SlideShare a Scribd company logo

Aws90 ch06 thermal

Download as PPT, PDF
C
chowdavaramsaiprasad

This chapter discusses performing steady-state thermal analyses in ANSYS Workbench Simulation. It covers geometry elements, contact types for assemblies, environmental loads and supports, solving models, and results postprocessing. It also describes the basics of steady-state heat transfer analysis including Fourier's Law and the assumptions made in this type of analysis.

Engineering
1 of 40
Downloaded 13 times
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
Thermal Analysis Chapter Six
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-2 Chapter Overview • In this chapter, performing steady-state thermal analyses in Simulation will be covered: – Geometry and Elements – Contact and Types of Supported Assemblies – Environment, including Loads and Supports – Solving Models – Results and Postprocessing • The capabilities described in this section are generally applicable to ANSYS DesignSpace Entra licenses and above, except for an ANSYS Structural license. – Some options discussed in this chapter may require more advanced licenses, but these are noted accordingly. – It is assumed that the user has reviewed Chapters 1-3 prior to this chapter. (Chapters 4-5 are optional)
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-3 Basics of Steady-State Heat Transfer • For a steady-state (static) thermal analysis in Simulation, the temperatures {T} are solved for in the matrix below: This results in the following assumptions: – No transient effects are considered in a steady-state analysis – [K] can be constant or a function of temperature • Temperature-dependent thermal conductivity can be input for each material property – {Q} can be constant or a function of temperature • Temperature-dependent film coefficients can be input for convective boundary conditions ( )[ ]{ } ( ){ }TQTTK =
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-4 Basics of Steady-State Heat Transfer • Fourier’s Law provides the basis of the previous equation: – This means that the thermal analysis Simulation solves for is a conduction-based equation. • Heat flow within a solid (Fourier’s Law) is the basis of [K] • Heat flux, heat flow rate, and convection are treated as boundary conditions on the system {Q} • No radiation is currently considered • No time-dependent effects are currently considered – Heat transfer analysis is different from CFD (Computational Fluid Dynamics) • Convection is treated as a simple boundary condition, although temperature-dependent film coefficients are possible. • If a conjugate heat transfer/fluid problem needs to be analyzed, one must use ANSYS CFD tools instead. • It is important to remember these assumptions related to performing thermal analyses in Simulation.
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-5 Physics Filters • Before proceeding to a detailed discussion on performing thermal analyses in Simulation, it is useful to point out that if a thermal-only solution is to be performed, the Physics Filter can be useful to filter the GUI. – Under “View menu > Physics Filter,” unselect the “Structural” option. Now, the available options in the Simulation GUI will only reflect thermal analyses. – This applies to options in the “Environment” and “Solution” levels only. – If a thermal-stress simulation is to be performed, do not turn off any physics filters since both structural and thermal options may be required. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-6 A. Geometry • In thermal analyses, all types of bodies supported by Simulation may be used. – Solid, surface, and line bodies are supported by all products which support thermal analyses. • For surface bodies, thickness must be input in the Details view of the Geometry branch • The cross-section and orientation of line bodies is defined within DesignModeler and is imported into Simulation automatically. Although the cross-section and orientation is defined, this information is meant for structural analyses, and the actual thermal link element will have an ‘effective’ cross-section based on the input properties. • No heat flux or vector heat flux output is available with line bodies. Only temperature results are available for line bodies. – The “Point Mass” feature is not applicable in thermal analyses • Point Mass is described in Chapter 4, Linear Structural Analysis. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-7 … Geometry • It is important to understand assumptions related to using shell and line bodies: – For shell bodies, through-thickness temperature gradients are not considered. A shell body should be used for thin structures when it can be safe to assume temperatures on top and bottom of surface are the same. • Temperature variation will still be considered across the surface, just not through the thickness, which is not explicitly modeled. – For line bodies, thickness variation in the cross-section is not considered. A line body should be used for beam- or truss- like structures, where the temperature can be assumed to be constant across the cross-section. • Temperature variation will still be considered along the line body, just not through the cross-section, which is not explicitly modeled. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-8 … Material Properties • The only required material property is thermal conductivity. – Material input is under the “Engineering Data” tab, and material assignment is per part under the “Geometry” branch – Thermal Conductivity is input under the Engineering Data tab. Temperature-dependent thermal conductivity can be input as a table. – Other material input is not used in thermal. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x If any temperature-dependent material properties exist, this will result in a nonlinear solution. This is because the temperatures are solved for, but the materials are dependent on the temperatures, so it is not linear.
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-9 B. Assemblies – Solid Body Contact • When importing assemblies of solid parts, contact regions are automatically created between the solid bodies. – Surface-to-surface contact allows non-matching meshes at boundaries between solid parts – Contact enables heat transfer between parts in an assembly Model shown is from a sample Inventor assembly. ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-10 … Assemblies – Contact Region • In Simulation, the concept of contact and target surfaces are used for each contact region. – One side of the contact region is comprised of “contact” face(s), the other side of the region is made of “target” face(s). – Heat flow is allowed between contact and target faces (based on the contact normal direction) • When one side is the contact and the other side is the target, this is called asymmetric contact. On the other hand, if both sides are made to be contact & target, this is called symmetric contact. However, the designation of which side is contact or target is unimportant in thermal analysis. • By default, Simulation uses symmetric contact for solid assemblies. • For ANSYS Professional licenses and above, the user may change to asymmetric contact, as desired. ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-11 … Assemblies – Contact Region • As noted in the previous slide, heat flows within a contact region in the contact normal direction – No heat spreading is considered in the contact/target interface • Heat spreading is considered within shell or solid elements at the contact or target surfaces because of Fourier’s Law • Heat flow within the contact region is in the contact normal direction only • This means that, regardless of the definition of the contact region, heat flows only if a target element is present in the normal direction In the figure on the left, the solid green double-arrows indicate heat flow within the contact region. Heat flow only occurs if a target surface is normal to a contact surface. The light, dotted green arrows indicate that no heat transfer will occur between parts. ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-12 … Assemblies – Contact Region • In Simulation, various contact behaviors exist – The contact “Type” is meant for structural applications – If the parts are initially in contact, heat transfer will occur between the parts. If the parts are initially out of contact, the parts will not transfer heat between each other. – Based on the contact type, whether heat will be transferred between contact and target surfaces is outlined below: – The pinball region is automatically defined and set to a relatively small value to accommodate small gaps which may present in the model. The pinball region will be discussed next. Initially Touching Inside Pinball Region Outside Pinball Region Bonded Yes Yes No No Separation Yes Yes No Rough Yes No No Frictionless Yes No No Contact Type Heat Transfer Between Parts in Contact Region? ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-13 … Assemblies – Contact Region • The pinball region may be input and visualized in ANSYS Professional licenses and above. – If the target nodes lie within the pinball region and the contact is bonded or no separation, then heat transfer will occur (solid green lines) – Otherwise, no heat transfer will occur between nodes (dotted green lines) In this figure on the right, the gap between the two parts is bigger than the pinball region, so no heat transfer will occur between the parts Pinball Radius ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-14 … Assemblies – Thermal Conductance • By default, a high thermal contact conductance (TCC) is defined between parts of an assembly – The amount of heat flow between two parts is defined by the contact heat flux q: where Tcontact is the temperature of a contact “node” and Ttarget is the temperature of the corresponding target “node” located in the contact normal direction. – By default, TCC is set to a relatively ‘high’ value, based on the largest material conductivity defined in the model KXX and the diagonal of the overall geometry bounding box ASMDIAG. This essentially provides ‘perfect’ conductance between parts. ( )contacttarget TTTCCq −⋅= ASMDIAGKXXTCC /000,10⋅= ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-15 … Assemblies – Thermal Conductance • Perfect thermal contact conductance between parts means that no temperature drop is assumed at the interface. • One may want to include finite thermal conductance instead – Two surfaces (at different temperatures) in contact experience a temperature drop across the interface. The drop is due to imperfect contact between the two surfaces. The imperfect contact, and hence the finite contact conductance, can be influenced by many factors such as: • surface flatness • surface finish • oxides • entrapped fluids • contact pressure • surface temperature • use of conductive grease ∆T T x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-16 … Assemblies – Thermal Conductance • In ANSYS Professional licenses and above, the user may define a finite thermal contact conductance (TCC) if the Pure Penalty or Augmented Lagrange Formulation is used. – The thermal contact conductance per unit area is input for each contact region in the Details view, as shown below. – If thermal contact resistance is known, invert this value and divide by the contacting area to obtain TCC value. – When this is done, there will now be a temperature drop between the contact and target surfaces for a contact region. If “Thermal Conductance” is left at “Program Chosen,” near- perfect thermal contact conductance will be defined. The user can change this to “Manual” to input finite thermal contact conductance instead, which is the same as including thermal contact resistance at a contact interface. ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-17 … Assemblies – Thermal Conductance • If using symmetric contact, the user does not need to account for a ‘double’ thermal contact resistance. – Input values as normal • MPC bonded contact allows for perfect thermal contact conductance. – In this case, no thermal contact conductance is used nor defined because ‘contact’ is related via constraint equations. – The contact “node” and corresponding target “node” will have the same temperature because of perfect contact conductance. ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x Do not use “Normal Lagrange” formulation for thermal analyses. If selected, the ANSYS solver will actually use “Augmented Lagrange” with a ‘perfect’ thermal contact conductance.
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-18 … Assemblies – Surface Body Contact • For ANSYS Professional licenses and above, mixed assemblies of shells and solids are supported – Allows for more complex modeling of assemblies, taking advantage of the benefits of shells, when applicable ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-19 … Assemblies – Surface Body Contact • Edge contact is a subset of general contact – For contact including shell faces or solid edges, only bonded or no separation behavior is allowed. – For contact involving shell edges, only bonded behavior using MPC formulation is allowed. • For MPC-based bonded contact, user can set the search direction (the way in which the multi-point constraints are written) as either the target normal or pinball region. • If a gap exists (as is often the case with shell assemblies), the pinball region can be used for the search direction to detect contact beyond a gap. • MPC results in perfect contact conductance ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-20 … Assemblies – Spot Weld • Spot welds provide a means of connecting shell assemblies at discrete points for heat transfer – Spotweld definition is done in the CAD software. Currently, only DesignModeler and Unigraphics define spotwelds in a manner that Simulation supports. – Spotwelds can also be created in Simulation manually, but only at discrete vertices. ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x DesignModeler x Pro/ENGINEER Unigraphics x SolidWorks Inventor Solid Edge Mechanical Desktop CATIA V4 CATIA V5 ACIS (SAT) Parasolid IGES
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-21 C. Loads • There are three types of loads in thermal analyses: – Heat Loads: • These loads pump heat into the system. • Heat loads can be input as a known heat flow rate or heat flow rate per unit area or unit volume. – Adiabatic Condition: • This is the naturally-occurring boundary condition, where there is not heat flow through the surface. – Thermal Boundary Conditions: • These boundary conditions act as heat sources or heat sinks with a known temperature condition. • These can be either a prescribed temperature or a convection boundary condition with a known bulk temperature. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-22 … Heat Loads • Heat Flow: – A heat flow rate can be applied to a vertex, edge, or surface. The load gets distributed for multiple selections. – Heat flow has units of energy/time (i.e., power). • Heat Flux: – A heat flux can be applied to surfaces only. – Heat flux has units of energy/time/area (i.e., power/area) • Internal Heat Generation: – An internal heat generation rate can be applied to bodies only. – Heat generation has units of energy/time/volume A positive value for heat load will add energy to the system. Also, if multiple loads are present, the effect is cumulative. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-23 … Adiabatic Conditions • Perfectly Insulated: – Perfectly insulated condition is applied to surfaces – Can be thought of as a zero heat flow rate loading – This is actually the naturally-occurring condition in thermal analyses, when no load is applied. • Usually, one does not need to apply a perfectly insulated condition on surfaces since that is the natural behavior for a regular surface. • Hence, this loading is meant to be used as a way to remove loading on specified surfaces. For example, it may be easier for a user to apply heat flux or convection on all surfaces, then use the perfectly insulated condition to selectively ‘remove’ the loading on some surfaces (such as those in contact with other parts). ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-24 … Thermal Boundary Conditions Thermal boundary conditions present a known local or ‘remote’ temperature condition. • At least one type of thermal boundary condition must be present. Otherwise, the steady-state temperature will be infinite if only heat is pumped into a system! • Also, Given Temperature or Convection load should not be applied on surfaces that already have another heat load or thermal boundary condition applied to it. – If applied on an entity which also has a heat load, the temperature boundary condition will override. – Perfect insulation will override thermal boundary conditions. • Given Temperature: – This imposes a temperature on vertices, edges, or surfaces. – Temperature is the degree of freedom solved for, but this fixes the temperature on selected entities to a given value. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-25 … Thermal Boundary Conditions • Convection: – Applied to surfaces only. – Convection relates a ‘ambient temperature’ with the surface temperature: where the convective heat flux q is related to a film coefficient h, the surface area A, and the difference in the surface temperature Tsurface & ambient temperature Tbulk. – Meant to provide a simplified way of accounting for heat transport from a fluid. “h” and “Tbulk” are user-input values. – The film coefficient h can be constant or input from a file (next) ( )ambientsurface TThAq −= ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-26 … Thermal Boundary Conditions • Temperature-Dependent Convection (continued): – If film coefficient h is input from a file, this can be a constant or temperature-dependent value h(T). • Define a convection boundary condition under the Environment branch and define the Type to be “Temperature-Dependent”. Next, select “New Convection…” for the Correlation. The “Engineering Data” tab will open and the Coefficient Type can then be defined for the new convection load. • Determine what temperature is used for h(T) first, for temperature- dependent film coefficients. Temperature can be: – Average film temperature T=(Tsurface+Tbulk)/2 – Surface temperature T= Tsurface – Bulk temperature T= Tbulk – Difference of surface and bulk temperatures T=(Tsurface-Tbulk) ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x Select the temperature- dependency from the pull-down menu
