CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Turbulent Boundary condition, viscosity ratio and length scale (http://www.cfd-online.com/Forums/fluent/108088-turbulent-boundary-condition-viscosity-ratio-length-scale.html)

Bollonga October 14, 2012 17:37

Turbulent Boundary condition, viscosity ratio and length scale
 
3 Attachment(s)
Hi everybody,

I am simulating a 2D inclined flat plate with an angle of attack of 70. 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.

Ive tried different approaches Ive 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.

RodriguezFatz October 15, 2012 04:46

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?

Bollonga October 15, 2012 07:49

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

RodriguezFatz October 15, 2012 10:04

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.

Bollonga October 15, 2012 10:33

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

RodriguezFatz October 15, 2012 10:51

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?

Bollonga October 15, 2012 11:02

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.

cfd seeker October 15, 2012 12:16

@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

Bollonga October 15, 2012 12:47

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.

cfd seeker October 15, 2012 13:04

Quote:

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

Quote:

Any references where I could find that turbulent length scale-BL thickness relationship and also BL thickness formulae for inclined flat plates?
A simple google search guides me here....http://en.wikipedia.org/wiki/Boundary-layer_thickness

cfd seeker October 15, 2012 13:07

Quote:

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

RodriguezFatz October 15, 2012 13:13

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:

Bollonga October 15, 2012 13:40

1 Attachment(s)
@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

cfd seeker October 15, 2012 13:49

Quote:

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)?
It refers to the BL thickness

Quote:

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

cfd seeker October 15, 2012 13:52

Quote:

Originally Posted by Bollonga (Post 386744)
@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

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

Bollonga October 16, 2012 05:42

2 Attachment(s)
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

RodriguezFatz October 16, 2012 06:44

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?

Bollonga October 16, 2012 07:18

1 Attachment(s)
@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.

Bollonga October 17, 2012 02:59

2 Attachment(s)
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 30 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!

RodriguezFatz October 17, 2012 03:23

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.


All times are GMT -4. The time now is 16:34.