order upwind some time later.
Second order implicit for transient formulation.
The problem is persistent whatever I use.

I'm using k-e standart model with standart wall function and there is no prism layer around the plate. You can download my mesh from this link:
https://dl.dropbox.com/u/6986695/PS_2D.msh

What should I try next?

Thanks a lot for your help

I started a new Fluent project, imported your mesh and used the settings you wrote. I don't see any TVR limitation after 6s. How long do I have to run the simulation?

At first glance your grid looks much too coarse. What is the name of the plate boundary?

By the way: You do have a prism layer around the plate.

I'm sorry I sent you an old mesh that I had used before. The current mesh that gives me TVR limitation is this one.
https://dl.dropbox.com/u/6986695/PS_2D_9_10.msh
The name of the plate boundary is panel_wall. TVR limitation appears at 5s aproximately.

Thanks a lot

Ok, TVR limitation starts to appear upstream the plates' upper and lower ends. Maybe you could refine the grid there. I let the simulation run over night and will see what it shows tomorrow...
What happens if you use a prism layer aroung the plate?

Yes, that is exactly what I'm trying this afternoon. I'll put an inflation layer around the plate and run the case with the same setup. I'll share the results with you as soon as I get them.

@Bollonga
Few points
1. There is a large transition in mesh size at the interface of structured and unstructured part of mesh....it can cause problems...try to correct it

2. BTW why you are using hybrid mesh for this simple case? it is very easy to get fully structured mesh for this case(I can help you in this)

3. Turbulent length scale=0.4*$($= B.L thickness) is a very good approximation for external flows. Analytical formulas are available to calculate B.L thickness for the flat plate

Hi cfd seeker,

1. Okay, I'll try to refine the structured mesh at the transition sides.

2. I'm using hybrid mesh because I'm using ansys workbench meshing application and it is not easy to do structured meshes for irregular areas. I haven't too much experience with Icem though (I don't have gambit installed). I'll be glad if you could help me with that.

3. Any references where I could find that turbulent length scale-BL thickness relationship and also BL thickness formulae for inclined flat plates?

Thanks, it's been of great help.

Ok attach your geometry file here in parasolid format or .tin( .tin is icem format)

A simple google search guides me here....http://en.wikipedia.org/wiki/Boundary-layer_thickness

ohhh hold on....the link in the above post will give you B.L thickness formulae but the relation b/w length scale and B.L thickness can be found in Fluent's user manual

If you have ICEM, you should really use it. It is absolutely perfect for such simple geometries, since the basic structure of the blocks will be pretty simple, too.
If you don't know how to use it, take 2 days and you will be able to mesh your stuff.
Use these tutorials of an airfoil:
http://www.youtube.com/watch?v=tYrbScUH9RE
(part 1 of 3, watch the others too)
Also, you can import the geometry from Ansys Geometry module to ICEM by using the "workbench reader" import utility in ICEM. Be sure you already named all inlets, outlets... in Ansys Geometry. They will be read in ICEM and forwarded to Fluent.

Edit: You only need Ansys Meshing if you have no clue at all, but want some fancy colored pictures anyway, regardless of the correctness of your results. :cool:

@cfd seeker

I have attached the geometry in parasolid format .x_t

From Fluent users guide:
"For wall-bounded flows in which the inlets involve a turbulent boundary layer, choose the Intensity and Length Scale method and use the boundary-layer thickness, delta, to compute the turbulence length scale, L, from L=0.4delta. Enter this value for L in the Turbulence Length Scale field."

Does delta refers to BL thickness at the inclined plate surface? or to an inlet BL condition (that will be next step in my simulation)?

From wikipedia:
delta=0.382*x/Re^0.2
As my plate is not paralell to the flow, should I use free stream velocity to get Re (Reynolds number) or a local velocity paralell to the plate?
I guess x is the plate length.

