Week 11 - Louver/Grille characterization

Aim: To design and evaluate the flow domain comprising a portion of the Hexa grille inside the domain. To study the parametric method, the parameter trails, and the primary and compound functions are to be reported for the challenge.

Objective:

• The cabinet has 160mm in length with the inlet and outlet openings at the ends the cross-sectional area is (7.363mm x 12.7mm)and four symmetry walls are on the other sides.
• The model includes a portion of the Hexa grille placed in streamwise directions at the center of the channel.
• The grill has one complete hexagonal hole in the middle and this pattern has been chosen for four
• quarters of hexagonal holes located around it as it forms a periodic region which is enough to measure the loss coefficient.
• We find only one part of the entire Hexa grille structure in a flow domain from the figure above

 Introduction:

• A grille is a vent cover through which air is blown into or out of a room for circulation back to the central heating or cooling unit.
• Grills are an important feature of any electronics enclosure be it natural convection cooling or forced convection. While designing the enclosure for electronics cooling, the thermal engineer is always concerned about the trade-off between thermal performance and fan power. As grills impact the fan power, it becomes necessary to characterize grills so that one can design a fan and select the best appropriate location for it.

Difference between Louver and grille

• Louvers, or dampers, are often attached to the back of a heat register. These adjustable louvers/dampers can open or close the register to open and close the flow of air as shown in Fig. (a)
• A grille has no damper to control airflow, so air is left to flow freely. Grilles do not have the damper normally found on registers as shown in Fig. (b).

Fig. (a) Louver used in a house           Fig (b) Grille used in Car

Simulations of electrical equipment, enclosed electronics components, and electrical systems are typical applications where grilles are used. The grille loss coefficient is a parameter whose value is a function not just of the free area ratio, but also of other parameters such as grille design, Reynolds number, grille thickness, and flow regime (laminar or turbulent). Icepak has an automatic mode that calculates the loss coefficient as a function of the free area ratio. However, this calculation is based on empirical correlations in the fully turbulent flow regime. Since most applications are for natural convection in the transitional flow regime it is important to develop a methodology to take into account the appropriate flow regime. For a more complicated grille design (chevron, louvers, etc.) a wind tunnel simulation is needed to characterize its pressure loss. Then, it is important to have a methodology to obtain accurate and consistent results.

Problem Description:  

The model includes a cabinet that is 160 mm in length with inlet and outlet openings at the two ends (with a cross-sectional area of 7.363 mm x 12.7 mm), and four symmetry walls on the other sides. The model also includes a part of the Hexa-grille placed at the center of the channel in the streamwise direction, as shown in Figure: Problem Specification (p. 198). The grille has one full hexagonal hole at the center and four quarter hexagonal holes placed around it. This pattern was selected because it forms a periodic region and is sufficient to calculate the loss coefficient. 

we are considering only a single part of the whole Hexa-grille structure into a flow domain.

Geometry:

First, after creating a new project in the icepack, we need to build a cabinet by creating a new project in the icepack gives us a cabinet for simulation results. To that cabinet, we need to do the necessary changes as per our requirements. In our case, the cabinet or flow domain should be 240 mm in length The cabinet height and width are the same as the Hexa grille we produce. For the Hexa grille layout, the real measurements are 7.363 mm x 12.7 mm x 1 mm

Cabinet: It creates a fluid region around the model for which the governing equations are solved.

• Shape - Prism.
• Specified By - Start/end.
• Start Xs - 0 mm. 
• Start Ys - 0 mm.
• Start Zs - -80 mm.
• End Xe - 12.7 mm.
• End Ye - 7.363 mm.
• End Ze - 80 mm.

Properties - The wall type for the cabinet is defined.

• Min X - Wall.
• Max X - Wall.
• Min Y - Wall.
• Max Y - Wall.
• Min Z - Opening.
• Max Z - Opening.

Block

• Shape - Polygon.
• Specified By - Start/end.
• Plane - X-Y.
• Height - 1mm.

Now the above polygon is mirrored

• After giving openings and the symmetric walls for all four sides of the cabinet, we need to provide the parametric function to the flow.
• We need to give a parametric function for the flow in the Min-Z direction.

Defining Reynolds number:

• Define a velocity parameter at the inlet opening in terms of the Reynolds number Re.
• The velocity at the inlet opening in terms of the Reynolds number Re, which is customarily
  used in loss coefficient plots in lieu of velocity, is calculated as

Where Re = Reynolds number

= density of air

= velocity of air

L = characteristic length

= Dynamic viscosity

Here, L = D_h = 4A/P

D_h = (4*(12.7*7.363)*1e-6) / ((2*12.7+2*7.363)*1e-3)

D_h = 0.009321 m

D_h = 9.322e-3 mm.

