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]

Correct me if i'm wrong but this section should not be fill with air, right  ? 

[Anonymous]

It can be solid or air. Because we are not going to do anything with the inside volume. It should be completely isolated from the outdoor wind and air flow around the equipment. 

[frederic.gaillard.7]

Hello Cyrus, 

If this region is not revelant to the analysis it should be suppressed from the mesh for basically two reason: 

• You will save computational time
• you have unrealistic behavior inside the building and the solver seems to struggle to compute the solution in this area

I was able to run a flow simulation without ''major problem'' 

velocity fieldsGrid MeshConvergence Plot

According to your convergence plot there is something going on at the early stage of the simulation. It's hard for me to give you an explanation about this odd behavior.

I will try to solve your thermal problem with a simpler geometry. I will give you some news when i succeed. 

Fred

[Anonymous]

Thank you again Fredric.

Few questions:

The region you are referring to is it inside the building? I thought in our model all the building elements were suppressed. But apparently some regions were not. How do we detect this region that is not suppressed?

It looks like you used 5m/s for velocity as compared to 10 mph. Could you please confirm.  I believe lower  velocity would have  a significant impact on the results.

Did you use external volume to set up a wind tunnel? Is the wind from north and not northwest?

I assume you used CFD 2019, so we would not be able to use your version of the CFZ file in CFD 2018.

Would you be able to send me the screenshot of the settings you used for you simulation.

Cyrus.

[frederic.gaillard.7]

Hello Cyrus, 

The region you are referring to is it inside the building? I thought in our model all the building elements were suppressed. But apparently some regions were not. How do we detect this region that is not suppressed?

When a region is suppressed it appears in blue when you are in the mesher. As i pointed before, we are able to see velocity/pressure field inside your building which confirm the presence of a fluid. 

unwanted fluid

It looks like you used 5m/s for velocity as compared to 10 mph. Could you please confirm.  I believe lower  velocity would have  a significant impact on the results.

I did not paid attention to the boundary condition when i was simulating sry about that. But you are right it will affect the result significantly. 

Did you use external volume to set up a wind tunnel?

No, personally i never use this tool to create external volume. My external volume is created in the CAD. It's easier to apply constraint on the different volume and avoid small gap like you have experienced.

Is the wind from north and not northwest?

Again i did not paid attention to this parameter, but i will suggest you to apply one velocity BC and one pressure BC on the outlet of your system. Just rotate your building to recreate the NW wind 🙂

I assume you used CFD 2019, so we would not be able to use your version of the CFZ file in CFD 2018.

Would you be able to send me the screenshot of the settings you used for you simulation.

I use v2019.1 so yeah unfortunately you won't be able to open my CFZ. 

i'm currently working on simplified version of your model to check and evaluated these aspects : 

• Continuity 
• overconstrained model
• Thermal Modelisation

I will come back to you tomorrow. 

If you think it can help you, i can share the results of my oversimplified model through google drive but you will need to switch to the 2019.1 version. 

Hope it helps
Fred

[frederic.gaillard.7]

Hello Cyrus, 

I was able to stabilize the thermal solution of your analysis with two flag : 

thermal_advection_scheme = 1

resid_heat_flux_calc = 0

Flag Manager
I change some parameter on the solver 

• Change to a steady state solution mode
• Uncheck hydrostatic pressure.
  • Any specific reason why you enable this hydrostatic pressure ? In my perspective it might not be necessary to taking care of this parameter since the weight of the fluid is negligible. If it is for a natural convection matter simply use a gravity vector as well as an air variable proprety (material editor) check these following link for more information : 
    • Hydrostatic Pressure 
    • Natural Convection 

About the simulation, i kept a simple mesh, so there still place for improvement here. Here is some image of my result

Basic Flow SimulationBasic Flow Simulation - close upThermal SimulationHydrostatic Pressure

The two first image are from a simulation where only flow was simulated (0.01% error on the continuity equation)

The third was a shot of the temperature where heat and flow were considered 

The fourth was the effect of the hydrostatic pressure. As you can see, i have recirculation at the of my model. Air leave and enter through the pressure BC. That is the main reason why i unchecked this parameter. 

i join a step file of a simplified model of your geometry, it is an easy way to make a proof of concept of your problem. I also join a the 2019cfz file

Hope It helps
Fred

[Anonymous]

Thank you Fredric,

Is there a possibility to save  and send the files in the older version (CFD 2018) ?

[frederic.gaillard.7]

Hello Cyrus, 

Just for following about what we discuss last time, the idea was to modelize a frame in the ''air-cooled chiller room''.

The frame (in gray) , supressed from the mesh, will have a heat flux boundary inside this space and it will allow to withdraw heat from this same space. This way, the chilling effect will be roughly approximated. Be careful about the sign of the heat flux value :

( + ) positive value simulate a flux who is leaving the control volume 

( - ) negative value, heat is injected inside the control volume.  

Simulate the impeller inside the air cooled chiller room  might be a good idea for at least one chiller.  You will have a better understanding of the physic involved. 

For proof of concept or validation don't hesitated to use simpler geometry. 

Keep me posted of your progress
fred