Thank you

It refers to the BL thickness

always use free stream velocity to calculate Re. No
yes "x" is plate length in your case(plate length in flow direction)

I will try on your geometry tomorrow morning in the office because don't have ansys available at home

Hi everybody,

I've done a new mesh with a prism layer around the plate with a total height of 0.2m, 7 layers and 1.2 growth rate. The mesh is still hybrid.
I've used 0.026m of turbulence length scale, resulting from formula above.
I've run the simulation with this setup:
- pressure-velocity coupling: coupled
- gradient: green-gauss cell based
- pressure: 2nd order
- momentum: 2nd order
- k and e: 1st order and changed to 2nd order at 10.5s
- 0.01s timestep gave divergence, so I run it with 0.005s and it went well (all residuals are 1e-6)

I'm attaching a picture of TVR at 9,5s, just before limitation appears, and at 55.28s, when limitation is spread in all the wake.

1. TVR limitation has started at 10s aprox, later than previous simulations in which it started at 5s. Can it be due to coarse mesh in the wake?

2. I have also drag and lift coeficients from monitors, they are higher than values from literature (Fage and Johansen, 1926). My normal force coefficient Cn is 1.54 aprox while Fage and Johansen is 1.034. My Re no is bigger, but this case should be Re no independent as it has clearly defined separation points.

3. How should I choose the wall function? Is y+ relevant in this problem? I've seen recommendations for y+ that are very restrictive regarding mesh size.

Thanks

3)
y+ is always more or less important.
Normally, values (velocity, energy,...) have very strong gradients / changes near the wall. If you use a wall function, you imply that these values behave quite similar near the wall for all different setups. The values close to the wall are not calculated but taken from analytical functions, such as v_x(y+). This saves a lot of computational power, since you can omit all those gridpoints at the wall. But: If your first grid point (closest to the wall) is actually too far away from the wall, these analytical functions can only provide complete garbish. That's why it is important to have the closest grid point (y+) close enough to the wall, that it satisfies the domain of definition of your wall functions.

You can just run a simulation and make "->Results->Plots->XY plot". Choose "Turbulence" and "y+" for y-Axis function and your plate for x-axis. Now you see the value of y+ along your relevant surface.

2) You should first get numerics right, than compare results.
1) Yes. Your mesh is pretty small. Couldn't you afford to just make it a bit larger and add some points?

@RodriguezFatz

1) I'll make my domain longer downstream and finer the mesh.

3) I attach a xy-plot of y+ at panel_wall. According to Fluent Users guide, for standar wall functions 30<y+<300. I'm having several values over 300 so I'm going to refine the prism layer.

I'll share results as soon as I get them. Thank you.

Hi

I've refined my mesh and prism layer around the plate (My mesh now has 57920 nodes) and have run the case with the same set-up as before. Results are still the same, TVR limitation appears between 5 and 6s and spreads all over the wake. I attach a picture of TVR at 23.7s. What can be the problem?

I have references that get good results for a coarser mesh and with less computational effort than me.
http://www.waset.org/journals/ijmae/v6/v6-60.pdf
There, flow over a flat plate at 30º is being simulated. The plate is 0.15m length and freestream velocity is 15.25m/s. The mesh is finer but it's in similar proportion to my mesh size. The author has 150 divisions in the plate surface and so do I. Can it be a scale issue? Even if my problem is much bigger it requires similar cell sizes?

By the way, y+ seems better now, even too low in some points. I attach the plot.

Thanks for the help!

Correct me if I'm wrong, but you say your plate has a length of 9.3m and velocity is 10m/s. In the paper the plate has a length of 0.1511m and velocity is 15.25m/s. Now, Reynolds number is 40 times higher in your case. You cannot compare the needs for the meshes then.

You are right, my Re no is 40.4 times higher. Should I try with a finer mesh so? I'm considering to reduce scale to get a similar case to the one in the reference and compare results. And once then go back to the current scale.

Just reduce your inlet velocity by a factor of 40 and give it a try. If you don't have any problems then, you know that your grid needs some refinement for your current case. (Don't forget to enlarge the timestep, when you reduce the velocity)

Well, I’ve run the case for 0.25 m/s, using the same solver setup and different time steps: 1, 2 and 4 s. Convergence criteria 1e6 as before.
I comment a few things:

1) Almost no TVR limitation, just a few cells (small vortexs) at some iterations.

