Workshop 3 Room Temperature Study Introduction to CFX Pardad Petrodanesh.Co Lecturer: Ehsan Saadati ehsan.saadati@gmail.com www.petrodanesh.ir

Introduction In this workshop you will be analyzing the effect of computers and workers on the temperature distribution in an office. In the first stage airflow through the supply air ducts will be simulated and the outlet conditions for the duct will be used to set the inlet conditions for the room. Although both components could be analyzed together, separating the two components allows different room configurations to be analyzed without solving the duct flow again.

Duct Simulation The operating conditions for the flow are: The working fluid is Air Ideal Gas Fluid Temperature = 21 [C] Inlet: 0 [atm] Total Pressure Outlet: 0.225 [kg/s] (per vent) Inlet vent1 vent2

Starting CFX in Workbench Open Workbench Drag CFX into the Project Schematic from the Component Systems toolbox Change the name of the system to duct Save the project as RoomStudy.wbpj in an appropriate directory Double-click Setup

Import Mesh The first step is to import the mesh that has already been created: Right-click on Mesh in the Outline tree and select Import Mesh > ICEM CFD Select the file duct_mesh.cfx5 Make sure Mesh Units are in m and click Open to import the mesh

Create Domain You can now create the computational domain: Double-click on Default Domain in the Outline tree to edit the domain On the Basic Settings tab, set the Fluid 1 Material setting to Air Ideal Gas Switch to the Fluid Models tab Set the Heat Transfer Option to Isothermal Heat Transfer is not modeled, but since the working fluid is an ideal gas we need to provide a temperature so its properties can be calculated Set the Fluid Temperature to 21 [C] Change the Turbulence Model Option to Shear Stress Transport Click OK to commit the changes to the domain

Create Boundary Conditions Now create the following boundary conditions: INLET Boundary Condition Name: INLET Boundary Type: Inlet Location: INLET Mass and Momentum Option: Total Pressure (stable) Relative Pressure: 0 [Pa] VENT2 Boundary Condition Name: VENT2 Boundary Type: Outlet Location: VENT2 Mass and Momentum Option: Mass Flow Rate Mass Flow Rate: 0.225 [kg/s] VENT1 Boundary Condition Name: VENT1 Boundary Type: Outlet Location: VENT1 Mass and Momentum Option: Mass Flow Rate Mass Flow Rate: 0.225 [kg/s]

Solver Control Double click on Solver Control from the Outline tree Enable the Conservation Target toggle Click OK to commit the settings The default Conservation Target is 1%. This means that the global imbalance for each equation must be less than 1% (i.e. (flux in – flux out)/flux in < 1%). The solver will not stop until both the Residual Target and the Conservation Target have been met (or Max. Iterations is reached).

Monitor Point Monitor points are used to monitor quantities of interest during the solution. They should be used to help judge convergence. In this case you will monitor the velocity of the air that exits through the vent. One measure of a converged solution is when this air has reached a steady- state velocity. Double click on Output Control from the Outline tree Switch to the Monitor tab and enable the Monitor Options toggle Under Monitor Points and Expressions, click the New icon Keep the default name Monitor Point 1 Set the Option to Expression

Monitor Point In the Expression Value field, type in: areaAve(Velocity w)@VENT1 Click OK to create the Monitor Point

Write Solver File You can now save the project and proceed to write a definition file for the solver: Close CFX-Pre to return to Project window Save the project Right-click on Solution and select Edit Choose Start Run

CFX Solver Manager Examine the residual plots for Momentum and Mass and Turbulence Examine the User Points plot When the run finished close the Solver Manager View the results in CFD-Post by double-clicking Results in the Project window Monitor point Residual plot

CFD-Post Now we will export a Boundary Condition profile from the outlet regions for use in the next simulation. Select File > Export Change the file name to vent1.csv Use the browse icon to set an appropriate directory Set Type as BC Profile and Locations as VENT1 Leave Profile Type as Inlet Velocity and click Save Similarly export a BC profile of VENT2 to the file named vent2.csv Quit CFD-Post and return to the Project Schematic