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-27 … Thermal Boundary Conditions • Temperature-Dependent Convection (continued): • After the type of temperature-dependency is selected, the user may input the film coefficients and temperatures in a table. The values are plotted on a graph, as shown below. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x If any temperature-dependent convection load is applied, this will result in a nonlinear solution since the surface temperature is solved for, but the film coefficient h is based on a function of the surface temperature. The only exception is if the film coefficient h is based on a function of the bulk temperature only. In Simulation, the bulk temperature is constant and input by the user, so this load will not be nonlinear. Right mouse click on the table to add or delete values.
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-28 … Thermal Boundary Conditions • Temperature-Dependent Convection (continued): • The convection data can also be imported from a file. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-29 … Thermal Loads Summary • For some structural users, it may be useful to provide an analogy of structural and thermal analyses: – There are some types of loads that do not have any analogy • There is no thermal equivalent for inertial loads such as rotational velocity or acceleration • The analogy of convective boundary condition is a ‘foundation stiffness’ support in structural terms, similar to a grounded spring Structural Thermal Natural Condition No external force Perfectly Insulated (No heat flow rate) Direct Given Displacement Given Temperature Indirect Convection Direct Force Heat Flow Per Area Pressure Heat Flux Per Volume Thermal Expansion Internal Heat Generation Inertial Loads Acceleration Boundary Conditions Load
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-30 D. Solution Options • Solution options can be set under the “Solutions” branch: – The ANSYS database can be saved if “Save ANSYS db” is set • Useful if you want to open a database in ANSYS – Two solvers are available in Simulation • The default solver is automatically chosen and does not usually need to be changed. • The “Iterative” solver can be efficient for solving large models whereas the “Direct” solver is a robust solver and handles any situation. • The ability to change the default solver is under “Tools > Options… > Simulation: Solution > Solver Type” – The “Weak Springs” and “Large Deflection” options are meant for structural analyses only, so they can be ignored for a thermal analysis. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-31 … Solution Options – Informative settings show the user the status of the analysis: • For a regular thermal analysis, the “Analysis Type” will be set to “Static Thermal.” If structural supports and results are present, then the analysis type will be “Thermal Stress.” • A nonlinear solution will be required if temperature-dependent (a) material properties or (b) convection film coefficients are present. This means that several internal iterations will be run to achieve heat equilibrium. • The solver working directory is where scratch files are saved during the solution of the equations. By default, the TEMP directory of your Windows system environment variable is used, although this can be changed in “Tools > Options… > Simulation: Solution > Solver Working Directory”. – Any solver messages which appear after solution can be checked afterwards under “Solver Messages”ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-32 … Solving the Model • To solve the model, request results first (covered next) and click on the “Solve” button on the Standard Toolbar – By default, two processors (if present) will be used for parallel processing. To change this, use “Tools > Options… > Simulation: Solution > Number of Processors to Use” – Recall that if a “Solution Information” branch is requested, the details of the solution output can be examined. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-33 … Solving the Model • To perform a thermal-stress solution, simply add structural support(s) and request structural results, then solve the model. – Structural loads are optional but can also be added. – Simulation will know that a thermal-stress analysis is to be performed (under Details view of the Solution branch). The following will be performed automatically: • A steady-state thermal analysis will be performed • The temperature field will be mapped back onto the structural model • A structural analysis will be performed – See Chapter 4 for details on Structural Analyses – Simulation automates this type of coupled-field solution, so the user does not have to worry about the above details. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-34 E. Results and Postprocessing • Various results are available for postprocessing: – Temperature – Heat Flux – “Reaction” Heat Flow Rate • In Simulation, results are usually requested before solving, but they can be requested afterwards, too. – If you solve a model then request results afterwards, click on the “Solve” button , and the results will be retrieved. A new solution is not required for retrieving output of a solved model.
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-35 … Temperature • Temperature contour plots can be requested: – Temperature is the degree of freedom solved for, and it is the most basic output request. – Temperature is a scalar quantity and, therefore, has no direction associated with it. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-36 … Heat Flux • Heat flux contour or vector plots are available: – Heat flux q is defined as and is related to the thermal gradient ∇T. The heat flux output has three components and can aid the user in seeing how the heat is flowing. – The magnitude plotted as contours: “Total Heat Flux” – The magnitude & direction as vectors: “Vector Heat Flux” • Recall that wireframe is best for viewing vectors – Components of heat flux can be requested with “Directional Heat Flux” and can be mapped on any coordinate system. TKXXq ∇⋅−= ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-37 … Reaction Heat Flow Rate • Reaction heat flow rates is available for any Given Temperature or Convection boundary condition – Recall that both given temperature and convection supply a known temperature, either directly or indirectly. Hence, this acts as a heat source/sink, and the amount of heat flowing in (positive) or out (negative) of the support can be output. – For each individual Given Temperature or Convection load, the Reaction heat flow rate is printed in the Details view after a solution. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-38 … Reaction Heat Flow Rate • The “Worksheet” tab for “Environment” branch has a tabular summary of reaction heat flow rates. – If a thermal support shares a vertex, edge, or surface with another thermal support or load, the reported reaction heat flow rate may be incorrect. This is due to the fact that the underlying mesh will have multiple supports applied to the same nodes. The solution will still be valid, but the reported values may not be accurate because of this. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-39 F. Workshop 6 • Workshop 6 – Thermal Analysis • Goal: – Analyze the pump housing shown below for its heat transfer characteristics.
Aws90 ch06 thermal

