1 / 27

Introduction to CFX

Workshop 6 Electronics Cooling with Natural Convection and Radiation. Introduction to CFX. Pardad Petrodanesh.Co Lecturer: Ehsan Saadati ehsan.saadati@gmail.com www.petrodanesh.ir. Goals.

amber
Download Presentation

Introduction to CFX

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. Workshop 6Electronics Cooling withNatural Convection and Radiation Introduction to CFX PardadPetrodanesh.Co Lecturer: Ehsan Saadati ehsan.saadati@gmail.com www.petrodanesh.ir

  2. Goals • This workshop models the heat dissipation from a hot electronics component fitted to a printed circuit board (PCB) via a finned heat sink. The PCB is fitted into a casing, which is open at the top and bottom. • Initially only the heat transfer via convection and conduction will be modelled. The effect of thermal radiation will then be included at a later stage.

  3. Loading Mesh (Workbench) • Open a new Workbench project and save it as HeatSink.wbpj • Look in the Component Systems section of the toolbox and drag a CFX system onto the Project Schematic • Double-click Setup to start CFX-Pre • In CFX-Pre, right-click Mesh and select Import Mesh > ANSYS Meshing • Select HeatSink.cmdb and click Open

  4. Separate interfaces are required for each domain because when radiation is added, emissivity will be set differently at each domain interfaces Options • In the tree expand Case Options, double-click General and ensure that Automatic Default Domains is switched on and Automatic Default Interfaces is active. • Set the Interface Method to One Per Domain Pair. Click OK.

  5. Create Fluid Domains First add a domain for the fluid region. The effects of buoyancy must be included, as the flow is driven by natural convection. The buoyancy reference density represents the density at the ambient conditions. • Right-click on Flow Analysis 1 and insert a new domain named Fluid • Open the details for Fluid and set the Location to Fluid • Set the Material to Air Ideal Gas • Switch the Buoyancy option to Buoyant and set the directional components to (0, -g, 0) • Click on the expression button to enter –g • Set the Reference Density to 1.1093 [kg m^-3] • Click the Fluid Models tab • Set Heat Transfer to Thermal Energy and Turbulence to None (Laminar) • Click OK

  6. Creating Materials CFX contains a library of many materials, but for this case we will create user materials for the component and Printed Circuit Board (PCB). • In the tree right-click on Materials and select Insert > Material. Name it ComponentMat • Define the material as a Pure Substance in the CHT Solids Material Group • Enable Thermodynamic State and select Solid • This must be set to allow it to be used in a solid domain • Click the Material Properties tab and set Density to 1120 [kg m^-3] • Select Specific Heat Capacity and set it to 1400 [J kg^-1 K^-1] • Expand Transport Properties and set Thermal Conductivity to 10 [W m^-1 K^-1] • Select OK

  7. Creating Materials • Repeat steps 1-7 to create PCBMat using • Density = 1250 [kg m^-3] • Specific Heat Capacity = 1300 [J kg^-1 K^-1] • Thermal Conductivity = 0.35 [W m^-1 K^-1]

  8. When all 4 domains are created the Default Domain will automatically be removed from the tree. Separate interfaces between each domain will have been automatically created, rather than combined into a single interface. Create Solid Domains This case contains three different solid parts that use different materials. Each part will be created as a different domain. • Insert a new domain called HeatSink • Set the Location to HeatSink • Set the Domain Type to Solid Domain with the Material set to Aluminium • Click OK to create the domain • Note that an interface between the two domains is automatically created • Repeat steps 1-4 to create a solid domain called Component located at IC using the Material ComponentMat, and a further solid domain called PCB located at PCB using PCBMat

  9. Adding Energy Source • In the tree right-click on the Component domain and select Insert > Subdomain, using the name Chip • Set the Location to IC so the subdomain occupies the whole of the Component domain • Switch to the Sources tab and check the Sources box and the Energy box • Set the Option to Total Source, enter75 [kg m^2 s^-3] then click OK The component is generating 75 [W] of heat which must be added to the simulation. To add this energy source in CFX, a subdomain must be created.

