CFX Intro 14.5 WS11 Room Temperature Study [PDF]

Zitiervorschau

Workshop 11 Room Temperature Study 14. 5 Release

Introduction to ANSYS CFX © 2012 ANSYS, Inc.

December 17, 2012

1

Release 14.5

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.

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 2

Postprocessing

Summary Release 14.5

Operating Conditions • The operating conditions for the flow are given below: – – – –

The working fluid is Air Ideal Gas Fluid Temperature = 21 [C] Inlet: 0 [atm] Total Pressure Outlet: 0.225 [kg/s] (per vent)

vent2 Inlet

vent1

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 3

Postprocessing

Summary Release 14.5

Starting CFX in Workbench • Open Workbench • Drag a CFX system into the Project Schematic from the Component Systems toolbox

• Change the name of the system to duct • Save the project as RoomStudy.wbpj in your working directory • Double-click Setup

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 4

Postprocessing

Summary Release 14.5

Importing the Mesh The first step is to import a mesh

• Right-click on Mesh in the Outline tree and select Import Mesh > ICEM CFD

• Select the file duct_mesh.cfx5 (workshop_input_files\WS_11_ Room Temperature Study)

• Make sure Mesh Units are in m and click Open to import the mesh

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 5

Postprocessing

Summary Release 14.5

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 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] • Click OK to commit the changes to the domain Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 6

Postprocessing

Summary Release 14.5

Boundary Conditions • Now create the following boundary

• VENT1 Boundary Condition

conditions

– – – –

• INLET Boundary Condition – Name: INLET – Boundary Type: Inlet – Mass and Momentum Option: Total

–

Pressure (stable) Relative Pressure: 0 [Pa]

–

Name: VENT1 Boundary Type: Outlet Location: VENT1 Mass and Momentum Option: Mass Flow Rate Mass Flow Rate: 0.225 [kg/s]

• VENT2 Boundary Condition – – – – –

Name: VENT2 Boundary Type: Outlet Location: VENT2 Mass and Momentum Option: Mass Flow Rate Mass Flow Rate: 0.225 [kg/s] Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 7

Postprocessing

Summary Release 14.5

Solver Control • Double-click on Solver Control from the Outline tree • Enable the Conservation Target toggle 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.

• Click OK to commit the settings

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 8

Postprocessing

Summary Release 14.5

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 one of the vents. 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 Objects toggle

• Under Monitor Points and Expressions click the Add new item button

• Keep the default name Monitor Point 1 • Set the Option to Expression • In the Expression Value field type: areaAve(Velocity w)@VENT1

• Click OK to create the monitor point Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 9

Postprocessing

Summary Release 14.5

Solution You can now save the project and proceed to write a definition file for the solver

• Close CFX-Pre to return to the Project Schematic window

• Save the project • Right-click Solution and select Edit • Click Start Run when the CFX-Solver Manager appears

• Examine the User Point. The velocity becomes steady toward the end of the run.

• Close the CFX-Solver Manager • In Workbench right-click Results and select Edit Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 10

Postprocessing

Summary Release 14.5

Export 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

• Close CFD-Post and return to the Project Schematic Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 11

Postprocessing

Summary Release 14.5

Summary The first part of the workshop simulated some upstream ductwork and the exit velocity profiles from the ductwork exit were exported. Now those profiles will be used as the inlet conditions to a larger simulation involving a room with heat sources

• Details of the next simulation:

vent2

outlet

– The working fluid is Air Ideal Gas – The temperature of the computer monitors is – –

30 [C] The flow through the vent of each computer is 0.033 [kg/s] at 40 [C] For the ceiling vents the velocity profile data are used and the temperature is 21 [C]

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 12

vent1

Postprocessing

Summary Release 14.5

Room Simulation Setup in Workbench • Drag a CFX system into the Project Schematic from the Component Systems toolbox

• Change the name of the system to room • Double-click Setup in the room system

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 13

Postprocessing

Summary Release 14.5

Importing the Mesh The first step is to import a mesh

• Right-click on Mesh in the Outline tree and select Import Mesh > ICEM CFD

• Select the file room.cfx5 • Make sure Mesh Units are m and click Open to import the mesh

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 14

Postprocessing

Summary Release 14.5

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 ]

)

Buoyancy must be included in order to model natural convection due to density variations. The buoyancy force is represented by a momentum source, which is a function of density differences relative to the buoyancy reference density. The buoyancy reference density should be chosen so that the source is not large. For a single-phase simulation the reference density should be an average value for the domain. Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 15

Postprocessing

Summary Release 14.5

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 Initialization tab Check the Domain Initialization box Set the Temperature Option to Automatic with Value and Temperature to 21 [C]

• Click OK to commit the changes to the domain

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 16

Postprocessing

Summary Release 14.5

Profile Data Initialization • Select Tools > Initialize 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). These functions can be used in the definition of boundary conditions.