More Related Content

PPT
CFD & ANSYS FLUENT
MD SHUJAN ALI
 
PPT
Aws100 ch06 thermal
chowdavaramsaiprasad
 
PPTX
12 transient analysis theory
chowdavaramsaiprasad
 
PPTX
13 r1-transient analysis methodology
chowdavaramsaiprasad
 
PPTX
11 (l)random vibrations methodology
chowdavaramsaiprasad
 
PPTX
11 generalsisation of fluent
chowdavaramsaiprasad
 
PPTX
12 l1-harmonic methodology
chowdavaramsaiprasad
 
PPTX
11 types of solvers
chowdavaramsaiprasad
 
CFD & ANSYS FLUENT
MD SHUJAN ALI
 
Aws100 ch06 thermal
chowdavaramsaiprasad
 
12 transient analysis theory
chowdavaramsaiprasad
 
13 r1-transient analysis methodology
chowdavaramsaiprasad
 
11 (l)random vibrations methodology
chowdavaramsaiprasad
 
11 generalsisation of fluent
chowdavaramsaiprasad
 
12 l1-harmonic methodology
chowdavaramsaiprasad
 
11 types of solvers
chowdavaramsaiprasad
 

What's hot (20)

PDF
Cfd analysis of horizontal plate in fluent
Khusro Kamaluddin
 
PPTX
Learning ANSYS Fluent R19 using modeling a Fluidized Bed with nano particles
Hamed Hoorijani
 
PDF
HLPW2-sasanapuri
Vijay Kumar
 
PPT
Fluent and Gambit Workshop
khalid_nitt
 
PPTX
CFD Introduction using Ansys Fluent
savani4611
 
PPTX
Design of robust plant layout for dynamic plant layout problem2
National Institute of Technology Calicut
 
PDF
Fvm fdm-fvm
Parhamsagharchi
 
PPTX
Solar cell Modeling with Scaps 1-D
shubham mishra
 
PPTX
Fluid Mechanics in CFD Perspective
George Mathew Thekkekara
 
PDF
International Journal of Computational Engineering Research(IJCER)
ijceronline
 
PPT
Fem lecture
Muhammad Mohsin Waseem
 
PPT
Finite element method
Santosh Chavan
 
PPTX
Numerical methods for 2 d heat transfer
Arun Sarasan
 
PPTX
CAD Softwares
sgrsoni45
 
PDF
Lecture 13 modeling_errors_and_accuracy
Javier Antonio Cárdenas Oliveros
 
PPTX
FEA good practices presentation
Mahdi Damghani
 
PPTX
IEEE APE
Utsav Yagnik
 
PDF
CFD Troubleshooting Guide
Hashan Mendis
 
PPT
Introduction to FEA and applications
Padmanabhan Krishnan
 
PPTX
Finite Element Method
Bharat sharma
 
Cfd analysis of horizontal plate in fluent
Khusro Kamaluddin
 
Learning ANSYS Fluent R19 using modeling a Fluidized Bed with nano particles
Hamed Hoorijani
 
HLPW2-sasanapuri
Vijay Kumar
 
Fluent and Gambit Workshop
khalid_nitt
 
CFD Introduction using Ansys Fluent
savani4611
 
Design of robust plant layout for dynamic plant layout problem2
National Institute of Technology Calicut
 
Fvm fdm-fvm
Parhamsagharchi
 
Solar cell Modeling with Scaps 1-D
shubham mishra
 
Fluid Mechanics in CFD Perspective
George Mathew Thekkekara
 
International Journal of Computational Engineering Research(IJCER)
ijceronline
 
Fem lecture
Muhammad Mohsin Waseem
 
Finite element method
Santosh Chavan
 
Numerical methods for 2 d heat transfer
Arun Sarasan
 
CAD Softwares
sgrsoni45
 
Lecture 13 modeling_errors_and_accuracy
Javier Antonio Cárdenas Oliveros
 
FEA good practices presentation
Mahdi Damghani
 
IEEE APE
Utsav Yagnik
 
CFD Troubleshooting Guide
Hashan Mendis
 
Introduction to FEA and applications
Padmanabhan Krishnan
 
Finite Element Method
Bharat sharma
 
Ad

Similar to Aws90 ch06 thermal (20)

PPT
AWS90_Ch06_Thermal.ppt
SandeepBhatia69
 
PPTX
IABU-UNIT99-LA04-Thermal Abaqus Documentation
Prasanna389554
 
PPTX
ANSYS.pptx
samygs1
 
PPTX
Introduction to ANSYS Workbench
nagesh surner
 
PDF
Finite element using ansys
jivanpawar5
 
PDF
Engineering System Modelling and Simulation Lab
Vishal Singh
 
PDF
midas NFX 2013: Towards a New Generation of Mechanical FEA Solution
MIDAS Information Technology
 
PDF
Transient thermal analysis of a clutch plate in Ansys
Rahul Shedage
 
PPT
Electro Thermal IC Simulation With Saber
domnitei
 
PDF
ANSYS AIM
Ekin ERSAN
 
PDF
Ansys icepak r160 update p4
CY N
 
PDF
vol2no10_10
Muyideen Dele Adewale
 
PDF
midas NFX 2015 is Released. Accurate FEA whenever you need!
MIDAS Information Technology
 
PDF
What's new in midas NFX 2015
Cyprien Rusu
 
PDF
STUDY AND ANALYSIS OF TREE SHAPED FINS BY USING FLUENT
Ijripublishers Ijri
 
PPT
Anasys Full.ppt
Rama Krishna
 
PDF
Casa lab manual
BHARATNIKKAM
 
PDF
Mech_HT_18.0_WS04.1_Radiating_System.pdf
jntuhcej
 
PDF
Arjan Ghosh Mechanical Portfolio
Arjan Ghosh
 
PPTX
Residual stress laser_welding
Ashutosh Srivastava
 
AWS90_Ch06_Thermal.ppt
SandeepBhatia69
 
IABU-UNIT99-LA04-Thermal Abaqus Documentation
Prasanna389554
 
ANSYS.pptx
samygs1
 
Introduction to ANSYS Workbench
nagesh surner
 
Finite element using ansys
jivanpawar5
 
Engineering System Modelling and Simulation Lab
Vishal Singh
 
midas NFX 2013: Towards a New Generation of Mechanical FEA Solution
MIDAS Information Technology
 
Transient thermal analysis of a clutch plate in Ansys
Rahul Shedage
 
Electro Thermal IC Simulation With Saber
domnitei
 
ANSYS AIM
Ekin ERSAN
 
Ansys icepak r160 update p4
CY N
 
vol2no10_10
Muyideen Dele Adewale
 
midas NFX 2015 is Released. Accurate FEA whenever you need!
MIDAS Information Technology
 
What's new in midas NFX 2015
Cyprien Rusu
 
STUDY AND ANALYSIS OF TREE SHAPED FINS BY USING FLUENT
Ijripublishers Ijri
 
Anasys Full.ppt
Rama Krishna
 
Casa lab manual
BHARATNIKKAM
 
Mech_HT_18.0_WS04.1_Radiating_System.pdf
jntuhcej
 
Arjan Ghosh Mechanical Portfolio
Arjan Ghosh
 
Residual stress laser_welding
Ashutosh Srivastava
 
Ad

Recently uploaded (20)

PPTX
UNIT-1 - COAL BASED THERMAL POWER PLANTS
Chandra Kumar S
 
DOCX
573137875-Attendance-Management-System-original
AYUSHMANAV
 
PPTX
OOP with Java - Java Introduction (Basics)
Rashmi T V
 
PDF
Mohammad Mahdi Farshadian CV - Prospective PhD Student 2026
Educational Group Mohammad Farshadian
 
PPTX
CARTOGRAPHY AND GEOINFORMATION VISUALIZATION chapter1 NPTE (2).pptx
abhi1361yadav
 
PPTX
FINAL REVIEW FOR COPD DIANOSIS FOR PULMONARY DISEASE.pptx
rubeshbme
 
PPTX
CYBER-CRIMES AND SECURITY A guide to understanding
Davies Chacko
 
PDF
Well-logging-methods_new................
ZafriFarid
 
PPTX
Internet of Things (IOT) - A guide to understanding
Davies Chacko
 
PPTX
Lesson 3_Tessellation.pptx finite Mathematics
quakeplayz54
 
PDF
Mitigating Risks through Effective Management for Enhancing Organizational Pe...
IJAEMSJORNAL
 
DOCX
ASol_English-Language-Literature-Set-1-27-02-2023-converted.docx
AYUSHMANAV
 
PPTX
UNIT 4 Total Quality Management .pptx
gokuld13012005
 
PDF
Structs to JSON How Go Powers REST APIs.pdf
Emily Achieng
 
PPTX
Recipes for Real Time Voice AI WebRTC, SLMs and Open Source Software.pptx
Alberto González Trastoy
 
PPT
Project quality management in manufacturing
BarMusaTetik
 
PPTX
IOT PPTs Week 10 Lecture Material.pptx of NPTEL Smart Cities contd
ssusera400e8
 
PPTX
Sustainable Sites - Green Building Construction
mhdumerali
 
PPTX
bas. eng. economics group 4 presentation 1.pptx
kiribakimoses1993
 
PPTX
Geodesy 1.pptx...............................................
abhi1361yadav
 
UNIT-1 - COAL BASED THERMAL POWER PLANTS
Chandra Kumar S
 
573137875-Attendance-Management-System-original
AYUSHMANAV
 
OOP with Java - Java Introduction (Basics)
Rashmi T V
 
Mohammad Mahdi Farshadian CV - Prospective PhD Student 2026
Educational Group Mohammad Farshadian
 
CARTOGRAPHY AND GEOINFORMATION VISUALIZATION chapter1 NPTE (2).pptx
abhi1361yadav
 
FINAL REVIEW FOR COPD DIANOSIS FOR PULMONARY DISEASE.pptx
rubeshbme
 
CYBER-CRIMES AND SECURITY A guide to understanding
Davies Chacko
 
Well-logging-methods_new................
ZafriFarid
 
Internet of Things (IOT) - A guide to understanding
Davies Chacko
 
Lesson 3_Tessellation.pptx finite Mathematics
quakeplayz54
 
Mitigating Risks through Effective Management for Enhancing Organizational Pe...
IJAEMSJORNAL
 
ASol_English-Language-Literature-Set-1-27-02-2023-converted.docx
AYUSHMANAV
 
UNIT 4 Total Quality Management .pptx
gokuld13012005
 
Structs to JSON How Go Powers REST APIs.pdf
Emily Achieng
 
Recipes for Real Time Voice AI WebRTC, SLMs and Open Source Software.pptx
Alberto González Trastoy
 
Project quality management in manufacturing
BarMusaTetik
 
IOT PPTs Week 10 Lecture Material.pptx of NPTEL Smart Cities contd
ssusera400e8
 
Sustainable Sites - Green Building Construction
mhdumerali
 
bas. eng. economics group 4 presentation 1.pptx
kiribakimoses1993
 
Geodesy 1.pptx...............................................
abhi1361yadav
 

Aws90 ch06 thermal

  • 2. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-2 Chapter Overview • In this chapter, performing steady-state thermal analyses in Simulation will be covered: – Geometry and Elements – Contact and Types of Supported Assemblies – Environment, including Loads and Supports – Solving Models – Results and Postprocessing • The capabilities described in this section are generally applicable to ANSYS DesignSpace Entra licenses and above, except for an ANSYS Structural license. – Some options discussed in this chapter may require more advanced licenses, but these are noted accordingly. – It is assumed that the user has reviewed Chapters 1-3 prior to this chapter. (Chapters 4-5 are optional)
  • 3. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-3 Basics of Steady-State Heat Transfer • For a steady-state (static) thermal analysis in Simulation, the temperatures {T} are solved for in the matrix below: This results in the following assumptions: – No transient effects are considered in a steady-state analysis – [K] can be constant or a function of temperature • Temperature-dependent thermal conductivity can be input for each material property – {Q} can be constant or a function of temperature • Temperature-dependent film coefficients can be input for convective boundary conditions ( )[ ]{ } ( ){ }TQTTK =
  • 4. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-4 Basics of Steady-State Heat Transfer • Fourier’s Law provides the basis of the previous equation: – This means that the thermal analysis Simulation solves for is a conduction-based equation. • Heat flow within a solid (Fourier’s Law) is the basis of [K] • Heat flux, heat flow rate, and convection are treated as boundary conditions on the system {Q} • No radiation is currently considered • No time-dependent effects are currently considered – Heat transfer analysis is different from CFD (Computational Fluid Dynamics) • Convection is treated as a simple boundary condition, although temperature-dependent film coefficients are possible. • If a conjugate heat transfer/fluid problem needs to be analyzed, one must use ANSYS CFD tools instead. • It is important to remember these assumptions related to performing thermal analyses in Simulation.
  • 5. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-5 Physics Filters • Before proceeding to a detailed discussion on performing thermal analyses in Simulation, it is useful to point out that if a thermal-only solution is to be performed, the Physics Filter can be useful to filter the GUI. – Under “View menu > Physics Filter,” unselect the “Structural” option. Now, the available options in the Simulation GUI will only reflect thermal analyses. – This applies to options in the “Environment” and “Solution” levels only. – If a thermal-stress simulation is to be performed, do not turn off any physics filters since both structural and thermal options may be required. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 6. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-6 A. Geometry • In thermal analyses, all types of bodies supported by Simulation may be used. – Solid, surface, and line bodies are supported by all products which support thermal analyses. • For surface bodies, thickness must be input in the Details view of the Geometry branch • The cross-section and orientation of line bodies is defined within DesignModeler and is imported into Simulation automatically. Although the cross-section and orientation is defined, this information is meant for structural analyses, and the actual thermal link element will have an ‘effective’ cross-section based on the input properties. • No heat flux or vector heat flux output is available with line bodies. Only temperature results are available for line bodies. – The “Point Mass” feature is not applicable in thermal analyses • Point Mass is described in Chapter 4, Linear Structural Analysis. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 7. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-7 … Geometry • It is important to understand assumptions related to using shell and line bodies: – For shell bodies, through-thickness temperature gradients are not considered. A shell body should be used for thin structures when it can be safe to assume temperatures on top and bottom of surface are the same. • Temperature variation will still be considered across the surface, just not through the thickness, which is not explicitly modeled. – For line bodies, thickness variation in the cross-section is not considered. A line body should be used for beam- or truss- like structures, where the temperature can be assumed to be constant across the cross-section. • Temperature variation will still be considered along the line body, just not through the cross-section, which is not explicitly modeled. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 8. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-8 … Material Properties • The only required material property is thermal conductivity. – Material input is under the “Engineering Data” tab, and material assignment is per part under the “Geometry” branch – Thermal Conductivity is input under the Engineering Data tab. Temperature-dependent thermal conductivity can be input as a table. – Other material input is not used in thermal. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x If any temperature-dependent material properties exist, this will result in a nonlinear solution. This is because the temperatures are solved for, but the materials are dependent on the temperatures, so it is not linear.
  • 9. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-9 B. Assemblies – Solid Body Contact • When importing assemblies of solid parts, contact regions are automatically created between the solid bodies. – Surface-to-surface contact allows non-matching meshes at boundaries between solid parts – Contact enables heat transfer between parts in an assembly Model shown is from a sample Inventor assembly. ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 10. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-10 … Assemblies – Contact Region • In Simulation, the concept of contact and target surfaces are used for each contact region. – One side of the contact region is comprised of “contact” face(s), the other side of the region is made of “target” face(s). – Heat flow is allowed between contact and target faces (based on the contact normal direction) • When one side is the contact and the other side is the target, this is called asymmetric contact. On the other hand, if both sides are made to be contact & target, this is called symmetric contact. However, the designation of which side is contact or target is unimportant in thermal analysis. • By default, Simulation uses symmetric contact for solid assemblies. • For ANSYS Professional licenses and above, the user may change to asymmetric contact, as desired. ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 11. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-11 … Assemblies – Contact Region • As noted in the previous slide, heat flows within a contact region in the contact normal direction – No heat spreading is considered in the contact/target interface • Heat spreading is considered within shell or solid elements at the contact or target surfaces because of Fourier’s Law • Heat flow within the contact region is in the contact normal direction only • This means that, regardless of the definition of the contact region, heat flows only if a target element is present in the normal direction In the figure on the left, the solid green double-arrows indicate heat flow within the contact region. Heat flow only occurs if a target surface is normal to a contact surface. The light, dotted green arrows indicate that no heat transfer will occur between parts. ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 12. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-12 … Assemblies – Contact Region • In Simulation, various contact behaviors exist – The contact “Type” is meant for structural applications – If the parts are initially in contact, heat transfer will occur between the parts. If the parts are initially out of contact, the parts will not transfer heat between each other. – Based on the contact type, whether heat will be transferred between contact and target surfaces is outlined below: – The pinball region is automatically defined and set to a relatively small value to accommodate small gaps which may present in the model. The pinball region will be discussed next. Initially Touching Inside Pinball Region Outside Pinball Region Bonded Yes Yes No No Separation Yes Yes No Rough Yes No No Frictionless Yes No No Contact Type Heat Transfer Between Parts in Contact Region? ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 13. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-13 … Assemblies – Contact Region • The pinball region may be input and visualized in ANSYS Professional licenses and above. – If the target nodes lie within the pinball region and the contact is bonded or no separation, then heat transfer will occur (solid green lines) – Otherwise, no heat transfer will occur between nodes (dotted green lines) In this figure on the right, the gap between the two parts is bigger than the pinball region, so no heat transfer will occur between the parts Pinball Radius ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x
  • 14. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-14 … Assemblies – Thermal Conductance • By default, a high thermal contact conductance (TCC) is defined between parts of an assembly – The amount of heat flow between two parts is defined by the contact heat flux q: where Tcontact is the temperature of a contact “node” and Ttarget is the temperature of the corresponding target “node” located in the contact normal direction. – By default, TCC is set to a relatively ‘high’ value, based on the largest material conductivity defined in the model KXX and the diagonal of the overall geometry bounding box ASMDIAG. This essentially provides ‘perfect’ conductance between parts. ( )contacttarget TTTCCq −⋅= ASMDIAGKXXTCC /000,10⋅= ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 15. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-15 … Assemblies – Thermal Conductance • Perfect thermal contact conductance between parts means that no temperature drop is assumed at the interface. • One may want to include finite thermal conductance instead – Two surfaces (at different temperatures) in contact experience a temperature drop across the interface. The drop is due to imperfect contact between the two surfaces. The imperfect contact, and hence the finite contact conductance, can be influenced by many factors such as: • surface flatness • surface finish • oxides • entrapped fluids • contact pressure • surface temperature • use of conductive grease ∆T T x
  • 16. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-16 … Assemblies – Thermal Conductance • In ANSYS Professional licenses and above, the user may define a finite thermal contact conductance (TCC) if the Pure Penalty or Augmented Lagrange Formulation is used. – The thermal contact conductance per unit area is input for each contact region in the Details view, as shown below. – If thermal contact resistance is known, invert this value and divide by the contacting area to obtain TCC value. – When this is done, there will now be a temperature drop between the contact and target surfaces for a contact region. If “Thermal Conductance” is left at “Program Chosen,” near- perfect thermal contact conductance will be defined. The user can change this to “Manual” to input finite thermal contact conductance instead, which is the same as including thermal contact resistance at a contact interface. ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x
  • 17. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-17 … Assemblies – Thermal Conductance • If using symmetric contact, the user does not need to account for a ‘double’ thermal contact resistance. – Input values as normal • MPC bonded contact allows for perfect thermal contact conductance. – In this case, no thermal contact conductance is used nor defined because ‘contact’ is related via constraint equations. – The contact “node” and corresponding target “node” will have the same temperature because of perfect contact conductance. ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x Do not use “Normal Lagrange” formulation for thermal analyses. If selected, the ANSYS solver will actually use “Augmented Lagrange” with a ‘perfect’ thermal contact conductance.
  • 18. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-18 … Assemblies – Surface Body Contact • For ANSYS Professional licenses and above, mixed assemblies of shells and solids are supported – Allows for more complex modeling of assemblies, taking advantage of the benefits of shells, when applicable ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x
  • 19. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-19 … Assemblies – Surface Body Contact • Edge contact is a subset of general contact – For contact including shell faces or solid edges, only bonded or no separation behavior is allowed. – For contact involving shell edges, only bonded behavior using MPC formulation is allowed. • For MPC-based bonded contact, user can set the search direction (the way in which the multi-point constraints are written) as either the target normal or pinball region. • If a gap exists (as is often the case with shell assemblies), the pinball region can be used for the search direction to detect contact beyond a gap. • MPC results in perfect contact conductance ANSYS License Availability DesignSpace Entra DesignSpace Professional x Structural Mechanical/Multiphysics x
  • 20. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-20 … Assemblies – Spot Weld • Spot welds provide a means of connecting shell assemblies at discrete points for heat transfer – Spotweld definition is done in the CAD software. Currently, only DesignModeler and Unigraphics define spotwelds in a manner that Simulation supports. – Spotwelds can also be created in Simulation manually, but only at discrete vertices. ANSYS License Availability DesignSpace Entra DesignSpace x Professional x Structural Mechanical/Multiphysics x DesignModeler x Pro/ENGINEER Unigraphics x SolidWorks Inventor Solid Edge Mechanical Desktop CATIA V4 CATIA V5 ACIS (SAT) Parasolid IGES
  • 21. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-21 C. Loads • There are three types of loads in thermal analyses: – Heat Loads: • These loads pump heat into the system. • Heat loads can be input as a known heat flow rate or heat flow rate per unit area or unit volume. – Adiabatic Condition: • This is the naturally-occurring boundary condition, where there is not heat flow through the surface. – Thermal Boundary Conditions: • These boundary conditions act as heat sources or heat sinks with a known temperature condition. • These can be either a prescribed temperature or a convection boundary condition with a known bulk temperature. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 22. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-22 … Heat Loads • Heat Flow: – A heat flow rate can be applied to a vertex, edge, or surface. The load gets distributed for multiple selections. – Heat flow has units of energy/time (i.e., power). • Heat Flux: – A heat flux can be applied to surfaces only. – Heat flux has units of energy/time/area (i.e., power/area) • Internal Heat Generation: – An internal heat generation rate can be applied to bodies only. – Heat generation has units of energy/time/volume A positive value for heat load will add energy to the system. Also, if multiple loads are present, the effect is cumulative. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 23. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-23 … Adiabatic Conditions • Perfectly Insulated: – Perfectly insulated condition is applied to surfaces – Can be thought of as a zero heat flow rate loading – This is actually the naturally-occurring condition in thermal analyses, when no load is applied. • Usually, one does not need to apply a perfectly insulated condition on surfaces since that is the natural behavior for a regular surface. • Hence, this loading is meant to be used as a way to remove loading on specified surfaces. For example, it may be easier for a user to apply heat flux or convection on all surfaces, then use the perfectly insulated condition to selectively ‘remove’ the loading on some surfaces (such as those in contact with other parts). ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 24. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-24 … Thermal Boundary Conditions Thermal boundary conditions present a known local or ‘remote’ temperature condition. • At least one type of thermal boundary condition must be present. Otherwise, the steady-state temperature will be infinite if only heat is pumped into a system! • Also, Given Temperature or Convection load should not be applied on surfaces that already have another heat load or thermal boundary condition applied to it. – If applied on an entity which also has a heat load, the temperature boundary condition will override. – Perfect insulation will override thermal boundary conditions. • Given Temperature: – This imposes a temperature on vertices, edges, or surfaces. – Temperature is the degree of freedom solved for, but this fixes the temperature on selected entities to a given value. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 25. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-25 … Thermal Boundary Conditions • Convection: – Applied to surfaces only. – Convection relates a ‘ambient temperature’ with the surface temperature: where the convective heat flux q is related to a film coefficient h, the surface area A, and the difference in the surface temperature Tsurface & ambient temperature Tbulk. – Meant to provide a simplified way of accounting for heat transport from a fluid. “h” and “Tbulk” are user-input values. – The film coefficient h can be constant or input from a file (next) ( )ambientsurface TThAq −= ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 26. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-26 … Thermal Boundary Conditions • Temperature-Dependent Convection (continued): – If film coefficient h is input from a file, this can be a constant or temperature-dependent value h(T). • Define a convection boundary condition under the Environment branch and define the Type to be “Temperature-Dependent”. Next, select “New Convection…” for the Correlation. The “Engineering Data” tab will open and the Coefficient Type can then be defined for the new convection load. • Determine what temperature is used for h(T) first, for temperature- dependent film coefficients. Temperature can be: – Average film temperature T=(Tsurface+Tbulk)/2 – Surface temperature T= Tsurface – Bulk temperature T= Tbulk – Difference of surface and bulk temperatures T=(Tsurface-Tbulk) ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x Select the temperature- dependency from the pull-down menu
