Patran 2008 R1 Interface To Md Nastran Preference Guide Volume 2: Thermal Analysis

Patran 2008 r1 Interface To MD Nastran Preference Guide Volume 2: Thermal Analysis

Main Index

Corporate

Europe

Asia Pacific

MSC.Software Corporation 2 MacArthur Place Santa Ana, CA 92707 USA Telephone: (800) 345-2078 Fax: (714) 784-4056

MSC.Software GmbH Am Moosfeld 13 81829 Munich, Germany Telephone: (49) (89) 43 19 87 0 Fax: (49) (89) 43 61 71 6

MSC.Software Japan Ltd. Shinjuku First West 8F 23-7 Nishi Shinjuku 1-Chome, Shinjuku-Ku Tokyo 160-0023, JAPAN Telephone: (81) (3)-6911-1200 Fax: (81) (3)-6911-1201

Worldwide Web www.mscsoftware.com

Disclaimer This documentation, as well as the software described in it, is furnished under license and may be used only in accordance with the terms of such license. MSC.Software Corporation reserves the right to make changes in specifications and other information contained in this document without prior notice. The concepts, methods, and examples presented in this text are for illustrative and educational purposes only, and are not intended to be exhaustive or to apply to any particular engineering problem or design. MSC.Software Corporation assumes no liability or responsibility to any person or company for direct or indirect damages resulting from the use of any information contained herein. User Documentation: Copyright 2008 MSC.Software Corporation. Printed in U.S.A. All Rights Reserved. This notice shall be marked on any reproduction of this documentation, in whole or in part. Any reproduction or distribution of this document, in whole or in part, without the prior written consent of MSC.Software Corporation is prohibited. The software described herein may contain certain third-party software that is protected by copyright and licensed from MSC.Software suppliers. Contains IBM XL Fortran for AIX V8.1, Runtime Modules, (c) Copyright IBM Corporation 1990-2002, All Rights Reserved. MSC, MSC/, MSC Nastran, MD Nastran, MSC Fatigue, Marc, Patran, Dytran, and Laminate Modeler are trademarks or registered trademarks of MSC.Software Corporation in the United States and/or other countries. NASTRAN is a registered trademark of NASA. PAM-CRASH is a trademark or registered trademark of ESI Group. SAMCEF is a trademark or registered trademark of Samtech SA. LS-DYNA is a trademark or registered trademark of Livermore Software Technology Corporation. ANSYS is a registered trademark of SAS IP, Inc., a wholly owned subsidiary of ANSYS Inc. ACIS is a registered trademark of Spatial Technology, Inc. ABAQUS, and CATIA are registered trademark of Dassault Systemes, SA. EUCLID is a registered trademark of Matra Datavision Corporation. FLEXlm is a registered trademark of Macrovision Corporation. HPGL is a trademark of Hewlett Packard. PostScript is a registered trademark of Adobe Systems, Inc. PTC, CADDS and Pro/ENGINEER are trademarks or registered trademarks of Parametric Technology Corporation or its subsidiaries in the United States and/or other countries. Unigraphics, Parasolid and I-DEAS are registered trademarks of UGS Corp. a Siemens Group Company. All other brand names, product names or trademarks belong to their respective owners.

P3*2008R1*Z*NATHM*Z* DC-USR

Main Index

Contents Patran Interface to MD Nastran Thermal Patran Interface to Nastran Thermal,

1

Overview Introduction

2

Using this Guide

3

Thermal Material Properties 5 Conductivity 5 Specific Heat and Heat Capacitance 5 Density 5 Thermal Loads and Boundary Conditions Temperature Boundary Conditions 7 Normal Heat Flux 7 Directional Heat Flux 8 Nodal Source 8 Volumetric Heat Generation 8 Basic Convection 8 Advection, Forced Convection 8 Radiation to Space 9 Radiation Enclosures 10 Contact Conduction 10

7

Thermal Analysis 11 Steady-State Analysis 11 Initial Conditions in Steady-State Analysis 12 Transient Analysis 13 Initial Conditions in Transient Analysis 13 Steady-State and Transient Convergence Criteria References

2

Getting Started - A Guided Exercise Introduction Objectives Start Patran

Main Index

15

18 19 21

14

ii Patran Interface to MD Nastran Thermal

Create a Database

22

Create a Rectangular Geometric Surface Mesh the Surface with Elements

25

26

Modify the Mesh (Reduce the Number of Elements) Specify Material Properties

29

Assign Element Properties

30

Define the Temperature at the Plate’s Bottom Edge Apply Heat Flux to the Plate’s Right Edge

34

Apply Convection to the Plate’s Left Edge

37

Perform a Steady-State Thermal Analysis

40

Visualize the Thermal Results (Contour Plot)

3

41

Building A Model Introduction

46

Finite Elements 47 Nodes 47 Finite Elements 49 Multi-Point Constraints Coordinate Frames

50 51

Material Library 52 Materials Form 53 Constitutive Models 55 Solid Properties 56 Fluid Properties 56 Phase Changes 56 Heat Generation1 56 Finite Element Properties 57 Element Properties Form 58 Conductors and Grounded Conductors 60 Capacitors and Grounded Capacitors 60 Beam and Rod Elements with General Section 60 Curved General Section Beam 61 Curved Pipe Section Beam 62

Main Index

27

32

CONTENTS iii

Tapered Section Beam 62 Pipe Section Rod 63 Flow Tube 63 2D Shell Elements 64 2D Axisymmetric Solid Elements 65 3D Solid Elements 65 Loads and Boundary Conditions 66 Loads and Boundary Conditions Form 66 Input Data Forms--Basic and Advanced Options 69 Two Application Regions 70 Surface Area 71 Spatial Dependence 71 Temperature Dependence 71 Time Dependence 71 Temp(Thermal) 73 Initial Temperature 75 Applied Heat--Normal Fluxes 76 Applied Heat--Directional Fluxes 77 Transient Analysis 78 Incident Thermal Vector 78 Applied Heat--Nodal Source 79 Applied Heat--Volumetric Generation 80 Applied Heat--Total Heat 80 Convection--To Ambient 81 Convection--Flow Tube To Ambient 82 Convection--Coupled 85 Convection--Coupled Flow Tube 87 Convection--Coupled Advection 90 Convection--Duct Flow 93 Radiation--Ambient Space 96 Radiation--Ambient Nodes 97 Radiation--Enclosures 98 Load Cases

4

101

Running a Thermal Analysis Introduction

104

Review of the Analysis Form Analysis Form 106 Translation Parameters

Main Index

109

105

iv Patran Interface to MD Nastran Thermal

Numbering Options

111

Solution Types 113 Solution Parameters 114 Radiation Parameters 115 View Factor Parameters 115 Solution Parameters for Transient Analysis 117 Direct Text Input

119

Subcases 121 Subcase Parameters 123 Steady-State Subcase 123 Thermal Contact Table 126 Transient Subcase Parameters 128 Structural Heat Subcase Parameters 130 Output Requests 130 Direct Text Input 133 Subcase Select

5

135

Results Processing and Visualization Overview

138

Reading Thermal Analysis Results 139 Read Output2 Form 141 Results File Formats 143 Supported OUTPUT2 Results 143 Attach XDB Form 146 Results File Formats 147 Supported MSC.Access Results 147 Results Visualization Options Contour Plots 151 Vector Output Definitions 152 XY Plots 153

6

Read Input File Review of Read Input File Form Read Input File Form 163 Entity Selection Form 164 Define Offsets Form 166 Selection of Input File 167

Main Index

150

162

CONTENTS v

Summary Data Form 168 Reject Card Form 169 Data Translated from the NASTRAN Input File Conflict Resolution

7

170

171

Example Problems Overview

174

Example 1 - Transient Thermal Analysis 175 Objectives 175 Define Time Dependent Functions 177 Create a Transient Load Case 181 Apply Time Varying Heat Flux to the Plate’s Right Edge 182 Apply Transient Volumetric Heat Generation Inside the Plate 185 Select Solution Type 189 Specify the Default Initial Temperature 190 Define Time Steps 190 Select a Transient Load Case 192 Perform a Transient Thermal Analysis 192 Visualize the Transient Results (Contour Plot) 194 Visualize the Transient Results (XY Plot) 195 Modify the XY Plot 197 Example 2 - Free Convection on Printed Circuit Board 200 Problem Description 200 Modeling 201 Create the Surfaces of Printed Circuit Board and Electronic Components 203 Extrude the Surfaces to Create Solids 204 Mesh the Solids 205 Specify Materials 206 Define Element Properties 208 Discussion of Results 213 Example 3 - Forced Air Convection on Printed Circuit Board Problem Description 214 Modeling 214 Discussion of Results 230 Example 4 - Thermal Contact Resistance Problem Description 231 Modeling 232

Main Index

231

214

vi Patran Interface to MD Nastran Thermal

Discussion of Results 240 Example 5 - Typical Avionics Flow Problem Description 241 Modeling 242 Discussion of Results 260

241

Example 6 - Radiation Enclosures Problem Description 261 Modeling 261 Discussion of Results 271

261

Example 7 - Axisymmetric Flow in a Pipe Problem Description 273 Modeling 274 Discussion of Results 289 Example 8 - Directional Heat Loads Problem Description 290 Modeling 291 Discussion of Results 300

273

290

Example 9 - Thermal Stress Analysis from Directional Heat Loads Problem Description 302 Modeling 303 Discussion of Results 309 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate Problem Description 310 Modeling 310 Discussion of Results 328

A

Files Files

B

332

Error Messages Error Messages

C

334

Supported Commands File Management Statements

Main Index

336

310

302

CONTENTS vii

Executive Control Statements Case Control Commands Bulk Data Entries

337

338

339

Patran Interface to MD Nastran Thermal

Main Index

343

viii Patran Interface to MD Nastran Thermal

Main Index

Chapter 1: Overview Patran Interface to MD Nastran Thermal

1

Main Index

Overview

J

Introduction

J

Using this Guide

J

Thermal Material Properties

J

Thermal Loads and Boundary Conditions

J

Thermal Analysis

J

References

2

15

3

11

5 7

2

Patran Interface to MD Nastran Thermal Introduction

1.1

Introduction The Patran MD Nastran Heat Transfer Preference supports the full range of thermal analysis capabilities available within MD Nastran. These capabilities include: • conduction in one, two, and three dimensions • fundamental convection • one dimensional advection • radiant exchange with space • radiant exchange in enclosures • specified temperatures • surface and volumetric heat loads • elements of thermal control systems • contact conduction

MD Nastran can span the full range of thermal analysis from system-level analysis of global energy balances to the detailed analysis associated with temperature and thermal stress limit levels. Within the integrated Patran-MD Nastran environment, you can simulate linear, nonlinear, steady-state, and transient thermal behavior. You can apply loads and boundary conditions either on the model’s geometry or on its finite element entities. MD Nastran’s sophisticated solution strategy automatically addresses the existence and extent of nonlinear behavior and adjusts the solution process accordingly.

Main Index

Chapter 1: Overview 3 Using this Guide

1.2

Using this Guide This guide is written for both new and experienced users of Patran and MD Nastran. It provides: • practical, “how to” descriptions of thermal modeling, analysis, and results processing and

visualization techniques • descriptions of the relevant Patran menu forms • basic engineering concepts and theory associated with MD Nastran's thermal solution

capabilities The Patran on-line help system provides logical and efficient access to all of this material. The remainder of Overview (Ch. 1), describes heat transfer basics. It discusses the concepts of thermal material properties, loads and boundary conditions, steady-state and transient analysis, and convergence criteria. Getting Started - A Guided Exercise (Ch. 2), is designed to familiarize users quickly with the basic Patran menu interfaces to thermal modeling, steady-state analysis, and results processing. Before beginning, please review the Guided Tour at the top of the Patran on-line help system. Building A Model (Ch. 3), describes Patran's menu forms for each phase of thermal modeling: • Meshing the geometric model with finite elements • Defining material properties • Specifying element properties • Applying loads and boundary conditions Running a Thermal Analysis (Ch. 4), describes how to select steady-state or transient analysis solution types, define solution and subcase input data, select load cases, and submit the MD Nastran analysis job. Results Processing and Visualization (Ch. 5), describes how to retrieve MD Nastran thermal analysis results into the Patran database. This chapter also summarizes the options for sorting and graphically rendering analysis results as contour or XY plots. Example Problems (Ch. 7), presents more advanced engineering problems covering the following

applications: • Transient thermal analysis (using the same flat plate model, plate.db, created in Getting Started - A Guided Exercise (Ch. 2)) • Free convection on a printed circuit board • Forced air convection on a printed circuit board • Thermal contact resistance • Typical avionics flow • Radiation enclosures • Axisymmetric flow in a pipe • Directional heat loads

Main Index

4

Patran Interface to MD Nastran Thermal Using this Guide

• Thermal stress analysis from directional heat loads • Thermal stress analysis of bi-metallic plate Files (App. A), describes the files created when using the Patran MD Nastran thermal preference product. Error Messages (App. B) describes general error and diagnostic messages. Supported Commands (App. C) describes the MD Nastran input data used “behind the scenes,” including

File Management Statements, Executive Control Statements, Case Control Commands, and Bulk Data Entries.

Main Index

Chapter 1: Overview 5 Thermal Material Properties

1.3

Thermal Material Properties MD Nastran thermal material properties include thermal conductivity, constant pressure specific heat, density, dynamic viscosity, internal heat generation, and temperature range and latent heat quantities associated with phase change phenomena. Conductivity Thermal conductivity is an intrinsic property of all materials and in the absence of any other mode of heat transfer, provides the proportionality constant between the flow of heat through a region and the temperature gradient maintained across the region (Fourier’s Law). Thermal conductivity is generally a mild function of temperature, decreasing with increasing temperature for solids and generally increasing with increasing temperature for liquids and gases. Additionally, within a solid, thermal conductivity can vary due to material orientation (anisotropy). Preferential paths for heat flow can result. MD Nastran allows for temperature-dependent and directionally dependent thermal conductivity. Specific Heat and Heat Capacitance Specific heat is another intrinsic material property. When multiplied by the volume and density of material, the quantity of interest is referred to as heat capacitance. Given a closed thermodynamic system, heat capacitance provides the proportionality constant between heat added or subtracted from the system and the resultant temperature rise or fall of the system (dq = C * dT). Since heat capacitance only multiplies the time derivative of temperature in the heat conduction equation, specific heat is usually only relevant in the solution of transient thermal phenomenon. We will note later that advection introduces a pseudo-transient flavor even in steady-state analysis and therefore the specific heat and density of the advecting fluid are needed in these calculations. Specific heat is also slightly temperature dependent. However, in typical heat transfer problems, the largest variations in specific heat are generally attributed to materials changing phase. Density For the purpose of conserving mass, the density cannot be allowed to vary with temperature. Since grid points are fixed in space in MD Nastran thermal analysis, if the density were to change with temperature, Density*Volume would also be changing, thus altering the system mass.

Main Index

6

Patran Interface to MD Nastran Thermal Thermal Material Properties

Table 1-1 provides several sets of consistent units which may be used by MD Nastran for the various

material properties. Table 1-1 Table 1-2

Typical Units for Thermal Material Properties Thermal Conductivity

Table 1-3

W Table 1-4 / m -

Btu/h r-fto F

o

C Table 1-5

Specific Heat

Table 1-6

J/ Table 1-7 k go

Btu/l bmoF

C Table 1-8

Density

Table 1-9

k Table 1-10 g/ m

lbm/ft 3

3

Main Index

Table 1-11

Dynamic Viscosity

Table 1-12

k Table 1-13 g/ m s e c

lbm/ft -hr

Table 1-14

Enthalpy

Table 1-15

J/ k g

Table 1-16

Btu/l bm

Table 1-17

Latent Heat

Table 1-18

J/ k g

Table 1-19

Btu/l bm

Chapter 1: Overview 7 Thermal Loads and Boundary Conditions

1.4

Thermal Loads and Boundary Conditions MD Nastran supports a full range of thermal boundary conditions and heat loads, starting with simple temperature constraints and heat flux boundary conditions, and moving on to more complicated heat transfer mechanisms associated with contact, convection and radiation. All of the thermal boundary conditions can be modeled as functions of time. Thermal boundary conditions can be applied to finite element entities as well as geometric entities and include the following:

Table 1-20 Table 1-21

Typical Units for Thermal Loads and Boundary Conditions Temperature

Table 1-22

o

C

o

Table 1-23

o

F

o

R

K Table 1-24

Normal Heat Flux

Table 1-25

W/m Table 1-26

Btu/hr-ft2

Table 1-27

Directional Heat Flux

Table 1-28

W/m Table 1-29

Btu/hr-ft2

Table 1-30

Nodal Source

Table 1-31

W

Btu/hr

Table 1-33

Volumetric Generation

Table 1-34

W/m Table 1-35

Btu/hr-ft3

Table 1-36

Convection Heat Flow

Table 1-37

W/m Table 1-38

Btu/hr-ft2

Table 1-39

Advection Heat Flow

Table 1-40

W

Btu/hr

Table 1-42

Convection Heat Transfer Coefficient

Table 1-43

W/m Table 1-44 2-oC

Btu/hr-ft2oF

Table 1-45

Radiation to Space

Table 1-46

W/m Table 1-47

Btu/hr-ft2

Table 1-48

Radiation Enclosure

Table 1-49

W/m Table 1-50

Btu/hr-ft2

Note:

Note:

2 2

Table 1-32

3 2

Table 1-41

2 2

When applying flux type loads or boundary conditions to nodal points, the units will still be those flux, i.e., loads per unit area. Patran’s input data forms for thermal loads and boundary conditions require you to specify an associated nodal area.

Temperature Boundary Conditions Temperature constraints can only be applied to nodal points. Temperature constraints can be defined as constant, spatially varying, or time varying. Normal Heat Flux Normal heat flux is defined using the nodal, element uniform, or element variable loading operations. As with temperature boundary conditions, heat flux loads can be made to vary with space or time.

Main Index

8

Patran Interface to MD Nastran Thermal Thermal Loads and Boundary Conditions

Directional Heat Flux MD Nastran supports vector heat flux from a distant radiant heat source. This capability allows you to model phenomena such as diurnal or orbital heating. The required input for this capability includes: • the magnitude of the flux vector • the absorptivity of the surface on which the flux is being applied • the vector components of the flux vector

The absorptivity can be dependent on temperature. The magnitude and components of the heat flux can be defined as constant, spatial varying, or time varying. Nodal Source Heat can be applied directly on nodal points (or “grid points” in MD Nastran terminology). Nodal source heat can be defined as constant, spatially varying in a global sense, or time varying. Volumetric Heat Generation Volumetric heat can be applied to one or more conduction elements and can be defined as constant, spatially varying, or time varying. The Patran MD Nastran interface also includes a heat generation multiplier for specifying temperature dependence. The multiplier feature is available in the input form used to specify the material property data. Basic Convection Basic convection boundaries can be defined. The approach to basic convection heat transfer in MD Nastran is to define the basic convection via a heat transfer coefficient and associated ambient temperature. The film coefficient is user specified and is available from a number of sources, including Reference 1. (p. 14). The film coefficient can be defined as a function of temperature; the ambient temperature can be defined as a function of time. Advection, Forced Convection Advection, forced convection, is a complicated heat transfer phenomenon that includes aspects of heat transfer as well as fluid flow. MD Nastran supports 1D fluid flow, which allows for energy transport due to streamwise advection and diffusion. Heat transfer between the fluid stream and the surroundings may be accounted for through a forced convection heat transfer coefficient based on locally computed Reynolds and Prandtl numbers; see Reference 1. (p. 14) and Reference 2. (p. 14) for more information on the underlying theory of this type of convection. The input for forced convection includes: • the mass flow rate of the fluid • the diameter of the fluid pipe • the material properties of the fluid

Main Index

Chapter 1: Overview 9 Thermal Loads and Boundary Conditions

The calculation of the heat transfer coefficient between the fluid and the adjoining wall requires the specification of a film temperature. By default, this temperature will be internally calculated as the average of the temperatures of the fluid and the adjoining wall. Additional forced convection inputs consist of the type of convection relationship used to calculate the energy transport and the method of calculating the heat transfer coefficient at the tube wall. There are two choices with respect to the energy transport. The default method includes advection and streamwise diffusion, and its theoretical basis is the Streamwise-Upwind Petrov-Galerkin method, or SUPG. There are also two choices for picking the method for calculating the heat transfer coefficient that applies between the fluid and the adjacent wall. The default method uses the following equation: h = Coef • Re

Expr

• Pr

Expp

(1-1)

The second method, chosen by picking the alternate formulation option, uses the following equation: k Expr Expp • Pr h =  --- • Coef • Re  d

(1-2)

h

=

=the heat transfer coefficient between the fluid and the adjacent wall (internally calculated)

Coef

=

=a constant coefficient

Re

=

=the Reynolds number based on the diameter (internally calculated)

Pr

=

=the Prandtl number (internally calculated)

Expr

=

=the Reynolds number convection exponent

Expp

=

=the Prandtl number convection exponent

k

=

=the fluid conductivity

d

=

=the tube diameter

Radiation to Space Radiation to space is a boundary condition that defines radiant exchange between a surface and blackbody space. The inputs required for radiation to space are the absorptivity and emissivity of the surface, the ambient temperature of space, and the radiation view factor between the surface and space (usually equal to 1.0). The absorptivity and emissivity can both be temperature dependent. The ambient temperature can vary with time. The exchange relationship is defined to be: 4

q = σ • View fac • ( ε e T e – α e T amb )

Main Index

4

(1-3)

10

Patran Interface to MD Nastran Thermal Thermal Loads and Boundary Conditions

q

=

=the net energy flux in W/m2 (internally calculated)

σ

=

=the Stefan-Boltzmann constant which has the value 5.668x10-8 W/m2 oK4 [0.1714x10-8 Btu/h ft2 oR4]

Viewfac

=

=the view factor

εe

=

= the emissivity

αe

=

=the absorptivity (usually

Te

=

=the temperature of the element (internally calculated)

Tamb

=

=the ambient temperature of space (user specified)

αe = εe )

Calculation of radiation exchange requires that the temperatures be defined on an absolute scale (Kelvin or Rankine). If the temperatures input in a problem involving radiation are either Celsius or Fahrenheit, an internal conversion can be defined. Radiation Enclosures Radiation Enclosure exchange is similar to the Radiation to Space boundary condition; however, this type of boundary condition takes into account the radiation exchange between discrete surfaces. As a result, subsequent to building a finite element mesh, the geometric relationship (view factor) between individual finite element surfaces must be determined. For enclosure radiation the view factors between surfaces are internally calculated. Also, for enclosure radiation, the absorptivity is taken as being equal to the emissivity (Kirchhoff’s Identity). Calculation of the radiation view factors can be the most computationally intensive operation in heat transfer analysis. MD Nastran has implemented a unique set of algorithms for solving this problem which provides for both reasonable performance while maintaining an accurate calculation. To help facilitate this calculation, the Can Shade and Can Be Shaded options have been added for those situations where the shading is known. These options can help reduce the calculation time for radiation enclosures. Patran also allows you to define multiple radiation enclosures. The view factors within each Radiation Enclosure will be independently calculated from the view factors of the other enclosures. In general, good view factor calculations require a reasonable surface mesh. Since the accuracy of the view factors tends to decrease as the distance between elements is reduced and becomes on the order of the element size, a mesh which prevents this sizing issue is recommended and is generally not too restrictive. Contact Conduction If contact bodies are present in the model for a SOL 153, 159 or 600 analysis heat transfer will occur between the contact bodies based on the properties defined on the contact bodies or via the contact table accessible from the subcase parameters for. as the bodies get closer the contact changes from radiation to convection to conduction. See the MSC Nastran Quick Reference Guide for more information.

