Recirculation in the outlet even with the extended surfaces

[Anonymous]

Hello everyone,

I have an extended surfaces in the outlet and inlet to avoid recirculation, however when I see the velocity vector it looks like some of the air is coming into the system from outlets.

The solution looks quite instable.

Also, in order to simulate damper in the exhaust, do I use volumetric flow rate with reverse direction?

Please see the attached model.

Thank you in advance.

-Parshu 

[frederic.gaillard.7 · Accepted solution]

Hello @Anonymous, 

You will need more mesh on your outlet. Try to refine the outlet surfaces with a 0.25 uniform factor, and then clic spread. I'm running your simulation, few thing are not set correctly. 
fred

[Anonymous]

Thank you for the reply.

Okay I will set 0.25 factor for mesh in the outlet and run again. Please let me know if I need to make any other changes.

-Parshu

[frederic.gaillard.7 · Accepted solution]

Hi again, 

I run your simulation. For the moment,  I disable heat transfert analysis and keep only flow analysis. I, also suppress all solid part from your model to decrease the number of element. The steady state solution will converge faster this way. Once your flow is correctly resolve you can add the thermal analysis, this way you will reach the solution more quickly, it is generally a good practice.  

1. I was able to eliminate the recirculation simply by adding refinement factor of 0.5 & uniform, on every outlet surface. Clic ''spread'' right after.

2. i agree, your solution doesn't look stable. The lack of meshing in critical region might be the cause. I will try to enhance the mesh near the internal fan and on your deflector  

3. ''Also, in order to simulate damper in the exhaust, do I use volumetric flow rate with reverse direction?'' not sure to understand what you trying to achieve here. 
Fred

[frederic.gaillard.7 · Accepted solution]

Hello @Anonymous, 

I ran your model over night, i focus only on flow analysis and i supress every solid part within the model. 

I think there is something wrong in your boundary conditions. You apply two volumetric flow rate one who enter in the model the other who's leaving the model. You should suppress the volumetric flow rate BC  who's driving the fluid outside the model (remplace it by a P=0 BC) Keep the other one at 370CFM ! 

Right now your convergence pattern acting very sillyI also check your mass balance on every intlet/outlet, here what i found 

Intlet (1) = 210.4 g/s 

Intlet (2) = -113.7 g/s

Outlet (1) = -1.2 g/s

Outlet (2) = -1.3 g/s

Outlet (3) = -1.2 g/s

Outlet (4) = -1.3 g/s
your mass balance is 45% off !  You can not have reliable result with this actual setup. 
Hope it helps 
Fred 

[Anonymous · Accepted solution]

Hello,

Thank you so much for your input.

The outlet in the top has an exhaust fan and a damper, which controls the amount of air going out of the system. If I put P=0 in the top exhaust, I cannot control the amount of air going out from top exhaust.

Is there any other way than having P=0 at top exhaust to simulate the function of a damper?

[frederic.gaillard.7 · Accepted solution]

Hello @Anonymous , 

For the damper you can run transciently and applying a transient pressure BC who's time dependant. I choose piecewise linear but you have other mathematical function. 

If it's more suitable for you, you can inverse your volumetric flow rate BC : Keep  your VFR BC at the outlet to simulate your damper correctly and change the other VFR BC for a pressure BC at the entry of your system. 
Keep in mind that if you have multiple volumetric flow rate boundary condition there need to be unidirectional 
(they're all coming into your model or they're all driving the flow outside of your model)

**  **

I just ran your simulation with the new setup and i still have a non-existent  pressure,  that is not normal ! 

Is your gemetry are correctly designed ? 

it is the first time that i saw this behavior not sure what could be the cause. 
Thank 
Fred

[Anonymous · Accepted solution]

Thank you again.

I will try to have pressure BC in the inlet instead of VFR and volumetric flow in the outlet.

I will get back to you when I get the result.

I appreciate your help.

-Parshu