Chapter Six Thermal Analysis.

Chapter Six Thermal Analysis

Chapter Overview In this chapter, performing steady-state thermal analyses in Design 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) February 2, 2004 Inventory #002010 6-2

Basics of Steady-State Heat Transfer
A steady-state thermal analysis is performed to determine the thermal response under applied steady-state loads Temperatures and heat flow rate are usually the items of interest, although heat fluxes can be reported as well. The general thermal equation is as follows: where t is time and {T} is temperature, [C] is the specific heat (thermal capacitance) matrix, [K] is the conductivity matrix, and {Q} is the heat flow rate load vector. In a steady-state analysis, all time-dependent terms are removed. However, nonlinearities are still present: February 2, 2004 Inventory #002010 6-3

For a steady-state thermal analysis in Design 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 February 2, 2004 Inventory #002010 6-4

Fourier’s Law provides the basis of the previous equation: This means that the thermal analysis Design 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 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 Design Simulation. February 2, 2004 Inventory #002010 6-5

A. Geometry In thermal analyses, most types of bodies supported by Design Simulation may be used. Solid and surface 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 Line bodies are only supported under ANSYS Professional licenses and above. The cross-section and orientation of line bodies is defined within DesignModeler and is imported into Design 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. LINK33 support in DS later February 2, 2004 Inventory #002010 6-6

… 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. LINK33 support in DS later February 2, 2004 Inventory #002010 6-7

… Elements Used In Design Simulation, the following elements are used:
Solid bodies are meshed with 10-node tetrahedral or 20-node hexahedral elements SOLID87 and SOLID90 Surface bodies are meshed with 4-node quad shell elements SHELL57 using real constants (SHELL131 or SHELL132 are currently not used.) Line bodies are meshed with 2-node line elements LINK33 using real constants An equivalent cross-sectional area, as defined in DesignModeler, is used for LINK33 For thermal-stress analyses, a coupled-field element is not used. The thermal-stress analysis is performed sequentially, so the above thermal elements are used, then the temperature field is read into corresponding structural elements. February 2, 2004 Inventory #002010 6-8

… Material Properties The only required material property is thermal conductivity. Material input is under the “Engineering Data” branch, and material assignment is per part under the “Geometry” branch Thermal Conductivity is input as a sub-branch of the material property. Temperature-dependent thermal conductivity can be input as a table. Specific heat can be input as well, but it is currently not used. Other material input is not used in thermal. 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. February 2, 2004 Inventory #002010 6-9

… Material Properties Thermal conductivity is input into ANSYS as MP commands. For temperature-dependent thermal conductivity, the appropriate MPTEMP and MPDATA commands are issued Although specific heat may be defined in the “Engineering Data” branch, it is currently unused and not passed to ANSYS No MP,C command is written for specific heat February 2, 2004 Inventory #002010 6-10

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 February 2, 2004 Inventory #002010 6-11 Model shown is from a sample Inventor assembly.

… Assemblies – Contact Region
In Design 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, Design Simulation uses symmetric contact for solid assemblies. For ANSYS Professional licenses and above, the user may change to asymmetric contact, as desired. February 2, 2004 Inventory #002010 6-12

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. February 2, 2004 Inventory #002010 6-13

In Design Simulation, various contact behaviors exist In general, 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. February 2, 2004 Inventory #002010 6-14

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 February 2, 2004 Inventory #002010 6-15

… 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. February 2, 2004 Inventory #002010 6-16

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 DT T x February 2, 2004 Inventory #002010 6-17

In ANSYS Professional licenses and above, the user may define a finite thermal contact conductance (TCC) 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. February 2, 2004 Inventory #002010 6-18

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, because constraint equations are used, no thermal contact conductance is used nor defined. The contact “node” and corresponding target “node” will have the same temperature because of perfect contact conductance. February 2, 2004 Inventory #002010 6-19