• In the Cabinet, we need to give the parametric function to one of the openings, i.e., cabinet_default_side_minz in the model manager.
• Select the Z-velocity as we kept the opening in the Z-direction, and set the value to "$Re*1.84e-5/9.322e-3"

• After clicking done, a dialogue box will appear to ask the initial value of Re, and we need to give an initial value of Re as 10.
• Now we need to give another 8 Re variables in the Run optimization -> Setup -> select parametric trials -> go to -> Design variables -> give the required values in the Discrete values box as " 10 50 100 500 1000 2000 3000 4000"
• Note: The gap between the numbers must be maintained. 
• So the changes we made look like this:

• The above figure represents the total number of trials we are going to run in the simulation.
• It initially starts with the Reynolds number 10, keeps on calculating all the variables, and ends up with the variable 4000.

Defining the report that includes pressures and velocities:

We need to first create the variables in the summary report to calculate the pressure and velocity which are also visible in the domain of the primary and compound functions.

1. In the Define summary report panel, click New
2. In the Objects drop-down list, select cabinet_default_side_minz and click Accept.
3. In the Value drop-down list, select UZ
4. Now we need to create new parameters for the other opening also: for that
5. Repeat steps (1) and (2), then select Pressure in the Value drop-down list.
6. Then repeat steps 1 and 4 for the Cabinet_default_side_maxz
7. Click the Close button to accept the settings and close the panel.
8. The summary report we set up looks as:

• Now go to Run optimization -> Functions. Here we need to provide the inputs for the primary functions, those we have set up in the summary report.
• Here is the primary function, we need to create four definitions. Which are: Static pressure in and out, and velocity in and out.
• We add the definitions by clicking the New button there.

• For the Compound functions, the same as the primary function click the New button to create the definitions.
• Here in the compound function, we need to create and find the Dynamic pressure in and out (Pd_in, Pd_out) and the total pressure in and out (Ptot_in, and Ptot_out), and as well as the K_loss factor.

For Dynamic pressure inlet:

• 0.5*1.16*$V_in*$V_in

For Dynamic pressure outlet:

• 0.5*1.16*$V_out*$V_out

For Total pressure inlet:

• $Pstat_in+$Pd_in

For Total pressure outlet:

• $Pstat_out+$Pd_out

For K_loss:

• ($Ptot_in-$Ptot_out)/$Pd_out

• Now, click Done to save and close the parameters and optimization dialogue box.
• After completing the mesh settings, click the Run button above to calculate or start the solution.

Meshing:

• Here we generated a Non-conformal mesh with the mesh assemblies separately option.
• As we created the assembly for the blocks, means for the single Hexa-grille, we have to give the slack values in the Z-direction.
• Particularly in Z-direction for is, our interest in finding flow domain is in Z-direction and if we provide the slack values to X and Y-directions the assembly can go outside of the cabinet.
• So, we only give the slack values in the Z-direction.

• For even better refinement near the walls of the Hexa-grille, we have incorporated the object parameter values also.

Here polygon blocks are selected and per object, params are defined as shown below

• Now using these settings in the meshing parameters, we can generate the mesh using the Mesher-HD type with the Normal mesh.

• The mesh generates 628488 elements and 686319 nodes to form an acceptable mesh.
• The below figure is the formation of the Mesh in the Z-direction, which is the flow direction in the flow domain.

• The solid type of mesh object Hexa-grille is, in this, we can see the mesh lines on the top side is matching with another side of the solid body.

Mesh Quality

Mesh quality is also checked and it is seen that mesh generated is of good quality.

• It is the measure of mesh quality defined by face alignment index = C0 C1.f
• C0 & C1 are the centroids of two adjacent elements and are normal vectors to the face between the two elements.
• Range of face alignment 0 (bad) to 1 (good) & value greater than 0.1 (preferred) & value greater than 0.15 provide better results.
• The min value of the model is 0.718 which is ideal for the results.
• The preferable volume of mesh to be greater than 1e-13 for single precision solver & greater than 1e-15 for double precision.
• Max / Min cell volume should be less than 10^7 for single precision & must be less than 10^12 for double precision since very small volume create divergence of the solution.
• The volume of the mesh greater than 10^-14 & Max / Min cell ratio is around 420 which is in the required range & single precision can be used for this model.
• It determines how close to the ideal & is based on the equilateral volume. A value greater than 0.5 provides good cell quality.

