# Scaling down a building

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 5, 2011, 09:03 Scaling down a building #1 Member   Faisal Durrani Join Date: Nov 2009 Location: England Posts: 62 Rep Power: 16 Hello guys, I am looking at using LES to model natural ventilation inside a building. I am supposed to model a building with occupants. Obviously i can not model the building with the same dimensions. I am thinking of scaling down the dimensions of the building. But dont know how to scale down the heat source (occupants). I mean initially the building has around 33W/m^2..... so if i scale down my building what should be the heat source then? Thank you, you experts out there.

 July 5, 2011, 20:15 #2 Senior Member   Julien de Charentenay Join Date: Jun 2009 Location: Australia Posts: 231 Rep Power: 17 Hi Faisal, I don't understand the statement that you "can not model the building with the same dimensions". Does it has to do with using LES and having to resolve turbulent scales? Anyway to answer your question, the heat source within the building is usually expressed as W/m2 of floor area (or net lettable area). Consequently, the heat source should readily scale with the spatial scale: If the spacial scale is 1m (real) to 1cm (model-1:100), then the heat source in your building would scale from 33 W/m2 (real) to 33 W/cm2 (or 0.033 W/m2 in the model). Hope this help. Julien __________________ --- Julien de Charentenay

 July 6, 2011, 06:31 #3 Member   Faisal Durrani Join Date: Nov 2009 Location: England Posts: 62 Rep Power: 16 Thank you julian for your kind reply. I said "i can not model the building with its same dimensions" because i am thinking resolving a 3m building will take longer than resolving a 3cm building right? Or will it take the same amount of time if the grid resolution is the same... meaning splitting the both the geometries to lets say 10 million nodes. Thank you.

 July 6, 2011, 21:33 #4 Senior Member   Julien de Charentenay Join Date: Jun 2009 Location: Australia Posts: 231 Rep Power: 17 Faisal, If all quantities are scaled properly (i.e space, velocity, and loads), it should not take "longer" to solve the 3m building than the 3cm building provided that the number of control volumes in your mesh remains the same. In my opinion, scaling makes sense for an experimental setup but not for a simulation. Scaling need conserve the correct non-dimensionalised parameters are conserved. Not withstanding the above and considering that you are wishing to undertake LES, there is one aspect that is affected by the scaling - provided that air thermodynamic properties are conserved: - The mesh resolution (i.e. the smallest scale resolved by your mesh, in other words the physical size of the small cells) will be lower for the 3cm building. If the viscosity is not changed between the 3m and 3cm building one can then assume that the 3cm building simulation will have a better resolution of the turbulence spectra. But, in my opinion, the viscosity may have to be changed for the smaller building to scale with Reynolds number. In short, I would recommend you run on the 3m building (i.e not scaled). You will need to check that the mesh resolution is sufficient for LES purposes. You might be able to run a steady-state solution, extract the turbulent length scale from the turbulent kinetic energy and dissipation, and compare it with the mesh resolution or you can try to do it a posteriori (mesh sensitivity study or extract of turbulent kinetic energy spectra for example). I hope that I did not confuse you too much. Kind regards, Julien __________________ --- Julien de Charentenay

 July 7, 2011, 06:23 #5 Member   Faisal Durrani Join Date: Nov 2009 Location: England Posts: 62 Rep Power: 16 Hello Julien, firstly sorry for spelling your name wrong in the last post of mine. Secondly you seem to be a very experienced person in the field of CFD. You answer has helped cleared out a lot. I am using LES because I will be looking at transient behavior of plumes etc. Seconly I have access to a 72-processors computer so I can easily do LES simulations. What I do is the first I run a RANS simulation on the mesh i intend to use. For that mesh i plot L/delta i.e. (turbulence kinetic energy^3/2/Turbulence eddy dissipation)/(Volume^1/3)..by plotting this value i see where in the mesh the value is higher and lower than 12. If the value is above 12 in the area its ok for LES and if its below 12 i have to increase the resolution over there. Then once happy with the mesh I run LES simulations. But thanks again for your kind help. I wish I reach a point where I have enough knowledge to answer questions like you can. What exactly is your job in Australia? Because if Australia is big on CFD engineers I might just come there after my PhD because England is not in much need of CFD engineers

July 7, 2011, 13:02
#6
Senior Member

andy
Join Date: May 2009
Posts: 263
Rep Power: 17
Quote:
 Originally Posted by faisal_durr Seconly I have access to a 72-processors computer so I can easily do LES simulations.
A few days on 72 processors may or may not be sufficient depending on how much of the flow field is required to be resolved to get reliable LES simulations.

Quote:
 Originally Posted by faisal_durr What I do is the first I run a RANS simulation on the mesh i intend to use. For that mesh i plot L/delta i.e. (turbulence kinetic energy^3/2/Turbulence eddy dissipation)/(Volume^1/3)..by plotting this value i see where in the mesh the value is higher and lower than 12. If the value is above 12 in the area its ok for LES and if its below 12 i have to increase the resolution over there. Then once happy with the mesh I run LES simulations.
Successful engineering simulations with LES tend to require that most of the fluid motion that creates turbulence is accurately resolved in time. This is straightforward for the "large eddies" away from solid surfaces but usually becomes impractical near solid surfaces. In these regions stronger assumptions about the turbulence are usually introduced and these can become the factor limiting the accuracy of the overall simulation but this does depend on the type of flow.

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post [foam-extend.org] Error compiling OpenFOAM-1.6-ext Canesin OpenFOAM Installation 137 January 20, 2016 15:56 Jenny CFX 6 December 10, 2013 04:52 Tanay OpenFOAM Installation 9 September 23, 2011 12:40 faisal_durr ANSYS Meshing & Geometry 1 July 6, 2011 15:39 darenyang OpenFOAM Installation 0 April 29, 2009 05:55

All times are GMT -4. The time now is 16:47.

 Contact Us - CFD Online - Privacy Statement - Top