Main Index

Chapter 1: Overview 11 Thermal Analysis

1.5

Thermal Analysis Thermal problems can be categorized as steady-state or transient, linear or nonlinear. Transient analyses are characterized by solution evolution over time, and in addition to energy exchange with the environment, involves thermal energy storage. Steady-state analyses are concerned with state point solutions to fixed boundary condition problems. Nonlinearities enter into both steady-state and transient solutions through several areas. The most common nonlinearity is associated with temperature dependent material properties, in particular thermal conductivity and specific heat. Other nonlinearities are introduced from application of boundary conditions principally convection and radiation. All nonlinear analyses necessarily involve solution iteration, error estimation, and some form of convergence criteria. MD Nastran attempts to do this as efficiently and trouble free as possible.

Steady-State Analysis The most general form of the steady-state heat balance equation is as follows: 4

[ K ] { u } + [ ℜ ] { u + T abs } = { P } + { N }

(1-4)

[K]

=

=the heat conduction matrix

[ℜ]

=

=the radiation exchange matrix

{u}

=

=the vector of unknown temperatures

Tabs

=

=the temperature offset from absolute required for radiation calculations (absolute temperature)

{P}

=

=the vector of constant applied heat flows

{N}

=

=the vector of temperature dependent heat flows

This equation is inherently nonlinear due to the presence of the fourth power law radiation term. In addition to the radiation term, many other nonlinearities may be introduced into this equation through the coefficient matrices and boundary condition terms. Specifically, nonlinearities are introduced by specifying the material properties and boundary conditions as temperature dependent as discussed in the Thermal Material Properties, 5 and Thermal Loads and Boundary Conditions, 7. MD Nastran applies a Newton-Raphson iteration scheme for the solution of these nonlinear equations. This process leads to the following form of the heat balance equation: i

i

[ KT ] { ∆ u } = { R }

Main Index

i

(1-5)

12

Patran Interface to MD Nastran Thermal Thermal Analysis

[ KT ]

=

i

=the tangential conductance matrix i

=

{R}

3 δN  i i i i { ∆ u } ≅ [ K ] + 4 [ R ] { u + T a b s } –  -------   δu 

=

i

=the residual vector {P}i + {N}i - [K]i {u}i - [R]i {ui + Tabs}4

At each iteration, the left-hand side matrix and the right-hand side vector are computed based on the temperature from the previous iteration temperatures i

{∆u} = {u

(u

i+1

i+1

)

i

(u ) .

By solving for the unknown vector

i

(∆u ) ,

the new

can be determined:

i

–u}

(1-6)

or {u}

i+1

= {∆u} + {u}

i

(1-7)

Because of the expense of performing matrix decompositions, MD Nastran recalculates the residual vector at each iteration, but only recalculates the tangent matrix when convergence is illusive or if it will lead to improvement in the iteration efficiency. MD Nastran will attempt to achieve an optimum converged solution by balancing various solution aspects such as: load bisection, residual updates, tangent matrix updates, line searches, and BFGS updates. Further description of the methods employed can be found in Reference 2. (p. 14). For steady-state analysis, the defaults for controlling the nonlinear solution should be sufficient for most problems. For those problems where additional control is required, the convergence tolerances for Temperature, Load, and Work can be overridden. See Steady-State and Transient Convergence Criteria, 14 for more information. Initial Conditions in Steady-State Analysis Since the nonlinear equations are solved by an iterative scheme, careful consideration of the initial conditions can have a significant effect on how quickly a problem will converge, or if it will converge at all. The initial conditions provide the starting point temperatures for the iterative solution method. Clearly, if we were able to exactly guess the solution to our problem, the process would converge on the first iteration, as it must for linear analysis. Although this is highly unlikely, a good initial guess can speed up the convergence process significantly. For highly nonlinear problems, good initial temperature estimates may be required in order to achieve convergence. See Initial Conditions in Transient Analysis, 13 for more information.

Main Index

Chapter 1: Overview 13 Thermal Analysis

Transient Analysis The most general form of the transient heat balance equation is: 4 [ B ] { u· } + [ K ] { u } + [ ℜ ] { u + T abs } = { P } + { N }

(1-8)

where, in addition to the terms already defined in the steady-state equation, we have: [B] = the heat capacity matrix.

(1-9)

du u· = -----dt

(1-10)

Because of its transient behavior, this equation must be integrated over time. The numerical method implemented for performing the time integration is Newmark’s method. As in the steady-state case, this equation also can be extensively nonlinear due to radiation and temperature-dependent material properties and boundary conditions. As a result, nonlinear iterations are also required for the solution of this equation. The iteration is performed within each time step until a converged solution for that time step is achieved (see Reference 2. (p. 14) for more details). Transient analysis requires specifying the total solution time. Solution time is defined by the initial time step size and total number of time steps requested. The total solution time is determined from their product. Because MD Nastran employs an automatic time stepping scheme (i.e., the time step is varied by the solver as the solution progresses), the actual number of time steps used may ultimately be quite different from the input request. In any event, the total amount of solution time will be approximately equal to the initially calculated product within some small tolerance of the last time step size. The advantage of using the adaptive time step algorithm is the potential for significantly reduced run times. To avoid inaccurate results or unstable solutions, the proper choice of the initial time step is required. A responsible initial time step is dependent on a number of factors, including the spatial size of the element mesh and the thermal diffusivity of the material. The selection criteria is: ρ ⋅ Cp 1 ∆ t 0 ≅ ------ ⋅ ∆ x 2 ⋅ -------------k 10

(1-11)

∆ t0

=

=the initial time step

∆x

=

=the mesh size

ρ

=

=the density

Cp

=

=the specific heat

k

=

=the conductivity

Initial Conditions in Transient Analysis Initial conditions define the temperature starting point for a transient analysis. Every node in the problem must have an initial temperature explicitly defined. Any node that does not have an initial temperature

Main Index

14

Patran Interface to MD Nastran Thermal Thermal Analysis

defined will automatically have a temperature of 0.0 assigned to it. This default temperature can be changed in the Solution Parameters form for the given application, either steady-state or transient analysis. Caution must be exercised when specifying initial conditions relative to any specified temperatures defined via a boundary condition. The initial condition temperature for these nodal points must match the (Implicit and Explicit) boundary condition temperature at time equal to zero. Failure to match these temperatures will cause an initial jump in the solution that can make convergence difficult to achieve. Fortunately, the default analysis setup will automatically enforce these temperatures to be equal at the start of the problem.

Steady-State and Transient Convergence Criteria As discussed previously, the solution of the nonlinear equations requires an iteration scheme. Efficient iteration schemes are highly dependent on convergence criteria and error estimation. Convergence criteria provide a means of measuring solution error relative to some predetermined acceptable level. For each iteration performed during the solution process, error levels are calculated and compared with preset tolerances. Three convergence criteria are available within MD Nastran that measure error based on temperature, load, and work. These criteria apply to steady-state and transient solutions alike. Four recommendations regarding nonlinear convergence can be made: 1. For most problems, use the default criteria selection with their default tolerance values. 1. If the analysis is transient and involves any time-varying temperature boundary conditions, you must use the temperature convergence criteria. 1. Convergence may be enhanced by increasing the numerical tolerance levels from their default values. 1. For highly nonlinear transient problems, the maximum number of iterations per time step may be increased. The defaults for controlling the nonlinear solution should be sufficient for most problems. However, for those problems requiring additional control, the convergence tolerances for Temperature, Load, and Work can be overridden. (In the solution of heat transfer problems, a convergence criteria based on WORK is realistically just a mathematical construct representing an extension of the equations used in the comparable structural solver.)

Main Index

Chapter 1: Overview 15 References

1.6

References 1. Holman, J. P., Heat Transfer, Sixth Edition, McGraw-Hill Book Company, 1986. 2. Chainyk, Mike, MSC/NASTRAN Thermal Analysis User’s Guide, Version 68, The MacNealSchwendler Corporation, 1994. 3. Peterson, Ken (ed.), MSC/NASTRAN Encyclopedia, Online Documentation CD-ROM, The MacNeal-Schwendler Corporation, 1995.

Main Index

16

Patran Interface to MD Nastran Thermal References

Main Index

Chapter 2: Getting Started - A Guided Exercise Patran Interface to MD Nastran Thermal

2

Main Index

Getting Started - A Guided Exercise

J

Introduction

J

Objectives

J

Start Patran

J

Create a Database

J

Create a Rectangular Geometric Surface

J

Mesh the Surface with Elements

J

Modify the Mesh (Reduce the Number of Elements)

J

Specify Material Properties

29

J

Assign Element Properties

30

J

Define the Temperature at the Plate’s Bottom Edge

J

Apply Heat Flux to the Plate’s Right Edge

34

J

Apply Convection to the Plate’s Left Edge

37

J

Perform a Steady-State Thermal Analysis

40

J

Visualize the Thermal Results (Contour Plot)

18 19 21 22 25

26

41

27

32

18

Patran Interface to MD Nastran Thermal Introduction

2.1

Introduction This guided exercise shows you in step-by-step fashion the basics of MD Nastran thermal modeling, analysis, and results visualization using Patran. By intention, the geometry is simple, as are the applied loads and boundary conditions. We will create the geometry for a rectangular metal plate, mesh it with quadrilateral elements, specify material and element properties, apply thermal loads and boundary conditions, run a steady-state thermal analysis to determine temperature distributions, and visualize the results using Patran’s postprocessor. Before attempting this exercise, please complete the guided tour provided at the top of the Patran on-line help system. It gives you an overview of the Patran user interface, including the layout of the main form, the various application selections, the use of menus and forms, mouse picking, and basic modeling operations. Although the menu options for thermal analysis differ from those for structural analysis, Patran has a common look-and-feel across both disciplines.

Main Index

Chapter 2: Getting Started - A Guided Exercise 19 Objectives

2.2

Objectives The objectives in this exercise are to: • Create a new database defined for MD Nastran thermal analysis. • Define geometry for a rectangular plate. • Mesh the structure with quadrilateral elements. • Modify the mesh. • Define the plate’s material as aluminum. Specify a thermal conductivity of 204 W/m-oC, specific

heat of 896 J/kg-oC, and a density of 2707 kg/m3. • Define the plate’s thickness to be 0.1 m. • Clean up the display. • Apply a temperature of 50 oC to the bottom edge of the plate. • Apply heat flux of 5000 W/m2 to the right edge of the plate. • Apply to the left edge of the surface a convection boundary condition with heat transfer

coefficient of 10.0 W/m2-oC and ambient temperature of 20 oC. • Perform a steady-state thermal analysis using MD Nastran within the Patran system.

Main Index

20

Patran Interface to MD Nastran Thermal Objectives

• Visualize the temperature distribution as a contour plot.

1m

Aluminum Plate K = 204 W/m-oC Cp = 896 J/kg-oC

ρ = 2707 kg/m3 h = 10.0 W/m2-oC 3m

q = 5000.0 W/m2

Tamb = 20.0 oC

Thickness = 0.1 m

T = 50 oC

Main Index

Chapter 2: Getting Started - A Guided Exercise 21 Start Patran

2.3

Start Patran To begin the Patran modeling session from your workstation’s XTERM window, enter the command patran or patran & (if you want to run the application in the background).

Main Index

22

Patran Interface to MD Nastran Thermal Create a Database

2.4

Create a Database From Patran’s main form, pull down the File menu and select New.

Patran File Group Viewport Viewing Display Preferences Tools File

Help

s

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results New...Ctrl N Open... Ctrl O Close Ctrl W $#Save Session file patran.ses.01 Ctrl S started recording at 25 $#Save Recorded by Patran 03:36:58 PM a Copy $# FLEXlm Initialization complete. Acquiring license(s)... Utilities hp, 2 Import... Export... Session Print... Report... Quit Ctrl Q s

Main Index

© XY

Chapter 2: Getting Started - A Guided Exercise 23 Create a Database

A form will appear called New Database.

New Database Template Database Name /patran/patran3/template.db New Database Name Change Template ...

NOTE: If only the MD Nastran Preference is accessed by the model, the

mscnastran_template.db

Modify Preferences... Filter /tmp/*.db Apply

Filter

can be used as template database to save disk space.

Cancel

Directories

Database List mdl.db

/tmp/. /tmp/..

New Database Name

STEP 1: Position the cursor inside the New Database Name databox. Type in the word plate.

plate OK

Filter

STEP 2: Click on OK.

Main Index

Cancel

24

Patran Interface to MD Nastran Thermal Create a Database

The New Model Preferences form will appear, which will display MD Nastran as the default analysis solver.

New Model Preferences Model Preferences For: plate.db Tolerance u

Based on Model

uu Default

Approximate Maximum Model Dimension: 10.0 Analysis Code: MD Nastran Analysis Type: STEP 3: Toggle the Analysis Type setting to Thermal.

Thermal OK

Reset

STEP 4: Click on OK.

Main Index

Chapter 2: Getting Started - A Guided Exercise 25 Create a Rectangular Geometric Surface

2.5

Create a Rectangular Geometric Surface Click on the Geometry application. The Geometry form will appear. Geometry

Action: Object: Method:

Create Surface XYZ

STEP 1: Change the settings to: Action:Create Object:Surface Method:XYZ

Surface ID List 1 Surface Type PATRAN 2 Convention

Refer. Coordinate Frame

STEP 2: Under Vector Coordinate List, we can enter the desired XYZ dimensions for our surface. Type <1 3 0> in the databox. Note: you must use angle brackets to define vectors. You must use square brackets to define coordinates. Make sure to provide a space between each number.

Coord 0 Vector Coordinates List STEP 3: Make sure that the Origin Coordinate List is [0 0 0], which is the default.

<1 3 0>

Auto Execute Origin Coordinates List [0 0 0]

-ApplyY Z X

STEP 4: Click on Apply.

Main Index

26

Patran Interface to MD Nastran Thermal Mesh the Surface with Elements

2.6

Mesh the Surface with Elements Click on the Finite Elements application. The Finite Elements form will appear.

Finite Elements Action:

Create

Object:

Mesh

Type:

STEP 1: Toggle the Object setting to Mesh.

Surface

Output Ids Node Id List 1 Element Id List 1

The Global Edge Length is 0.1, which is the default setting. We will leave this value as is for now. (We will change it later, after we mesh the surface.) The global edge length specifies the physical length of each element. If you are making 10 elements to comprise 1 unit (for example, 1 m) in length, you would specify an edge length of 0.1 to create 300 elements.

Global Edge Length 0.1 Element Topology Quad4 Quad5 Quad8

STEP 2: Click inside the databox under the heading Surface List. You can now use the mouse to click on the actual surface you want to mesh. Click anywhere on the surface we have made.

Mesher u

IsoMesh uu Paver IsoMesh Parameters... Node Coordinate Frames...

Surface List Surface 1

-Apply-

Y Z X

STEP 3: Click on Apply. A mesh of 300 quadrilateral elements will be generated on the surface with elements automatically numbered.

Main Index

Chapter 2: Getting Started - A Guided Exercise 27 Modify the Mesh (Reduce the Number of Elements)

2.7

Modify the Mesh (Reduce the Number of Elements) At this point, we will invoke Patran's undo feature so that we can make a coarser mesh. The mesh we have just created (300 elements) is excessive for our example.

Table 2-1 STEP 1: Click on the erasure icon at the top right corner of the Patran main form. The word undo will appear, and Patran will automatically delete the created mesh (the last specified action).

STEP 2: Click on the paintbrush icon. The words Refresh Graphics will appear, and the geometric surface will be regenerated exactly as it appeared before we applied the mesh.

Main Index

28

Patran Interface to MD Nastran Thermal Modify the Mesh (Reduce the Number of Elements)

Output IDs Node ID List 1 Element ID List 1 Global Edge Length 0.2

STEP 3: Note that the Finite Elements form is still visible. Change the Global Edge Length from 0.1 to 0.2. This will create elements of 0.2 units (meters) in length, which will result in a coarser mesh of 75 quadrilateral elements. Click on Apply.

The resulting mesh (75 elements) is now more to our liking.

Y Z X

Main Index

Chapter 2: Getting Started - A Guided Exercise 29 Specify Material Properties

2.8

Specify Material Properties Our material for this exercise will be aluminum. Click on the Materials application. The Materials form will appear with certain default options.

Materials Action:

Create

Object:

Isotropic

Method:

Manual Input

*

Filter

STEP 1: Type in alum under Material Name.

Existing Materials

Input Options Constitutive Model:

Solid properties

Property Name Material Name alum Description Date: 22-May-96

Time:16:13:13

Code: MD Nastran Type:

Value

Thermal Conductivity =

204

Specific Heat =

896

Density =

2707

Temperature Dependent Fields:

Thermal Input Properties ...

Change Material Status ...

Current Constitutive Models:

-ApplySTEP 2: Click on Input Properties.

Main Index

STEP 4: Click on Apply.

Clear

Cancel

STEP 3: The Input Options form will appear. Edit the form to specify a thermal conductivity of 204, specific heat of 896, and a density of 2707.

30

Patran Interface to MD Nastran Thermal Assign Element Properties

2.9

Assign Element Properties Our next task is to specify a thickness of 0.1 to our aluminum elements. Click on the Properties application. The Element Properties form will appear. Element Properties Action:

Create

Dimension:

2D

STEP 1: Click inside the Property Set Name databox. Type in the name plate.

Shell

Type:

STEP 2: Click on Input Properties. Existing Property Sets

STEP 3: The Input Properties form appears. The word alum will appear within the Material Property Sets listbox. Click on this word. The Material Name databox will now appear as m:alum. Property Set Name plate

STEP 4: Type in 0.1 in the Thickness databox.

Input Properties

Input Properties ...

Stan. Homogeneous Plate(CQUAD4) Property Name Value Material Name

Application Region Select Members

Value Type Mat Prop Name

m:alum

CID

[Material Orientation]

Surface 1 Thickness

Add

0.1

Real Scalar

Remove

Application Region Surface 1

-Apply-

Material Property Sets alum

STEP 5: Click on OK.

OK

STEP 6: From the Element Properties form, click on the Select Members databox. Patran will display two icons to the left of the Element Properties form. The first icon represents surface or face; the second represents 2D element. The two options allow you to apply properties either on the geometric entity (in this case, the surface) or on the finite elements.

Main Index

Chapter 2: Getting Started - A Guided Exercise 31 Assign Element Properties

STEP 7: We will apply properties directly on the geometry. Pick the top icon; it will turn black when you pick it.

Application Region Select Members Surface 1

Add

Remove

STEP 8: Now click anywhere on the geometric surface. The surface will be highlighted in red. The Select Members databox will now appear as Surface 1.

Application Region STEP 9: Click on Add at the bottom of the Element Properties form.

Surface 1

-Apply-

Main Index

STEP 10: Click on Apply.

32

Patran Interface to MD Nastran Thermal Define the Temperature at the Plate’s Bottom Edge

2.10

Define the Temperature at the Plate’s Bottom Edge Click on the Loads/BCs application. The Loads/Boundary Conditions form will appear. Create

Action: Object:

STEP 1: Change the settings to: Action:Create Object:Temp (Thermal) Type:Nodal

Temp (Thermal)

Type:

Nodal

Analysis Type: Thermal Current Load Case: Default... Type:

Static

Existing Sets

STEP 2: Type in a New Set Name in the databox. We will call it tempbc.

Input Data Boundary Temperature 50

New Set Name

tempbc

Spatial Fields

STEP 3: Click on Input Data. The Input Data form will appear. Reset

Input Data... . Select Application Region..

-Apply-

Main Index

OK

STEP 4: Click in the Boundary Temperature databox and type in 50.

Cancel

STEP 5: Click on OK.

STEP 6: Click on the Select Application Region. The Select Application Region form will appear.

Chapter 2: Getting Started - A Guided Exercise 33 Define the Temperature at the Plate’s Bottom Edge

STEP 7: Under Geometry Filter, the default setting is Geometry. To the left, five options are given, represented as icons: Geometric entity, Point or Vertex, Curve or Edge, Surface or Face, Solid.

Select Application Region

u

STEP 8: Click on Curve or Edge. This icon will become black, indicating that it has been selected.

Geometry Filter Geometry

uu FEM

Application Region Select Geometry Entities Surface 1.4 Add

Remove

STEP 9: With your mouse, position the cursor on the bottom edge of the surface. Click on the edge. You will see Surface 1.4 appear in the Select Geometry Entities databox. This means we have selected Edge number 4 in Surface number 1.

Application Region

STEP 10: Click on Add.

OK

STEP 11: Click on OK. You must also click on Apply located on the Loads/Boundary Conditions form.

Note: A label on the bottom of your model will appear showing a boundary condition of 50 oC applied to the desired edge of the surface.

Main Index

34

Patran Interface to MD Nastran Thermal Apply Heat Flux to the Plate’s Right Edge

2.11

Apply Heat Flux to the Plate’s Right Edge We will now apply heat flux to the model using the Loads/Boundary Conditions form.

Load/Boundary Conditions Create

Action: Object: Type:

Applied Heat

STEP 1: Change the settings to: Object:Applied Heat Type:Element Uniform Option:Normal Fluxes

Element Uniform

Option: Normal Fluxes Analysis Type: Thermal Current Load Case: Default... Type:

Static

Existing Sets

New Set Name

flux

STEP 2: Click inside the New Set Name databox. Type in the name flux.

Target Element Type: 2D

Input Data... .

STEP 3: Because the problem is a 2D one, we need to toggle the Target Element Type setting to 2D. Even though we are applying heat flux along an edge, which we normally think of as 1D, our finite element problem is 2D; i.e., we are modeling heat conduction in two dimensions.

Select Application Region..

-ApplySTEP 4: Click on the Input Data button. The Input Data form will appear.

Main Index

Chapter 2: Getting Started - A Guided Exercise 35 Apply Heat Flux to the Plate’s Right Edge

Input Data Form Type:

Basic

Surface Option:

Edge

Edge Heat Flux

STEP 5: Toggle the Surface Option setting from Top to Edge.

5000 STEP 6: Click inside the databox under Edge Heat Flux. Type in 5000.

Spatial Fields

Reset OK

Cancel STEP 7: Click on OK.

Next, click on Select Application Region located on the Loads/Boundary Conditions form.

Main Index

36

Patran Interface to MD Nastran Thermal Apply Heat Flux to the Plate’s Right Edge

STEP 8: Two icon choices will appear, Surface and Edge. Click on the bottom icon, Edge.

Select Application Region

u

Geometry Filter Geometry

uu

FEM

Application Region Select Surfaces or Edges Surface 1.3 Add

STEP 9: Position the cursor over the right edge of the surface and click on this edge with the mouse. Patran will insert Surface 1.3 in the databox under the heading Select Surfaces or Edges.

