1. Workshop 3 Room Temperature Study (Part 1)
Introductory FLUENT Training

2. Introduction
In this introductory workshop you will be analyzing the effect of computers and workers on the temperature distribution in an office. In the first stage, the simulation of airflow through the duct will be carried out and then the outlet conditions for the duct will be saved and provided as the profile data for the inlet condition(s) of the room

3. Duct Simulation: Description
The operating and boundary conditions for the flow are:
The working fluid is Air
Fluid Temperature = 294 K
Inlet: K
Outlet: kg/s (per vent)
Inlet
Vent 2
Vent 1
Inlet

4. Starting FLUENT in Workbench
Open the Workbench (Start > Programs > ANSYS 12.0 > ANSYS Workbench)
Drag FLUENT into the project schematic
Change the name to Duct
Double click on Setup
Choose 3D and Double Precision under Options and retain the other default settings

5. Import Mesh
This starts a new FLUENT session and the first step is to import the mesh that has already been created:
Under the File menu select Import> Mesh
Select the file duct.msh and click OK to import the mesh
After reading the mesh, check the grid using Mesh>Check option
or by using Check under Problem Setup>General

6. Setting up the Models
Select Pressure Based, Steady state solver Problem Setup>General>Solver
Specify Turbulence model
Problem Setup > Models > Viscous
Double click and Select k-omega (2 eqn) under Model and SST under k-omega model and retain the default settings for the other parameters
Make sure that the Energy Equation is disabled
Problem Setup > Models> Energy

7. Materials Define the materials. Problem Setup > Materials
Double click on air to open Create/Edit Materials panel
By default, Density and Viscosity of air are set as kg/m3 and e-05 kg/(m-s) respectively
Retain those values and close the panel

8. Operating Conditions
Under Problem Setup >Cell Zone Conditions (operating conditions are also in BC panel)
Click on Operating Conditions… and set the Operating Pressure (Pascal) to

9. Boundary Conditions Under Problem Setup > Boundary Conditions
Select inlet under Zone and choose Pressure-Inlet from the drop down menu under Type
Now double click on inlet under Zone
Input all the parameters in Momentum tab as shown below

10. Boundary Conditions Under Problem Setup > Boundary Conditions
Select vent1 under Zone and choose mass-flow-inlet from the drop down menu under Type
Now double click on vent1 under Zone
Input all the parameters in Momentum tab as shown below

11. Boundary Conditions Under Problem Setup > Boundary Conditions
Select vent2 under Zone and choose mass-flow-inlet from the drop down menu under Type and set the conditions similar to that of vent1
NOTE: Under the Direction Specification Method, we may also use Outward Normal condition for both the vents

12. Solution Methods
Set the Solution methods which decides the Pressure-Velocity coupling.
Under Solution>Solution Methods setup the parameters as shown in the image.

13. Solution Controls
Under Solution>Solution Controls setup the parameters as shown below

14. Monitors Residual Monitoring Solution > Monitors
Double click on Residuals (By default it is on)
Enable Plot under Options. Deselect Check Convergence for all the variables.

15. Monitors Surface Monitors
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 door. One measure of a converged solution is when this air has reached a steady- state temperature.
Solution > Monitors > Surface Monitors
Click on Create to create a new surface monitor
Type ‘velocity-monitor’ under Name
Enable Printing and Plotting of monitors by marking check boxes under Options
Select Area-Weighted Average from the drop-down menu under Report Type
Select Velocity… as the Field Variable and select Velocity Magnitude under Velocity variable

16. Monitors Select one of the vents as the Surfaces to be monitored
Click on OK to create the monitor and to close the panel
We can also write the above values to a file by clicking the check box next to Write.

17. Write Case File
You can now save the project and proceed to write a case file for the solver:
To save the project
File>Save Project
To write the case files
File>Export>Case..