• Similarly initialize profile data for vent 2 by choosing vent2.csv

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 17

Postprocessing

Summary Release 14.5

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 Switch to the Boundary Details tab • Change the Option for Mass And Momentum to Cart. Vel. Components. Expressions based on the function VENT1 automatically appear • Set the Heat Transfer Option to Static Temperature with a value of 21 [C]

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 18

Postprocessing

Summary Release 14.5

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 Mass And Momentum Option: Cart. Vel. Components 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] Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 19

Postprocessing

Summary Release 14.5

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: workers Boundary Type: Wall Location: MONITORS Heat Transfer Option: Temperature Fixed Temperature: 37 [C] Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 20

Postprocessing

Summary Release 14.5

Boundary Conditions • computerVent boundary condition: – Name: computerVent – Boundary Type: Inlet – Location: COMPUTER1VENT, COMPUTER2VENT, COMPUTER3VENT, – – – –

COMPUTER4VENT (to select multiple locations click on Ctrl button while making selection) Mass and Momentum Option: Mass Flow Rate Mass Flow Rate: 0.132 [kg/s] Heat Transfer Option: Static Temperature Static Temperature: 40 [C]

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 21

and then hold down the

Postprocessing

Summary Release 14.5

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.

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 22

Postprocessing

Summary Release 14.5

Solver Control • • • • •

Edit Solver Control from the Outline tree

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

– The default value 0.01 is applicable here

• Click OK to commit the settings

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 23

Postprocessing

Summary Release 14.5

Monitor Point 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 temperature.

• Edit Output Control from the Outline tree • Switch to the Monitor tab and enable the Monitor Objects toggle

• Under Monitor Points and Expressions click the Add new item icon

• Enter the Name as temp • Set the Option to Expression • In the Expression Value field type in: massFlowAve(Temperature)@outlet

• Click OK to create the monitor point Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 24

Postprocessing

Summary Release 14.5

Solution Save the project and write a definition file:

• Close CFX-Pre to return to the Project Schematic window and save the project 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

• 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

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 25

Postprocessing

Summary Release 14.5

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 (shown on next slide)

– The residual target of 1e-4 was met at

– –

about 290 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. Introduction

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 26

Postprocessing

Summary Release 14.5

CFX Solver Manager Residual plots for Mass and Momentum and Heat Transfer

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 27

Postprocessing

Summary Release 14.5

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, VMom, W-Mom, P-Mass and H-Energy equations It took 722 iterations to satisfy the Conservation Target of 1% for the HEnergy equation – see the Plot Monitor 1 tab

• Close the CFX-Solver Manager • View the results in CFD-Post by double-clicking Results for the same room Results system Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 28

Postprocessing

Summary Release 14.5

Temperature Plot Start by creating a ZX Plane at Y = 1.2 [m] • Select Location > Plane from the toolbar

• On the Geometry tab in the Details window set the Method to ZX Plane

• Set Y to 1.2 [m] • On the Color tab set Mode to Variable

• Set Variable to Temperature • Set Range to Local and click Apply

– Observe how the warm air collects under the table Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 29

Postprocessing

Summary Release 14.5

Temperature Plots 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

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 30

Postprocessing

Summary Release 14.5

Vector Plots Plot vectors plots on the planes that you created:

• Insert> Vector • On the Geometry tab in the Details window, set Location to Plane 2

• On the Symbol tab, set the Symbols Size to 3

• Click Apply • After observing the flow behavior on Plane 2, switch the Location to Plane 4

• Click Apply Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 31

Postprocessing

Summary Release 14.5

Further Steps 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

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 32

Postprocessing

Summary Release 14.5

Summary • This workshop has shown the steps needed to set up a simulation that includes:

– Profile Boundary Condition export and import – Buoyant flow – Heat Transfer

• Of particular note is that, for heat transfer problems, it is very important to consider the domain imbalance in a system. In this case the solution needed to proceed for more than double the number of iterations that would have been needed to converge to 1e-4.

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solving 33

Postprocessing

Summary Release 14.5