2) Y+ very small, from 0.1 to 1.8. First layer of prism layer should be higher for SWF. (see picture)

3) Epsilon residuals in some iterations can’t go under 1e6.

4) Turbulence intensity drops too fast so close to the inlet. (see picture) I’ve read in the forum that if TI drops too much it means that equilibrium between k and e is wrong because I have too much dissipation, e is over estimated. I guess I need a higher amount of TI in the inlet so I get the desired value at the plate? But if I put too much TI and initialize the solution from the inlet it may start with TVR limitation from the beginning.

5) Lift and drag keep oscillating even if I have left time enough for the flow to run the entire domain for twice (3200s at 0.25 m/s) (see pictures)

I’m gonna try to simulate at the same scale as the reference, with same Re number and try to get a correct y+ value. Once then I'll have to try again the real scale. Any suggestions?

Thanks a lot

Hey,

2) With an y+ of that size: If you can afford that mesh (by means of computational power) you can just use the "enhanced wall treatment" instead of wall functions.
4) I don't know much about that, but what you write sounds reasonable. You say, that TE drops on the way from your inlet to your plate, correct? Now, shouldn't you fix your k and e at the inlet in a way, that the 10% TI is sustained? Or isn't that possible?
5) Your plate has a much higher angle than in the paper, right? Isn't it possible that lift and drag are strongly time dependent? Looks like you have strong oscillations in the wake...

Sorry I was busy for 2 days, I worked on your geometry and I guess I got the good blocking.min quality is 0.8 which is very good but you have to work yourself on the edge parameters and refine/coarsen the mesh in the appropriate areas and finally put BC's and export the mesh in fluent. I am attaching few pics and project files of ICEM

If your are fully resolving the boundary layer(wall y+ <=1) then better use Enhanced Wall Treatment instead of wall functions.
One more suggestion...use SST kw model instead of k-epsilon because angle of attack in your case is very high and there is significant amount of flow separation and k-epsilon model does not properly capture separation instead SST kw model is more recommended in such a situation.
Another point....if turbulent viscosity limit is exceeding in few cells then you don't need to worry as long as your lift and drag are in agreement with experimental results

Regards

@cfdseeker Thank you very match for the files! That will help me a lot to learn more about ICEM.
As this case has a clear separation point at the edge of the plate, is there a big diference between k-e and k-omega?

@rodrigeuzfatz @cfdseeker I've run the case at a smaller scale and almost didn't have any TVR limitations, just few cells away from the plate at some iterations, nothing to worry about.
y+ is still too low, I prefer to coarsen my inflation layer and use a wall function instead of using the enhanced wall treatment in order to reduce computational effort.
Force coefficients don't oscillate as much as they did before, they are still a bit higher than in literature but I guess I have to resolve near wall flux properly before.
I've read something about TI decay in Fluent users guide (7.2.2), there are some equations to estimate k and e from TI decay and distance.

Is there a way to get time-averaged variables along the plate wall? The only way I know to do that is to write an xy-plot file for each time, and then calculate the mean value. However, I need to save many .dat files to have a good resolution.

I'll share further results. Regards.

yes it has been thoroughly discussed in literature that there is a mark difference b/w k-e and k-w.Standard k-e and RNG k-e under predicts separation,Realizable k-e is a bit better in capturing separation but SST kw is best model recommended for this case

No no don't do it my opinion....Enhanced wall treatment is best in capturing flow separation especially at such high angle of attacks. SST kw by default use enhanced wall treatment. My opinion is to run the case on this mesh(wall y+ <=1) using SST kw model. I am quite sure that you will get much better results in this case

Okay, I'll try SST k-w model with the finner mesh, the thing is y+ distribution around the plate reaches very different values. There's always a minimum at the stagnation point in the front face and at two corners but there are peaks at the back face and the two other corners that goes over 1 in the finner case (see y+ picture at comment #23)
1) Do I have to get y+<=1 along all the wall? as the case is strongly time dependent, do I have to look at time-averaged y+ or just the maximum?