18. Initialization
Before starting the calculations we must initialize the flow field in the entire domain
Solution > Monitors > Solution Initialization
Initializing the flow field with near steady state conditions will result in faster convergence
In this case, from the flow rate and the area of the duct we can get an estimate of the velocity at steady state
Click on Initialize to initialize the solution

19. FMG Initialization
Flow convergence can be accelerated if a better initial solution is used at the start of the calculation. The Full Multigrid initialization (FMG initialization) can provide this initial and approximate solution at a minimum cost to the overall computational expense.
Note: FMG initialization is not available through GUI
Press  <Enter>  in the console to get the command prompt ( >).
Enter the text commands and input responses outlined in green, as shown, accepting the default values by pressing  <Enter>  when no input response is given
Note: The FMG initialized flow field can be inspected using FLUENT's postprocessing tools.

20. FMG Initialization

21. Run Calculations
The solution process can be started in the following manner
Solution >Run Calculation
Enter 200 for Number of Iterations and click on Calculate
During the iteration process, both the residual plot and monitor plots will be shown in different windows. If the velocity monitor is not changing we can stop the iterations. You may specify further iterations if the monitors are still changing significantly.
The magnitude of change of a monitor per iteration can be observed from the console (enabled by clicking on Print to Console while creating the monitor)
Note: Iterations can be stopped in between using the Cancel button.

22. Residue & Monitor plots
The results included are obtained after running for 370 iterations.

23. Other Checks (optional)
We can check the mass balance at the inlet and outlet boundary as follows:
Results > Reports> Fluxes
Click on Setup…
A new dialogue box for Flux Reports will come
Select Mass Flow Rate under Options
Select inlet, vent1,vent2 together under Boundaries
Click on Compute
Mass flow rate on all these boundaries will be printed and we can see that the Net Results is in the order of e-06 which indicates very good convergence

24. Exporting the Profile at the Outflow boundary
We need to export the outflow velocity profile at the Vents to provide the same as an input for the room case.
Exporting the Profile:
Export the velocity profile at vent1 from the file menu
File>Export>Profile…
Select vent1 from Surfaces
Select X,Y,Z Velocity and Turbulent Kinetic energy(k) and Specific dissipation rate (Omega)as the Values to be exported
Save the file as vent1.prof

25. Exporting the Profile at the Outflow boundary
Similarly export the Velocity profile of vent2 and save the file as vent2.prof

26. Write Case & Data File
You can now save the project and proceed to write a case file for the solver:
To save the project
File>Save Project
To write the case/data files
File>Export>Case & Data..

27. Workshop 3 Room Temperature Study (Part 2)
Introductory FLUENT Training

28. Room: Operating Conditions
The operating conditions for the flow at room are:
The working fluid is Air
Worker Temperature = 310 K
Computer Monitor Temperature = 303 K
Computer Vent: K (per computer)
Ceiling Vents: profile data, Temperature=294 K

29. Room Geometry and Details
Vent 2
Outlet
Vent 2
Workers
Monitors
Computer CPU

30. Starting FLUENT in Workbench
Return to the Project window
Drag FLUENT into the Project Schematic
Change the name to Room
Double click on Setup
Choose 3D and Double Precision under Options and retain the other default settings

31. Import Mesh
This starts a new FLUENT session and the first step is to import the mesh that has already been created:
Under the File menu select Import> Mesh
Select the file duct.msh and click OK to import the mesh
After reading the mesh, check the grid using Mesh>Check option
or by using Check under Problem Setup>General

32. Reading the Profiles
Read the profile files that were written in the Duct’s case at Vent Boundaries
Under the File menu select Read> Profile
Select the file vent1.prof and click OK to read the profile
Similarly read vent2.prof file

33. Models
Select Pressure Based, Steady state solver Problem Setup>General>Solver
Specify turbulence model Problem Setup > Models > Viscous Double click and Select k-omega (2 eqn) under Model and SST under k-omega model and retain the default settings for the other parameters
Enable the Energy Equation. Problem Setup > Models> Energy

34. Materials Define the materials. Problem Setup > Materials
Double click on air to open Create/Edit Materials panel
Select incompressible-ideal-gas from the dropdown menu of Density
Retain other default values of Specific heat and Viscosity. Select ‘Change/Create’ to implement the changes then Close
NOTE: The incompressible ideal gas law for density is used when pressure variations are small enough that the flow is fully incompressible but you wish to use the ideal gas law to express the relationship between density and temperature

35. Operating Conditions Problem Setup >Cell Zone Conditions
Click on Operating Conditions… and set the Operating Pressure (Pascal) to
Enable Gravity and specify Z-component of Gravitational Acceleration as m/s2
Enter Operating Density as kg/m3
Note: Enabling gravity will allow the solver to take into account the buoyancy effect due to the change in the density of the air.

