Introduction to CFX. Workshop 3 Room Temperature Study презентация

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)

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
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
The first step is to import the mesh that has already been created:

Create 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
You can now create the computational domain:

Create 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]
Now create the following boundary conditions:
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

Monitor Point
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 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.

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

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

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
CFX Solver Manager
Monitor point
Residual plot

CFD-Post
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
Now we will export a Boundary Condition profile from the outlet regions for use in the next simulation.

Operating Conditions
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]
The operating conditions for the flow in the room are:

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
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
The first step is to import the mesh that has already been created:

Create 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 ]
You can now create the computational 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

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
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]
Now create the following 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.
Create Boundary Conditions

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
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 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.

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

Write Solver File
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 …
You can now save the project and proceed to write a definition file for the Solver:
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
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.
Now you can view the solution for the previously solved case.

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
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)
Start by creating a ZX Plane at Y = 1.2 [m]

CFD-Post
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
Using the same procedure, create several other planes displaying the temperature profile:

CFD-Post
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
Plot vector plots on the planes that you created: