y+ Value & Aspect Ratio {Wind Tunnel Model}
 

Hi, I am modeling a wind tunnel test with ICEM and Fluent.
Basically it is a box (cube=building) in a box (wind tunnel).


I need to describe as good as possible the turbulences and the detached flows around the bluff-body, especially in the corners.

In Fluent I will use different models, starting from kepsilon.

Question_1: I will need to have y+=1 close to the walls of the building, how can I do it?

I've already done a really coarse mesh to make an attempt and Fluent gives me values of the wall shear stress of ~0.03 Pa.

I tought then just to apply the formula

y+=[density*y*sqrt(shear_stress/density)]/viscosity

In my case, looking for y wich will be the dimension of the first step of the grid close to the wall:

density=1.225
shear_stress_wall=0.03
y+=1
viscosity=1.789*10^(-5)

yields to y=0.00009332 m

Does it make sense?
After the first cell how much can I increase the step distance?


Thank you very much, I attach a really coarse mesh as an example.

Question_2: Trying to make a mesh less coarse than the first one Fluent gives me a warning on the aspect ratio. But considering I have to model thevoundary layer and that the steps have to increase far from the walls for CPU reasons, I will always get low aspect ratio!
Suggestions?


Thank you very much for any reply!

Fabio

Considering that the cube is 0.5m*0.5m, assuming 0.00009~0.0001 would mean to have every edge of the cube divided in 5000 parts, and it would lead to an enormous number of elements for Fluent!

I hope I am making a mistake somewhere.. any reply will be really appreciated!

thanks,

Fabio

Try this for your y+ calculations, should make it much easier in predicting your wall spacing

http://geolab.larc.nasa.gov/APPS/YPlus/

Hi, thanks.
Actually I've already seen that page looking for something on the web, but I didn't understand what the Ref. Length is, so I don't know how to use it.

Do you know what the Ref. Length is?

Thanks,

Fabio

Hi FabioT

I have performed some simulation about the wind loadings on bulidings.

I think the empirical formula based on my knowledge to calculate the y plus is not accurate.

I have an empirical case for your refference.

When the inflow is 7.5m/s, rng k-e turbulence model is applied and the grid first layer heights equal to 0.0001m, the y plus will approximate 1.

Hi bluelc, thanks!

Where did you get that value from? Can you send me any reference?

Actually the wind speed in my case will be 15 m/s, and it will probably change the value of y+!

Any suggestions?

Actually, having such a small value of y+ will lead to a really fine mesh. Does anybody know how long will a simulation take (of course, it will depend on the CPU).

Thank again,

Fabio

Reference length is the characteristic length of your geometry. For a wing, it is the mean aerodynamic chord, for an airfoil it is just the chord. For this box, it would be the edge length.

What I mentioned is based on my simulation results.

Ok, thanks.
And what do you think about the wind speed?

How long did your simulations took and with what kind of CPU? Thanks,

Fabio

Wind speed is proportional to the Reynolds Number. So, the increase of wind speed requires smaller boundary layer grids height, but the relationship is not linear.

The CPUs I used are XEON 5430 * 16 in 2 cluster node. For a 2,500,000 grids problem, I think 15 hours is enough supposing no crash occurred.

This is not right... For your Y+, we are only concerned with the distance normal to the wall, not the size along the wall. (by the way, you should calculate it from your Re using your average building edge length).

Once you know your Y+, you should create an OGrid around your building and then setup the edge for the OGrid to have a spacing at the wall of 0.0001 and a growth rate of 1.2 away from the wall.

OGrid is better than Hgrid for this boundary layer because the refinement is localized exactly where it needs to be and won't propagate out in all directions.

Along the other edges of the building you should have a much larger and more reasonable size, it may not need to be much finer than your coarse example, except that you may want it to refine closer to the corners using a bi-geometric or bi-exponential mesh law.

You may also want to put an Ogrid in the block behind your building so you can refine locally and capture turbulent flow features. Optionally, you could use 2 to 1 refinement in the block behind the building.

Good answer!

Hi, thanks.

Of course, I don't want the edge to be divided in constant steps.

I agree that I have to worry only about the distance normal to the walls, but the floor is a wall, too. This is why I need to refine the mesh long the edge of the building.
I have already tried to use a "Spline" distribution along the edge, but it gives me errors at the corners (see attached images of some failed attempts). I think the reason is that ICEM has to approximate the distribution and doesn't match the corners, but I don't know how to fix it.