Solver:

• The three-dimensional steady-state Navier-Stokes equations for the model are solved within the computational domain using the Fluent solver available in ANSYS Icepak. The following settings are applied to the solver:
  1. Variables solved: Flow (velocity, pressure) and Temperature
  2. Radiation: On
     1. Model: Surface-to-surface radiation
  3. Flow regime: Turbulent
  4. Model: Zero equation model
  5. Time variation: Steady
  6. Solution initialization
     1. X velocity: 0
     2. Y velocity: 0.000980665 m/s
     3. Z velocity: 0
  7. Temperature: Ambient (20 deg. C)
  8. Natural convection
     1. Density model: Boussinesq approximation
     2. Operating pressure: 101325 N/m2
     3. Operating density: 1.225 Kg/m3
     4. Gravity vector: 9.80665 m/s^2 directed along the negative Y-axis
  9. Number of iterations: 1000
  10. Convergence criteria
      1. Flow: 1e-7
      2. Energy: 1e-7
      3. Joule heating: 1e-7
  11. Configuration: Parallel
      1. Number of processors: 4
      2. GPU computing: Enabled
      3. Number of GPUs: 1
  12. Discretization scheme
      1. Pressure: Standard
      2. Momentum: First
      3. Temperature: First
      4. Under-relaxation factors
      5. Pressure: 0.3
      6. Momentum: 0.7
      7. Temperature: 1
      8. Viscosity: 1
      9. Body forces: 1
      10. Joule heating potential: 1
  13. Linear solver settings
      1. Pressure - Type: V, Termination criterion: 0.1, Residual reduction tolerance: 0.7, Stabilization: None
      2. Momentum - Type: flex, Termination criterion: 0.1, Residual reduction tolerance: 0.7
      3. Temperature - Type: F, Termination criterion: 0.1, Residual reduction tolerance: 0.7, Stabilization: None
      4. Joule heating potential - Type: F, Termination criterion: 0.1, Residual reduction tolerance: 0.7, Stabilization: None
  14. Precision: Double

• So, the flow regime can automatically change from laminar when the Reynolds number is calculated until 2000 to Turbulence when the Reynolds number is calculated for 3000 and 4000.

Residuals:

The residuals of the following equations are plotted against the number of iterations:

1. Continuity equation
2. X-Momentum equation
3. Y-Momentum equation
4. Z-Momentum equation
5. Energy equation

Here the residual plot defines each and every oscillation as the solution for Re 10,50,100 Calculated for other

Reynolds numbers are converged and started.

• Here each and every oscillation in the residual plot describes that the solution for Re 10, 50, 100 .... is converged and started calculated for other Re's.

Results:

• The results for the parametric study for the variable Reynolds number is given in a table. The table contains results for all the functions that we have created.

• Here from the above table, we can clearly see that the increase in the Reynolds number increases the value of the velocity and as well as the pressure also.
• The above table is called as the summary report of the optimized data of the variables.
• The summary report of the primary functions are:

• Here in this table, we can see the max and min velocity and pressures at both openings of the flow domain or cabinet.
• The min and max velocity at the inlet opening is 7.89 m/s, and the pressure is 23.36 N/m2.
• The min. velocity at outlet opening is 4.99 m/s and max. velocity is 9.82 m/s. 
• The Max. pressure at the outlet is almost equal to 0 N/m2. (actual is 0.0058N/m2) means we have a normal or ambient pressure is located in that region.
• If we see the pressure, there will be a massive drop in the pressure. Any type of obstruction, restriction, or roughness in the system will cause resistance to airflow and cause a pressure drop. ... The maximum pressure drop from the supply side to the points-of-use will occur when the compressed air flow rate and temperature are highest.

K_loss:

• The loss coefficient (ζ) is a dimensionless number (characteristic coefficient) to calculate the head loss (HL).

.

Where v = Characteristic flow velocity in the relevant hydraulic component (usually the flow velocity in the cross-section of the connection downstream of the component)

g = Acceleration due to gravity

Zeta = loss coefficient

• Plot the loss coefficient, K_loss, against the Reynolds number, Re.
• In the Parametric trials panel, click the Plot button to open the Selection panel.
• In the Selection panel, select Re as the x-axis variable, and click Okay.
• In another Selection panel which automatically opens up, select K_loss as the y-axis variable, and
  Click Accept.

• After selecting the Re on the x-axis and K_loss on the y-axis, the plot will appear as shown in the above figure.
• From the above plot, we can say that as the Reynolds number is increasing the loss coefficient is also decreasing.
• After it reaches the turbulence area the K_loss becomes almost stagnant which changes at the rate of 1e-3.

Velocity Contours:

• The max. velocity recorded inside the flow domain is 11.565 m/s.
• In the figure, we can see how the velocity and flow are behaving on the walls of the Hexa-grille and in the neighboring area.
• We can see how the velocity is increasing from the walls of the Hexa-grille to the edges and then in the flow domain area.
• The max. velocity recorded in the Uz direction is 12.14 m/s.

Velocity Vectors:

Pressure Contours:

Conclusion:

• It can be observed that the loss coefficient is having very large value at low velocity but decreases drastically with an increase in speed.