Remove

Application Region STEP 10: Click on Add.

OK

STEP 11: Click on OK. Be sure to click on Apply located on the Loads/Boundary Conditions form. 5000.

Y Z X

Main Index

50.00

50.005000.

A yellow flag will appear on the right edge of your surface indicating that a heat flux of 5000 W/m2 has been applied along the right edge.

Chapter 2: Getting Started - A Guided Exercise 37 Apply Convection to the Plate’s Left Edge

2.12

Apply Convection to the Plate’s Left Edge We will now apply a convection boundary condition to the left edge of the plate--again, using the Loads/Boundary Conditions form. Load/Boundary Conditions

Action:

Create

Object:

Convection

Type:

Option:

STEP 1: Change the settings to: Object:Convection Type:Element Uniform Option:To Ambient

Element Uniform To Ambient

Analysis Type: Thermal Current Load Case: Default... Type:

Static

Existing Sets

New Set Name

conv

STEP 2: Click inside the New Set Name databox and type in conv.

Target Element Type: 2D

STEP 3: Toggle the Target Element Type setting to 2D.

Input Data... . Select Application Region..

-Apply-

Main Index

STEP 4: Click on the Input Data button. The Input Data form will appear.

38

Patran Interface to MD Nastran Thermal Apply Convection to the Plate’s Left Edge

STEP 5: Change the Surface Option setting to Edge.

Input Data STEP 6: Click inside the Edge Convection Coef databox and type in 10.

STEP 7: Type in an Ambient Temperature of 20.

Surface Option:

Edge Convection Coef 10

Form Type:

Basic

* Temperature Function

Ambient Temperature 20

Spatial Fields

STEP 8: Click on OK.

Edge

OK

Temperature Dependent Fields

Reset

Cancel

Next, click on Select Application Region located on the Loads/Boundary Conditions form.

Main Index

Chapter 2: Getting Started - A Guided Exercise 39 Apply Convection to the Plate’s Left Edge

STEP 9: Two icon choices will appear, Surface and Edge. Click on the bottom icon, Edge.

Select Application Region Geometry Filter u Geometry uu

FEM

Application Region

STEP 10: Position the cursor over the left edge of the surface and click on this edge with the mouse. Patran will insert Surface 1.1 in the databox under Select Surfaces or Edges.

Select Surfaces or Edges Surface 1.1 Add STEP 11: Click on Add.

Remove

Application Region

STEP 12: Click on OK. Be sure to click on Apply located on the Loads/Boundary Conditions form.

OK

10.00

5000.

A green label will appear confirming that you have applied a convection coefficient of 10.0 W/m2-oC at this location of your model. Y Z X

Main Index

5000. 10.00 50.00 Select50.00 Menu

40

Patran Interface to MD Nastran Thermal Perform a Steady-State Thermal Analysis

2.13

Perform a Steady-State Thermal Analysis We are now ready to submit the model for MD Nastran steady-state thermal analysis. Click on the Analysis application located on the Patran main form. The Analysis form will appear. Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Code: MD Nastran Type: Thermal

STEP 1: Change the settings to: Action:Analyze Object:Entire Model Method:Full Run Note: The Full Run Method will run the job in the background. If Method is changed to Analysis Deck, Patran will translate the MD Nastran input file but will not run the job.

Available Jobs plate

Job Name STEP 2: Make sure that the Job Name setting is plate.

plate Job Description MD Nastran job created on 18-Apr-96 at 13:58:15 Translation Parameters... Solution Type... Direct Text Input... Subcase Create...

Note: In the background, Patran will submit the needed input data information to the MD Nastran solver. The heartbeat icon at the top right of Patran main form will turn blue, indicating that Patran’s forward translator and MD Nastran are active in the background. (In your XTERM windows, from which you launched Patran, you can similarly note a message indicating that MD Nastran has been executed.) When the analysis is completed, you are ready to visualize the results.

Subcase Select... Apply

Main Index

STEP 3: Click on Apply.

Chapter 2: Getting Started - A Guided Exercise 41 Visualize the Thermal Results (Contour Plot)

2.14

Visualize the Thermal Results (Contour Plot) MD Nastran has now finished its processing, and the thermal results are ready to be displayed. To visualize the results in Patran, you must first access the OUTPUT2 results data created by MD Nastran. Analysis

Action:

Read Output2

Object:

Result Entities

Method:

Translate

STEP 1: Change the settings to: Action:Read Output2 Object:Result Entities Method:Translate

Code: MD Nastran Type: Thermal Available Jobs plate

Job Name STEP 2: Make sure that the Job Name setting is plate.

plate Job Description MD Nastran job created on 18-Apr-96 at 13:58:15 Translation Parameters... Select Results File...

STEP 3: Click on the Select Results File button. A new form will appear called Select File that lists all the available output2 files. (Note that these files all have the extension .op2). STEP 4: Double click on the file called plate.op2.

Apply

Main Index

STEP 5: Click on Apply. The heartbeat will change to the color blue, indicating that postprocessing is underway.

42

Patran Interface to MD Nastran Thermal Visualize the Thermal Results (Contour Plot)

When the heartbeat becomes green again, click on the Results application selection located on the Patran main form. The Results Display form will appear. Results

Action: Object:

Create Quick Plot

Select Result Cases Default, Default, PW PW Linear:100. Linear : 100.%%ofofLoLoa

STEP 1: In the Results form, make sure the Default, PW Linear : 100. % of Load selection is highlighted in the Select Result Cases listbox.

Select Fringe Result Heat Fluxes, Temperature Gradients, Temperatures,

Quantity:

STEP 2: Within the Select Fringe Result listbox, highlight Temperatures.

Magnitude

Select Deformation Result

Animate STEP 3: Click on Apply.

-Apply-

Main Index

Chapter 2: Getting Started - A Guided Exercise 43 Visualize the Thermal Results (Contour Plot)

A contour plot displaying temperature distributions will appear as follows:

Select the Save and Close operations from the File menu to save your plate.db file. We will perform a transient thermal analysis on this model in Example Problems (Ch. 7). You have now learned the basics of steady-state thermal analysis using Patran and MD Nastran. Example 1 - Transient Thermal Analysis (Ch. 7) builds on this example. The remaining examples in Example Problems (Ch. 7) describe more advanced applications.

Main Index

44

Patran Interface to MD Nastran Thermal Visualize the Thermal Results (Contour Plot)

Main Index

Chapter 3: Building A Model Patran Interface to MD Nastran Thermal

3

Main Index

Building A Model

J

Introduction

J

Finite Elements

J

Coordinate Frames

J

Material Library

J

Finite Element Properties

J

Loads and Boundary Conditions

J

Load Cases

46 47 51

52

101

57 66

46

Patran Interface to MD Nastran Thermal Introduction

3.1

Introduction Building a model for heat transfer analysis can be divided into several steps:

Import or create the geometry

You can either import the geometry for your model from a CAD definition or create it within Patran. For a complete description of this process, see Patran Reference Manual, Part 2: Geometry Modeling.

Define the finite element mesh

The objective of this step is to subdivide the geometry into nodes and elements. Temperatures are calculated at the nodal points in the analysis. Heat conduction takes place within the elements. This step is described briefly in Finite Elements, 47. For more complete information, see Patran Reference Manual, Part 3: Finite Element Modeling.

Define material properties

In a steady-state conduction analysis, the thermal conductivity of one or more materials must be defined. In a transient analysis, the specific heat and density of the materials must also be defined. Sophisticated analyses may also require latent heat or fluid viscosity to be defined. This step is described in Material Library, 52.

Define element properties

The elements that define the heat conduction paths in the body can be characterized geometrically as 1D, 2D, 3D, or axisymmetric. All elements have associated material properties. In addition, one-dimensional elements must have their cross-sectional properties defined, and shell elements must have their thickness defined. This step is described in Finite Element Properties, 57.

Define loads and boundary conditions

Defining loads and boundary conditions is often the most difficult step in building a model for thermal analysis. In a steady-state analysis, fixed temperatures can be specified at any nodal points in the model. This applies to structural nodal points as well as ambient nodal points. In a transient analysis, temperatures specified on nodal points may be fixed or time varying. In addition to specifying temperatures, you can apply numerous other boundary conditions, including several forms of convection and radiation. Applied surface or volumetric heat flux or heat flow are described as thermal loads. Initial temperatures are specified for two primary reasons. In a transient analysis, the full mathematical description of the Fourier problem requires the statement of the initial condition, for heat transfer the beginning temperature. In a nonlinear steady-state analysis, the MD Nastran solver necessarily employs an iterative scheme in solving the system equations, and it requires a starting temperature to initialize the process. For more information, see Loads and Boundary Conditions, 66.

Main Index

Chapter 3: Building A Model 47 Finite Elements

3.2

Finite Elements The Finite Elements Application in Patran provides options for creation of nodes, elements, and multipoint constraints in the thermal finite element model.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

© XY

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

For more information on how to create finite element meshes, see Mesh Seed and Mesh Forms (p. 25) in the Reference Manual - Part III. For information on the concepts of multi-point constraints, see the Patran Thermal User’s Guide, Volume 1: Thermal/Hydraulic Analysis.

Nodes Nodes in Patran will translate into unique GRID Bulk Data entries in MD Nastran. Nodes can be created either directly using the Node object, or indirectly using the Mesh object. Each node has associated Reference (CP) and Analysis (CD) coordinate frames. The ID is taken directly from the assigned node ID. The X1, X2, and X3 fields (Node Location List) are defined in the specified CP coordinate frame. If

Main Index

48

Patran Interface to MD Nastran Thermal Finite Elements

no reference frame is assigned, the global system is used. The PS and SEID fields on the translated GRID entry are left blank.

Finite Elements Action:

Create

Object:

Node

Method:

Edit

Node ID List 1

Analysis Coordinate Frame Coord 0 Refer. Coordinate Frame Coord 0

Associate with Geometry Auto Execute Node Location List

(0 0 0)

-Apply-

Main Index

The analysis frame (CD of the GRID) is the ID of the which the loads and boundary conditions are define reference coordinate system for any output in vecto temperature gradients and heat fluxes. The coordinate system in which the node location is GRID) can be the reference coordinate frame, the a frame, or a global reference (blank), depending on forward translation parameter “Node Coordinates.”

Chapter 3: Building A Model 49 Finite Elements

Finite Elements The Finite Elements application in Patran assigns element connectivity, such as Quad/4 (CQUAD4), for standard finite elements. The type of MD Nastran element to be created is not determined until the element properties are assigned. See the Element Properties Form, 58 for details concerning the MD Nastran element types. Elements can be created either explicitly using the Element object or implicitly using the Mesh object.

Finite Elements Action:

Create

Object:

Mesh Surface

Type: Output IDs Node ID List 1

Element ID List

Elements not referenced by an element property region that is recognized by the Patran MD Nastran forward translator will not be translated.

1 Global Edge Length 0.1 Element Topology Quad4 Quad5 Quad8 Mesher

u

IsoMesh

uu Paver

IsoMesh Parameters... Node Coordinate Frames...

Surface List

-Apply-

Main Index

50

Patran Interface to MD Nastran Thermal Finite Elements

Multi-Point Constraints Multi-point constraints (MPCs) can also be created from the Finite Elements menu. These are special element types that define a rigorous algebraic relationship between several specified nodes. The forms for creating MPCs are found by selecting MPC as the Object on the Finite Elements form. For MD Nastran thermal analysis, the MPC object is used to implement temperature coupling. Finite Elements Action:

Create

Object:

MPC

Method:

Explicit (Thermal)

Analysis Preferences: Code: MD Nastran Type: Thermal MPC ID 2

Define Terms...

Creates an explicit MPC between a dependent grid point and one or more independent grid points. This constraint is used to specify a grid point temperature to be a weighted combination of any number of other grid point temperatures. The dependent term consists of a node ID, while an independent term consists of a coefficient and a node ID. An unlimited number of independent terms can be specified, while only one dependent term can be specified; A1T1+A2T2+ ...AnTn = 0 where T1 must be defined to be the dependent node temperature.

-Apply-

Note: 1. Patran automatically sets the A1 field on the MPC entry to -1.0. 2. When specifying initial temperature conditions, the nodal temperatures associated with the node points in an MPC must identically satisfy the MPC constraint equation.

Main Index

Chapter 3: Building A Model 51 Coordinate Frames

3.3

Coordinate Frames Coordinate frames will generate a unique CORD2R, CORD2C, or CORD2S Bulk Data entry, depending on the specified coordinate frame type. The CID field is defined by the Coord ID assigned in Patran. The RID field may or may not be defined, depending on the coordinate frame construction method used in Patran. The A1, A2, A3, B1, B2, B3, C1, C2, and C3 fields are derived from the coordinate frame definition in Patran. Only Coordinate Frames that are referenced by nodes, element properties, or loads and boundary conditions can be translated. For more information on creating coordinate frames, see Creating Coordinate Frames (p. 393) in the Geometry Modeling - Reference Manual Part 2.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

Main Index

© XY

52

Patran Interface to MD Nastran Thermal Material Library

3.4

Material Library The Materials form will appear when you select Materials from the main form. The selections made on the Materials menu will determine which material form appears, and ultimately, which MD Nastran material will be created. The following pages give an introduction to the Materials form and details of all the material property definitions supported by the Patran MD Nastran Thermal Application Preference. Only material records that are referenced by an element property region will be translated. References to externally defined materials will result in special comments in the MD Nastran input file, e.g., materials that property values are not defined in Patran. The Patran MD Nastran forward translator will perform material type conversions when needed. This translation applies to both constant material properties and temperature-dependent material properties.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

Main Index

© XY

Chapter 3: Building A Model 53 Material Library

Materials Form This form appears when you select Materials from the main menu. The Materials form provides options for specifying MD Nastran material data. Materials Create

Action:

Isotropic

Object:

Manual Input

Method:

*

Defines the basic material directionality and can be set to Isotropic, 2D Orthotropic, 3D Orthotropic, 2D Anisotropic, or 3D Anisotropic.

Filter

Existing Materials

Lists the existing materials with the specified directionality.

Material Names Defines the material name. A unique material ID will be assigned during translation.

Description DATE: 01-Apr-92 Time: 17:08:02

Code:

MD Nastran

Type:

Thermal Input Properties...

Change Material Status...

Main Index

Describes the material that is being created.

Indicates the active analysis code and analysis type. These selections are made on the Preferences>Analysis (p. 431) in the Patran Reference Manual. Generates a form that is used to define the material properties. Generates a form that is used to indicate the active portions of the material model. By default, all portions of a created material model are active.

54

Patran Interface to MD Nastran Thermal Material Library

The following table outlines the material properties for MD Nastran thermal analysis. Object Isotropic

Constitutive Model Solid properties

Fluid properties

Phase changes

2D Orthotropic

3D Orthotropic

MAT4, MATT4

MAT4, MATT4

MAT4

Input Data

Temp Dep

Thermal Conductivity

yes

Specific Heat

yes

Density

no

Thermal Conductivity

yes

Specific Heat

yes

Density

no

Dynamic Viscosity

yes

Reference Enthalpy

no

Phase Change Temperature

no

Phase Change Temp. Range

no

Latent Heat

no

Heat generation

MAT4, MATT4

Heat Generation Multiplier

yes

Solid properties

MAT5, MATT5

Thermal Conductivity Kx/Kr

yes

Thermal Conductivity Ky/Kz

yes

Specific Heat

yes

Density

no

Heat generation

MAT5, MATT5

Heat Generation Multiplier

yes

Solid properties

MAT5, MATT5

Thermal Conductivity Kx

yes

Thermal Conductivity Ky

yes

Thermal Conductivity Kz

yes

Specific Heat

yes

Density

no

Heat Generation Multiplier

yes

Heat generation

Main Index

MD Nastran Bulk Data

MAT5, MATT5

Chapter 3: Building A Model 55 Material Library

Object

MD Nastran Bulk Data

Constitutive Model

2D Anisotropic

3D Anisotropic

Solid properties

MAT5, MATT5

Input Data

Temp Dep

Thermal Conductivity Kxx

yes

Thermal Conductivity Kxy

yes

Thermal Conductivity Kyy

yes

Specific Heat

yes

Density

no

Heat generation

MAT5, MATT5

Heat Generation Multiplier

yes

Solid properties

MAT5, MATT5

Thermal Conductivity Kxx

yes

Thermal Conductivity Kxy

yes

Thermal Conductivity Kxz

yes

Thermal Conductivity Kyy

yes

Thermal Conductivity Kyz

yes

Thermal Conductivity Kzz

yes

Specific Heat

yes

Density

no

Heat Generation Multiplier

yes

Heat generation

MAT5, MATT5

Constitutive Models The material properties for isotropic materials are divided into different categories called constitutive models, as follows: Solid Properties, 56 Fluid Properties, 56 Phase Changes, 56 Heat Generation1, 56

For a single material, you only need to define the constitutive models and properties necessary for the particular analysis. For example, in a steady-state analysis of a simple solid, you need only define the thermal conductivity. The phase changes and heat generation constitutive models need to be defined only when these effects are present in the analysis.

Main Index

56

Patran Interface to MD Nastran Thermal Material Library

Solid Properties Thermal conductivities may be defined for isotropic, orthotropic, and anisotropic materials. When the 2D orthotropic material is used in an axisymmetric analysis, the conductivity Kr applies to the radial direction and the conductivity Kz is along the axis of symmetry. The conductivities may be defined as functions of temperature by creating temperature-dependent functions in the Fields application and then referencing these functions on the Materials form. Density and specific heat define the heat capacity of the body and are needed only in transient analysis. Fluid Properties The dynamic viscosity is used in the calculation of the Reynolds (Re) and Prandtl (Pr) number in forced convection/advection applications and applies only to the Flow Tube element. The fluid specific heat, thermal conductivity, and density are also required for the formulation of the advective Streamwise Upwind Petrov Galerkin (SUPG) elements. This is the case even for steady-state analysis.

Recall

Cp µ DVρ Re = ------------ and Pr = ----------µ K

(3-1)

Phase Changes1 To model a phase change, you need to specify the latent heat and a finite temperature range over which the phase change is to occur. You also need to specify the lower boundary of the transition temperature as well as the reference enthalpy. The reference enthalpy is defined as the enthalpy corresponding to a zero temperature if the heat capacity Cp is a constant. If the heat capacity is temperature dependent, then the enthalpy must be defined at the lowest temperature value in the tabular field. For pure materials, the temperature range over which the phase change takes place can be quite small, whereas for solutions or alloys the range can be quite large. Numerically, the wider the range the better. It is not recommended to make this range less than a few degrees. Heat Generation1 The heat generation multiplier allows the definition of a temperature-dependent rate of volumetric heat generation to be defined. Usually a temperature-dependent function will be defined in Fields and selected on the Materials form. The value defined by this field will multiply the rate of heat generation defined on the Applied Heat, Volumetric Generation LBC. If the heat generation is not temperature dependent, only the Volumetric Generation LBC needs to be defined.

1

If you define this constitutive model, you must also define a constitutive model for Solid Properties.

Main Index

Chapter 3: Building A Model 57 Finite Element Properties

3.5

Finite Element Properties The Element Properties form appears when you select Properties from the main form. There are several option menus available when creating element properties. The selections made on the Element Properties menu will determine which element property form appears, and ultimately, which MD Nastran element will be created. The following pages give an introduction to the Element Properties form and details of all the element property definitions supported by the Patran MD Nastran Thermal Application Preference.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

Main Index

© XY

58

Patran Interface to MD Nastran Thermal Finite Element Properties

Element Properties Form This form appears when you select Element Properties from the main menu. There are four option menus on this form. Each will determine which MD Nastran element type will be created and which property forms will appear. The individual property forms are documented later in this section. For a full description of this form, see Element Properties Forms (p. 67) in the Patran Reference Manual. Element Properties Create

Action: Dimension:

1D

Type:

Beam

Use this option menu to define the element’s dimension. Th options are: 0D (point elements) 1D (bar elements) 2D (tri and quad elements) 3D (tet, wedge, and hex elements)

Existing Property Sets This option menu depends on the selection made in the Dimension option menu. Use this menu to define the genera type of element, such as: Shell versus Axisym Solid

Property Set Name

Option (s): General Section

Input Properties... Application Region Select Members

Add Application Region

Main Index

Remove

This option is only presented for 1D Beam and Rod elements.

Chapter 3: Building A Model 59 Finite Element Properties

The available element types are described briefly in the table below. Dimension 0D

Type

Option

• Grounded

Elem Type

Input Data

CELAS1

Thermal Conductance

CDAMP1

Thermal Capacitance

CBAR

Material Name

Conductor • Grounded

Capacitor 1D

• Beam

• General

Section Area • Curved w/

CBEND

General Section

Material Name Center of Curvature Area

• Curved w/

CBEND

Pipe Section

Material Name Center of Curvature Mean Pipe Radius Pipe Thickness

• Tapered

CBEAM

Material Name

Section Cross Sect. Areas • Rod

• General

CROD

Material Name

Section Area • Pipe

CTUBE

Material Name

Section Outer Diameter @ Node [Outer Diam. @ Node 2] Pipe Thickness • Conductor

CELAS1

Thermal Conductance

• Capacitor

CDAMP1

Thermal Capacitance

• Flow Tube

CHBDYP

Material Name Hydraulic Diam. at Node 1 [Hydraulic Diam. at Node 2]

Main Index

60

Patran Interface to MD Nastran Thermal Finite Element Properties

Dimension 2D

Type

Option

• Shell

Elem Type

Input Data

CQUAD4,8

Material Name

CTRIA3,6

[Material Orientation] Thickness

• Axisym

CTRIAX6

[Material Orientation]

Solid Material Name 3D

• Solid

CHEXA

Material Name

CPENTA CTETRA Conductors and Grounded Conductors These elements provide a simple conductance link between either two nodes in the model or a node and a zero temperature heat sink. The only property to be defined is the thermal conductance of the link. This value can either be real or a reference to an existing field definition. Capacitors and Grounded Capacitors These elements provide a simple thermal capacitance link between either two nodes in the model or a node and a zero temperature heat sink. The only property to be defined is the thermal capacitance of the link. This value can either be real or a reference to an existing field definition. Beam and Rod Elements with General Section These elements provide a simple conductance and capacitance link between two nodes in the model. Heat is conducted only along the length of the element; no heat is transferred across the cross section. The referenced material and cross-sectional area must be defined. Cross-sectional area can be defined either as a real value or as a reference to an existing field definition.

Main Index

Chapter 3: Building A Model 61 Finite Element Properties

Curved General Section Beam Figure 3-1 Input Properties Curved General Sec. Beam (CBEND) Property Name

Value

Material Name

Defines the material for the element.

Mat Prop Name Vector

Center of Curvature Area

Real Scalar

The center of curvature of the pipe bend can be defined as a vector from the first node to the center or by selecting an existing node located at the center.

Defines the cross-sectional area of the element. This value can be either a real value or a reference to an existing field definition.

Material Property Sets m

OK

Main Index

Value Type

62

Patran Interface to MD Nastran Thermal Finite Element Properties

Curved Pipe Section Beam Figure 3-2 Input Properties Curved Pipe Section Beam (CBEND) Property Name

Value

Material Name

Defines the material for the element.

