CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   modelling wind movement (http://www.cfd-online.com/Forums/star-ccm/67363-modelling-wind-movement.html)

 charltonjames August 12, 2009 18:15

modelling wind movement

Hi All,

thanks for the help everyone. i appear to have successfully generated a volume mesh for my city square, which is enclosed within a box. I have changed one of the sides of the box into an inlet and the opposite to an outlet (i hope thats right). I wish to now model wind movement within the square, it doesnt have to be precise now, just a pretty pattern or two will do. Although i dont fully know what is best way to show wind movement within CCM+ is, from my weeks experience with the software, im thinking a nice vector diagram.

So any suggestions on what to do next?

Cheers

James

 highnelly August 13, 2009 05:32

Hi,

You need to set up you inlet to represent an atmospheric boundary layer, although you probably know this already, (if not look up Journal of wind eng. and indust. aerodyn. in sciencedirect to get plenty of recent references; look up Bert Blocken).

Other than inlet and ground, I would have pressure outlets on all other surfaces of the box, and make sure tick the extrapolate option for backflow on these boundaries that are aligned with your wind-flow.

After that you can solve and get some pretty pics.

The following are the equations you need fro your wind profile in a rural (barren location) so they may need to be modified for city region:

where is your ref vertical height, is your roughness height, is von Karman constant; is your ref wind speed, is turb model constant; and is your frictional velocity.

 charltonjames August 14, 2009 04:52

Hi highnelly, thanks for the help!!

I have a couple of follow up questions if you dont mind. I cant find the extrapolate option for backflow, could you please guide me to were this option is. Also, i have the inlet set as a velocity inlet, is that correct?

I have carried out a test on my model using the simple flow tutorial within CCM+ as a basis and it appears that the flow is entering the volume in one small funnel. Is there a way that i could specify wind entering the volume for the whole inlet face?

Any other suggestions would be gratefully appreciated.

Regards

James

 highnelly August 14, 2009 06:13

1 Attachment(s)
Hi,

When you change the boundary type to pressure outlet; go to physics conditions/backflow option/extrapolate; (maybe you need to initialise the solution first before it comes available)

Its important to use this option for the pressure boundaries aligned with the flow.

So, in you box you will have 3 pressure boundaries and and 1 inlet similar to the image i have attached, which is similar to your setup except the box is sliced down the sym plane. (just click on the face and change the boundary condition to whatever you want in properties)

Also, If you want any accuracy you must set up the wind profile at the inlet, using field functions is the easiest way. However, if you just want pretty pics, then change the wind velocity and direction on the default inlet to whatever you want and away you go.

 charltonjames August 14, 2009 07:25

Thanks highnelly, you are being very helpful!!! I will try out your suggestions. At present i am not trying to create an accurate wind environment, i will need to do more research into formulers etc first. Im simply trying to show wind entering the city in a certain direction at a set speed, say 6 m/s or something like that. Could you please confirm where i set the wind velocity and direction. Is this within Regions > Region 1 > inlet > etc..... or is it within my Continua > Physics 1 > etc....

I have set my physics 1 as follows;

Three Dimensional is selected (from the Space group box).
Gas in the Motion group box

Coupled Flow in the Flow group box

Constant Density in the Equation of State group box

Turbulent in the Viscous Regime group box.

Select K-Epsilon Turbulence in the Reynolds-Averaged Turbulence group box

Does that sound ok to you???

Thanks again

James

 highnelly August 14, 2009 08:01

I would advise you use the segregated flow model, with high y+ standard k-e turbulence until u get a better understanding for what is needed.

In Region 1 I assume that you have many patches; some of these belong to the city and some to the outer box. I would advise that you clear your meshes and combine the faces that represent your city. This will reduce your number of boundaries (I presume that all the buildings will have the very same wall conditions). Then you will in effect have the city boundary, the ground boundary and the 3 outlet and one wind boundaries. Rename all these to whatever, i.e. wind for inlet, atmosphere? for outlets.

once you have this done you go to the specific boundary and set the mesh and physic conditions. It sounds like you went with the default mesh size and skipped this bit but it is advisable that you put larger cell size on your box boundaries than on your city. On your wind boundary you set the conditions you want.

If you want a finer mesh in different areas you can use volumetric controls

 charltonjames August 14, 2009 10:09

Thanks again!! i think i am sorted now.

I have the following boundaries;
• City - wall type
• Ground - wall type
• Wind (West) - Velocity Inlet
• North Atmosphere - Pressure Outlet
• South Atmosphere - Pressure Outlet
• Sky Atmosphere - Pressure Outlet
• East Atmosphere - Pressure Outlet
I have a generated a volume mesh, with different mesh sizes for the city and the surrounding boxes.

I have set up a physic model as follows;
• Three Dimensional is selected (from the Space group box)
• Gas in the Material group box
• Stationary in the Motion group box
• Segregated Flow in the Flow group box
• Constant Density in the Equation of State group box
• Steady in Time group box.
• Turbulent in the Viscous Regime group box.
• K-Epsilon Turbulence in the Reynolds-Averaged Turbulence group box
I have also, set the wind speed within Regions > Region 1 > Wind > to 6.0 mph.

The backflow option for the pressure outlets aligned with the flow have been set to extrapolate.

So, i guess now i want to set up a new scalar scene, select my parts and change the little blue bar to show velocity. Then initialize solution before i Run!!

Is that correct? Do you have any other suggestions??

Thanks again,

James

 highnelly August 14, 2009 12:48

yes it sounds good for a rough calculation.

If you want to get more detail in specific areas you will need to refine the mesh. Use volumetric controls for that.

Also, I dont know if you have prism layers in your final mesh. These are essential for good convergence and to hold accurate the assumptions that go with the wall conditions. try to keep y+ 30-60.

Strar-CCM+ is the nicest software I have used for this type of simulation (although anything is nicer than Phoenics i guess), so Enjoy

let me know if you need anymore help or there may be others that can advise more on this!!

 plainstyle May 10, 2010 02:52

Log law Wind profile?

Hi anyone managed to set log-law wind profile for simulations of this type?