I like your idea of the O-Grid, but I am not sure how to do it. Do I need to make a bigger box before doing the o-grid or there is a way to do it from the blocking I already have?

What is the offset of the O-grid that I have to choose in you opinion?

Thanks for the replies!
Best,

Fabio

Ogrid.
 

Your blocking edges appear to be surface projected. You should associate them with the curves along the edges of the building.

Your Ogrid can be along the surface also. (you do not need to refine along the edges of the building).

TO apply the Ogrid, go into Split Edges => OGrid.

For Select Blocks, add/select everything in the fluid domain.

For Select Faces, add/select all the boundary faces except the buildings and the ground. Basically, this should mean just your inlet, side walls, outlet and top of the box. You can use the from corners selection method to make this a very quick process. (pick the diagonal corners of the FF box).

Hit apply. (Ogrid is easy and powerful. Try some tutorials to learn more).

It will give a default thickness to the Ogrid based on the geometry, no the flow conditions. You can rescale Ogrid if you wish (under edit Blocks). The ideal height of the Ogrid is a bit more than the total thickness of your boundary layer. I usually start with the default and then adjust if my post processing suggests that my boundary layer is not contained within my Ogrid.

Experts can use Ogrid in fancier ways to generate a more efficient mesh or better capture expected flow patterns... Explore.

Hi PSYMN

I have a question. How to attach a 3D high quality prism mesh around an internal wall (no thickness)?

Thanks in advance.

Stair Step
 

Hey Bluelc... Try not to hijack a thread with something unrelated. You can always create a new thread and then send me a private message with a link so I will be sure to go look at it.

I have been off traveling for a while, but decided to take a couple hours for CFD Online today.

In this case, I assume you are really asking for prisms that extend over the entire surface and don't taper off as they approach the edge. You need 12.1 and you need to turn off the "stair step" option under Advanced Prism Options.

Attachment 4761

Be aware that Some solvers prefer the stair stepping "on" approach (don't like all the pyramids in one place).

Other tricks include creating a construction surface that extends beyond your surface. Prism that and then delete the shells. This creates an effect like prisms trailing behind your surface. Here is a screen shot of it done behind a sharp trailing edge of a wing, but it would work just as well for a baffle...
Attachment 4762

This is good because it takes the pyramids away from the critical edge of the baffle... you can then let them stair step out...

Hi, I think you are right.
Can anybody tell me how to fix it?

I attach a couple of pics that show the problem! Basically the problem is that the mesh does not respect the geometry (but I'm pretty sure I've associated the surfaces and the edges, too). I want the mesh on the boundaries to be on the plane of the sides of the box.

Of course, the finer the mesh the worste the effect!

Thanks a lot, PSMYN you can answer me in the email as well, as you prefer!

Have a good day,

Fabio

Any answer?
Please let me know.

Thanks a lot.

Hands on help...
 

Hello Fabio,

I will actually be in your area at the EnginSoft ANSYS user conference on the 20th and 21st of October.

http://www.caeconference.com/event.html

Will you be attending?

My comments on your model...

1) You don't need to chop up the geometry to match the blocking... The blocking works nicely and more flexibly without all this geometry work. I recreated your geometry from scratch using the script (run it with file => Replay), you could edit the script to adjust the box sizes or location, etc. you will see that without being constrained to the curves, I can adjust my blocking for optimal quality.

2) You could have prevented Ogrid along your inlet and outlet face... You don't need Ogrids there, so it is a waste. When you create Ogrid, Face those blocks...

Attachment 4866

3) You didn't associate the edges of your blocking with your curves... This is what caused the problems in your above images. I actually just used the auto associate as you will see in the replay script... But usually, you would use Blocking => Associate => Edge to Curve...

4) Then I played with the edge params... Matching edges and copying distributions to parallel so that my mesh transitioned smoothly (your original mesh was good element quality, but horrible transition quality...)

It is pretty easy to mesh models like this in ICEM CFD.

Attachment 4867

You could also go more complicated if you wanted to. In this case, I put the Ogrid in a different way... The first wrapped around the box and a block behind it... Then I put one around just the box. Then I put one inside the two blocks behind the box... Next I could put the tunnel boundary layer thru, etc. Adding each Ogrid in the ICEM CFD way is pretty easy. Adding those in any other hexa mesher would be very difficult.

Attachment 4868

And the more complicated the model is, the further ahead ICEM CFD gets.