Value Type Mat Prop Name Vector

Center of Curvature Mean Pipe Radius

Real Scalar

Pipe Thickness

Real Scalar

The center of curvature of the pipe bend can be defined as a vector from the first node to the center or by selecting an existing node located at the center.

The distance from the centroid of the pipe cross section of the midwall of the pipe. This value can either be a real value or a reference to an existing field definition.

Material Property Sets m Wall thickness of the pipe. This value can either be a real value or a reference to an existing field definition.

OK

Tapered Section Beam The Tapered Section beam allows different cross-sectional areas at each end of the beam. Both areas are entered in the Cross Sect. Areas databox separated by either spaces or a comma. If only one area is defined, the cross-sectional area is assumed to be constant at that value.

Main Index

Chapter 3: Building A Model 63 Finite Element Properties

Pipe Section Rod Figure 3-3 Defines the tube OD at each end of the element. These values can either be real values or references to existing field definitions. The Outer Diameter at Node 1 property is required. The Outer Diameter at Node 2 Property is optional.

Input Properties Pipe Section Rod (CTUBE) Property Name

Value

Value Type

Material Name

Mat Prop Name

Outer Diameter @ Node

Real Scalar

[Outer Diam. @ Node 2]

Real Scalar

Pipe Thickness

Real Scalar

Defines the material to be used. When entering data here, a list of all materials currently in the database is displayed. You can either pick one from the list with the mouse, or type the name in.

Specifies the wall thickness of the pipe. This value can be either real or a reference to an existing field definition.

OK

Flow Tube This element defines heat transfer based on 1D fluid flow. A material with the Fluid constitutive model defined must be selected. In addition, the diameters of tube at each end must be defined; if only the diameter at node 1 is defined, the tube diameter is assumed to be constant at that value. The value for the

Main Index

64

Patran Interface to MD Nastran Thermal Finite Element Properties

diameter may either be real or a reference to an existing field definition. The Flow Tube elements can be referenced in the Loads/BCs application to support several types of forced convection and advection conditions. 2D Shell Elements These elements provide for conduction and heat capacitance within a planar area. Heat is not transferred through the thickness of the shell. Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. You can either select one from the list using the mouse or type in the name.

Input Properties Stan. Homogeneous Plate (CQUAD4) Property Name

Value

Value Type Mat Prop Name

Material Name [Material Orientation]

CID

Thickness

Real Scalar

Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This scalar value can either be a constant value in degrees, a vector, or a reference to an existing coordinate system. This property is optional.

Defines the thickness, which will be uniform over each element. This value can either be real or a reference to an existing field definition.

OK

Main Index

Chapter 3: Building A Model 65 Finite Element Properties

2D Axisymmetric Solid Elements These elements are used to model heat conduction in a body that is symmetric about a particular coordinate axis. When defining the model with Patran, this axis must be the global z-axis and the radial axis must be the global x-axis (i.e., the elements must lie in the x-z plane). The only element property required is the material. An optional material orientation allows you to define the orientation for any nonisotropic material within the element. You can specify temperature boundary conditions, initial temperatures, and nodal and volumetric heat loads on the element’s boundaries or interior. You can specify exchange type boundary conditions (convection and radiation) on the boundaries of the geometry. With Version 68 of MD Nastran, if convection or radiation boundary conditions are applied to 6-node triangular axisymmetric elements, the heat flux results associated with these elements cannot be postprocessed in Patran. To postprocess boundary heat fluxes, the 3-node triangular axisymmetric elements must be used instead. 3D Solid Elements These elements provide for conduction and heat capacitance within a volume. A material property must be selected to define the thermal conductivity, density, and specific heat.

Main Index

66

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

3.6

Loads and Boundary Conditions The Loads and Boundary Conditions form will appear when you select Loads/BCs from the main form. When you create a loads and/or boundary condition, there are several option menus. The selections made on the Loads and Boundary Conditions menu will determine which loads and/or boundary conditions form appears, and ultimately, which MD Nastran loads and/or boundary conditions will be created. The following pages give an introduction to the Loads and Boundary Conditions form and details of all the loads and boundary conditions supported by the Patran MD Nastran Thermal Application Preference.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

© XY

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

Loads and Boundary Conditions Form This form appears when you select Loads/BCs from the main menu. The Loads/Boundary Conditions form provides options to create the various MD Nastran loads and/or boundary conditions. For a

Main Index

Chapter 3: Building A Model 67 Loads and Boundary Conditions

definition of full functionality, see Loads and Boundary Conditions Form (p. 27) in the Patran Reference Manual. Load/Boundary Conditions

Action:

Create

Object:

Convection

Indicates the category of heat loads or boundary condition. The choices are Temp (Thermal) for prescribing temperatures, Initial Temperature, Boundary Temperature, Applied Heat, Convection, Radiation, and Contact.

Type:

Element Uniform

Option:

Coupled

Analysis Type:

Thermal

Current Load Case:

Indicates the specific type for each general category of loads/boundary condition. The choices for each Object are shown on page 68.

Default... Type:

The Type options are Nodal, Element Uniform, and Element Variable. Nodal is applied explicitly to nodes. Element Uniform defines a constant value to be applied over an entire element, element face, or element edge. Element Variable defines a value that varies across an entire element, element face, or element edge.

Static Loads or boundary conditions defined here are associated with the Current Load Case. By default, this is a static (steady-state) load case called Default. To create heat loads or boundary conditions for a transient analysis, you must create a Time-Dependent load case in the Load Cases application.

Existing Sets

New Set Name

Target Element Type: Region 2:

2D

Nodal Input Data...

Select Application Region...

-Apply-

Main Index

Generates either a Static or Transient Input Data form, depending on the current Load Case Type selected. The Application Region is the piece of geometry or set of nodes or elements to which the loads or boundary condition is applied. Most Loads/BCs have a single region. However, options are provided for advanced users to define complex convection or radiation exchange between two application regions.

68

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

The following table outlines the options for creating MD Nastran thermal loads and boundary conditions: Object

Option

• Temp

Type

Target Element Type

Region 2

Nodal

--

--

Nodal

--

--

Nodal

--

--

Element Uniform

1D, 2D, 3D

--

Nodal

--

--

Element Uniform

1D, 2D, 3D

--

• Nodal Source

Nodal

--

--

• Volumetric

Element Uniform

1D, 2D, 3D

--

• Total Heat

Element Uniform

1D, 2D, 3D

• To Ambient

Nodal

--

--

Element Uniform

1D, 2D, 3D

--

Element Uniform

1D

--

Nodal

--

Nodal

Element Uniform

1D, 2D, 3D

Nodal, 1D, 2D, 3D

• Coupled Flow Tube

Element Uniform

1D

Nodal, 1D, 2D, 3D

• Coupled Advection

Element Uniform

1D, 2D, 3D

1D

• Duct Flow

Element Uniform

1D

2D, 3D

• Ambient Space

Nodal

--

--

Element Uniform

1D, 2D, 3D

--

Nodal

--

Nodal

Element Uniform

1D, 2D, 3D

Nodal 1D, 2D, 3D

Nodal

--

--

Element Uniform

1D, 2D, 3D

--

Element Uniform

1D, 2D, 3D

(Thermal) • Initial

Temperature • Applied Heat

• Normal Fluxes

Element Variable • Directional Fluxes

Generation • Convection

• Flow Tube To

Ambient • Coupled

• Radiation

• Ambient Nodes

• Enclosures

• Contact

• Deformable • Rigid Body

Main Index

Chapter 3: Building A Model 69 Loads and Boundary Conditions

Input Data Forms--Basic and Advanced Options Many of the input data forms have a Basic format and an Advanced format. The default is the Basic format, but you can change the format to Advanced using the option menu at the top of the form. Many of the advanced forms contain a databox called Control Node ID. If an existing node is selected in this databox, the temperature at this node during the analysis is used as an implicit load multiplier, depending on the exact application. Another advanced option is the Film Node ID that appears on forms for defining convection boundary conditions. This option allows an existing node to be selected. The temperature of this node during the analysis is used to define the temperature of the fluid used in determining the temperature-dependent fluid material properties involved in the calculation of the convection heat transfer coefficient.

Main Index

70

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Two Application Regions Two application regions provide advanced options for convection and radiation boundary conditions with complex exchange mechanisms. Application Region 1 defines a convecting or radiating surface, while Application Region 2 specifies a set of nodes to which the heat is transferred.

Select Application Region Geometry Filter u Geometry uu

Defines the coupling methods of two application regions. The Patran MD Nastran Thermal Application Preference ignores this option and always applies a closest approach algorithm to associate the companion region with Application Region 1.

FEM

Order:

Selection

Application Region Select Geometry Entities

Add

Selects geometry or finite element entities by graphical picks or text input to the databox.

Remove

Application Region

Adds geometry or finite element entities to the activated Application Region. Removes geometry or finite element entities from the activated Application Region.

Surface 1

Active List

Activates the selection of Application Region 1.

Companion Region Surface 2.4

Active List

Activates the selection of Application Region 2.

OK Note:

Main Index

When applying any of the convection or radiation forms involving two application regions, both regions must use the same geometry filter.

Chapter 3: Building A Model 71 Loads and Boundary Conditions

Surface Area The total amount of heat radiated or convected from a surface or input from a heat source depends on the area of the surface. For nodal loads and boundary conditions, the nodal area must be defined explicitly. For faces of 2D or 3D elements, the area is calculated from the relative locations of the nodal points. For the edge of a shell element, the area is calculated from the nodal points location and the shell thickness. For general or tapered beam elements, the rod element, or the curved beam with general section, the area is calculated as: ( 4. • π • cross_sectional_area ) • beam_length

For the rod or curved beam with pipe section, the area is calculated as: 2 • π • radius • beam_length

For directional flux or radiation enclosure on 1D elements, the Patran MD Nastran forward translator will automatically calculate the projected area based on the normal vector specified for the given elements. Spatial Dependence Many of the quantities defined on the Loads/BCs forms are allowed to vary as a function of the model’s spatial coordinates. This variation is described by first defining a spatial field using the Fields application and then selecting this field from the Spatial Fields listbox on the Loads/BCs Input Data form. Creation of spatial fields is described in more detail in Fields Forms (p. 210) in the Patran Reference Manual. Temperature Dependence Many of the quantities defined on the Loads/BCs forms are also allowed to vary as a function of temperature. An example is Convection Coefficient. The convection coefficient can take on different values depending on the surface or fluid temperatures at each point in the model. All quantities that are allowed to vary as a function of temperature have a second databox on the Loads/BCs Input Data form with the *Temperature Function label above it. This indicates that the temperature function multiplies the value in the databox to its immediate left (this value may be a constant or may come from a spatial field). Functions of temperature are described by defining a temperature-dependent field in the Fields application. To create this Field, you must set the Object to Material Property. You may then select the created field from the Temperature Dependent Fields listbox on the Loads/BCs Input Data form. For convenience, if you have specified a temperature-dependent function but do not specify any value in the far left column, Patran will assign a default value of 1.0 to that databox. Time Dependence When the Current Load Case is Time Dependent (set from the Load Cases application), a time-dependent field listbox appears on the far right column of the Loads/BCs Input Data form. This column contains databoxes that allow the time dependence of the quantities in the far left column of the Input Data form to be defined. Just as for spatial and temperature dependencies, you must first create a time dependence in the Fields application. To create the field in the Fields application, you must set the Object to Non

Main Index

72

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Spatial and the Method to Tabular Input. You must also define a set of time-load multiplier pairs. This field can then be selected from the Time Dependent Fields listbox on the Loads/BCs Input Data form. For convenience, if you have specified a time-dependent function but do not specify any value in the far left column, Patran will assign a default value of 1.0 to that databox.

Main Index

Chapter 3: Building A Model 73 Loads and Boundary Conditions

Temp(Thermal) Forms associated with the Temp(Thermal) Object allow you to define nodal temperatures that remain constrained during the analysis. The Temp(Thermal) Input Data forms for steady-state (Static) and transient (Time Dependent) load cases are shown below.

Main Index

74

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Input Data In a steady-state analysis, you may input a constant value or select a previously created Spatial Field that defines the temperature as a function of location in the model.

Boundary Temperature

Spatial Fields spatial_fld1 spatial_fld2

In a transient analysis, in addition to the constant value or Spatial Field, you may also select a previously created Time Dependent Field that describes how the temperature changes as an explicit function of time.

Reset OK

Cancel

Input Data Boundary Temperature

*Time Function

Spatial Fields

Time Dependent Fields

spatial_fld1 spatial_fld2

time_fld1 time_fld2

OK

Main Index

Reset

Cancel

Chapter 3: Building A Model 75 Loads and Boundary Conditions

The input option is described in the table below. Input Data

Dependence

Boundary Temperature

spatial, time

Description Defines temperature boundary conditions.

Initial Temperature Initial temperature is required in a time-dependent analysis. In a nonlinear steady-state analysis, initial temperatures are input as an initial guess to improve the convergence rate and often to provide initialization for the nonlinear iterative solution scheme. As a user convenience, if most of the initial nodal temperatures are to be the same, you can define this temperature using the Default Init Temperature databox in the Solution Parameters form invoked from the Analysis application. Any initial temperatures defined using this Initial Temperature option in Loads/BCs will take precedence over the default value defined in the Analysis application. The Input Data form for Initial Temperature is very similar to the form for steady-state temperature shown above. The input option is described in the table below. Input Data Initial Temperature

Main Index

Dependence spatial

Description Defines initial condition temperatures for transient analysis. May also be used to define an initial guess in a nonlinear steady-state analysis.

76

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Applied Heat--Normal Fluxes This option applies a heat flux either to nodes or elements on the surface of a body. Input Data Form Type:

If the Form Type is toggled from Basic to Advanced Node ID databox appears.

Advanced

Surface Option:

Top

Top Surf Heat Flux

For 2D elements, the heat flux can be applied to the bottom, or edge of the surface.

Control Node ID

Spatial Fields

Reset OK

Cancel

The following table describes the options for defining a heat flux. Input Data Heat Flux

Dependence spatial, time

Description Defines a heat flux.

[Top Surf, Bottom Surf, spatial, time Edge] Heat Flux

When the Target Element Type on the main form is set to 2D, this databox appears to define a heat flux applied on the top, bottom, or edge of a boundary surface.

Nodal Area

--

Appears only when the LBC type is Nodal. Defines the area of a boundary surface associated with the node.

Control Node ID

--

An advanced option that defines a control node. See Input Data Forms--Basic and Advanced Options, 69.

Main Index

Chapter 3: Building A Model 77 Loads and Boundary Conditions

Applied Heat--Directional Fluxes This option applies a thermal vector flux from a distant source onto the surface of a body. Steady-StateAnalysis

Figure 3-4 Input Data Form Type: Absorptivity

Basic

* Temperature Function

Heat Flux

Incident Thermal Vector <

When the load type is Nodal or the target element type is 1D, you must specify a vector defining the “surface normal.”

>

Normal Vector <

>

Nodal Area

Spatial Fields

OK

Main Index

Temperature Dependent Fields

Reset

Cancel

When the load type is Nodal, you must specify the area associated with the node.

78

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Transient Analysis For a time-dependent load case, the Input Data form with the Form Type changed from Basic to Advanced and the Thermal Vec Type changed to Transient is shown below. Input Data Surface Option:

Top

Top Surf Absorptivity

Form Type:

Advanced

Thermal Vec Type: Transient

* Temperature Function

Top Surf Heat Flux

* Time Function

Incident Thermal Vector

DirCos e1(t) of Thermal Vec

<

> Control Node ID

DirCos e2(t) of Thermal Vec

DirCos e3(t) of Thermal Vec

Spatial Fields

Temperature Dependent Fields

Time Dependent Fields

temp_fld1 temp_fld2

time_fld1 time_fld2

OK

Reset

Cancel

Incident Thermal Vector The incident thermal vector defines the direction from the surface to the heat source. In steady-state analysis, you may use any of the standard Patran vector tools to define this vector. In a transient analysis, two options are available and controlled with the Thermal Vec Type menu: 1. If only the magnitude of the heat flux changes as a function of time in the analysis, you may choose Thermal Vec Type Constant and select a previously defined field in the * Time Function databox to describe this change. 2. If the direction of the vector also changes as a function of time, the Thermal Vec Type menu must be set to Transient. The form changes to display three databoxes titled DirCos ei(t) of Thermal Vec. Separate time-dependent fields can be selected for these three boxes to define the change of direction as a function of time.

Main Index

Chapter 3: Building A Model 79 Loads and Boundary Conditions

The following table describes the options for the forms shown on page 77 through page 78. Input Data

Dependence

Description

Absorptivity

spatial, temp

Defines the absorptivity of the surface.

[Top Surf, Bottom Surf, Edge] Absorptivity

spatial, temp

When the target element type is 2D, a toggle and databox appear to define the absorptivity of the top, bottom, or edge of a boundary surface.

Heat Flux

spatial, time

Defines the heat flux quantity.

[Top Surf, Bottom Surf, Edge] Heat Flux

spatial, time

When the target element type is 2D, a toggle and databox appear to define a heat flux applied on the top, bottom, or edge of a boundary surface.

Incident Thermal Vector

--

Defines the fixed direction incident thermal vector.

DirCos e1(t) of Thermal Vec

time

Defines the time function of the direction cosine e1 of the incident thermal vector.

DirCos e2(t) of Thermal Vec

time

Defines the time function of the direction cosine e2 of the incident thermal vector.

DirCos e3(t) of Thermal Vec

time

Defines the time function of the direction cosine e3 of the incident thermal vector.

Normal Vector

spatial

When the load type is Nodal or the target element type is 1D, a vector defining the “surface normal” must be entered.

Nodal Area

--

When the load type is Nodal, the area associated with the node must be entered.

Control Node ID

--

An advanced option that defines a control node. See Input Data Forms--Basic and Advanced Options, 69.

Applied Heat--Nodal Source This option applies a heat flow directly to one or more nodes in the model. Input Data Nodal Source

Main Index

Dependence spatial, time

Description Defines the heat applied to the nodes.

80

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Applied Heat--Volumetric Generation This option defines a rate of heat generation within the volume of a conduction solid. This heat generation rate can be made a function of temperature by assigning a temperature field to the Heat Generation Multiplier option of the material associated with this solid. Input Data

Dependence

Description

Volumetric Heat Generation spatial, time

Defines the volumetric heat generation in conduction elements.

Control Node ID

An advanced option that defines a control node. See Input Data Forms--Basic and Advanced Options, 69.

--

Applied Heat--Total Heat This option defines a rate of heat generation within the volume of a conduction solid. This heat generation rate can be made a function of temperature by assigning a temperature field to the Heat Generation Multiplier option of the material associated with this solid. Input Data

Dependence

Description

Total Heat

spatial, time

Defines the total heat (power) applied to a surface or element face. The total heat value given is divided by the total area of the application region (for surface entities). If the application region is geometry, then the value displayed graphically on the geometry is the actual given value. If the application region is FEM (or Geometry, but displayed on the associated FEM) then the value displayed is the given value divided by the total area of the application region. This is the value that will be written to the MD Nastran QBDY3 entry.

Control Node ID

--

An advanced option that defines a control node. See Input Data Forms--Basic and Advanced Options, 69.

Main Index

Chapter 3: Building A Model 81 Loads and Boundary Conditions

Convection--To Ambient This option allows for the definition of the most basic form of convection boundary condition. Heat is exchanged between the surface of the body and a surrounding media, the temperature of which is known. The form for a steady-state load case and 2D element type are shown below.

Input Data Surface Option:

Form Type:

Top

Top Surf Convection Coef

Advanced

* Temperature Function

Ambient Temperature

Reference Temperature Option u

Formula Type Option u

q=h(Ts-Ta)**EXPF*(Ts-Ta)

uu q=h(Ts**EXPF-Ta**EXPF)

Average Temp (Ts+Ta)/2

uu Surface Temp (Ts) uu Ambient Temp (Ta) uu Film Temperature

Convection Exponent (EXPF)

Spatial Fields

OK

Main Index

Temperature Dependent Fields

Reset

Cancel

82

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

The options for this convection boundary condition are shown in the table below. Input Data

Dependence

Description

Convection Coefficient

spatial, temp, time

Defines free convection heat transfer coefficient.

[Top Surf, Bottom Surf, Edge] Convection Coeff

spatial, temp, time

When the target element type is 2D, a toggle and databox appear to define the free convection heat transfer coefficient of the top, bottom, or edge of a boundary surface.

Ambient Temperature

time

Defines ambient temperature.

Nodal Area

--

When the LBC type is Nodal, this databox appears to define the area of the boundary surface.

Formula Type Option

--

An advanced option for defining a customized form of the free convection formula: q = h (Ts-Ta)(expf+1) or q = h (Tsexpf - Taexpf) By default, the first form is chosen with EXPF equal 0.0.

Convection Exponent

--

An advanced option for defining EXPF in the above equation.

Reference Temperature Option

--

An advanced option for defining the temperature used in calculating the convection coefficient. The options are: average of surface and ambient temperatures, surface temperature, ambient temperature, or temperature at a userdefined node. By default, this reference temperature is taken as the average of surface and ambient temperatures.

Film Node ID

--

An advanced option for selecting an existing node for fluid film temperature.

With MSC.Nastran Version 68, the Patran MD Nastran Forward Translator will average the values for Surface Temp (Ts) and Ambient Temp (Ta) to acquire the Average Temp (Ts+Ta)/2. Average Temp will be used as the temperature at which the temperature dependent heat transfer coefficient will be determined. Convection--Flow Tube To Ambient Two basic heat transport mechanisms take place when the Flow Tube element is used. The first involves the transport of heat in the streamwise direction from the upstream fluid elements to the downstream fluid elements. We refer to this as heat transport due to advection. The second heat transfer mechanism involves heat transport into or out of the working fluid along the fluid tube boundary. We refer to this as heat transfer due to forced convection. The transport of heat energy by advection is a function of the mass flow rate (mdot) and the specific heat of the fluid. In the typical case we can ignore the small amount of heat transfer resulting from conduction in the fluid1; energy is then transported at the rate: mdot * Cp * T. The heat transfer at the stream tube 1 MD Nastran does not ignore the component of heat transfer in the fluid due to conduction.

Main Index

Chapter 3: Building A Model 83 Loads and Boundary Conditions

boundary, then, must be equal to (mdot * Cp * T)in - (mdot * Cp * T)out, where in and out refer to the inlet and exit states of the fluid stream. Typically, the inlet temperature is specified and the exit temperature is determined as part of the solution. The forced convection part of the problem allows the fluid stream tube to communicate with the surrounding environment. You can determine the heat transfer coefficient for a particular problem externally, or use the generalized correlations available through the preference and MD Nastran heat transfer solver. The particular application has a lot to do with the viability of either approach. A practical example of the use of Flow Tube to Ambient is the situation of analyzing a flow tube in a free stream of large mass flow and essentially constant temperature. A flow tube in an automobile radiator is a good example where the flow tube models the flow stream in the tubing (engine coolant) and the ambient environment is that of the air rushing across the tubes at the local air temperature. Physical Model

Flow out

Flow in

Ambient Flow Stream At Temperature T∞ = Constant

Finite Element Representation Forced convection resistance T∞

1 Res = ------hA

. m cp

Tin

Main Index

Tout

84

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

The Input Data form for a transient load case is shown below.