By the way, these guys get very good results for a vertical plate in the same conditions as me (just a little geometry difference) using k-e with different wall treatments and they don't use a prism layer around the wall.
http://www.waset.org/journals/waset/v61/v61-49.pdf
2) What are they doing that I'm missing?

I've run the case with SST k-w model, no TVR limitations appeared. The problem is I'm still having wrong force coeficients. Time averaged values are the same as in all previous simulations: Cd=2.979 and Cl=-1.071 while literature ones are Cd=1.945 and Cl=-0.708.
I've been looking at Cp distribution at the plate and made the time average over a complete vortex sheddind cycle. I've compared it to literature values and my Cp's at the back face are much lower (see attached pictures), that's why my Cd and Cl are higher. So I must be simulating something wrong at the wake, could it be because of wrong y+ values at the back face? (see picture of instantaneous y+ at Cd max time) What can be the reason for too low pressure at the back face?

Thanks a lot for your help guys

You don't need to worry about this, its a normal situation. Wall y+ are dependent on wall shear stress and Re. No. As the Re. No is changing along the length of plate so wall y+ will be different at each point

Not really. It should be in between 1 and 5

Are you sure that your case is Fully turbulent and transition is not taking place?

I'm not pretty sure if transition is taking place. How can I asure that the case is fully turbulent?
I've increased TI from 10% to 25% at the inlet and let the same turbulent lenght scale (TLS) of 9e-4 m and results are the same.
Now I'm running a case with 25% of TI at the inlet but a TLS of 5e-5 m to make it more diffusive to see if something changes.

I think using the hexa mesh will solve your problem. What do you think?

Can you tell me the following info:

1. Reynolds number

2. Time step and no of time steps and how you have determined them?

3. How you are making the time-average Cd and Cl. How many time steps and total time you are taking into account for this purpose?

4. How you are ensuring the convergence

5. Domain extent is good enough? Have you made the sensitivity analysis to domain extent?

Hi far,

I've already solved TVR limitations by scaling the problem and using a better turbulence lenght. k-e standar with standar wall function and k-w with enhanced wall treatment are not showing this limitation.

The problem is both models give too low pressure at the near wake and so drag and lift coeficients are higer than they should be.

I'm now playing with BC for TI(%) and T length scale to see if results change, but force over the plate is not changing so far. I think it may be related to turbulence model or its parameters.

Here you can see that a relative coarse mesh with k-e gives good results for a vertical plate.

Thanks

What do you mean by scaling the problem?

I've just seen your last comment.

1) Re no is 1.55e5 (plate length=0.15m, u=15m/s)

2) I've tried several timesteps: 5e-4, 1e-3, 2e-3 and eventually I'm using 25e-4. I let the flow goes several times all along the domain (6.25 m long) that is 800 timesteps. But I've have checked that mroe iterations don't change the result.

3) Once the coefficients are constante I've measured the period of a cycle of lift and drag force, they are almost 0.07s and I've writen a Cp file every 0.001s. I've made the average for each point and got the time-averaged Cp distribution for a complete cycle.

4) Residuals are 1e-5.

5) Now it's 41.6*L long and 27.7*L where L is the plate length 015m. I've tried a larger one and results are the same.
3)

By scaling I mean to reduce the scale of the mesh.
My real plate is 9.13m but I wanted to compare with literature experiments for a 0.15m plate. So I reduced mine to have the same length.
The real scale problem gave TVR limitation but the same mesh with reduced scale gave no problem.

What is the value of density and viscosity and why you choose these values?

How did you determine the time step size? Is it according to any method available in literature?

Do you wanna try the hexa mesh? I have made one. In this mesh, Y+ is 1 (good for transition model as well) but requires more time steps. You may need the transition model for better prediction of Cd.

http://imageshack.us/a/img42/8580/57979604.png


http://imageshack.us/a/img560/5580/32506684.png