Operating Conditions The operating conditions for the flow in the room are: The working fluid is Air Ideal Gas Computer Monitor Temperature = 30 [C] Computer Vent Flow Rate: 0.033 [kg/s] @ 40 [C] (per computer) Ceiling Vents: Profile Data, Temperature=21 [C] outlet vent1 vent2

Starting Room Simulation in Workbench Drag CFX into the Project Schematic from the Component Systems toolbox Change the name of the system to room Double-click Setup in the room system

Import Mesh The first step is to import the mesh that has already been created: Right-click on Mesh in the Outline tree and select Import Mesh > ICEM CFD Select the file room.cfx5 Make sure the Mesh Units are in m and click Open to import the mesh

Create Domain You can now create the computational domain: Edit Default Domain from the Outline tree On the Basic Settings tab, set the Fluid 1 Material setting to Air Ideal Gas Set the Buoyancy Option to Buoyant. Set the Buoyancy settings as shown: Gravity X Dirn. = 0 [ m s^-2 ] Gravity Y Dirn. = 0 [ m s^-2 ] Gravity Z Dirn. = -g (first, click the Enter Expression icon ) Buoy. Ref. Density = 1.185 [ kg m^-3 ] Enabling Buoyancy allows for natural convection due to density variations. The buoyancy force is a function of density variations relative to the buoyancy reference density. Since density variations can be very small, using a reference density help avoid round-off errors. The reference density should be a typical fluid density in the domain.

Create Domain Switch to the Fluid Models tab Change the Heat Transfer Option to Thermal Energy Change the Turbulence Model Option to Shear Stress Transport Switch to the Initialisation tab Check the Domain Initialisation box Set the Temperature Option to Automatic with Value. Set the Temperature to 21 [C] Click OK to commit the changes to the domain For most cases, setting an initial condition for domain temperature is not necessary since the solver can automatically calculate initial conditions. However, if you input a value that is closer to the final solution than what the solver would automatically calculate, you will reach a converged solution faster.

Profile data initialization Select Tools >Initialise Profile Data and choose the Data File as vent1.csv. Click OK CFX-Pre reads the file and creates functions that point to the variables available in the file (see the User Functions section in the Outline tree). Boundary conditions can be set by referencing these functions. E.g. VENT1.Velocity u(x,y,z) refers to the Velocity u value in the VENT1 function with the local coordinate values x, y and z passed in as the arguments. Any value with the correct dimensions can be passed in as an argument, but usually the local coordinates are used. Similarly initialise profile data for vent 2 by choosing vent2.csv

Create Boundary Conditions Now create the following boundary conditions: vent1 Boundary Condition Name: vent1 Boundary Type: Inlet Location: VENT1 Select Use Profile Data and choose VENT1 as the Profile Name Click Generate Values This will create expressions for the Mass and Momentum option on the Boundary Details tab that reference the profile functions On the Boundary Details tab check that the expressions make sense Heat Transfer Option: Static Temperature Static Temperature: 21 [C]

Create Boundary Conditions vent2 Boundary Condition Name: vent2 Boundary Type: Inlet Location: VENT2 Select Use Profile Data and choose VENT2 as the Profile Name Click Generate Values The Mass and Momentum Option will be automatically updated Heat Transfer Option: Static Temperature Static Temperature: 21 [C] workers Boundary Condition Name: workers Boundary Type: Wall Location: WORKERS Heat Transfer Option: Temperature Fixed Temperature: 37 [C]

Create Boundary Conditions outlet Boundary Condition Name: outlet Boundary Type: Opening Location: OUTLET Mass and Momentum Option: Opening Pres. and Dirn Relative Pressure: 0 [Pa] Heat Transfer Option: Opening Temperature Opening Temperature: 21 [C] monitors Boundary Condition Name: monitors Boundary Type: Wall Location: monitors Heat Transfer Option: Temperature Fixed Temperature: 30 [C]

Create Boundary Conditions computerVent Boundary Condition Name: computerVent Boundary Type: Inlet Location: COMPUTER1VENT, COMPUTER2VENT, COMPUTER3VENT, COMPUTER4VENT Mass and Momentum Option: Mass Flow Rate Mass Flow Rate: 0.132 [kg/s] Heat Transfer Option: Static Temperature Static Temperature: 40 [C]

Create Boundary Conditions computerIntake Boundary Condition Name: computerIntake Boundary Type: Outlet Location: COMPUTER1INTAKE, COMPUTER2INTAKE, COMPUTER3INTAKE, COMPUTER4INTAKE Mass and Momentum Option: Mass Flow Rate Mass Flow Rate: 0.132 [kg/s] Mass Flow Update Option: Constant Flux This enforces a uniform mass flow across the entire boundary region, rather than letting a natural velocity profile develop. It is used here to make sure the flow rate through each intake is the same.