36. Boundary Conditions
Under Problem Setup > Boundary Conditions
Select vent1 under Zone and choose velocity-inlet from the drop down menu under Type. For this boundary we will specify the parameters using the previously read profile file
Now double click on vent1 under Zone
Go to Momentum tab, set Components as Velocity Specification Method
Select vent1 x-velocity from the dropdown menu for X-Velocity. (make sure you select the velocity variable “vent1 x-velocity” not the grid variable”vent1 x”. Do likewise for all the other variables (y-velocity, z- velocity, turbulent kinetic energy and specific dissipation rate).
In the Thermal tab, set a constant Temperature of 294K:

37. Boundary Conditions Under Problem Setup > Boundary Conditions
Similarly, select vent2 under Zone and set all the quantities. This time choose the profile quantities starting with vent2

38. Boundary Conditions
Under Problem Setup > Boundary Conditions
Select outlet under Zone and choose Pressure-outlet from the drop down menu under Type. For this boundary we will specify the parameters using the previously read profile file
Now double click on outlet under Zone
Go to Momentum tab, set Gauge Pressure (Pascal) as 0
Set the backflow conditions for the turbulence quantities to have a Backflow Turbulent Intensity and Backflow Turbulent Viscosity Ratio of 5% and 5 respectively
In the Thermal tab, set a constant Backflow Total Temperature of 294 K

39. Boundary Conditions Under Problem Setup > Boundary Conditions
Select computer1intake under Zone and choose Mass-Flow inlet from the drop down menu under Type.
Set the Mass Flow Rate as kg/s and keep the Direction Specification Method as Outward Normals
Set Turbulent Intensity (fraction) and Turbulent Viscosity Ratio as 5% 10 respectively

40. Boundary Conditions
To save time, the conditions for computer1 can be copied over to the boundary conditions for the other 3 computers in the simulation.
Make sure that the inlets for the other computers are all of type mass- flow-inlet
In the Boundary Conditions Panel, click the Copy... button. This will open the Copy BCs panel
In the From Zone list, select the zone that has the conditions you want to copy: computer1intake
In the To Zones list, select the zones to which you want to copy the conditions to: computer2intake, computer3intake, computer4intake
Click Copy. FLUENT will set all of the boundary conditions for the zones selected in the To Zones list to be the same
as the conditions for the zone selected in
the From Zone list.

41. Boundary Conditions Under Problem Setup > Boundary Conditions
Repeat the instructions on the previous 2 slides in order to set the conditions for the computer vents.
So, first make sure all vents are of type ‘mass-flow-inlet’.
Set the conditions for computer1vent as in the image below.
In the Thermal tab, set a constant temperature of 313 K
Copy this boundary condition from computer1vent to the other 3 computers.

42. Boundary Conditions Under Problem Setup > Boundary Conditions
Select monitors under Zone and choose wall from the drop down menu under Type.
Now double click on monitors under Zone
Go to Momentum tab, set it as Stationary wall with No Slip
In the Thermal tab, set a constant Temperature of 303 K

43. Under Problem Setup > Boundary Conditions
Select workers under Zone and select wall from the drop down menu under Type.
Double-click on workers under Zone.
On the Momentum tab, specify a stationary wall with no slip.
On the Thermal tab, set a constant wall temperature of 310 K.