Input Data Form Type:

Advanced

Mass Flow Rate

* Time Function

Ambient Temperature

* Time Function

Heat Transfer Coefficient

Reference Temperature Option uu

Average Temp (Ts+Ta)/2

Formula Type Option

uu

u

h=coef*Re**Expr*Pr**Expp

uu

Surface Temp (Ts) Ambient Temp (Ta)

uu

h=k/d*coef*Re**Expr*Pr**

u

Reynolds Exponent

Film Temperature

Film Node ID

Prandtl Exponent, Heat In Time Dependent Fields Prandtl Exponent, Heat Out

OK

time_fld1 time_fld2

Reset

Cancel

The following table describes the options for defining this convection boundary condition. Input Data

Dependence

Description

Mass Flow Rate

time

Defines mass flow rate within the flow tube element.

Ambient Temperature

time

Defines ambient temperature.

Heat Transfer Coefficient

--

Defines the constant coefficient used for forced convection. A default value 1.e-20 will be defined if this data is not specified.

Main Index

Chapter 3: Building A Model 85 Loads and Boundary Conditions

Input Data Formula Type Option

Dependence --

Description An advanced option to define forced convection formula type: h=coef*Reexpr*Prexpp or h=coef*Reexpr*Prexpp*k/d By default, the first form is chosen with EXPR and EXPP equal to 0.0.

Reynolds Exponent

--

An advanced option to define the Reynolds number convection exponent EXPR.

Prandtl Exponent, Heat In

--

An advanced option to define the Prandtl number convection exponent EXPPI for heat transfer into the working fluid.

Prandtl Exponent, Heat Out

--

An advanced option to define the Prandtl number convection exponent EXPPO for heat transfer out of the working fluid.

Reference Temperature Option

--

An advanced option for defining the temperature used in calculating material properties for the fluid. The options are: average of surface and ambient temperatures, surface temperature, ambient temperature, or temperature at a userdefined node. By default, this reference temperature is taken as the average of surface and ambient temperatures.

Film Node ID

--

An advanced option for selecting an existing node for fluid film temperature.

With MSC.Nastran Version 68, the Patran MD Nastran Forward Translator will average the values for Surface Temp (Ts) and Ambient Temp (Ta) to acquire the Average Temp (Ts+Ta)/2. Average Temp will be used as the temperature at which the temperature dependent heat transfer coefficient will be determined. Convection--Coupled This advanced option for applying a convection boundary condition allows for the explicit definition of the convecting surface (Application Region 1) and a set of nodes (Application Region 2) between which heat is exchanged by convection. Mathematically, the exchange mechanism is similar to that for Convection to Ambient, except here Application Region 2 may be something other than basic ambient fluid points and their temperatures need not be specified in the description of the problem. The temperatures in Application Region 2 may be part of the solution. In addition, there does not need to be

Main Index

86

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

a one-to-one correspondence between nodal points in Region 1 and those in Region 2. The Input Data form for a steady-state load case is shown below.

Input Data Form Type: Advanced Convection Coefficient

* Temperature Function

Reference Temperature Option

u Average Temp (Ts+Ta)/2 uu Surface Temp (Ts)

Formula Type Option

u

uu Ambient Temp (Ta) uu Film Temperature

q=h(Ts-Ta)**EXPF*(Ts-Ta)

uu q=h(Ts**EXPF-Ta**EXPF)

Application Region 2

Convection Exponent (EXPF)

Spatial Fields

OK

Temperature Dependent Fields

Reset

Cancel

Application Region 1

The input options for coupled convection are shown in the table below. Input Data

Dependence

Description

Convection Coefficient

spatial, temp, time

Defines free convection heat transfer coefficient.

[Top Surf, Bottom Surf, Edge] Convection Coeff

spatial, temp, time

When the target element type is 2D, a toggle and databox appear to define the free convection heat transfer coefficient of the top, bottom, or edge of a boundary surface.

Nodal Area

--

When the LBC type is Nodal, this databox appears to define the area of the boundary surface.

Main Index

Chapter 3: Building A Model 87 Loads and Boundary Conditions

Input Data Formula Type Option

Dependence --

Description An advanced option for defining a customized form of the free convection formula: q = h (Ts-Ta)(expf+1) or q = h (Tsexpf - Taexpf) By default, the first form is chosen with EXPF equal 0.0.

Convection Exponent

--

An advanced option for defining EXPF in the above equation.

Reference Temperature Option

--

An advanced option for defining the temperature used in calculating the convection coefficient. The options are: average of surface and ambient temperatures, surface temperature, ambient temperature, or temperature at a userdefined node. By default, this reference temperature is taken as the average of surface and ambient temperatures.

Film Node ID

--

An advanced option for selecting an existing node for fluid film temperature.

With MSC.Nastran Version 68, the Patran MD Nastran Forward Translator will average the values for Surface Temp (Ts) and Ambient Temp (Ta) to acquire the Average Temp (Ts+Ta)/2. Average Temp will be used as the temperature at which the temperature dependent heat transfer coefficient will be determined. Convection--Coupled Flow Tube This is an advanced extension of the Convection, Flow Tube to Ambient boundary condition. In this application, the advection flow tube is attached to nodal points associated with a structure as opposed to simply an ambient environment. The flow tube in this application transports energy downstream in the mdot * Cp * T sense. Flow tube relations related to forced convection heat transfer at the tube boundaries are associated with this model. In this case, the convection area is the area associated with the flow tube perimeter, and it is the user’s responsibility to coordinate this area with that of the attached structure. It is important to realize that if the flow tube relationships are used (as opposed to a user-supplied h), the

Main Index

88

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

tube input diameters are used in the calculation of the Reynolds number and subsequently in calculating the heat transfer coefficient.

Application Region 1 (Flow Tube) mdot

1 Res = ------hA Convection Resistance

Application Region 2 (Structure)

When this capability is applied, there must be general correspondence (one flow tube element for every structural element grid point pair) between the flow tube node points in Application Region 1 and the

Main Index

Chapter 3: Building A Model 89 Loads and Boundary Conditions

structural node points in Application Region 2. The Input Data form for a steady-state load case is shown below.

Input Data Form Type: Advanced Mass Flow Rate

Heat Transfer Coefficient

Reference Temperature Option u

Average Temp (Ts+Ta)/2

Formula Type Option

uu

Surface Temp (Ts)

u

uu

Ambient Temp (Ta)

uu

Film Temperature

uu

h=coef*Re**Expr*Pr**Expp h=k/d*coef*Re**Expr*Pr**

Reynolds Exponent

Prandtl Exponent, Heat In

Prandtl Exponent, Heat Out

OK

Reset

Cancel

The input options for coupled flow tube convection are described in the table below. Input Data

Dependence

Description

Mass Flow Rate

time

Defines mass flow rate in the Flow Tube element.

Heat Transfer Coefficient

--

Defines the constant coefficient used for forced convection. A default value 1.e-20 will be defined if this data is not specified.

Main Index

90

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Input Data Formula Type Option

Dependence --

Description An advanced option to define forced convection formula type: h=coef*Reexpr*Prexpp or h=coef*Reexpr*Prexpp*k/d By default, the first form is chosen with EXPR and EXPP equal to 0.0.

Reynolds Exponent

--

An advanced option for defining the Reynolds number convection exponent EXPR in the above equation.

Prandtl Exponent, Heat In

--

An advanced option for defining the Prandtl number convection exponent EXPPI for heat transfer into the working fluid.

Prandtl Exponent, Heat Out

--

An advanced option for defining the Prandtl number convection exponent EXPPO for heat transfer out of the working fluid.

Reference Temperature Option

--

An advanced option for defining the temperature used in calculating material properties for the fluid. The options are: average of surface and ambient temperatures, surface temperature, ambient temperature, or temperature at a userdefined node. By default, this reference temperature is taken as the average of surface and ambient temperatures.

Film Node ID

--

An advanced option for selecting an existing node for fluid film temperature.

With MSC.Nastran Version 68, the Patran MD Nastran Forward Translator will average the values for Surface Temp (Ts) and Ambient Temp (Ta) to acquire the Average Temp (Ts+Ta)/2. Average Temp will be used as the temperature at which the temperature dependent heat transfer coefficient will be determined. Convection--Coupled Advection This advanced option enables the connection between an advection stream and a structural surface. For this capability, the forced convection tube relationships are essentially turned off by setting the constant coefficient for forced convection to 1.E-20. The convection connection between the flow stream and the surface is determined from basic convection; Q = h * A * (T1 - T2). Here the internally calculated area A is the area associated with the structural surface elements. The user must specify the value of the heat transfer coefficient, h. In steady-state analysis, the flow tube diameters are of little consequence for this capability since no Reynolds Numbers or heat transfer coefficients are determined internally. In transient analysis, the fluid speed needs to be produced by the correct choice of fluid properties and tube diameter. There need not be any particular correspondence between the nodes on the flow tube and those on the

Main Index

Chapter 3: Building A Model 91 Loads and Boundary Conditions

surface elements; Patran uses a closest approach algorithm to associate the surface elements with the stream tube elements. The Input Data form for a steady-state load case is shown below.

Input Data Form Type: Advanced * Temperature Function

Convection Coefficient

Mass Flow Rate

Reference Temperature Option u

Average Temp (Ts+Ta)/2

Formula Type Option

uu

Surface Temp (Ts)

u

uu

Ambient Temp (Ta)

uu

Film Temperature

q=h(Ts-Ta)**EXPF*(Ts-Ta)

uu q=h(Ts**EXPF-Ta**EXPF)

Convection Exponent (EXPF)

Spatial Fields

OK

Main Index

Temperature Dependent Fields

Reset

Cancel

92

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

T = 0.0

Res → ∞

Flow Tube

1 Res = ------hA

In MD Nastran terms, the flow tube ambient points are brought together and set to 0.0 degrees temperature. The forced convection resistance is set to a large number (negligible heat transfer coefficient). The connection between the fluid and structure is affected through basic convection with a user-specified heat transfer coefficient. The input options are described in the table below. Input Data

Dependence

Description

Convection Coefficient

spatial, temp, time

Defines free convection heat transfer coefficient.

[Top Surf, Bottom Surf, Edge] Convection Coeff

spatial, temp, time

When the target element type is 2D, a toggle and databox appear to define the free convection heat transfer coefficient of the top, bottom, or edge of a boundary surface.

Mass Flow Rate

time

Defines the mass flow rate of the flow tube elements.

Nodal Area

--

When the LBC type is Nodal, this databox appears to define the area of the boundary surface.

Main Index

Chapter 3: Building A Model 93 Loads and Boundary Conditions

Input Data Formula Type Option

Dependence --

Description An advanced option for defining a customized form of the free convection formula: q = h (Ts-Ta)(expf+1) or q = h (Tsexpf - Taexpf) By default, the first form is chosen with EXPF equal 0.0.

Convection Exponent

--

An advanced option for defining EXPF in the above equation.

Reference Temperature Option

--

An advanced option for defining the temperature used in calculating the convection coefficient. The options are: average of surface and ambient temperatures, surface temperature, ambient temperature, or temperature at a userdefined node. By default, this reference temperature is taken as the average of surface and ambient temperatures.

Film Node ID

--

An advanced option for selecting an existing node for fluid film temperature.

With MSC.Nastran Version 68, the Patran MD Nastran Forward Translator will average the values for Surface Temp (Ts) and Ambient Temp (Ta) to acquire the Average Temp (Ts+Ta)/2. Average Temp will be used as the temperature at which the temperature dependent heat transfer coefficient will be determined. Convection--Duct Flow This feature enables the user to associate a 1D fluid stream with a surface or duct composed of 2D or 3D (shell or solid) elements. When specifying the duct flow attributes, the target element type is 1D and the region-2 specification will be 2D or 3D. It would be good modeling practice to provide flow stream element discretization level of approximately the same level as the adjoining structure with respect to the streamwise direction. Fluid connections can only be made between the flow tube and 3 noded triangular elemental surfaces or 4 noded quadrilateral elemental surfaces. The structural surface may represent a physically more complex geometry composed of surface fins. The increased area associated with extended surfaces can be accounted for in duct flow by using the Extended Surface Multiplier on the Input Data menu. The actual convection surface area will equal the area calculated by the code from the elemental areas times this surface multiplier. On this same menu, mass flow rate refers to the duct mass flow rate (total flow). The proper treatment of the heat transfer coefficient relationship depends on the input for the flow tube diameters, defined in this application as the hydraulic diameters (DH). The flow tube hydraulic diameter is the dimension used in internally calculating the Reynolds Number. It will also automatically be used as the diameter in the Input Data, Formula Type Option equation for the heat transfer coefficient. With this formulation, the advection flow heat transfer coefficient is based on the gross dimensions of the structure and is input to the code through the input of hydraulic diameter. It is the user’s responsibility to determine an appropriate DH. The mass flow rate and fluid material properties represent the actual

Main Index

94

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

total/real flow characteristics for the duct. The actual elemental surface area flow attachment is accounted for internally through the triangle and quadrilateral surface element area calculations and may be enhanced by the extended surface multiplier to represent a finned surface.

Input Data Mass Flow Rate

* Time Function

Heat Transfer Coefficient

Reference Temperature Option Average Temp (Ts+Ta)/2 Surface Temp (Ts)

Extended Surface Multiplier

Ambient Temp (Ta) Film Temperature

Formula Type Option h=coef*Re**Expr*Pr**Expp

Film Node ID

h=k/d*coef*Re**Expr*Pr** Reynolds Exponent Prandtl Exponent, Heat In

Time Dependent Fields

Prandtl Exponent, Heat Out

OK

Reset

Input Data

Dependence

Cancel

Description

Mass Flow Rate

time

Defines mass flow rate in the Flow Tube element.

Heat Transfer Coefficient

--

Defines the constant coefficient used for forced convection. A default value 1.e-20 will be defined if this data is not specified.

Extended Surface Multiplier

--

Defines extended area factor for surface fins.

Main Index

Chapter 3: Building A Model 95 Loads and Boundary Conditions

Input Data Formula Type Option

Dependence --

Description An advanced option to define forced convection formula type: h=coef*Reexpr*Prexpp or h=coef*Reexpr*Prexpp*k/d By default, the first form is chosen with EXPR and EXPP equal to 0.0.

Reynolds Exponent

--

An advanced option for defining the Reynolds number convection exponent EXPR in the above equation.

Prandtl Exponent, Heat In

--

An advanced option for defining the Prandtl number convection exponent EXPPI for heat transfer into the working fluid.

Prandtl Exponent, Heat Out

--

An advanced option for defining the Prandtl number convection exponent EXPPO for heat transfer out of the working fluid.

Reference Temperature Option

--

An advanced option for defining the temperature used in calculating material properties for the fluid. The options are: average of surface and ambient temperatures, surface temperature, ambient temperature, or temperature at a userdefined node. By default, this reference temperature is taken as the average of surface and ambient temperatures.

Film Node ID

--

An advanced option for selecting an existing node for fluid film temperature.

Main Index

96

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Radiation--Ambient Space This option defines a boundary condition for a surface exchanging radiant energy with an ambient temperature in space. The Input Data form for 3D element types is shown below. Input Data

Emissivity

* Temperature Function

Absorptivity

* Temperature Function

Ambient Temperature

View Factor

Spatial Fields

Temperature Dependent Fields

OK

Input Data

Reset

Dependence

Cancel

Description

Emissivity

spatial, temp

Defines surface emissivity.

[Top Surf, Bottom Surf, Edge] Emissivity

spatial, temp

When the target element type is 2D, a toggle and databox appear to define the emissivity of the top, bottom, or edge of a boundary surface.

Absorptivity

spatial, temp

Defines surface absorptivity.

[Top Surf, Bottom Surf, Edge] Absorptivity

spatial, temp

When the target element type is 2D, a toggle and databox appear to define the absorptivity of the top, bottom, or edge of a boundary surface.

Ambient Temperature

time

Defines ambient temperature.

Main Index

Chapter 3: Building A Model 97 Loads and Boundary Conditions

Input Data

Dependence

Description

View Factor

spatial, time

Defines radiation view factor between the surface and the ambient space. The default value is 1.0.

Nodal Area

--

When the LBC type is Nodal, this databox appears to define the area of the boundary surface.

Radiation--Ambient Nodes This is an advanced option for applying a radiation boundary condition to a surface. You select both the surface (Application Region 1) and a set of nodes that define the temperature to which the surface is exchanging heat by radiation (Application Region 2). Input Data

Dependence

Description

Emissivity

spatial, temp

Defines surface emissivity.

[Top Surf, Bottom Surf, Edge] Emissivity

spatial, temp

When the target element type is 2D, a toggle and databox appear to define the emissivity of the top, bottom, or edge of a boundary surface.

Absorptivity

spatial, temp

Defines surface absorptivity.

[Top Surf, Bottom Surf, Edge] Absorptivity

spatial, temp

When the target element type is 2D, a toggle and databox appear to define the absorptivity of the top, bottom, or edge of a boundary surface.

View Factor

spatial, time

Defines radiation view factor between the surface and the ambient nodes. The default value is 1.0.

Nodal Area

--

When the LBC type is Nodal, this databox appears to define the area of the boundary surface.

Main Index

98

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Radiation--Enclosures This option defines a radiation boundary among a set of surfaces making up a cavity or enclosure. Each surface is defined independently using the form below. The surfaces are grouped to form an enclosure by specifying the same Enclosure ID (integer) on all surfaces making up the enclosure. Input Data Enclosure ID Emissivity

* Temperature Function

Surface Can Shade

Third Body Shading

Surface Can Be Shaded

Complete Enclosure

Normal Vector <

>

Nodal Area

Spatial Fields

OK

Input Data

Temperature Dependent Fields

Reset

Dependence

Cancel

Description

Enclosure ID

--

Defines the ID number of the radiation enclosure.

Emissivity

spatial, temp

Defines surface emissivity.

[Top Surf, Bottom Surf, Edge] Emissivity

spatial, temp

When the target element type is 2D, a toggle and databox appear to define the emissivity of the top, bottom, or edge of a boundary surface.

Surface Can Shade

--

Specifies if the face can shade other faces in the enclosure (default=yes).

Surface Can Be Shaded

--

Specifies if the face can be shaded by other faces in the enclosure (default=yes).

Normal Vector

spatial

When the load type is Nodal or the target element type is 1D, a vector defining the “surface normal” must be entered.

Main Index

Chapter 3: Building A Model 99 Loads and Boundary Conditions

Input Data

Dependence

Description

Nodal Area

--

When the LBC type is Nodal, this databox appears to define the area of the boundary surface.

Third Body Shading

--

Controls third body shading calculation (default=yes). When set at “no,” third body shadowing calculations will be ignored.

Complete Enclosure

--

In an enclosure that is not fully closed, energy may be radiated to entities outside the enclosure. Toggling this option from “no” (default) to “yes” specifies that all energy not exchanged among the surfaces of the enclosure will be radiated to a user-defined ambient temperature. When creating an enclosure it is sometimes not feasible to model everything that will be generating or receiving heat from a model. The user models everything that is of interest, and then simply wants to close the remainder of the his model with a single ambient element that will allow his view factors to sum to 1.0. This is done with a RADCAV card and can be accomplished by selecting the complete enclosure toggle. The ambient temperature of the open space is then entered, and now the analysis is able to complete with a total view factor of 1.0.

Ambient Temperature

--

This databox appears when the Complete Enclosure option is toggled to “yes” and is used to define the external temperature to which energy is exchanged with the enclosure.

Cavity 1

Figure 3-5

Main Index

Multiple Cavity Example

Cavity 2

100

Patran Interface to MD Nastran Thermal Loads and Boundary Conditions

Can Be Shaded, but cannot shade

Figure 3-6

Main Index

Can Shade, but cannot be shaded (Third Body Shadowing) Single Cavity Example

Can Be Shaded, but cannot shade

Chapter 3: Building A Model 101 Load Cases

3.7

Load Cases Load cases in Patran enable you to group a series of load sets into one load environment for your model. Load cases are selected when defining an analysis job. The usage within MD Nastran is similar. Patran uses the selected load cases to create the necessary SUBCASE commands in the Case Control Section of the NASTRAN input file. For information on how to define multiple static and/or transient load cases, see Load Cases Application (Ch. 5) in the Patran Reference Manual.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

Main Index

© XY

102

Patran Interface to MD Nastran Thermal Load Cases

Main Index

Chapter 4: Running a Thermal Analysis Patran Interface to MD Nastran Thermal

4

Main Index

Running a Thermal Analysis

J

Introduction

J

Review of the Analysis Form

J

Translation Parameters

J

Solution Types

J

Direct Text Input

J

Subcases

J

Subcase Select

104

113 119

121 135

109

105

104

Patran Interface to MD Nastran Thermal Introduction

4.1

Introduction To run a thermal analysis, you use the procedure described below.

Select the solution type

The solution type can be either steady-state or transient analysis.

Define the solution related input data

The purpose of this step is to change the default settings of job-related input data, such as Maximum Run Time, Default Initial Temperature, Radiation Parameters, and options for view factor calculations.

Define the subcase data

Similar to the previous step, the defaults for nonlinear iteration controls, time increments, and output requests can be altered in the Subcase Create section of the Analysis menu form.

Select load cases

This step selects load case(s) for an analysis job.

Submit the job

When a job is ready for analysis, the MD Nastran solver can be retrieved by clicking on the Apply button on the main Analysis form. You can modify the default settings of translation parameters, or you can insert additional data entries using the Direct Text Input form before submitting your analysis job.

Read the analysis results

The analysis results must be read into the Patran database by invoking the Read Output2 Action on the Analysis form. The results can then be processed by selecting the Results toggle on the Patran application selections.

To submit a single load case, steady-state analysis job to MD Nastran, you need only click on the Apply button on the main Analysis form. Patran will automatically control the appropriate default settings and other related selections. In the Patran MD Nastran Interface, a subcase can be thought of as a Patran load case with some additional parameters (e.g., Output Requests) associated with it. This association is further strengthened since the default subcases are created for each load case and have the same name as their associated load case. In this document, the terms “load case” and “subcase” are used interchangeably. When a specific form is referenced, Load case and Subcase are capitalized.

Main Index

Chapter 4: Running a Thermal Analysis 105 Review of the Analysis Form

4.2

Review of the Analysis Form The Analysis form appears when you select Analysis from the main form. To run an analysis, or to create an NASTRAN input file, select Analyze as the Action on the Analysis form. Other forms brought up by the Analysis form are used to define translation parameters, solution types, solution parameters, output requests, and load cases. These forms are described on the following pages. For further information, see The Analysis Form (p. 8) in the MSC.Patran Reference Manual. Patran

File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

Main Index

© XY

106

Patran Interface to MD Nastran Thermal Review of the Analysis Form

Analysis Form This form appears when you select Analysis from the main menu. When preparing for an analysis run, select Analyze as the Action. Analysis

Analyze

Action: Object:

Entire Model

Method:

Analysis Deck

Code: MD Nastran Type:

Actions can be set to: Analyze Read Output2 (p. 125) Read Input File (p. 545) in the Patran Interface

to MD Nastran Preference Guide (support is limited for thermal analysis) Delete (Ch. 6) in the Patran Interface to MD Nastran Preference Guide Monitor (Ch. 5) in the Patran Analysis Manager User’s Guide Abort (Ch. 6) in the Patran Analysis Manager User’s Guide

Thermal

Available Jobs my_job Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual.

