[Far]

Originally Posted by Bollonga

Thanks a lot. How big are the files?

I've managed to export your mesh in 2D, but it gives error when importing it in parallel mode. An error message says:

Build Grid: Aborted due to critical error.

There are also several messages in the command window saying:

4:WARNING: cell id 28340 of thread 24 has NULL face pointer 3.
Primitive Error at node 4: Build Grid: Aborted due to critical error.

Which can be the reason?

This is because of meshing error which is not acceptable to fluent. Did you turn off the solid and vorfn blocks before exporting the mesh?

[Bollonga]

Originally Posted by Far

This is because of meshing error which is not acceptable to fluent. Did you turn off the solid and vorfn blocks before exporting the mesh?

How can I do that?

[Far]

But there should not be error in mesh as I have used it for simulation in Fluent and shown in this thread.

[Bollonga]

Hello everybody,

In this month I've made some progress with the flat plate, the key was using k-epsilon Realizable with enhanced wall treatment, and I got CD and CL way more similar to the literature ones.

Now I'm learning to use Icem (v13) because I need an optimal mesh to do the 3D case.

However, I've encountered a problem when exporting my mesh to fluent. It's a 2D hex mesh with a blocking strategy. When I try to open it in Fluent it gives this message:

FLUENT reveiced fatal signal (ACCESS VIOLATION)

I've read that I should use serial processor instead of paralell, but the message is still there. I've made some reading in the internet and read that all edges must be related to curves. I have some interior edges that I don't know to which curve relate.

I upload the geometry and icem files in the following link, but I would like to know how to solve that. Thanks in advance.

https://dl.dropbox.com/u/6986695/PS_2D_Icem.zip

[Bollonga]

Now I have solved the previous problem, it was due to some mesh setting I was skipping.

But now I'm facing new problems. I've done my 2D hex mesh, I export it to fluent and when I try to read it it gives many messages saying:

Skipping zone (not referenced by grid)

So I get all zones deleted. I've tried with the fix option in Icem, and it's supposed to have fixed many things, but I'm still getting the same problem. I've made a search at the forum but got no useful tip.

Your help would be much appreciated.

[Bollonga]

I've solves those problems with the help of people in the geometry and meshing forum. Thanks anyway! Now I'm gonna try the 3D simulation, I'll inform about my results!

[Bollonga]

Hi everybody!

Here I am again stuck with the 3D case of the flat plate.
I'm just trying to reproduce the air flow over a 0.15m flat plate inclined 70º. Flow speed is 15 m/s.
I've used k-epsilon Realizable with enhanced wall treatment and k-omega SST but both have failed. Simulation starts slowly (adaptive time-step from 1e-5 to 1e-6 s) but converging until it reaches some point in which it diverges sharply (see picture). It reaches Turbulent viscosity ratio limitation to 1e5 in too many cells.
I've remeshed the geometry but I always get similar results.

I know I can play with the material viscosity, so should I reduce the speed and viscosity to maintain the same Reynolds number and avoid this limitation? Is it an appropiate approach?

Any suggestion is highly appreciated!

[msaeedsadeghi]

The only problem is with the mesh. Try to make a better mesh.

[Bollonga]

Originally Posted by msaeedsadeghi

The only problem is with the mesh. Try to make a better mesh.

Does the mesh have to be much finer in all the wake? That would make the case very expensive.

I've observed that turbulent viscosity ratio limitation appears near the corners of the plate and then it's transported to the rest of the wake.
Maybe if I improve the mesh just there it won't reach the limitation?

[msaeedsadeghi]

Try to make an structured mesh if possible, else you should make a finer mesh.

[Bollonga]

Originally Posted by msaeedsadeghi

Try to make an structured mesh if possible, else you should make a finer mesh.

Sure, I'm using an hexa-mesh. I'm gonna refine the o-grid block around the plate and the areas near the body. I'll share my results here.

[Bollonga]

Besides using a finer mesh, for a turbulent intensity of 5% and 15 m/s in the inlet, which turbulent length scale should I use? I had good results in 2D with k-ep realizable and turbulent length scale of 0.05 m but that setup was giving problems for 3D.

[aditya.pandare]

I suggest you go for a y+ of under 10 and then use the enhanced wall function.
I agree to the suggestion of using icem cfd and getting a structured mesh (wont take more than 2 days to make this, even if u start from scratch)

I also suggest you try a still smaller timestep

if it still doesnt resolve the issue, go for severe underrelaxation for the first few timesteps.

[Bollonga]

I already have an hexa-mesh and first layer thickness of the o-grid block is pretty small so I guess I'll get y+<10.

I'm gonna try a smaller timestep using the adaptive timestep option, say from 1e-3 to 1e-8 s with 10 as maximum timestep factor and 0.1 as the minimum.

However, I would like to know which is the optimum solver configuration, I'm using this one:

Pressure-velocity coupling: PISO (skewness correction =1, neighbor correction =1, skewness-neighbor correction enabled)

Spatial discretization:
Gradient: Least Squares cell based
Pressure: PRESTO!
Momentum: Second Order Upwind
Turbulent Kinetic Energy: First Order Upwind (I'll change it to 2nd order later on)
Turbulent Dissipation rate: First Order Upwind (I'll change it to 2nd order later on)
Transient Formulation: First Order Upwind (in order to use adaptive timestep, I might change it to 2nd order when I'll get a constant timestep)

In case this doesn't work I'll change under relaxation factors as suggested by Aditya.

Originally Posted by aditya.pandare

if it still doesnt resolve the issue, go for severe underrelaxation for the first few timesteps.

The question is for how many iterations should I maintain the reduced under-relaxation factors? And which values should I use?

Thanks a lot guys!

[Far]

You need good mesh in wake region. did you make the domain extend study?

[Bollonga]

Originally Posted by Far

You need good mesh in wake region. did you make the domain extend study?

I did it for the 2D case, 13 times the plate chord downstream was appropiate .

To begin I've used a 1e-8 s timestep (adaptive timestep), 50 iterations for timestep and turbulent viscosity under-relaxation factor of 0.5 (the rest of them as default)

TVR limitation appears from the very first iteration. Divergence appears at only 7 iterations.

I'm initializing the solution from inlet (U=15m/s, TI=5% and TLS=0.05m).

I guess it might be due to bad initial condition... but I'm not sure. Any ideas?

[Far]

13 chords downstream with 70 deg inclination? I guess it is not enough...

Can you show velocity and pressure contours?

[Bollonga]

Originally Posted by Far

13 chords downstream with 70 deg inclination? I guess it is not enough...

Can you show velocity and pressure contours?

I've just checked the former 2D simulation an the domain extend is 30 times chord downstream. I attach static pressure and velocity magnitude images.

I guess I need a similar wake extend in the 3D case, but is initialization from inlet a correct approach?

[Far]

results look good but convergence plot not. Init from inlet is ok.

[aditya.pandare]

reduce the relaxation by an order of magnitude at the most.
use it until your residuals start decreasing (time-step wise).
this is a question of both judgement and trial-error; so try a few times; generally, using the reduced under-relaxn for a few time-steps after the reducing trend begins is sufficient.