Solver Control Edit Solver Control from the Outline tree Due to nature of this flow it will take a long time for a steady-state condition to be reached Increase the Max. Iterations to 750 Change the Timescale Control to Physical Timescale Set a Physical Timescale of 2 [s] Enable the Conservation Target toggle Click OK to commit the settings

Monitor Point Monitor points are used to monitor quantities of interest during the solution. They should be used to help judge convergence. In this case you will monitor the temperature of the air that exits through the outlet. One measure of a converged solution is when this air has reached a steady-state temperature. Edit Output Control from the Outline tree Switch to the Monitor tab and enable the Monitor Options toggle Under Monitor Points and Expressions, click the New icon Enter the Name as temp Set the Option to Expression

Monitor Point In the Expression Value field, type in: massFlowAve(Temperature)@outlet Click OK to create the Monitor Point

Write Solver File You can now save the project and proceed to write a definition file for the Solver: Close CFX-Pre to return to the Project window and save the project Select File > Import from the main menu in Workbench Set the file filter to CFX-Solver Results File Select the results file provided with this workshop, room_001.res Change the name of the system to room results … The solution will take several hours to solve on one processor. To save time, a results file is provided with this workshop. The Project Schematic shows that the room Solution has not been completed, so you cannot view the results in CFD-Post yet. To view the results for the file provided you’ll need to add the results to the project.

Project Schematic

CFX Solver Manager Now you can view the solution for the previously solved case. Right-click on Solution in the room results system and select Display Monitors Examine the residual plots for Momentum and Mass, Heat Transfer and Turbulence The Residual Target of 1e-4 was met at about 270 iterations, but the solver did not stop because the Conservation Target had not been met Examine the User Points plot Air temperature leaving through the outlet did not start to reach a steady temperature until >650 iterations. Using residuals as the only convergence criteria is not always sufficient.

Residual and Monitor plot Residual plot Monitor points

CFX Solver Manager Check the Domain Imbalances at the end of the .out file for each equation You can right click in the text monitor, select Find… and search for “Domain Imbalance” to find the appropriate section An imbalance is given for the U-Mom, V-Mom, W-Mom, P-Mass and H-Energy equations It took 653 iterations to satisfy the Conservation Target of 1% for the H-Energy equation – see the Plot Monitor 1 tab Close the Solver Manager View the results in CFD-Post by double-clicking Results in the Project Schematic from the room system

CFD-Post Start by creating a ZX Plane at Y = 1.2 [m] Select Location > Plane from the toolbar In the Details windows on the Geometry tab, set the Definition Method to ZX Plane Set Y to 1.2 [m] On the Colour tab set Mode to Variable Set Variable to Temperature Set Range to Local and click Apply Observe the temperature distribution (for example, how the warm air collects under the table)

CFD-Post Using the same procedure, create several other planes displaying the temperature profile: ZX Plane at Y = 2 [m] ZX Plane at Y = 5.1 [m] XY Plane at Z = 0.25 [m] When finished observing the temperature distribution, uncheck the visibility boxes of the planes that you created

CFD-Post Plot vector plots on the planes that you created: Click Insert > Vector from the main menu In the Details windows on the Geometry tab, set Location to Plane 2 and Symbols Size to 3.0 in Symbol tab Click Apply After observing the flow behavior on Plane 2, switch the Location to Plane 4

Further Steps (Optional) Time permitting, you may want to try the following: Observe the density variation at various planes Create a streamline from each of the vents You may want to adjust the values on the Limits tab (Max. Segments) Animate the streamlines Right-click on the Streamlines in the 3D viewer and select Animate Create an isosurface based on different temperatures (e.g., 22 [C], 24 [C], etc.) Calculate the areaAve of Wall Heat Flux on the workers Click Tools > Function Calculator