Job Name my_job Job Description MD Nastran job created on 01-Feb-93 at 14:32:43

Name of job. Patran will use this name as the base filename for all resulting MD Nastran files and message files.

List of already existing jobs. If you select one of these jobs, the name will appear in the Job Name listbox and all input data for this job will be retrieved from the database. You can submit an existing job again simply by selecting it and clicking on Apply. It is often convenient to select an existing job, modify the input data as desired, and click on Apply to submit the new job.

Main Index

Chapter 4: Running a Thermal Analysis 107 Review of the Analysis Form

Job Description MD Nastran job created on 01-Feb-93 at 14:32:43

Patran uses this text to generate the TITLE statement in the MD Nastran Executive Control Section.

Translation Parameters... Solution Type... Direct Text Input... Subcase Create...

Opens the Direct Text Input form; this form allows you to enter data directly for the File Management, Executive Control, Case Control, and Bulk Data sections of the NASTRAN input file.

Subcase Select... Analysis Manager...

Selects one or more subcases for the analysis job.

Opens the Patran Analysis Manager form.

Apply

Opens a form that allows you to choose either steadystate analysis or transient analysis and to specify settings for controlling the overall analysis job.

Main Index

108

Patran Interface to MD Nastran Thermal Review of the Analysis Form

The following table outlines the selections for the Analyze action. Object

Method

Entire Model

Full Run Check Run Analysis Deck Model Only

Current Group

Full Run Check Run Analysis Deck Model Only

Existing Deck

Full Run

The Object indicates which part of the model is to be analyzed. There are three choices for thermal analysis: Entire Model, Current Group, and Existing Deck. Entire Model

Indicates that the whole model is to be analyzed.

Current Group

Indicates that only part of the model is to be analyzed. To do this, you create a group of that part, confirm that it is the current group, then select Current Group as the Object. For more information, see The Group Menu (p. 262) in the Patran Reference Manual.

Existing Deck

Means that you wish simply to submit an existing input file to MD Nastran. To form the input filename, Patran appends the suffix “.bdf” to the jobname appearing in the Job Name listbox. This file must reside in the current directory.

The Method indicates how far the translation is to be taken.The methods are as follow: Full Run

Is the selected type if an Analysis Deck translation is performed, and the resulting input file is submitted to MD Nastran for complete analysis.

Check Run

Is the selected type if an Analysis Deck translation is performed, and the resulting input file is submitted to MD Nastran for a check run only.

Analysis Deck

Is the selected type if the Model Deck translation is performed, plus all load case, analysis type and analysis parameter data are translated. A complete input file, ready for MD Nastran, will be generated.

Model Only

Is the selected type if a Bulk Data file is created that contains only the model data including node, element, coordinate frame, element property, material property, and loads and boundary conditions data. The translation stops at that point.

Main Index

Chapter 4: Running a Thermal Analysis 109 Translation Parameters

4.3

Translation Parameters This subordinate form appears when you click on the Translation Parameters button on the Analysis form.

Defines the type of data output. “Print” specifies output of data to the MD Nastran print file (.f06). “OP2” specifies output of data to an MD Nastran OUTPUT2 file (.op2). “XDB” specifies output of data to an MSC.Access database (.xdb).

Translation Parameters Data Output Data Output:

OP2 and Print

OUTPUT2 Requests:

P3 Built In

OUTPUT2 Format:

Binary

Tolerances Division:

1.0e-08

Numerical:

1.0e-04

Writing:

1.0e-20

Specifies format of the MD Nastran OUTPUT2 (*.op2) files. Use “Text” format when the resulting OUTPUT2 file must be transported between heterogeneous computer platforms. Defines various tolerances used during translation. Division is used to prevent division-by-zero errors. Numerical is used to determine if two real values are equal. Writing is used to determine if a value is approximately zero when generating a Bulk Data entry field.

Bulk Data Format Card Format:

either

Minimum Signif. Digits:

4

Node Coordinates: MD Nastran Version:

reference frame 69

Write Properties on Element Entries Numbering Options... Bulk Data Include File... OK

Main Index

Defaults

Specifies type of OUTPUT2 commands. “P3 Built In” signals the use of MD Nastran internal OUTPUT2 commands geared toward Patran. These commands are also appropriate for PATRAN 2. “Alter File” specifies the use of an external alter file found on the Patran file path and following the “msc_v#_sol#.alt” naming convention. See Files (App. A) for more details. “CADA-X Alter” specifies the use of an LMS CADA-X specific alter file that is identical to the “Alter File” but with an additional “.lms” extension, e.g., “msc_v69_sol53.alt.lms”. “P2 Built In” specifies use of MD Nastran internal OUTPUT2 commands geared toward PATRAN 2.

Cancel

110

Patran Interface to MD Nastran Thermal Translation Parameters

Data Output OP2 and Print

Data Output:

P3 Built In

OUTPUT2 Requests:

Binary

OUTPUT2 Format: Tolerances Division:

1.0e-08

Numerical:

1.0e-04

Writing:

1.0e-20

Defines what type of fields are to be used in the Bulk Data entry. Entry format can be se to small, large, or either. If either is selected the Minimum Significant Digits value is use to determine whether the values on a particular Bulk Data entry can be placed in small fields or whether large fields are required. The small-field format consists of Bulk Data entry fields 8 columns wide; the large field format is 16 columns wide.

Bulk Data Format Card Format:

either

Minimum Signif. Digits:

4 reference frame

Node Coordinates: MD Nastran Version:

69

Brings up a subordinate form, Numbering Options, 111, which defines automatic numbering offsets and possible syntaxes fo encoded IDs.

Write Properties on Element Entries Numbering Options...

Brings up a standard file select form which allows you to select a file to be included in the Bulk Data Section of the NASTRAN inpu file.

Bulk Data Include File... OK

Defaults

Cancel

Writes CELAS2, CDAMP2, and CONROD Bulk Data entries instead of CELAS1, CDAMP1, and CROD entries.

Note:

Do not turn ON this option if your model has time varying temperature boundary conditions or conductor/capacitor elements.

Defines which version of MD Nastran is to be used. The version indicated here serves two purposes: to create the full name of the ALTER file to be used and to determine which Solution Sequence to be used. Be sure to specify only whole numbers and letters; e.g., 68 or 69. Defines which coordinate frame is to be used when generating the grid coordinates. The options are reference frame, analysis frame, or global. This setting should not affect the analysis. It only changes the method used in the

Main Index

Chapter 4: Running a Thermal Analysis 111 Translation Parameters

Numbering Options Patran allows you to define numbering offsets for IDs associated with model entities. To invoke this feature, you click on the Numbering Options button on the Translation Parameters form. Numbering Options Automatic Numbering Offsets: Element Properties:

0

Material Properties:

0

Data Tables: s: Load Sets:

0

Load Cases:

0

Control Sets:

0

Rigid Elements:

0

Scalar Points:

0

Indicates offsets for all IDs to be automatically assigned during translation. For example, if you type 100 into the Element Properties Offset box, the numbering of element properties in the resulting NASTRAN input file will begin at 101.

0

Begin. Contin. Marker:

+

Specifies the continuation mnemonic format used on multiple line Bulk Data entries. Activates recognition of IDs encoded into the name of any named entry, such as a material.

A

IDs Encoded in Names: Recognizes and uses an ID if, and only if, the name of the entity is an actual number, such as “105.” This option is ON by default.

Number Only Beginning Number

Recognizes an ID if the number begins the name, such as “52_shell_property.” This option is OFF by default.

Trailing Number Encoded Syntax Syntax Marker:

OK

Recognizes an ID if it directly follows the first occurrence of the specified syntax. For example, with this option activated and the specified syntax set to “.”, the ID assigned to a material given the name “Steel_1027.32” would be 32.

.

Defaults

Cancel

Recognizes an ID if it tails the name, such as “shell_property_52.” This option is OFF by default.

Main Index

112

Patran Interface to MD Nastran Thermal Translation Parameters

Note that both the Patran Neutral file reader and the Patran MD Nastran input file reader preserve the IDS of named entities with a “.” syntax, so that an MD Nastran PSHELL entry of ID 12 will be assigned the name “PSHELL.12.” This last option allows great continuity between input model data and output model data. This option is ON by default, and the default Syntax Marker is “.” Note:

Main Index

“The Encoded IDs” option currently only works for element properties and material properties.

Chapter 4: Running a Thermal Analysis 113 Solution Types

4.4

Solution Types Three solution types are supported in the Patran MD Nastran thermal interface: steady state, transient, and linear structural. The two thermal (only) analysis types employ nonlinear solution algorithms so that nonlinear material properties or boundary conditions can be included in the model. The linear structural analysis type (STRUCTURAL HEAT ANALYSIS) performs first a linear steady-state thermal analysis (SOL 153), then it performs a linear structural analysis (SOL 101) using the results of the thermal analysis as loading on the structural model. Use the form shown below to select the solution type. By default, a steady-state thermal analysis is requested.

Performs linear or nonlinear steady-state thermal analysis usin MD Nastran Solution Sequence 153.

Performs linear or nonlinear transient thermal analysis using MD Nastran Solution Sequence 159.

Performs linear structurall analysis using MD Nastran Solution Sequence 101, and the temperature results from a linear steady-state thermal analysis.

Brings up a form that controls various settings that pertain to th overall analysis process.

Displays the MD Nastran Solution Sequence number.

Main Index

114

Patran Interface to MD Nastran Thermal Solution Types

Solution Parameters The solution parameter form contains options and subordinate forms for defining parameters that affect the overall analysis. The Subcase Parameter forms, described below, are used for setting input data that control the analysis only within a single subcase. You should always review the settings on both forms before submitting an analysis. Requests that the model singularities be constrained automatically. Select the Solution Sequence. If a static analysis is being performed (SOL 153) the choices are SOL 153, 400, or 600. If a transient analysis is being performed (SOL 159) the choices are SOL 159, 400, or 600. Controls whether or not the input file is printed to the Nastran output file (f06). Maximum number of lines to be written to the Nastran output file (f06). Maximum number of CPU minutes the analysis job is allowed to run. The job will terminate when this limit is reached.

Buttons to bring up subordinate forms for additional parameters needed for radiation analysis. Select this button to specify what is to be output from the analysis.

Defines the default initial temperature for all node points which have not been given an initial temperature by the Initial Temperature object of Loads/BCs.

Main Index

Chapter 4: Running a Thermal Analysis 115 Solution Types

Radiation Parameters Figure 4-1

The value of “absolute temperature scale” may be entered directly or selected from the menu.

The value of the Stefan-Boltzmann constant must be input in units that are consistent with the rest of the model definition. Values in several different combinations of units are available for selection in the menu, or you can enter the value directly.

View Factor Parameters This subordinate form defines parameters and output options to calculate view factors. For all the radiation enclosures selected, the Patran MD Nastran forward translator automatically enables the Gaussian integration view factor calculation method by applying the terminology defined here. A more detailed description of the calculation of view factors can be found in the MD Nastran Thermal Analysis User’s Guide.

Main Index

116

Patran Interface to MD Nastran Thermal Solution Types

Figure 4-2 Defines the view factor sum that the enclosure will be set to if the view factor summation of the enclosure is greater than 1.0. No scaling is performed if this databox is left blank.

View Factor Parameters Defines Gaussian integration order for calculating net effective view factors in the presence of third-body shading.

View Factor Scale = Gaussian Int Order (3rd Body Shading):

4

Gaussian Int Order (Self Shading):

4

Discretization Level =

4

Error Tolerance =

0.1

Assumed Level of Calculation =

1.0e-10

Assumed Degree of Warpage =

0.01

Defines Gaussian integration order for calculating net effective view factors in the presence of self shadowing.

Defines the discretization level used in the semi-analytic contour integration method.

Defines the assumed level of calculation below which the numbers are considered to be zero.

Defines the assumed degree of warpage above which the actual value of Fii will be calculated. (For a flat surface Fii = 0.0)

Defines the error tolerance above which a corrected view factor is calculated using the semi-analytic contour integration method.

NOTE: See the MD Nastran Thermal Analysis User’s Guide for a description of error estimators for view factor calculation.

Main Index

Chapter 4: Running a Thermal Analysis 117 Solution Types

Defines diagnostic output request options for the radiation exchange surfaces. The output will be written to the NASTRAN output (f06) file.

Diagnostic Output Requests Grid Table and Element Connectivity Surface Diagnostics View Factor Calculation Diagnostics Output Device Option:

OK

Both

Defaults

Cancel

Defines the output device options (Both, Print, Punch, None) for printing or punching view factors onto RADLST/RADMTX entries. The printed view factors are written to the NASTRAN output (f06) file, while the punched view factors are written to a punch file, job_name.pch. If the FEM mesh and the application regions of loads and boundary conditions are not changed in subsequent runs, the lengthy view factor calculations may be skipped by including the RADLST/RADMTX punch files, which can be retrieved from the Bulk Data Include File menu in the Translation Parameters form.

Solution Parameters for Transient Analysis Figure 4-3

Main Index

118

Patran Interface to MD Nastran Thermal Solution Types

Controls the printout of model singularities.

Solution Parameters Transient Solution Parameters

Controls whether or not the input filefile is printed to the NASTRAN output (f06) file.

Print Out Singularities Data Deck Echo:

None

Maximum Printed Lines =

999999999

Maximum Run Time =

600

Default Init Temperature =

0.0

Maximum number of lines to be written to the NASTRAN output (f06) file.

Maximum number of CPU minutes the analysis job is allowed to run. The job will terminate when this limit is reached.

Radiation Parameters... The radiation and view factor input data forms are identical to those shown above for steady-state analysis.

View Factor Parameters...

OK

Defaults

Cancel

Defines the default initial temperature for all grid points which have not been given an initial temperature by the Initial Temperature Object of Loads/BCs.

Main Index

Chapter 4: Running a Thermal Analysis 119 Direct Text Input

4.5

Direct Text Input This form allows you to enter entries directly in the File Management, Executive Control, Case Control, and Bulk Data sections of the NASTRAN input file. The input file reader1 also creates these entries for any unsupported entries in the input file. If the data is entered by the user, the Write to Input file toggle default setting is ON. If the data comes from the input file reader, the default for the Input file toggle is OFF. A good practice is to review and edit the MD Nastran input entries. If they should be written to any input files subsequently created by the interface, the appropriate Write to Input file toggle should be set to ON. Text entered into the Case Control section is written to the input file before the first subcase. The Direct Text Input option on the Subcase Create form should be used to enter text directly within a subcase definition.

1

Main Index

The current input file reader provides limited support for thermal analysis.

120

Patran Interface to MD Nastran Thermal Direct Text Input

Switches to determine which data section the MSC ⁄NASTRAN input would be sent.

Direct Text Input

Bulk Data Section

uu

File Management Section

FMS Write To Input Deck

uu

Executive Control Section

EXEC Write To Input Deck

uu

Case Control Section

CASE Write To Input Deck

u

Bulk Data Section

BULK Write To Input Deck

OK

Saves the current setting and data for the four sections and closes the form.

Main Index

Clear

Clears the current form.

Reset

Resets the form back to the data values it had at the last OK.

Cancel

Resets all four forms back to its previous value and closes the form.

Chapter 4: Running a Thermal Analysis 121 Subcases

4.6

Subcases This form appears when you select the Subcase Create button on the Analysis form. The subcase is the MD Nastran mechanism for associating loads and boundary conditions, output requests, and various other input data to be used during part of a complete run.

Main Index

122

Patran Interface to MD Nastran Thermal Subcases

The Patran MD Nastran interface automatically associates default parameters and output requests with each Patran load case to create a subcase with the same name as the load case. You can access the Subcase Parameters and Output Requests forms to view or modify these defaults. Subcase Create Solution Sequence: 153 Available Subcases Default Convection_Case Radiation_Case 100_BTU_Heat_Load

Displays all the available subcases associated with the current Solution Sequence.

Subcase Name

Displays the subcase name that is being created, modified, or deleted. You can type in the subcase name or pick it from the Available Subcases listbox.

Default Subcase Description This is the default subcase

Displays the description of the current subcase The description can be 256 characters long.

Available Load Cases Default Convection_Case Radiation_Case 100_BTU_Heat_Load

Displays all the available loadcases in the curr database. Only one loadcase can be selected subcase.

Subcase Options Subcase Parameters... Output Requests...

These buttons bring up subordinate forms for additional input associated with the subcase.

Direct Text Input...

Apply

Main Index

Delete

Cancel

Chapter 4: Running a Thermal Analysis 123 Subcases

Note about Structural Heat Analysis: • There can be only two subcases. • First subcase has only thermal Loads/BCs (Case Control LOAD and SPC entries) and thermal

Output Requests (Case Control THERMAL entry). • Second subcase has only structural Loads/BCs (Case Control LOAD and SPC entries) and

structural Output Requests (Case Control STRESS entry). The temperatures from the thermal analysis (first subcase) are a part of the structural Loads/BCs (Case Control TEMPERATURE(LOAD) = ID (ID of the first subcase) entry). • Both thermal (Bulk Data MAT4 entry) and structural (Bulk Data MAT1 entry) material

properties must exist. The IDs of the MAT4 and MAT1 entries must be equal. • PARAM, HEATSTAT, YES in written to the Bulk Data section to enable this type of analysis.

To set up and perform a chained thermal-structural analysis in one run using SOL 101. The procedure is to: 1. With Patran Preferences set to MD Nastran, Structural, create and set up your structural LBCs and load case 1. Change the Patran Preferences to MD Nastran, Thermal, create and set up your thermal LBCs and load case 1. Set the Solution Type to STRUCTURAL HEAT ANALYSIS 1. Set up two Subcases, one referencing the structural load case and the other referencing the thermal load case. 1. Select the two Subcases in the order: Thermal, Structural 1. Submit the job The Nastran run is submitted as a SOL 101 with two Subcases. The first subcase is the heat transfer run to determine the temperature loading. The temperature results from the first subcase are used along with any other structural LBCs called out in the second subcase, which is a SOL 101 run. PARAM, HEATSTAT, YES is written to the input file.

Subcase Parameters The controls and parameters set on the Subcase Parameters forms apply to a single MD Nastran subcase within the overall analysis run. Steady-State Subcase This subordinate form appears when the Subcase Parameters button is selected on the Subcase Create form and the solution type is Steady State. This form provides for the definition of the input data that controls the solution of the nonlinear equations. Occasionally, when solving a set of nonlinear equations, it may not be possible to obtain a solution directly with the total heat load applied. Instead, the solution is obtained by applying the loading in

Main Index

124

Patran Interface to MD Nastran Thermal Subcases

increments, solving the system equations for the current fraction of the total load, and using that solution as the starting point for the next increment of load. This process continues until the desired total heat load is applied. It should be mentioned that the number of load increments has no effect on the accuracy of the solution-- it is merely a computational technique to aid in obtaining the solution efficiently. In linear or mildly nonlinear problems, a single increment is usually applied. In highly nonlinear problems, dozens of increments may be required to obtain a converged solution. This incremental procedure is only applicable with respect to applied heat loads and specified temperature boundary conditions. There is no incremental provision for convection or radiation boundary

Main Index

Chapter 4: Running a Thermal Analysis 125 Subcases

conditions. As a result, it is more common with highly nonlinear boundary conditions to exceed the nonlinear iteration limit. This defaults to 25 currently, but can be increased.

Number of increments over which the heat load is applied.

These parameters control aspects of the nonlinear equation solving process. For more information, see table on page 127.

The convergence criteria are used to determine when the solution is sufficiently accurate to be considered “converged.” See page 127 for more information.

See the next page for the contact table form.

Main Index

126

Patran Interface to MD Nastran Thermal Subcases

Thermal Contact Table

This data can optionally be defined for each individual contact pair (which is selected by clicking on the cell of the above contact body matrix) and is written to the BCTABLE bulk data entry. See the MD Nastran Quick Reference Guide for more information.

Main Index

Chapter 4: Running a Thermal Analysis 127 Subcases

The parameters controlling the steady-state solution process are discussed more fully in the table below. More extensive information can be found in the MD Nastran Thermal Analysis User’s Guide. Parameter Name Matrix Update Method

This option determines the strategy used to determine how often to update (reform) the nonlinear conductance and radiation matrices. The three options are Automatic, Semi-Automatic, and Controlled Iters. The optimum strategy would result in the lowest computational cost. When the Automatic option is selected, MD Nastran tries to select the most efficient strategy based on convergence rates. If Controlled Iters is selected, the matrices are updated after a prescribed number of iterations (determined by the Number of Iterations per Update parameter).

Number of Iterations per Update

When the Matrix Update Method is set to Controlled Iters, this is the number of iterations before the matrices are reformed.

Allowable Iterations per Increment

This parameter specifies the maximum number of allowed iterations in a load increment. If this number is exceeded, the load increment is halved and the iteration process repeated.

Convergence Criteria

The convergence criteria provide for the comparison of userrequested maximum levels of error and the error in the solution as estimated numerically. In this sense, the convergence criteria determine when the solution is sufficiently accurate to be considered converged. Any or all of the three convergence criteria listed below can be selected. When more than one criteria is selected, each one must be satisfied for convergence to be achieved.

Temperature Error

Indicates whether a temperature convergence criterion should be used. If Temperature Error is selected, the Temperature Tolerance field becomes active. A norm of the temperature increment vector calculated in the iteration must be less than this tolerance for a converged solution.

Temperature Tolerance

Load Error Load Tolerance

Work Error Work Tolerance

Main Index

Description

Indicates whether a load convergence criteria should be used. If Load Error is selected, the Load Tolerance field becomes active. A norm of the residual heat load vector must be less than this tolerance for a converged solution. Indicates whether a work convergence criteria should be used. If Work Error is selected, the Work Tolerance field becomes active. The incremental work associated with the iteration must be less than this tolerance for a converged solution.

128

Patran Interface to MD Nastran Thermal Subcases

Transient Subcase Parameters This subordinate form appears when you select the Subcase Parameters button on the Subcase Create form and the solution type is Transient. This form provides for the definition of the input data that controls the solution of the nonlinear time-dependent equations. The integration in time is carried out using Newmark’s method with variable time steps. An initial time step and the number of time steps must be input. Since the time increment is adjusted during the analysis,

Main Index

Chapter 4: Running a Thermal Analysis 129 Subcases

the actual number of time steps may not be equal to the input value. However, the total time duration will be close to the product of the input values.

Subcase Parameters Initial Time Step =

0.01

Number of Time Steps =

100

Initial time increment for the Newmark method.

This number is used along with the initial time step to calculate the total time duration.

Transient Nonlinear Iterations Matrix Update Method:

Adaptive

Number of Bisections per Update = Defines the maximum number of time step bisections to be used in each matrix update.

2 Allowable Iterations per Time Step = 10

The maximum number of allowed iterations in a time step.