  10. Boundary Conditions For this case all of the heat will be extracted by the air passing over the heat exchanger so all solid walls will be defined using adiabatic settings. Within the simulation heat can pass between all of the solid and fluid domains because interfaces have been automatically created. To allow air to enter or leave the simulation domain, the top and bottom face of the fluid domain are defined as openings. • Right-click on the Fluid domain and insert a new boundary called Walls and set the Boundary Type to Wall • Set the Location to Wall • Switch to the Boundary Details tab and check that Heat Transfer is set to Adiabatic then click OK • In the PCB domain rename PCB Default to PCBwalls and check that Heat Transfer is set to Adiabatic

  11. The Opening Pressure and Opening Temperature options set Total values when flow is entering the domain and Static values when flow is leaving. This is appropriate when the flow outside the domain is accelerated from rest before entering the domain but will have a velocity when leaving. Boundary Conditions • In the Fluid domain rename Fluid Default to Openings and check that the Location is set to be the two ends of the fluid domain • In the Basic Settings tab change the Boundary Type to Opening • In the Boundary Details tab set the Mass and Momentum option to Opening Pres. and Dirn with a relative pressure of 0 [Pa] • Set Heat Transfer to Opening Temperature at 45 [C]

  12. Solver Control • From the tree right-click Solver Control and select Edit • Increase the Max. Iterations to 500 • Leave the Fluid Timescale Control set to Auto Timescale • Leave Solid Timescale set to Auto Timescale • Note that solid regions will use a much larger timescale than fluid regions because only the energy equation is being calculated within the solid • Click OK

  13. Radiation Setup The next step is to redefine the model to include radiation effects. This will be set up as a second analysis that can be run after the convection only case using results from the initial simulation as starting conditions. This reduces the overall computational time, as the convection only case will be much closer to the end solution. Most of the settings will be the same as the original analysis so the first step will be to make a duplicate analysis. • Right-click on Flow Analysis 1 and rename it to Convection • Right-click on Convection and select Duplicate • Rename Copy of Convection to Radiation • This will form the basis of the radiation case

  14. Adding Radiation to the Air Domains The effects of radiation need to be included in the new analysis. In this case, the surface-to-surface model will be used so radiation is only passed from wall to wall and the fluid does not participate in any way. This saves computational time and is appropriate since air will not absorb or emit significant thermal radiation on these length scales. • In the Radiation analysis, edit theFluid domain • Switch to the Fluid Models tab • Under Thermal Radiation set theOption to Discrete Transfer • Set Transfer Mode to Surface to Surface • Click OK

  15. As the default value was all that was required in this case an alternative method of correcting this error would have been to right-click on the error message and select Auto Fix Physics. Updating the Boundary Conditions. Adding radiation will produce an error because additional information is now required at the Openings boundary. • Edit the boundary Openings. Make sure that it is the copy from the Radiation Flow Analysis that is being edited • Click the Boundary Details tab and see that Thermal Radiation has been added and is set to Local Temperature • Click OK to accept this addition to the boundary condition

  16. Radiation Emissivity Different materials will have different radiation emissivity values. These can be set at each of the boundaries around the Fluid domain within the Radiation analysis. The emissivity of a surface is a function of the material, surface finish and any coatings that may have been applied as well as local temperature and the radiation wavelength. • In the Fluid domain find theinterface boundary thatconnects the HeatSink to thefluid • Hint: boundaries arehighlighted in the viewerwhen selected • Open up that boundary andin the Boundary Details tabchange Emissivity to 0.3then click OK

  17. Radiation Emissivity Note that each interface object is shown at the flow analysis level. There are two interface boundaries (at the domain level) associated with each interface object. Here we are editing the emissivity values for the interface boundaries in the fluid domain. The interface boundaries in the solid domains do not have an emissivity, because there is no radiation in the solid domain (they are opaque!). • Find the interface boundary in the Fluid domain connecting the Component and Fluid domains and set Emissivity to 0.9 • Find the interface connecting the PCB to the Fluid domain and set Emissivity to 0.9 • Open the boundary Walls and set Emissivity to 0.9

