Hello,
i'm struggling to produce a good simulation with your model. TED et TKE are diverging quickly.
Did you read this article ?
Other point, your building are really detailled, a lot of feature doesn't had to be there, there are too tiny to have a real impact on the general result. I will suggest you to use a simpler geometry.
Fred
Hello,
I did not succeed to get rid of those unrealistic velocity. Here is what i try :
- uncheck hydrostatic pressure
- add a high flow rate at the intlet to avoid recirculation at the outlet (20'000CFM)
- refined mesh in critical area where high velocity occurs
I became suspicious about the geometry of your model and it might be the cause of your problem.
- My advice will be : extend your air volume, it must be longer ! Your boundary condition is too close to your building and it cause recirculation through your 0 pressure BC. This behavior will screw your continuity equation (mass conservation principle) Usually, in this type of analysis, the flow rate at the intlet, must be equal to the flow who's leaving the model. You have a good summary of those quantities in the results tab under the banner summary file.
- In the last scenario simulated, i was able to get rid of the recirculation by applying a really high flow rate (50'000CFM) the unrealistic velocities almost vanish (see picture below). If you use a smaller flow rate or velocity i.e 10mph you will need extra space to allow air to stabilize after passing near the building.
- The number of element in the last analysis was quite high (4'000'000) this is why i brought up the idea of using a simpler geometry... if you have a lot of computational power go ahead, but otherwise i might be worth it to clean up your geometry.
- Last point, check the mass balance of your simulated system it will give you some hint about the quality of your analysis.
i joint my CFZ
hope it helps
Fred
Hello @Anonymous,
Regarding to your questions :
- We used the Exterior Volume from the Geometry Tool to create the air volume around the building. But it dose not allow to close the gap below the building to model the ground. So the air flows under the building and obviously affects the air pattern around the building and the equipment. Is there a way to close the air gap below the building and the ground?
- From the last CFZ that i got, i dont see any air flow below the buiding. If i'm understanding your question correctly any CAD software can get rid of those gap by simply moving the air volume to the same level as the building lying. External volume can be created through the CAD as well
- We would need to assign heat generation (and rejection) to the 54 chillers on the roof. (see attached for air flow in & out of a typical chiller). Ambient air intake is from the 2 sides and hot air discharges from the top 2 slots (each slot representing where 10 propeller fans forcing the hot discharge air up into the atmosphere).
- how do we assign the KW to each slot (or disc)? Can this be done within a single solid element of the Chiller or do we have to create heat generating element(s) within the chiller. (For simple quick modeling, we are assigning a fixed amount of air flow to the side intakes and fixed amount of discharge air flow at a fixed higher temperature at the top. But this fixed temperature discharge method cannot take into account the variations of air intake temperature change when hot air recirculates back into the intake). We need a more accurate modeling.
- Heat element had to be created separatly because you will assign a thermal volumetric boundariy condition Remember, imposing boundary condition require surface that are external to the computational domain (i.e. velocity BC (m/s) or heat flux W/in^2 can not be defined onto internal surface of the model)
- How do we make sure the air buoyancy is correctly represented where hot air actually rise and does not get recirculated down into the air intake stream? Should we run the simulation as steady state, transient, …. etc.
- Here is the basic parameter to check if you want to take in account the effect of buoyancy. Make sure that the proprety of the air is setted to ''variable''.
- Do you use an initial condition ? If yes transient analysis is required otherwise use steady state analysis.
- http://help.autodesk.com/view/SCDSE/2019/ENU/?guid=GUID-50A1708F-4CB8-4EF9-9E85-6C947E44A7B2
- Here is the basic parameter to check if you want to take in account the effect of buoyancy. Make sure that the proprety of the air is setted to ''variable''.
- how do we assign the KW to each slot (or disc)? Can this be done within a single solid element of the Chiller or do we have to create heat generating element(s) within the chiller. (For simple quick modeling, we are assigning a fixed amount of air flow to the side intakes and fixed amount of discharge air flow at a fixed higher temperature at the top. But this fixed temperature discharge method cannot take into account the variations of air intake temperature change when hot air recirculates back into the intake). We need a more accurate modeling.
If somethig remain unclear don't hesitate.
Hope it helps
Fred
Hi @Anonymous ,
i will make a quick comment regarding your mesh problem :
you have a mesh diagnostics tool under the mesh sizing banner it will help you to spot the area where you need to refine the mesh. Unfortunately this is what i got when use the diagnostic tool on your model :
Long story short, you need more mesh on your surface to overcome this first difficulty. I was able to run the model by simply assign a surface mesh size of 100 (in manual mode) over your entire building.
I will come back to you tomorrow for the rest of your question as well as other recommandation.
fred
Hello Cyrus,
Let's take a step back!
I play around with your geometry and nothing good came from your simulated scenario. CAD Geometry, CFD parameterization are dead wrong here.
Objective
I'm a little bit confused regarding to your goal. I'm not even sure if i understand what your trying to achieve here.
- You are looking for the temperature inside your building ?
- The total heat transfered to the outside environment ?
- The cooling effect brought by the cold wind ?
- All of the above ?
Defining clearly your objective will help you to build a CAD model more suitable for your needs. All the detail does not need to appears in your geometry because some feature are often irrevelant to your objectives. Saying that, this lead me to the next topics your CAD Geometry....
CAD Model
In this particular case, your CAD model is the sources of all the problems :
- You have (a lot) of overlapping wall, small edge, tiny gap. This is not sustainable of a CFD analysis.
- you have too much feature designed (tiny object in a huge space) this will eventually lead to an expensive computational simulation.
Your geometry must be cleaned or reworked.
Air modelization inside your building
Another confusing point is what happen inside your building. Do you want to simulate the air ? if the answer is yes air has to be modeled. Right now it is modeled but only in localised area
Your cad geometry must be alligned with your goal or your objectives.
CFD Parameterization
Try to reflected on the following point :
- What are the local or global information required for the intended cfd simulation.
- What are the important flow physic to be solved
- What are the area of primary interest or domain of the flow calculation
- What level of validation is necessary for the cfd problem
This is more general comment more than trouble shooting specific issues but i think it will helps you.
Good luck and if you had other question don't hesistate.
Fred
Hello Cyrus,
You have a critical area right here , inside the building where air flowing at high speed. Is it correctly modeled ?
If it doesn't are you able to suppress the air volume in this area.
The tiny air gap below the building might be removed as well