Convergence Criteria Temperature Error Temperature Tolerance =

1.0e-02

Load Error Load Tolerance =

The convergence criteria are described above for the steady-state case. The temperature convergence criteria must be selected if the analysis involves any time varying temperature boundary conditions.

1.0e-03

Work Error Work Tolerance =

1.0e-06

Fixed Time Steps

Directs MD Nastran to use the initial time step for all time steps. This disables the automatic time stepping mechanism.

Exit on Failure to Converge OK

Cancel

If this toggle is ON, the run will terminate if the converge criteria are not met for any time step. If OFF, the run continues to the next time step.

Main Index

130

Patran Interface to MD Nastran Thermal Subcases

Structural Heat Subcase Parameters This subordinate form appears when you select the Subcase Parameters button on the Subcase Create form and the solution type is Structural Heat. This form provides for the definition of the input data that controls the solution of the linear structural equations. The parameters that can be set have to do with 1) Default Load Temperature, 2) Rotor Dynamics, 3) Contact Table, and 4) Solvers/Options..

Default Load Temperature is for specifying the temperature at nodes for which the temperature has not been specified using Loads/BCs. By clicking Enable Rotor Dynamics, and clicking Specify Rotor Speed, several things are to be specified. They are 1) Reference Rotor, 2) the units of the speed, and 3) Rotor Speed. Clicking the Contact Table button displays the Contact Table form. This form is used to specify what and how contact bodies are to be in contact. For example, rubber seal (flexible) contacts door (rigid). See Thermal Contact Table, 126 Clicking the Solvers / Options button displays the Solvers / Options form that is used to specify the Solver Type (for example, Nastran Default or an iterative method), a Preconditioner method (for example, Cholesky), Maximum Number of Iterations, and other parameters.

Output Requests The output requests forms allow you to define what result quantities will be written to the MD Nastran print file for viewing and the OUTPUT2 file for import into Patran. A reasonable set of default result quantities are predefined. The simplest way to change these is to use the Basic Output Requests form.

Main Index

Chapter 4: Running a Thermal Analysis 131 Subcases

More control over output quantities is provided for sophisticated users by changing the Form Type menu from Basic to Advanced. The Basic form is shown below. Output Requests The available output requests depend on the active Solution Sequence as indicated by this value.

SUBCASE NAME: SOLUTION SEQUENCE: 159 Form Type:

Basic This option menu is used to switch between the advanced and basic versions of this form.

Select Result Type Temperatures Heat Fluxes Applied Linear Loads Heats of Constraint Enthalpies Rate of Change of Enthalpies

Displays the appropriate result types that may be selected for the solution sequence indicated at the top of the form. The output requests are selected one at a time by clicking.

Output Requests THERMAL(SORT2,PRINT)=All FEM FLUX(SORT2,PRINT)=All FEM Displays the selected output requests for the subcase shown at the top of the form.

Deletes the output request highlighted in the Output Requests listbox.

Delete

OK

Defaults

Cancel

NOTE: The OK button accepts the output requests and closes the form. The Defaults button deletes all output requests and replaces them with defaults. The Cancel button closes the form without saving the output requests.

Main Index

132

Patran Interface to MD Nastran Thermal Subcases

When the Form Type is set to Advanced, the Output Requests form expands to the form below. The same result types are available in the Select Result Type listbox, but more options are available to control these. This listbox is used to select the group of nodes or elements to which the output requests relate.

Use this listbox to select the result type to be created.

Output Requests SUBCASE NAME: SOLUTION SEQUENCE: 153 Form Type:

Select Group(s)/SET All FEM

Advanced

Select Result Type Temperatures Heat Fluxes Applied Linear Loads Heats of Constraint

Options Sorting:

By Node/Element

Output Device Opt:

Print

Output Requests THERMAL(SORT1,PRINT)=All FEM FLUX(SORT1,PRINT)=All FEM

Create Intermediate Output Option:

No

Delete

OK

Defaults

Creates output requests for highlighted result types. It also modifies highlighted output requests. The button label changes to reflect the operation. Use this listbox to select output requests that are to be modified or deleted. NOTE: The ALL FEM set must be selected to request the heat flux output associated with loads and boundary conditions.

Main Index

Cancel

These options are appropriate for the highlighted result type. They also indicate the options that were selected for a highlighted output request. See Table 4-1.

Chapter 4: Running a Thermal Analysis 133 Subcases

Table 4-1

Output Request Form Options

Options Sorting

Label

Multiple Select Allowed

Descriptions

By Node/Element No

Output is presented as tabular listing of nodes/elements for each load step or time.

By Time/Load Step

No

Output is presented as tabular listing of load step/time for each node or element type.

No

Requests that the output be written to the NASTRAN output (f06) file.

Punch

No

Requests that the output be written to the punch file (job_name.pch).

Both

No

Requests that the output be written to the NASTRAN output (f06) file and the punch file (job_name.pch).

IntermediateO Yes utput Options

Once per subcase

Intermediate outputs are requested for every computed load increment. Applicable for steadystate analysis only.

No

Once per subcase

Intermediate outputs are requested for the last load of the subcase. Applicable for steady-state analysis only.

All

Once per subcase

Intermediate outputs are requested for every computed and user-specified load increment. Applicable for steady-state analysis only.

--

Once per subcase

An integer ‘n’ that specifies the percentage of intermediate outputs to be presented for transient analysis. Default = 100.

Output Device Print Options

Percent of Step Output

Direct Text Input This form is used to directly enter entries into the Case Control section for the defined subcase.

Main Index

134

Patran Interface to MD Nastran Thermal Subcases

Directly entered entries may potentially conflict with those created by the interface. Writing these entries to the file can be controlled with this toggle.

Direct Text Input Write To Input Deck

OK

Clear

Clears the current form. Saves the current setting and data and closes the form.

Main Index

Reset

Resets the form back to the data values it had at the last OK.

Cancel

Resets the form back to its previous value and closes the form.

Chapter 4: Running a Thermal Analysis 135 Subcase Select

4.7

Subcase Select This form appears when you select the Subcase Select button on the Analysis form. It allows you to select a sequence of subcases associated with an analysis job. The Default subcase is selected automatically. If multiple subcases are selected, the subcases selected must contain identical sets of convection, radiation boundary conditions, and fixed value temperature boundary conditions because these boundary conditions are not subcase selectable in MD Nastran thermal analysis. Subcase Select

Subcases For Solution Sequence:

153

Default Second-Load-Case Radiation-Case

Displays all the available subcases for the current solution sequence. The current solution sequence is displayed at the top of the form.

Subcases Selected: Default Displays all subcases that have been associated with the current jobname.

OK

Cancel

Within the current Patran MD Nastran design, only those boundary conditions referred to as loads are subcase selectable. All heat flux types and temperature boundary specifications are defined as thermal loads, whereas all occurrences of convection and radiation are defined as boundary conditions and are not subcase selectable. As a result, the use of multiple subcases in MD Nastran thermal analysis has limited utility and in general is not recommended.

Main Index

136

Patran Interface to MD Nastran Thermal Subcase Select

Main Index

Chapter 5: Results Processing and Visualization Patran Interface to MD Nastran Thermal

5

Main Index

Results Processing and Visualization

J

Overview

J

Reading Thermal Analysis Results

J

Results Visualization Options

138

150

139

138

Patran Interface to MD Nastran Thermal Overview

5.1

Overview Before postprocessing of thermal results can occur, the MD Nastran analysis results must be loaded into the Patran database through the Read Output2 or Attach XDB Action on the Analysis form. You can then display, sort, or retrieve the results using the following options:

Contour Plots (Fringe Plots)

Contour Plots can be made for temperatures (isotherms), temperature gradients, and heat fluxes. Since temperature gradients and heat fluxes are vector quantities, plotting their values on the geometry requires selecting the desired result quantity; magnitude, x-component, y-component, or z-component. Contour plots can be made for any steady-state solution, and any temporal solution state in a transient analysis.

XY Plots

The most common XY plot for heat transfer is the representation of nodal temperature versus time. On an elemental basis, temperature gradients and heat fluxes may also be represented as functions of time. In a general sense, the following XY plot types are available: • Results versus Global Variables • Results versus Another Result • Results versus Distances • Global Variables versus Global Variable • Result in Local System • Result in Arbitrary Path

Global variables include time and percent of load*. Results include: temperature, temperature gradients, and heat fluxes. * Percent of load refers to the nonlinear extreme solution technique of determining the result by incrementing the load toward its full level from a reduced initial condition or load.

Main Index

Chapter 5: Results Processing and Visualization 139 Reading Thermal Analysis Results

5.2

Reading Thermal Analysis Results The Analysis form will appear when you select Analysis from the main form.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

© XY

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

There are currently two Actions--Read Output2 and Attach XDB--for importing results. Selecting Read Output2 as the Action on the Analysis form allows the model and⁄or results data to be read into the Patran database from an NASTRAN OUTPUT2 file. Subordinate forms of the Analysis form will define translation parameters, which control the data to be translated, and the OUTPUT2 file from which to translate. The OUTPUT2 data files are created by placing a PARAM,POST,-1 entry in the MD Nastran Bulk Data section. Selecting Attach XDB as the Action on the Analysis form allows the results data from a MSC.Access database (an .xdb file) to be accessed. In this case the results are not read directly into the Patran database but instead remain in the MSC.Access database. Only what is termed as meta data is read into the Patran database. Meta data consists of the Result Case names, their associated subcases, primary and secondary result types, global variables, and the file location of the MSC.Access database or .xdb file. The Meta data is used to translate results when the user attempts to postprocess the model. Subordinate forms of the Analysis form will define translation parameters, which control the data to be accessed on attachment.

Main Index

140

Patran Interface to MD Nastran Thermal Reading Thermal Analysis Results

MSC.Access databases are created by placing a PARAM,POST,0 entry in the MD Nastran Bulk Data section. See following sections See following sections Use this option if results are to be attached using MASTER/DBALL direct results access. Use this option if SOL 600 results are to be attached using T16/19 direct results access.

Main Index

Chapter 5: Results Processing and Visualization 141 Reading Thermal Analysis Results

Read Output2 Form This form appears when you select Analysis from the main menu. Read Output2, as the selected Action, defines the type of data to be read from the MD Nastran results file into Patran. The Object choices are Result Entities, Model Data, or Both.

Main Index

142

Patran Interface to MD Nastran Thermal Reading Thermal Analysis Results

Defines how far the results translation will proceed. If Translate is selected, a job file containing information for the results translation control is created and then submitted for translation. If Control File is selected, the procedure will stop as soon as the control file is generated. Analysis

Read Output2

Action:

Result Entities

Object:

Translate

Method:

Code:

MD Nastran

Type:

Thermal

When the Object selected is Result Entities, the model data must already exist in the database. No results can be read into Patran if the associated node or element does not already exist. Model Data only reads the model data that exists in the results file. Both will first read the model data, then the result entities. If Model Data or Both are selected, you must ensure that there will not be any ID conflicts with existing model entities.

Available Job Names my_job

Defines the jobname to be used for this job. The same jobname used for the Analyze Action should be used for the Read Output2 Action. This will allow Patran to load the results directly into the load cases that were used for the analysis.

Job Name my_job Job Description MSC.Nastran job created on 18-Apr-96 at 13:58:15

Defines the tolerances used during model translation. The division tolerance is used to prevent division by zero errors. The numerical tolerance is used when comparing real values for equality. For Results Entities and Both Objects, the Translations Parameters form also specifies which version of the NASTRAN OUTPUT2 file will be read.

Translation Parameters... Select Results File...

Apply

Main Index

Selects the results file (*.op2) to be read. The form that is called up lists all files recognized as being MD Nastran results files. Even if there is only one .op2 file, it must be explicitly selected. Begins the translation of NASTRAN OUTPUT2 results into the Patran database for postprocessing.

Chapter 5: Results Processing and Visualization 143 Reading Thermal Analysis Results

Results File Formats The Patran MD Nastran interface supports several different OUTPUT2 file formats. The interface, running on any platform can read a binary format OUTPUT2 file produced by MD Nastran running on any of these same platforms. For example, a binary OUTPUT2 file produced by MD Nastran running on an IBM RS/6000 can be read by Patran running on DEC Alpha. Patran may be able to read binary format OUTPUT2 files from other platforms if they contain 32 bit, IEEE format entities (either Big or Little Indian). For platforms that do not produce OUTPUT2 files in these formats, Patran can read OUTPUT2 files created with the FORM=FORMATTED option in MD Nastran. This option can be selected from the Analyze/Translation Parameters form in Patran Analysis menu and directs MD Nastran to produce an ASCII format OUTPUT2 file that can be moved between any platforms. The Patran MD Nastran interface detects this format when the OUTPUT2 file is opened, automatically converts it to the binary format, and then reads the model and/or results into the Patran database. An OUTPUT2 file is created by MD Nastran by placing a PARAM,POST,-1 entry in the Bulk Data portion of the input file. The formatted or unformatted OUTPUT2 file is specified in the FMS section using an ASSIGN OUTPUT2 = filename, UNIT=#, FORM=FORMATTED (or UNFORMATTED) command. See Translation Parameters, 109. Supported OUTPUT2 Results The following table indicates all the possible results quantities that can be loaded into the Patran database during results translation from MD Nastran. The Primary and Secondary Labels are items selected from the postprocessing menus. The Type indicates whether the results are Scalar or Vector and determines which postprocessing techniques are available to view the results quantity. Data Block indicates which NASTRAN OUTPUT2 datablock the data comes from. The Description gives a brief discussion about the results quantity, such as whether it is a nodal or elemental result, and what type of output request will generate this datablock. Primary Level

Secondary Level

Type

Data Block

Description

Temperatures

S

OUGV1

Nodal temperatures

Applied Linear Loads

S

OPG1

Nodal applied linear loads

Heats of Constraint

S

OQG1

Nodal heats of constraint

Applied Load

S

OEF1

Heat flows from applied surface loads

Free Conv

S

OEF1

Heat flows from free convection

Forced Conv

S

OEF1

Heat flows from forced convection

Radiation

S

OEF1

Heat flows from radiation

Total

S

OEF1

Total heat flows into surface elems

Temperature Gradients

V

OEF1

Conduction element temperature gradients

Heat Fluxes

V

OEF1

Conduction element heat fluxes

Heat Flows

Main Index

144

Patran Interface to MD Nastran Thermal Reading Thermal Analysis Results

Secondary Level

Primary Level

Type

Data Block

Description

Enthalpies

S

OUGV1

Nodal enthalpies

Rate of Change of Enthalpies

S

OUGV1

Rate of change of nodal enthalpies

Heats of Constraint are the mathematical (non-physical) heat flow into or out of a nodal point which is associated with a user-specified temperature. In real-world analysis, we generally do not know the structural temperatures, but we do know something about the heat loads, convection and radiation boundaries, etc. We then invoke MD Nastran to calculate the temperatures. However, suppose we have results of an experiment in which a thermocouple is used to measure the boundary temperature. This temperature could then be applied as a boundary condition in the finite element model. In the experimental test, there may well be heat flow into or out of the boundary, but we have not made any attempt to qualify or quantify the heat flow mechanism because we actually measured the temperature. When the MD Nastran thermal analysis is performed, the heat of constraint output represents the heat flow that must occur at the physical boundary to support or maintain the measured temperature. In addition to standard results quantities, several Global Variables can be created. This table outlines Global Variables that may be created. Global Variables are results quantities where one value is representative of the entire model: Label

Type

Data Block

Description

Time

S

Oxxx

Time value of the time step

Percent of Load

S

Oxxx

Percent of load value for a nonlinear steady-state analysis

When reading model data from an NASTRAN OUTPUT2 file by selecting the Model Data Object, all the data that will be created in the Patran database and the location in the OUTPUT2 file from where it is derived are described in the following table: Item Nodes

Block GEOM1

Description Node ID Nodal Coordinates Reference Coordinate Frame Analysis Coordinate Frame

Main Index

Chapter 5: Results Processing and Visualization 145 Reading Thermal Analysis Results

Item Coordinate Frames

Block GEOM1

Description Coordinate Frame ID Transformation Matrix Origin Can be Rectangular, Cylindrical, or Spherical

Elements

GEOM2

Element ID Topology (e.g., Quad4 or Hex20) Nodal Connectivity

Main Index

146

Patran Interface to MD Nastran Thermal Reading Thermal Analysis Results

Attach XDB Form This form appears when you select Analysis from the main menu. Attach XDB, as the selected Action, defines the type of data to be read from the MD Nastran results file into Patran. The Object choices are Result Entities, Model Data, or Both. Action:

Attach XDB

Object:

Result Entities

Method:

Local

Code: MD Nastran

When the Object selected is Result Entities, the model data must already exist in the Patran database. Only metadata or catalog information such as Result Cases/Types, Global Variables, and file connection is read into the Patran database. The results data remains in the XDB file. The Model Data Object only imports Nodes, Elements, and Coordinate Systems. The Both selection will first read the model data, then the result entities. If Model Data or Both are selected, you must ensure that there will not be any ID conflicts with existing model entities.

Thermal

Type: Study:

Available Jobs my_job

Defines the jobname to be used for this job. The same jobname used for the Analyze Action should be used for the Attach XDB Action. This will allow Patran to load the results directly into the load cases that were used for the analysis.

Job Name my_job Job Description MSC.Nastran job created on 14-Apr-98 at 13:24:31

Selects the results file (MSC.Access database or xdb file) to be read. The form that is called up lists all files recognized as being MD Nastran results files. By default, all files with an xdb extension are listed on them. This can be changed with the filter. One may attach up to 20 .xdb files simultaneously. Defines the tolerances used during model translation. The division tolerance is used to prevent division by zero errors. The numerical tolerance is used when comparing real values for equality.

Select Results File... Translation Parameters...

Apply

Main Index

Begins the reading of the meta data from the MD Nastran xdb file for postprocessing.

Chapter 5: Results Processing and Visualization 147 Reading Thermal Analysis Results

Results File Formats The same basic issues exist for MSC.Access databases as for OUTPUT2 files. For example, the MSC.Access database (xdb file) may be exchanged between computer systems that have binary compatibility. That is, an XDB file generated on a SUN Machine may be used on an IBM/AIX, HPUX or SGI computers. However, in order to exchange the XDB file on binary incompatible machines, one needs to use the TRANS and RECEIVE utilities delivered with every installation of MD Nastran. TRANS converts an XDB file generated by MD Nastran to an “equivalent” character, i.e. ASCII, file which can be transported to another computer across the network via ftp or rcp. RECEIVE converts the character file back into the XDB format for postprocessing. For more information on TRANS and RECEIVE utilities, please consult the “Configuration and Operations Guide” for V70 of MSC.Nastran. A MSC.Access XDB database is created by MD Nastran by placing a PARAM,POST,0 entry in the Bulk Data portion of the input file. See Translation Parameters, 109. In this release, it is assumed that the geometry, loads, and results ouput all reside in the same physical XDB file. That is, "split" XDB databases are not supported. Supported MSC.Access Results The following tables list the currently supported quantities from the MSC.Access database (xdb file). The Primary and Secondary Labels are items selected from the postprocessing menus. The Type indicates whether the results are Scalar or Vector and determines which postprocessing techniques are available to view the results quantity. The Object indicates which MSC.Access object the data comes from. The Description gives a brief discussion about the results quantity, such as whether it is a nodal or elemental result, and what type of output request will generate this datablock. To get further information on the MSC.Access, i.e. XDB, objects supported in Patran, please use the ddlprt and ddlqry utilities delivered with every installation of MD Nastran. ddlprt is MSC.Access' on-line documentation. ddlqry is MSC.Access’ Data Definition Language (DDL) browser. See “Configuration and Operations Guide” for MSC.Nastran V70. Primary Level

Secondary Level

Type

Object

Description

Temperatures

S

THERR

Nodal temperatures

Applied Linear Loads

S

HTFLR

Nodal applied linear loads

Heats of Constraint

S

HTFFR

Nodal heats of constraint

Main Index

148

Patran Interface to MD Nastran Thermal Reading Thermal Analysis Results

Primary Level Heat Flows

Secondary Level

Type

Object

Description

Applied Load

S

QHBDY

Heat flows from applied surface loads

Free Conv

S

QHBDY

Heat flows from free convection

Forced Conv

S

QHBDY

Heat flows from forced convection

Radiation

S

QHBDY

Heat flows from radiation

Total

S

QHBDY

Total heat flows into surface elems

Temperature Gradients

V

Conduction element QBARR, QBEMR,QCON temperature gradients R, QHEXR,QPENR, QQD4R, QQD8R, QRODR, QTETR, QTUBR, QTX6R

Heat Fluxes

V

Conduction element heat fluxes QBARR, QBEMR, QCONR, QHEXR,QPENR, QQD4R, QQD8R, QRODR, QTETR, QTUBR, QTX6R

Enthalpies

S

ENTHR

Nodal enthalpies

Rate of Change of Enthalpies

S

ENRCR

Rate of change of nodal enthalpies

Heats of Constraint are the mathematical (non-physical) heat flow into or out of a nodal point which is associated with a user-specified temperature. In real-world analysis, we generally do not know the structural temperatures, but we do know something about the heat loads, convection and radiation boundaries, etc. We then invoke MD Nastran to calculate the temperatures. However, suppose we have results of an experiment in which a thermocouple is used to measure the boundary temperature. This temperature could then be applied as a boundary condition in the finite element model. In the experimental test, there may well be heat flow into or out of the boundary, but we have not made any attempt to qualify or quantify the heat flow mechanism because we actually measured the temperature.

Main Index

Chapter 5: Results Processing and Visualization 149 Reading Thermal Analysis Results

When the MD Nastran thermal analysis is performed, the heat of constraint output represents the heat flow that must occur at the physical boundary to support or maintain the measured temperature.

Main Index

150

Patran Interface to MD Nastran Thermal Results Visualization Options

5.3

Results Visualization Options The Results or XY Plot toggle, located on the Patran application selections, may be chosen to visualize thermal analysis results. The Results application displays contour plots and XY plots that can be sorted or grouped by various kinds of variables. The XY Plot application creates and manages the definitions of XY windows, curves, and titles. It also manages the display of XY plot information.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

The following pages describe how to process basic thermal results. For more information on postprocessing results, see Postprocessing Results and XY Plotting.

Main Index

© XY

Chapter 5: Results Processing and Visualization 151 Results Visualization Options

Contour Plots Thermal contours can be plotted using the Quick Plot object (default) selected from the Results application. If advanced features or XY plots are desired, the Fringe or Graph object must be used. Results

Action: Object:

Create Quick Plot

Select Result Cases Default, PW Linear : 100. % of Loa

Select Fringe Result Heat Fluxes, Temperature Gradients, Temperatures,

Quantity:

Magnitude

Selects the desired result case. This will fill out the Select Fringe Result listbox below. If this listbox is empty, no results exist in the database. Results can be imported from the Analysis application or with Import in the FIle pulldown menu.

After selecting a result case, the plot options are displayed. This listbox is used to select a desired contour plot.

Displays the result quantity options when a Vector result (Temperature Gradients or Heat Fluxes) is chosen in the Select Fringe Result listbox above. If the selected contour result is a scalar value, this menu does not appear. The possible result quantities are: Magnitude, X component, Y component, Z component

Select Deformation Result

Ignores this listbox for thermal analysis.