… Assemblies – Solid Body Contact
Internally, thermal contact for solid faces is defined with CONTA174 and TARGE170 elements. KEYOPT(1)=2 set for thermal DOF only KEYOPT(12) is based on contact type used For example, bonded type is KEYOPT(12)=5. KEYOPT(2), KEYOPT(5), KEYOPT(9), and FKN are also set. These contact settings are most critical for structural contact, so the various default settings are outlined in Chapter 4. Default thermal contact conductance (TCC) is based on highest value of thermal conductivity of materials and overall geometry size TCC=KXX*10,000/ASMDIAG KXX is of highest thermal conductivity value of used materials ASMDIAG is diagonal of overall ‘bounding box’ of assembly February 2, 2004 Inventory #002010 6-20

… Assemblies – Surface Body Contact
For ANSYS Professional1 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 February 2, 2004 Inventory #002010 6-21 1 For ANSYS Professional, surface contact supported with ANSYS 8.0 Service Pack 1 and above

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 February 2, 2004 Inventory #002010 6-22

Internally, any contact including an edge (solid body edge or surface edge) results in asymmetric contact with CONTA175 for the edge and TARGE170 for the edge/face Undocumented KEYOPT(1)=2 is set for thermal contact Contact involving solid edges default to pure penalty method Contact involving surface edges use MPC formulation. Instead of “target normal,” if search direction is “pinball region,” KEYOPT(5)=4 set on companion TARGE170 element. For bonded contact (default), both use KEYOPT(12)=5 and KEYOPT(9)=1. For surface faces in contact with other faces, standard surface-to- surface contact is used, namely CONTA174 and TARGE170 CONTA175 elements TARGE170 elements February 2, 2004 Inventory #002010 6-23

… Assemblies – Spot Weld
Spot welds provide a means of connecting shell assemblies at discrete points for heat transfer Although the ANSYS DesignSpace licenses support structural spot welds, these do not support thermal spot welds. Spotweld definition is done in the CAD software. Currently, only DesignModeler and Unigraphics define spotwelds in a manner that Design Simulation supports. Spotwelds can also be created in Design Simulation manually, but only at discrete vertices. LINK33 support in DS later February 2, 2004 Inventory #002010 6-24

… Assemblies – Spot Weld
Internally, spot welds are defined as a set of LINK33 elements. The spot weld is defined with one link element, and the top and bottom of the spot weld is connected to the shell or solid elements with a ‘spider web’ of multiple links. The LINK33 elements use same thermal conductivity as underlying materials but with a circular cross-section with radius=5*thickness of underlying shells Figure on right shows two spot welds between two sets of shell elements, which are made translucent for clarity. February 2, 2004 Inventory #002010 6-25

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. February 2, 2004 Inventory #002010 6-26

… Heat Loads Heat Flow: Heat Flux: Internal Heat Generation:
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. February 2, 2004 Inventory #002010 6-27

… 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). February 2, 2004 Inventory #002010 6-28

… 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. February 2, 2004 Inventory #002010 6-29

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) February 2, 2004 Inventory #002010 6-30

Temperature-Dependent Convection (continued): If film coefficent h is input from a file, this can be a constant or temperature-dependent value h(T). Select the Engineering branch and use the “Convection” toolbar to add or create a new convection file. 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) Select the temperature-dependency from the pull-down menu February 2, 2004 Inventory #002010 6-31

Temperature-Dependent Convection (continued): After the type of temperature-dependency is selected, the user may select the “Film Coefficient vs. Temperature” branch on the Outline Tree to input the film coefficients and temperatures in a table. The values are plotted on a graph, as shown below. 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 Design Simulation, the bulk temperature is constant and input by the user, so this load will not be nonlinear. February 2, 2004 Inventory #002010 6-32

… Thermal Loads in ANSYS
The internal representation of loads in ANSYS: Heat flow for an edge or vertex is a heat flow rate (F,,HEAT) Heat flux or heat flow for a surface is surface load (SF,,HFLUX) Internal heat generation is applied as a body load (BFE,,HGEN) Given temperature is applied as a constraint (D,,TEMP) Perfectly insulated condition internally removes any loads applied in Design Simulation on those surface(s). Convection is defined by surface effect SURF152 elements Bulk temperature and film coefficient is applied on the surface effect elements (SF,,CONV,film,bulk) If temperature-dependent film coefficients exist, these are defined with a temperature-dependent HF material property (MPDATA,HF). The film coefficient value applied will be “–HF_number,” and ANSYS knows to use the referenced HF material property number. KEYOPT(8) is set to be consistent with temperature evaluation of h(T), such as evaluate h(T) based on surface temperature. February 2, 2004 Inventory #002010 6-33

