ANSYS 12.0 官方培训手册-Introduction to CFX-PART G.ppt

ANSYS 12.0 Training ManualCFX 12.0,Introduction to CFXPart G Workshop 5-10, 163 Pages,Introduction to CFX,Workshop 6Electronics Cooling withNatural Convection and Radiation,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.,Goals,Loading Mesh (Workbench),Open a new Workbench project and save it as HeatSink.wbpjLook in the Component Systems section of the toolbox and drag a CFX system onto the Project SchematicDouble-click Setup to start CFX-PreIn CFX-Pre, right-click Mesh and select Import Mesh > ANSYS MeshingSelect HeatSink.cmdb and click Open,,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.,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 FluidOpen the details for Fluid and set the Location to FluidSet the Material to Air Ideal GasSwitch the Buoyancy option to Buoyant and set the directional components to (0, -g, 0)Click on the expression button to enter –gSet the Reference Density to 1.1093 [kg m^-3]Click the Fluid Models tabSet Heat Transfer to Thermal Energy and Turbulence to None (Laminar)Click OK,Create Fluid Domains,Creating Materials,In the tree right-click on Materials and select Insert > Material. Name it ComponentMatDefine the material as a Pure Substance in the CHT Solids Material GroupEnable Thermodynamic State and select SolidThis must be set to allow it to be used in a solid domainClick 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,CFX contains a library of many materials, but for this case we will create user materials for the component and Printed Circuit Board (PCB).,Creating Materials,Repeat steps 1-7 to create PCBMat usingDensity = 1250 [kg m^-3]Specific Heat Capacity = 1300 [J kg^-1 K^-1] Thermal Conductivity = 0.35 [W m^-1 K^-1],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 HeatSinkSet the Location to HeatSinkSet the Domain Type to Solid Domain with the Material set to AluminiumClick OK to create the domainNote that an interface between the two domains is automatically createdRepeat 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,Adding Energy Source,In the tree right-click on the Component domain and select Insert > Subdomain, using the name ChipSet the Location to IC so the subdomain occupies the whole of the Component domainSwitch to the Sources tab and check the Sources box and the Energy boxSet 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.,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 WallSet the Location to WallSwitch to the Boundary Details tab and check that Heat Transfer is set to Adiabatic then click OKIn the PCB domain rename PCB Default to PCBwalls and check that Heat Transfer is set to Adiabatic,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 domainIn the Basic Settings tab change the Boundary Type to OpeningIn 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],Solver Control,From the tree right-click Solver Control and select EditIncrease the Max. Iterations to 500Leave the Fluid Timescale Control set to Auto TimescaleLeave Solid Timescale set to Auto TimescaleNote that solid regions will use a much larger timescale than fluid regions because only the energy equation is being calculated within the solidClick OK,。