  18. Defining Configurations CFX-Pre now contains two separate setups for this project. It is necessary to indicate the order in which they run and how they are linked. This is achieved by setting up configurations. (Note that you could run each case separately, manually starting the radiation case from the convection solution.) • In the main tree expand Simulation Control then right-click on Configurations and select Insert > Configuration, accepting the default name • In the General Settings tab set the Flow Analysis to Convection and Activation Condition 1 to Start of Simulation • Click OK

  19. Defining Configurations • Insert a second configuration and set the Flow Analysis to Radiation. Set the Activation Condition to End of Configuration, and set Configuration Names to Configuration 1 • Switch to the Run Definition tab, select Configuration Execution Control then Initial Values Specification. Set the option to Configuration Results, using Configuration 1 • Click OK The convection case will run first, then when it finishes the .res file it created will be used to initialise the radiation simulation.

  20. Running the Simulation • Select File > Quit to exit CFX-Pre • Save the Project • In the Project Schematic, right-click on Solution and select Update • While the solver is running right-click on Solution again and select Display Monitors to check on progress

  21. Running the Simulation This case uses a multi-configuration setup so the first screen will show the global progress by showing which configuration is being run. • Change the Workspace from the current run to Configuration1_001 • The standard out file and residuals are displayed • This run will take a while to run so after a few iterations stop the run and the results provided will be used • Close the Solver Manager

  22. Open CFD-Post • From the Component Systems section of the Toolbox drag a Results system onto the Project Schematic • Right-click on the Results cell (B2) and select Edit • When CFD-Post opens, select File > Load Results and select HeatSink.mres. Use the option Load complete history as: Separate cases The results field in the existing CFX module is associated with the partially calculated results from your setup. To analyse the existing results you will add a new results field to the project.

  23. Case Comparison The case comparison tool allows two different setups to be shown side by side and any differences between the two cases identified. • In the tree edit Case Comparison • Enable the check-box Case Comparison Active and check that Case 1 is set to Configuration 1 and Case 2 is set to Configuration 2 • In the viewer a new view is created to display the difference between the convection only case and the case including radiation • Click Apply to enter comparison mode

  24. Temperature Temperature will be a key variable for any electronics cooling application so it will be displayed in several locations, such as within the flow, on the surfaces of the solid region and by extracting the maximum temperature within the component. When these plots are created they appear in the User Locations and Plots section of the tree. • Create a YZ plane using Location > Plane. Name it Centre, set X to 0 [m] and colour using the variable Temperature. • Create a contour plot using Insert > Contour or by clicking on . Use the fluid-solid interfaces as the location (use the ‘…’ icon and Ctrl key to select multiple locations from both configurations). Set the Variable to Temperature using the Global Range.

  25. Temperature • Move to the function calculator using the icon on the toolbar. Set the options to: Function = maxValLocation = ComponentCase = All Cases Variable = Temperature • Click Calculate • Note that with radiation (Configuration 2) the temperature in the solid is significantly lower than when radiation was not included. The cooling of the component is mirrored with an increase in the temperature of the walls around the fluid zone. This can be seen if you plot the temperature on the walls or use the Function Calculator with the areaAve function.

  26. Flow Displays To show the flow patterns a range of methods can be used including streamlines, vector plots and isosurfaces. • Switch off the visibility of the existing plots • Insert an isosurface using Location > Isosurface and set the Variable to Velocity with a value of 0.5 [m s^-1] • Gradually reduce the isosurface value to 0.2 [m s^-1] and notice that for the radiation case higher speed flow can be observed close to the fluid walls as well as the PCB

  27. Flow Displays • Insert a vector plot using Insert > Vector or click on • Set the location to Centre. Change the sampling to Equally Spaced with 1000 points • If you wish to see the pattern in the slow speed sections try going to the Symbol tab and select Normalize Symbols • Insert streamlines using Insert > Streamlines or by clicking on • Set Start From to Openings • Apply 100 equally spaced points and set the Direction to Forward and Backward

More Related