… 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 February 2, 2004 Inventory #002010 6-34

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 Design Simulation The default solver is automatically chosen. In thermal analyses, the user usually does not need to change the solver type. 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 > Control Panel > 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. February 2, 2004 Inventory #002010 6-35

… 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 > Control Panel > Solution > Solver Working Directory”. Any solver messages which appear after solution can be checked afterwards under “Solver Messages” February 2, 2004 Inventory #002010 6-36

… 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 set the number of processors, use “Tools > Control Panel > Solution > Number of Processors to Use” Recall that under “Worksheet” tab of the “Solution” branch, the details of the solution output can be examined. February 2, 2004 Inventory #002010 6-37

… 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. Design 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 Design Simulation automates this type of coupled-field solution, so the user does not have to worry about the above details. February 2, 2004 Inventory #002010 6-38

… Solution Options in ANSYS
The solver selection for direct vs. iterative: The solvers used are either the direct sparse solver (EQSLV,SPARSE) or the PCG solver (EQSLV,PCG) The JCG solver is not used in thermal analyses A simplified discussion between the two solvers: If given the linear static case of [K]{x} = {F}, Direct solvers factorize [K] to solve for [K]-1. Then, {x} = [K]-1{F}. This factorization is computationally expensive but is done once. Iterative solvers use a preconditioner [Q] to solve the equation [Q][K]{x} = [Q]{F}. Assume that [Q] = [K]-1. In this trivial case, [I]{x} = [K]-1{F}. However, the preconditioner is not usually [K]-1. The closer [Q] is to [K]-1, the better the preconditioning is, and this process is repeated - hence the name, iterative solver. For iterative solvers, matrix multiplication (not factorization) is performed. This is much faster than matrix inversion if done entirely in RAM, so, as long as the number of iterations is not very high (which happens for well-conditioned matrices), iterative solvers can be more efficient than sparse solvers. The main difference between the iterative solvers in ANSYS — PCG, JCG, ICCG — is the type of pre-conditioner used. February 2, 2004 Inventory #002010 6-39

Solver working directory: The ANSYS input file is written as “ds.dat” in the solver directory. The output file is “solve.out” and can be viewed in the “Worksheet” tab of the “Solution” branch. ANSYS is executed in batch mode (-b) as a separate process. During solution, the results file .rst is written. The results are also read in and XML results files are generated in batch mode. The XML files are then read into Design Simulation. All associated ANSYS files have default jobname of “file” and are deleted after solution, unless changed in “Tools > Control Panel > Solution > Save Ansys Files”. February 2, 2004 Inventory #002010 6-40

Some solution options are also defined: Solution control is used This is different from structural analyses in Design Simulation where Solution Control is turned off ANSYS shape checking is turned off (SHPP,OFF) If nonlinear, the number of substeps (NSUBST,1,10,1) and number of equilibrium iterations (NEQIT,20) are defined CNVTOL also set, where minimum reference heat flow rate is defined as 1e-6 W Only Design Simulation-supported results is output with OUTRES, not everything by default Results are later written to XML files in /POST1, which are then read back into Design Simulation. Hence, Design Simulation does not directly read the results from the .rth file February 2, 2004 Inventory #002010 6-41

E. Results and Postprocessing
Various results are available for postprocessing: Temperature Heat Flux “Reaction” Heat Flow Rate In Design 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. February 2, 2004 Inventory #002010 6-42

… 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. February 2, 2004 Inventory #002010 6-43

… 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. February 2, 2004 Inventory #002010 6-44

… 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. February 2, 2004 Inventory #002010 6-45

… 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. February 2, 2004 Inventory #002010 6-46

F. Workshop 6 Workshop 6 – Thermal Analysis Goal:
Analyze the pump housing shown below for its heat transfer characteristics. February 2, 2004 Inventory #002010 6-47

Chapter Six Thermal Analysis.

Similar presentations

Presentation on theme: "Chapter Six Thermal Analysis."— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

Chapter Six Thermal Analysis.

Similar presentations

Presentation on theme: "Chapter Six Thermal Analysis."— Presentation transcript:

Similar presentations

About project

Feedback