Reynolds Number and LES Resolution

[Saharrp95]

Dear developers,

Hello, I have a question and it would be highly appreciated if you could help me answer it.

In my simulation, the computational setup represents a small wind tunnel with dimensions of 0.6 m (x-direction) × 0.26 m (y-direction) × 0.09 m (z-direction). Air flow enters the tunnel at a velocity of 1 m/s, and a pine needle fuel bed is positioned at the center of the chamber.

How should the Reynolds number be properly defined for this configuration both for the boundary layer and around the particles, and what criterion or metric is typically used in Large Eddy Simulation (LES) to verify that the large-scale turbulent eddies are adequately resolved in such fire-simulation domains?

My focus mainly is on the metric that can be used for the LES.

Thank you in advance for your help.

[rmcdermo]

Ultimately, you need to show grid independence of your result. But within reason, you should aim for a y+ of O(100), which puts your first off wall grid cell in the log layer. Any other length scales in your problem need 10-20 cell for resolution. With a wind tunnel that is 9 cm tall, you probably need to be using 1-5 mm grid cells in z.

[Saharrp95]

A tunnel is a pipe. 0.26 x 0.09 is a hydraulic diameter of 0.13. Re_d at 1 m/s is ~9000. Pipe flow needs more than 4000 to be turbulent.

Based on this Reynolds number, the fully developed region begins approximately 2.7 m downstream. Since my domain length is only 0.6 m, the flow in my simulation is not fully developed. Considering this, can we also conclude that pipe flow typically requires a Reynolds number greater than 4000 to be turbulent?

Additionally, the U-velocity slice in Smokeview does not show any visible fluctuations in the flow field. Can this observation alone be used to determine whether the flow is turbulent or not?

&DEVC ..., QUANTITY='U-VELOCITY'. The output value also here is not fluctuating that much.

[AmirrezaHBSH]

A tunnel is a pipe. 0.26 x 0.09 is a hydraulic diameter of 0.13. Re_d at 1 m/s is ~9000. Pipe flow needs more than 4000 to be turbulent.

Based on this Reynolds number, the fully developed region begins approximately 2.7 m downstream. Since my domain length is only 0.6 m, the flow in my simulation is not fully developed. Considering this, can we also conclude that pipe flow typically requires a Reynolds number greater than 4000 to be turbulent?

Additionally, the U-velocity slice in Smokeview does not show any visible fluctuations in the flow field. Can this observation alone be used to determine whether the flow is turbulent or not?

&DEVC ..., QUANTITY='U-VELOCITY'. The output value also here is not fluctuating that much.

So, you mean that since the flow is not yet in the fully developed region, we cannot conclude that it is turbulent based on the critical Reynolds number of 9000?

[Saharrp95]

Yes, exactly. My duct length is 0.6 m, and I obtained these plots from FDS. As can be seen, the subgrid-scale kinetic energy is nearly zero, and the U-velocity shows minimal fluctuations. This observation is also consistent with the Smokeview slice files. @drjfloyd, based on this information, can we conclude that since the flow is not yet fully developed, the critical Reynolds number cannot be taken as 4000, and therefore the flow is laminar?

[drjfloyd]

What is the inlet condition for the wind tunnel you are modelling? If your fans are upstream of the tunnel inlet and there is no flow conditioning you probably have turbulent flow at the inlet.

[SaharRasoulpour]

What is the inlet condition for the wind tunnel you are modelling? If your fans are upstream of the tunnel inlet and there is no flow conditioning you probably have turbulent flow at the inlet.

Thank you for your response. In my setup, the fan is modeled as an air inlet positioned upstream of the domain, providing an inlet velocity of 1 m/s. The computational domain extends from x = 0 m to x = 0.6 m, with the vent located at x = 0.6 m.

[SaharRasoulpour]

I have another question, and I would really appreciate your help.

To evaluate the turbulence resolution M(x), I need to define devices (DEVCs) for the quantities U-VELOCITY, V-VELOCITY, W-VELOCITY, and SUBGRID KINETIC ENERGY. My question is: to obtain the value for a single computational cell, should I specify XB as a plane in one direction? If XB covers the entire domain, will the output represent a volume-averaged value? And is it possible to define a DEVC at a single point inside the domain?

[rmcdermo]

Use XYZ to define a point DEVC. I would not mess with fancy XB averaging, etc., in FDS. Just output your point values with high frequency (low DT_DEVC) and post process the points yourself.

[SaharRasoulpour]

Thank you for your response. So, when we specify a single point using XYZ, which location would be most appropriate for evaluating M(x)?

[marcosvanella]

If you ask for U-VELOCITY, V-VELOCITY, W-VELOCITY for a DEVC in a location XYZ, FDS will figure out the cell I,J,K where that point is located and give you the face velocities I,J,K in x, y and z directions respectively. These are the "high side" faces for that cell, in the staggered mesh. The SUBGRID KINETIC ENERGY will be the cell value for cell I,J,K.

[SaharRasoulpour]

Thank you for your explanation. So, each point or cell provides its own value of M(x), meaning this quantity varies throughout the domain. How can we determine which point gives a representative assessment of the entire domain? Also, if we specify XB for the entire domain, will M(x) correspond to the average value over all cells?