Autodesk CFD - Wind velocity at the end of wind tunnel is unusually high

[Anonymous]

Please see the attached image. We have noticed this condition for simulating a building exposed to 10 MPH wind form N and/or NW directions. The surface at the end of the tunnel with zero (0) pressure shows some unexcepted results with wind reversing direction towards the building at high velocities (600 to 800 MPH)!!!  We expected to see the wind speed stay the same or slow down as it gets to the other end.

Could you please help us with understanding what is going on ….and how to correct it? Support file is also attached.

[frederic.gaillard.7]

Hello, 

Your fluid recirculating through your 0 pressure boundary condition, and i think it induces those high velocity. 
unfortunately your support file is not available, can you share it again ? 
Try to compress your cfz file into a folder otherwise it wont work.

Thx 
fred 

[Anonymous]

I am trying to attach the zip file czf. But if the file is too large it may not go thru.

Also I tried to send you a link to a dropbox location via my office email. Please let me know if you could access it.

What is the best way to send you a link from the message board?

Thanks,

[frederic.gaillard.7]

Hello, 

In both scenario you have recirculation which is responsible for the high velocity. Lack of mesh could be the cause. 

Try to apply a finner mesh over your model. 

- uniform et dense mesh on your BC surface (velocity and pressure) 

- Refined meshing region around your building 

However not 100% sure if it will resolve this issue. 

Fred

[frederic.gaillard.7]

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

[Anonymous]

Hello Fredric,

We reviewed your suggestions. Also, regarding the simplification of the geometry. It has already been simplified to the extent that we could. We need the elements as shown in order to run the next phases of simulations when we assign high temperature discharge flow to the generators and the chillers on the roof.

We have not been able to find anything that could help with the extreme high velocity problem.

Is there any other suggestions you and others in the community can provide?

Thanks,

[frederic.gaillard.7]

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

critical area - high velocitycritical area - unrealistic pressure

I became suspicious about the geometry of your model and it might be the cause of your problem. 

1. 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. 
2. 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. 
3. 
4. 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. 
5. Last point, check the mass balance of your simulated system it will give you some hint about the quality of  your analysis. 

High Intel Flow Rate Refined

i joint my CFZ 
hope it helps 
Fred

[Anonymous]

Hello Fredric,

Thanks for the suggestions. I increased the volume and it helped greatly and the results make more sense now. I do however still see the velocity increases on the opposite (exiting side) of the wind. This time from 10MPH up to ~ 20 to 30 MPH.  But the air patterns are all stable and streamlined. Not sure why even any velocity increase!?

I also could not open your attached file with 2018 version of CFD.

Thank you.

[Anonymous]

I also wanted to share this screenshot from the latest simulation and the convergence plot. It has not yet shown flat lines. TED keep rising. Not sure if this is acceptable or if more time will help to flatten it.

Thanks,

[frederic.gaillard.7]

Hello @Anonymous , 

I use the 2019 version, unfortunately you can not open the CFZ that came from a more recent version. Since you start with v2018 i will suggest you to stick with this version, there is no need to switch to this specific version. What you can do is to share your lastest cfz and i will check for the high velocity on the exit side. 

About the TED. 

TKE and TED are involved in the turbulence modeling. TED specifically are responsible for the dissipation of turbulence.
Your convergence plot look fine : 

• the wavy profile of your TED is probably caused by a lack of mesh.
• the overall behavior of this curve is good. You will need an extra 100 iterations to appreciate a flattened line. Usually TKE and TED tend to be equal. 

Hope it helps 
Fred

[Anonymous]

Thanks again!

Few follow up questions:

1. 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?

2. 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). 

 A---> 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.

B---> 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. 

Thanks,

[frederic.gaillard.7]

Hello @Anonymous, 

Regarding to your questions :

1. 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?
   1. 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
2. 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). 
   1. 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.
      1. 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) 
   2. 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. 
      1. 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''.
         
         
      2. Do you use an initial condition ? If yes transient analysis is required otherwise use steady state analysis.
      3. http://help.autodesk.com/view/SCDSE/2019/ENU/?guid=GUID-50A1708F-4CB8-4EF9-9E85-6C947E44A7B2

If somethig remain unclear don't hesitate. 
Hope it helps 
Fred

[Anonymous]

Fredric,

Thanks for your timely feedbacks.

Please see the new attached CFD 2018 CFZ support file, and few screenshots.

This is the same building, with new arrangement for the rooftop chillers, (4-feet elevated and no canopies). The roof now is shown with screen walls (50% open louvers) and service platform (75% open grating). The air mass around the building was modeled with "Exterior Volume". The gap below the building is still there, we have not changed it in CAD file yet. The chillers also show "FIXED" hot air discharge at 130 F. We have not changed that yet to heat generation. … which we hope can change later on the next rounds of simulations.

As it is now, we are seeing problems with the meshing after the louvers and grate were added. We have tried many meshing refinements and diagnostics. But cannot figure out how to fix them.

Also, from the last post, we still have questions on what the best way is to change the fixed 130 F discharge temperature by adding internal heat generation source on the discharge surface of the chillers, which will allow for variable discharge air temperature.

Thanks for your timely feedbacks.

[frederic.gaillard.7]

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

[frederic.gaillard.7]

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 

This From your last CFZ shared you still have issue with your boundary condition. The 2 pressure boundary condition located next to each other will favorise recirculation. Ideally, for this type of analysis, impose 1 hard BC (velocity, flow rate) and one soft BC (0 pressure gage) 

In your first post i understood that several wind direction will be tested (N, NW). Regarding to my last suggestion i recommande you to change the orientation of your building and fix your flow/velocity and pressure boundary condition on designated surface.

For the moment i will not comment on the termal part of your simulation because there is more important issues. And generally it is irrevelant to add thermal layer if your flow had reciculation or irrealistic behavior. 

General Work Flow

Beginning with a simple geometry and gradually add layer of complexity is generally a faster way to success. This mean you have to go back-and-forth between cad and cfd software but it will point out rapidly the issues that you cfd analysis is facing. 

Try to reflected on the following point : 

1. What are the local or global information required for the intended cfd simulation.
2. What are the important flow physic to be solved
3. What are the area of primary interest or domain of the flow calculation
4. 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

[Anonymous]

Hello Fredric,

Sorry for any confusion. Please see the attached narrative.

[Anonymous]

Fredric,

We just suppressed the components called LOUVERS and GRATE resistance, and the meshing problem went away!

as we ran the simulation in steady state for 30 iteration. seems to be working, but not seeing the flat line in convergence yet. Now we are trying to run it longer and in transient to see what happens. Will let you know.

Would still like to see your feedback on the other matters.

Thanks,

[frederic.gaillard.7]

Hello Cyrus, 

Thank you very much for your detailled answer. It's more clear now!
i will try on my end and let you know if i found something. 

Fred

[frederic.gaillard.7]

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

[Anonymous]

Hi Fredric,

Nothing inside the building is critical. It should all be a solid block. I think we have already assigned the entire building as solid steel. Are you seeing a gap that is not closed and connect it to the outside air? What is the best way to find it, isolate it and suppress it?

Also, how can we isolate the gap under the building?

Thanks,