  • 27. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-27 … Thermal Boundary Conditions • Temperature-Dependent Convection (continued): • After the type of temperature-dependency is selected, the user may input the film coefficients and temperatures in a table. The values are plotted on a graph, as shown below. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x If any temperature-dependent convection load is applied, this will result in a nonlinear solution since the surface temperature is solved for, but the film coefficient h is based on a function of the surface temperature. The only exception is if the film coefficient h is based on a function of the bulk temperature only. In Simulation, the bulk temperature is constant and input by the user, so this load will not be nonlinear. Right mouse click on the table to add or delete values.
  • 28. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-28 … Thermal Boundary Conditions • Temperature-Dependent Convection (continued): • The convection data can also be imported from a file. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 29. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-29 … Thermal Loads Summary • For some structural users, it may be useful to provide an analogy of structural and thermal analyses: – There are some types of loads that do not have any analogy • There is no thermal equivalent for inertial loads such as rotational velocity or acceleration • The analogy of convective boundary condition is a ‘foundation stiffness’ support in structural terms, similar to a grounded spring Structural Thermal Natural Condition No external force Perfectly Insulated (No heat flow rate) Direct Given Displacement Given Temperature Indirect Convection Direct Force Heat Flow Per Area Pressure Heat Flux Per Volume Thermal Expansion Internal Heat Generation Inertial Loads Acceleration Boundary Conditions Load
  • 30. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-30 D. Solution Options • Solution options can be set under the “Solutions” branch: – The ANSYS database can be saved if “Save ANSYS db” is set • Useful if you want to open a database in ANSYS – Two solvers are available in Simulation • The default solver is automatically chosen and does not usually need to be changed. • The “Iterative” solver can be efficient for solving large models whereas the “Direct” solver is a robust solver and handles any situation. • The ability to change the default solver is under “Tools > Options… > Simulation: Solution > Solver Type” – The “Weak Springs” and “Large Deflection” options are meant for structural analyses only, so they can be ignored for a thermal analysis. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 31. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-31 … Solution Options – Informative settings show the user the status of the analysis: • For a regular thermal analysis, the “Analysis Type” will be set to “Static Thermal.” If structural supports and results are present, then the analysis type will be “Thermal Stress.” • A nonlinear solution will be required if temperature-dependent (a) material properties or (b) convection film coefficients are present. This means that several internal iterations will be run to achieve heat equilibrium. • The solver working directory is where scratch files are saved during the solution of the equations. By default, the TEMP directory of your Windows system environment variable is used, although this can be changed in “Tools > Options… > Simulation: Solution > Solver Working Directory”. – Any solver messages which appear after solution can be checked afterwards under “Solver Messages”ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 32. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-32 … Solving the Model • To solve the model, request results first (covered next) and click on the “Solve” button on the Standard Toolbar – By default, two processors (if present) will be used for parallel processing. To change this, use “Tools > Options… > Simulation: Solution > Number of Processors to Use” – Recall that if a “Solution Information” branch is requested, the details of the solution output can be examined. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 33. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-33 … Solving the Model • To perform a thermal-stress solution, simply add structural support(s) and request structural results, then solve the model. – Structural loads are optional but can also be added. – Simulation will know that a thermal-stress analysis is to be performed (under Details view of the Solution branch). The following will be performed automatically: • A steady-state thermal analysis will be performed • The temperature field will be mapped back onto the structural model • A structural analysis will be performed – See Chapter 4 for details on Structural Analyses – Simulation automates this type of coupled-field solution, so the user does not have to worry about the above details. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 34. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-34 E. Results and Postprocessing • Various results are available for postprocessing: – Temperature – Heat Flux – “Reaction” Heat Flow Rate • In Simulation, results are usually requested before solving, but they can be requested afterwards, too. – If you solve a model then request results afterwards, click on the “Solve” button , and the results will be retrieved. A new solution is not required for retrieving output of a solved model.
  • 35. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-35 … Temperature • Temperature contour plots can be requested: – Temperature is the degree of freedom solved for, and it is the most basic output request. – Temperature is a scalar quantity and, therefore, has no direction associated with it. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 36. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-36 … Heat Flux • Heat flux contour or vector plots are available: – Heat flux q is defined as and is related to the thermal gradient ∇T. The heat flux output has three components and can aid the user in seeing how the heat is flowing. – The magnitude plotted as contours: “Total Heat Flux” – The magnitude & direction as vectors: “Vector Heat Flux” • Recall that wireframe is best for viewing vectors – Components of heat flux can be requested with “Directional Heat Flux” and can be mapped on any coordinate system. TKXXq ∇⋅−= ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 37. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-37 … Reaction Heat Flow Rate • Reaction heat flow rates is available for any Given Temperature or Convection boundary condition – Recall that both given temperature and convection supply a known temperature, either directly or indirectly. Hence, this acts as a heat source/sink, and the amount of heat flowing in (positive) or out (negative) of the support can be output. – For each individual Given Temperature or Convection load, the Reaction heat flow rate is printed in the Details view after a solution. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 38. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-38 … Reaction Heat Flow Rate • The “Worksheet” tab for “Environment” branch has a tabular summary of reaction heat flow rates. – If a thermal support shares a vertex, edge, or surface with another thermal support or load, the reported reaction heat flow rate may be incorrect. This is due to the fact that the underlying mesh will have multiple supports applied to the same nodes. The solution will still be valid, but the reported values may not be accurate because of this. ANSYS License Availability DesignSpace Entra x DesignSpace x Professional x Structural Mechanical/Multiphysics x
  • 39. ANSYSWorkbench–SimulationANSYSWorkbench–Simulation Training Manual Steady-State Thermal Analysis March 29, 2005 Inventory #002215 6-39 F. Workshop 6 • Workshop 6 – Thermal Analysis • Goal: – Analyze the pump housing shown below for its heat transfer characteristics.

Editor's Notes

  • #7: LINK33 support in DS later
  • #8: LINK33 support in DS later
  • #21: LINK33 support in DS later