44. Set the Solver Controls
Solution Methods
Set the Solver Controls
Under Solution>Solution Methods setup the parameters as described below
Select Coupled Scheme
Specify the discretization schemes as shown below

45. Solution Controls Under Solution>Solution Controls
Set a Courant Number of 100 with Explicit Relaxation Factors for Momentum and Pressure as 0.25 each
Set Under Relaxation Factors of Density, Body Forces, Turbulent Kinetic Energy, Turbulent Viscosity and Specific Dissipation Rate as 0.5 each
Keep an Under Relaxation Factor of 1.0 for Energy

46. Monitors Residual Monitoring Solution > Monitors
Double click on Residuals (By default it is on)
Enable Plot under Options. Deselect Check Convergence for all the variables.

47. Monitors Surface Monitors Solution > Monitors > Surface Monitors
Click on Create to create a new surface monitor
Type ‘temperature-monitor’ under Name
Enable Printing and Plotting of monitors by marking check boxes under Options
Select Area-Weighted Average from the drop-down menu under Report Type
Select Temperature… as the Field Variable and select Static Temperature under Temperature

48. Monitors Select outlet under Surfaces
Click on OK to create the monitor and to close the panel

49. Write Case File
You can now save the project and proceed to write a case file for the solver:
To save the project
File>Save Project
To write the case files
File>Export>Case..

50. Solution > Monitors > Solution Initialization
Initialize the flow field with inflow conditions by selecting vent1from the dropdown menu under Compute from
Click on Initialize to initialize the solution

51. Run Calculations
The solution process can be started in the following manner
Solution >Run Calculation
Enter 100 for Number of Iterations and click on Calculate
Monitor the solution and see if the Temperature monitor is not changing further. You can instruct FLUENT to perform more iterations if the monitors are still changing significantly. You can stop iterating if the monitors are stabilized.

52. Residue & Monitor plots
The results included are obtained after running for 554 iterations.

53. Write Case & Data File
You can now save the project and proceed to write a case file for the solver:
To save the project
File>Save Project
To write the case/data files
File>Export>Case & Data..

54. Post processing(1)
We can create isosurfaces at various locations of the domain to examine the results at any location within the domain, not just at the boundaries.
An isosurface can be created in the following manner:
Select Surface>Iso-surface… from the toolbar
Select Mesh… under Surface of constant drop down menu and select Y-Coordinate under Mesh
If we click on Compute it will report the minimum and maximum values
Enter 2.4 under Iso-Values
Specify a surface name under New Surface Name
Clicking Create will generate the new surface
You may want to create more iso-surfaces at different critical locations to observe different parameters.

55. Post processing(2) Display the contours of Temperature:
Go to Results > Graphics and Animation
Select Contours under Graphics and click on Set Up…
Select Contours of Temperature… then Static Temperature
Select the Surfaces on which we wish to see the temperature
Zoom into the area of interest by using middle mouse button
Overlay a wireframe representation of the room:
On the Contours Panel, Check the Draw Mesh box.
Select Edges (not Faces), and Outline. Under Surface Types, select ‘Wall’ which will select all the walls.
Display then Close (mesh display panel) : Display (contours panel)
Display the Vectors of Velocity:
Select Vectors under Graphics and click on Set Up
Change the Scale to 15, and plot on the surface of interest.

56. Post processing(3)
We can also find out the Maximum and Minimum of a variable in the following way
Go to Results > Reports>Volume Integrals
Select Maximum under Report Type
Select Temperature… under Field Variable followed by Static Temperature
Select fluid-19 under Cell Zones
On clicking Compute, the maximum value of the Temperature is calculated.
Note: The location of Maximum temperature, say, can be found out by creating an iso-surface of temperature in the same process as mentioned in the slide-54

57. Post processing(4) Contours of Temperature on a plane at Y=2.4 m
Plane location
Contours of Temperature on a plane at Y=2.4 m

58. Results Summary
Mass Weighted Average of Temperature at Outlet: K
Minimum temperature in the domain: 293.6K
Maximum temperature in the domain: 313.1K (at the region near the outlet of Computer2vent)
Mass Weighted Average of Velocity at Outlet: m/s

59. Further Steps (Optional)
Following steps can be done so as get the flow patterns at various planes etc.
Observe the density variation at various planes
Create a streamline from each of the vents
Animate the streamlines
Create an isosurface based on different temperatures