Animate -Apply-

Main Index

Click on Apply to create the contour plot.

152

Patran Interface to MD Nastran Thermal Results Visualization Options

To create a contour plot: 1. Select the results case from the first listbox. 1. Select the fringe result from the second listbox. 1. If the fringe result is a vector quantity, select the scalar quantity (Magnitude, X component, Y component, or Z component) to be derived for the fringe. 1. Click on Apply. Vector Output Definitions Thermal vector results include temperature gradients and heat fluxes for conduction elements. Their result quantities are as follows: Result Quantity

Temperature Gradients

Heat Fluxes

Magnitude

{(dT/dx)2+ (dT/dy)2+ (dT/dz)2 } 1/2

{ qx2 + qy2 + qz2 } 1/2

X Component

dT/dx

qx = -k dT/dx

Y Component

dT/dy

qy = -k dT/dy

Z Component

dT/dz

qz = -k dT/dz

The sign convention for heat flow is as follows. Positive heat flow takes place as energy is transferred from a region of high relative temperature to a region of low relative temperature. Similarly, heat flux into the surface of a body is a positive quantity.

Main Index

Chapter 5: Results Processing and Visualization 153 Results Visualization Options

For example,

T=100.

K = Constant

T=0.

L=10. T=100. y

1

2

X=4.

X=6.

T=60. T=40. x T=0. X=0.

X=L=10.

T2 – T1 dT 40. – 60. --------------- = -------------------- = --------------------- = – 2. (Negative Gradient) dx 1 – 2 6. – 4. X2 – X1 qx

dT = – k ------------- = dx1 – 2 1–2

2⋅k

(Positive Flux)

XY Plots In transient thermal analysis, XY plotting is frequently applied to track the temperature-time history of grid points. You select this capability from the Results application using the Graph object. You can also

Main Index

154

Patran Interface to MD Nastran Thermal Results Visualization Options

use the Fringe object and the Report object for advanced features of contour plots and text report generation. Toggles the form to select the result case(s) from the first list box. This is the default form for the Graph object.

Results Display Results Action:

Create

Object:

Graph

Method:

-none-

Y vs X

-none-

-none-

-none-

Turns the Abbreviate Subcases toggle OFF if more than one subcase exists for a Result Case.

Select Result Case(s) transient, Time=60. transient, Time=140. transient, Time=220. transient, Time=380. transient, Time=540. transient, Time=700. transient, Time=860. transient, Time=1020.

Y:

Selects result cases for results postprocessing. NOTE: If nothing appears in this listbox, then the results are not successfully loaded into the database. Go back to the Analysis menu or pull down File Import to read in analysis results.

Selects the Y-axis value.

Result

Select Y Result Boundary Heat Flux, Radiation Boundary Heat Flux, Total Heat Fluxes, Temperature Gradients, Temperatures, , Position...((NON-LAYERED))

X:

Main Index

Selects a Global Variable.

Time

Apply

Selects the layer if more than one layer is associated with the result.

Selects the X-axis value.

Global Variable

Variable:

Lists result types for each selected load case. This listbox is used to select a result for postprocessing.

Reset

Chapter 5: Results Processing and Visualization 155 Results Visualization Options

The Target Entities form shown below is used to select target entities. Results Action:

Create

Object: Method:

-none-

Graph

Toggles the form to select the entities for which you wish to create an XY plot.

Y vs X

-none-

-none-

-none-

Target Entity: Selects entity type.

Nodes Select Nodes

Select (pick or type) entities.

Node 49:54

Apply

Main Index

Reset

156

Patran Interface to MD Nastran Thermal Results Visualization Options

To create a fundamental XY plot of temperature versus time: Results Action:

Create

Object: Method:

-none-

STEP 1: Select Graph object.

Graph Y vs X

-none-

STEP 4: Press the Target Entities icon to toggle the form to select target entities.

-none-

-none-

Select Result Case(s) transient, Time=60. transient, Time=140. transient, Time=220. transient, Time=380. transient, Time=540. transient, Time=700. transient, Time=860. transient, Time=1020.

Y:

STEP 2: For XY Plotting, we need a series of results data, such as the temperature results over a period of time from a transient analysis. You can select the result cases with a mouse click and drag over the time states of interest.

Result

Select Y Result Boundary Heat Flux, Radiation Boundary Heat Flux, Total Heat Fluxes, Temperature Gradients, Temperatures, , Position...((NON-LAYERED))

X: Variable:

Main Index

Global Variable Time

STEP 3: Choose Temperatures from the Select Y Result listbox.

Chapter 5: Results Processing and Visualization 157 Results Visualization Options

Results Action:

Create

Object: Method:

-none-

Graph Y vs X

-none-

-none-

-none-

Target Entity: STEP 5: Select Nodes as the target entity.

Nodes Select Nodes Node 49:54

STEP 6: Select (pick or type) Node IDs.

STEP 7: Click on Apply to create an XY plot.

Apply

Main Index

Reset

158

Patran Interface to MD Nastran Thermal Results Visualization Options

Delete an XY Window STEP 1: Select the XY Plot toggle on the Patran m

Patran up Viewport Viewing Display Preferences Tools

Help

try © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

n file patran.ses.01 started recording at 25 ed by Patran 03:36:58 PM Initialization complete. Acquiring license(s)...

Main Index

© XYPlot

Chapter 5: Results Processing and Visualization 159 Results Visualization Options

XY Plot Action: Object:

Delete

STEP 2: Select the Delete option.

XYWindow

XYWindow List window_1 window_2

STEP 3: Select the desired window(s) to delete from the XYWindow List listbox.

window_3 window_4

-Apply-

Main Index

STEP 4: Click on Apply.

160

Patran Interface to MD Nastran Thermal Results Visualization Options

Main Index

Chapter 6: Read Input File Patran Interface to MD Nastran Thermal

6

Main Index

Read Input File

J

Review of Read Input File Form

J

Data Translated from the NASTRAN Input File

J

Conflict Resolution

171

162 170

162

Patran Interface to MD Nastran Thermal Review of Read Input File Form

6.1

Review of Read Input File Form The Analysis form will appear when the Analysis toggle, located on the Patran main menu, is chosen.

Patran File Group Viewport Viewing Display Preferences Tools

Help

© Geometry © FEM © LBCs © Matls © Properties © Load Cases © Fields © Analysis © Results

© XY

$# Session file patran.ses.01 started recording at 25 $# Recorded by Patran 03:36:58 PM $# FLEXlm Initialization complete. Acquiring license(s)... hp, 2

Read Input File as the selected Action on the Analysis form allows much of the model data from a NASTRAN input file to be translated into the Patran database. A subordinate File Selection form allows the user to specify the NASTRAN input file to translate. This form is described on the following pages.

Main Index

Chapter 6: Read Input File 163 Review of Read Input File Form

Read Input File Form This form appears when the Analysis toggle is selected on the main menu. Read Input File, as the selected Action, specifies that model data is to be translated from the specified NASTRAN input file into the Patran database. Analysis

Action:

Read Input File

Object:

Model Data

Method:

Translate

Code:

MD Nastran

Type:

Structural

Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual.

Available Jobs List of already existing jobs.

Job Name simple Job Description

Name assigned to current translation job. This job name will be used as the base file name for the message file.

MSC.NASTRAN job created on 30-Jan-93 at 16:05:33

Entity Selection...

Activates a subordinate Entity Selection form which allows the user to specify the specific entry types to be read. Also defines ID offset values to be used during import.

Select Input File... Activates a subordinate File Select form which allows the user to specify the NASTRAN input file to be translated.

Main Index

164

Patran Interface to MD Nastran Thermal Review of Read Input File Form

Entity Selection Form This subordinate form appears when the Entity Selection button is selected on the Analysis form and Read Input File is the selected Action. It allows the user to specify which MD Nastran entity types to import.

Entity Selection Entity Packets Nodes Elements Material Properties Element Properties Coordinate Frames Load Sets Subcases MPC Data

Highlighted entity types will be imported.

Select None Select All Select All FEM Select All LBC

Activates the form to define ID offsets.

Define Offsets...

Reset OK

Main Index

Cancel

Chapter 6: Read Input File 165 Review of Read Input File Form

The following table shows the relation between the entity types listed above and the actual MD Nastran entry types effected. If an entity type is filtered out, it is treated as if those entries did not exist in the original input file. Entity Type

MD Nastran Entries

Nodes

GRID, GRDSET, SPOINT

Elements

BAROR, BEAMOR, CBAR, CBEAM, CBEND, CDAMP1, CDAMP2, CDAMP3, CDAMP4, CELAS1, CELAS2, CELAS3, CELAS4, CGAP, CHEXA, CMASS1, CMASS2, CMASS3, CMASS4, CONM1, CONM2, CONROD, CPENTA, CQUAD4, CQUAD8, CQUADR, CROD, CSHEAR, CTETRA, CTRIA3, CTRIA6, CTRIAR, CTRIAX6, CTUBE, CVISC, PLOTEL

Material Properties

MAT1, MAT2, MAT3, MAT8, MAT9

Element Properties

PBAR, PBCOMP, PBEAM, PBEND, PCOMP, PDAMP, PELAS, PGAP, PMASS, PROD, PSHEAR, PSHELL, PSOLID, PTUBE, PVISC

Coordinate Frames

CORD1C, CORD1R, CORD1S, CORD2C, CORD2R, CORD2S

Load Sets

FORCE, GRAV,MOMENT, PLOAD1, PLOAD2, PLOAD4, PLOADX1, RFORCE, TEMP, TEMPP1, TEMPRB, SPC, SPC1, SPCD

Subcases

LOAD, SPCADD, Case Control Section

MPC Data

MPC, RBAR, RBE1, RBE2, RBE3, RROD, RSPLINE, RTRPLT It should be noted that since the GRID entry is controlled with the Nodes filter, the grid.ps load set with the permanent single point constraint data will also be controlled by the Nodes filter.

Main Index

166

Patran Interface to MD Nastran Thermal Review of Read Input File Form

Define Offsets Form This subordinate form appears when the Define Offsets button is selected on the Entity Selection form. It allows the user to specify the ID offsets used when reading a NASTRAN input file. If selected, the value in the Maximum column will be used as the offset for the selected rows.

Minimum and Maximum IDs currently found in the Patran database.

Entity Label Offset Definition Input Offset Value Automatic Offset Define Label Offsets for Selected Entities: Existing ID Range in Db

Entity

Minimum

Maximum

Nodes

1

200

Elements

1

200

New ID

All offset data boxes can be selected at once by selecting this column header.

Offset

Material Properties Element Properties

ID offset value to be used during import. The new ID value will be the ID found in the NASTRAN input file plus this offset value.

Coordinate Frames Distributed Load Set IDs Node Force Load Set IDs Node Displacement Set IDs Bar element Init Displacement

Reset

OK

Cancel

All references made in the input file will also be offset. If a node references a particular CID as its analysis frame, then the reference will be offset as well. If the coordinate frame is defined in the same input file, the proper references should be maintained. The preference will be properly maintained. If the coordinate frame existed in the file prior to the import, then it needs to be the offset CID. If a coordinate frame with that CID is not found in the database, an error message will be issued.

Main Index

Chapter 6: Read Input File 167 Review of Read Input File Form

To determine which offset effects a particular MD Nastran entry type, refer to the table in the previous section. For Patran entities identified by integer IDs (nodes, elements, coordinate frames, and MPCs), the offset value is simply added to the MD Nastran ID to generate the Patran ID. For Patran entities identified by text names (materials, element properties, load sets, and load cases), the offset value is first added to the MD Nastran ID. The new integer value is then used to generate the Patran name per the naming conventions described in later sections.

Selection of Input File This subordinate form appears when the Select Input File button is selected on the Analysis form and Read Input File is the selected Action. It allows the user to specify which NASTRAN input file to translate. Select File Filter /bahamas/users/sprack/pf/main/*.bdf Files

Directories

/bahamas/users/sprack/pf/main/.

ids.bdf

/bahamas/users/sprack/pf/main/..

ids_1.bdf

/bahamas/users/sprack/pf/main/clip

north.bdf

Selected Input File /bahamas/users/sprack/pf/main/north.bdf

OK

Main Index

Filter

Cancel

168

Patran Interface to MD Nastran Thermal Review of Read Input File Form

Summary Data Form This form appears after the import of the NASTRAN input file has completed. It displays the number of entities imported correctly, imported with warnings, or not imported due to errors. These figures reflect the number of Patran entities created. In some cases, there is not a one-to-one relation between the original MD Nastran entities and the generated Patran entities. For example, when material orientations on several CQUAD4s are defined using references to varying MCIDs while still referencing the same PID, Patran needs to create a unique property set for each different MCID reference. When the OK button is selected, the newly imported data will be committed to the Patran database, and can not be undone. If there is any question as to whether or not this import was desired, review the graphics data prior to selecting OK on this form. If the import was not correct, select the undo button on the main menu bar before selecting OK on this form.

NASTRAN Input File Import Summary Imported

Imported with Warning

Nodes Elements Coordinate Frames Materials Element Properties Load Sets Load Cases MPCs

Reject Entries...

OK

Main Index

Not Imported

Chapter 6: Read Input File 169 Review of Read Input File Form

Reject Card Form During import of the NASTRAN input file, some entriess types might not be understood by Patran. Those entries are brought into Patran in the direct text input data boxes. Selecting the Reject Entries button on the Summary Data form will bring up this Reject Card Form. You can review these entries here.

Direct Text Import Bulk Data Section $ $CBEAM

215

MPCADD

100

213 101

214

0.

0.

1.

102

uu File Management Section

uu Case Control Section

uu Executive Control Section

u

Bulk Data Section

OK

Only card types not supported by Patran are sent to the reject card blocks. (This includes comments.) Entries which are otherwise recognized, but can not be imported due to syntax or invalid data errors are not sent to the reject blocks.

Main Index

170

Patran Interface to MD Nastran Thermal Data Translated from the NASTRAN Input File

6.2

Data Translated from the NASTRAN Input File For more information about which specific MD Nastran entry types can currently be read into Patran, see Data Translated from the NASTRAN Input File (p. 713) in the Patran Interface to MD Nastran Preference Guide.

Main Index

Chapter 6: Read Input File 171 Conflict Resolution

6.3

Conflict Resolution If an entity can not be imported into Patran because another entity already exists with that ID or name, then the conflict resolution logic is used. For more information, see Conflict Resolution (p. 724) in the Patran Interface to MD Nastran Preference Guide.

Main Index

172

Patran Interface to MD Nastran Thermal Conflict Resolution

Main Index

Chapter 7: Example Problems Patran Interface to MD Nastran Thermal

7

Main Index

Example Problems

J

Overview

J

Example 1 - Transient Thermal Analysis

J

Example 2 - Free Convection on Printed Circuit Board

J

Example 3 - Forced Air Convection on Printed Circuit Board

J

Example 4 - Thermal Contact Resistance

J

Example 5 - Typical Avionics Flow

241

J

Example 6 - Radiation Enclosures

261

J

Example 7 - Axisymmetric Flow in a Pipe

J

Example 8 - Directional Heat Loads

J

Example 9 - Thermal Stress Analysis from Directional Heat Loads

J

Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

174 175 200 214

231

273

290

310

302

174

Patran Interface to MD Nastran Thermal Overview

7.1

Overview This chapter provides ten examples that illustrate popular capabilities in Patran’s interface to the MD Nastran thermal solver. The first example, which describes transient thermal analysis, is an extension of the steady state modeling exercise given in Getting Started - A Guided Exercise (Ch. 2). This example contains step-by-step descriptions of the menu picks involved in the modeling process. Examples 2 through 10 are in easy to follow tutorial format. The actual menu structures are not shown since the expectation is for the user to follow along interactively with the Patran modeling system. The session files of the example problems described in this chapter are delivered with the software. To run an example problem: 1. Start Patran by entering the command p3. 1. From Patran’s main form, pull down the File menu and select Session -- Play. A Play Session File form will appear. 1. Select nastherm_exn.ses from the Session File List listbox. 1. Click on Apply. Patran will execute the modeling process and show you how to build the model.

Main Index

Chapter 7: Example Problems 175 Example 1 - Transient Thermal Analysis

7.2

Example 1 - Transient Thermal Analysis Objectives The objectives of this exercise are as follows: • Open the database created in Getting Started - A Guided Exercise (Ch. 2). • Define time dependent functions using the Field application. • Create a transient load case. Add two existing load sets (temperature and convection boundary

conditions) to this transient load case. • Apply time varying heat flux to the right edge of the plate. • Apply a transient volumetric heat generation inside the shaded area of the plate. • Select solution type as transient analysis. • Specify the default initial temperature. • Define time steps. • Select a transient load case. • Perform a transient thermal analysis using MD Nastran within the Patran system.

Main Index

176

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

• Postprocess the transient results (Contour and XY plots).

0.4 m

1m

Aluminum Plate k = 204 W/m-oC Cp = 896 J/kg-oC

ρ = 2707 kg/m3 h = 10.0 W/m2-oC

3m

o

Tamb = 20.0 C

q = qvol(t) W/m3

q = qflux(t) W/m2

Thickness = 0.1 m T0 = 50 oC

T = 50 oC

Main Index

Chapter 7: Example Problems 177 Example 1 - Transient Thermal Analysis

Open the Database Created in Chapter 2 File

Ctrl N Ctrl O Ctrl W Ctrl S s

STEP 1: From Patran’s main form, pull down the File menu and select Open. A form will appear called Open Database.

New Database Name

Open Database

Enable NFS Access s

New... Open... Close Save Save a Copy Utilities Import... Export... Session Print... Report... Quit

Filter /tmp/*.db Apply

Ctrl Q

Filter

Cancel

Directories

Database List plate.db

/tmp/.

/tmp/..

Existing Database Name

/tmp/plate.db OK

STEP 3: Click on OK.

Filter

Cancel

STEP 2: Within the Database List listbox, highlight plate.db. The database name will appear inside the Existing Database Name databox.

Define Time Dependent Functions Before applying time varying loads and boundary conditions, we need to define time dependent functions using the Field application. In this model, two time fields are defined, one for applied heat flux and one for volumetric heat generation.

Main Index

178

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Click on the Fields application. The Fields form will appear.

Fields Action:

Create

Object:

Non Spatial

Method:

STEP 1: Toggle the Object setting to Non Spatial.

Tabular Input

Existing Fields

Field Name STEP 2: Click inside the Field Name databox and type in flux_time.

flux_time

Table Definition Active Independent Variables Time (t) Frequency (f) Input Data ... [Options...]

-Apply-

Main Index

STEP 3: Click on the Input Data button.

Chapter 7: Example Problems 179 Example 1 - Transient Thermal Analysis

STEP 4: Fill in the table with the following values using the RETURN or ENTER key.

Time

Value

0

1 1.25 1.75 2 2

10 30 50 100

Time/Frequency Scalar Table Data Input Scalar Data

Time(t)

Value

1

0.00000E+00

1.00000E+00

2 3 4 5

1.00000E+01

1.25000E+00

3.00000E+01

1.75000E+00

5.00000E+01

2.00000E+00

1.00000E+02

2.00000E+00

6 7 8

STEP 5: Click on OK. You must also click on APPLY located on the Fields form.

Map Function to Table... OK

Main Index

180

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Similarly, a time dependent function for volumetric heating is defined as follows.

Fields Action:

Create

Object:

Non Spatial

Method:

Tabular Input

Existing Fields

Field Name qvol_time

STEP 6: Click inside the Field Name databox and type in qvol_time.

Table Definition Active Independent Variables Time (t) Frequency (f) Input Data ... [Options...]

STEP 7: Click on the Input Data button. Fill in the table with the following values using the RETURN or ENTER key.

Time

Value

0

10000 12000 13000 14000 14000

10 30 50 100

-Apply-

STEP 8: Click on OK. You must also click on APPLY located on the Fields form.

Main Index

Chapter 7: Example Problems 181 Example 1 - Transient Thermal Analysis

Create a Transient Load Case Our next task is to create a transient load case. Click on the Load Cases application. The Load Cases form will appear. Load Cases Action:

Create

*

Filter

Existing Load Cases Default

Load Case Name transient Make Current

STEP 1: Click inside the Load Case Name databox. Type in the name transient.

Load Case Type: Time Dependent Description

STEP 2: Toggle the Load Case Type setting to Time Dependent. Since the temperature and convection boundary conditions are not changed from the Getting Started example, we can associate these two load sets with the new load case directly.

Assigned Load/BCs Sets Appli_flux Conve_conv Temp _tempbc Temp_tempbc

STEP 3: Highlight Conve_conv and Temp_tempbc within the Assigned Load/BCs Sets listbox.

Prioritize Load/BCs -Apply-

Main Index

STEP 4: Click on Apply.

182

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Apply Time Varying Heat Flux to the Plate’s Right Edge At this point, we will impose a transient flux load on the plate’s right edge. The magnitude of this flux load is 5000 W/m2 multiplied by the time dependent function flux_time defined earlier under the Fields application. Click on the Loads/BCs application. Load/BoundaryConditions Create

Action: Object: Type:

Applied Heat STEP 1: Change the settings to: Action:Create Object:Applied Heat Method:Element Uniform Option:Normal Fluxes

Element Uniform

Option: Normal Fluxes Analysis Type: Thermal Current Load Case: transient... Type:

Time Dependent

Existing Sets flux

New Set Name

tran_flux

STEP 2: Click inside the New Set Name databox. Type in the nam tran_flux.

Target Element Type: 2D

STEP 3: Toggle the Target Element Type setting to 2D.

Input Data... . Select Application Region..

Main Index

STEP 4: Click on the Input Data button. The Input Data form will appear.

Chapter 7: Example Problems 183 Example 1 - Transient Thermal Analysis

Input Data Form Type:

Basic

Surface Option: STEP 5: Toggle the Surface Option setting from Top to Edge.

Edge

Edge Heat Flux

* Time Function

5000

f:flux_time

Spatial Fields

Time Dependent Fields qvol_time flux_time flux_time

STEP 6: Click inside the databox under Edge Heat Flux. Type in 5000.

OK

STEP 8: Click on OK.

Main Index

Reset

Cancel

STEP 7: Click on the flux_time in the Time Dependen Fields listbox. The *Time Function databox will now appear as f:flux_time.

184

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Next, click on Select Application Region located on the Loads and Boundary Conditions form.

STEP 9: Two icon choices will appear, Surface and Edge. Click on the bottom icon, Edge.

Select Application Region u

Geometry Filter Geometry

uu

FEM

Application Region Select Surfaces or Edges Surface 1.3 Add

Remove

Application Region

STEP 10: Position the cursor over the right edge of the surface and click on this edge with the mouse. Patran will insert Surface 1.3 in the databox under the heading Select Surfaces or Edges.

STEP 11: Click on Add.

OK

STEP 12: Click on OK. Be sure to click on Apply located on the Load/Boundary Conditions form.

Note: A yellow marker will appear on the surface’s right edge indicating that a heat flux load has been applied along the right edge.

Main Index

Chapter 7: Example Problems 185 Example 1 - Transient Thermal Analysis

Apply Transient Volumetric Heat Generation Inside the Plate The volumetric heating can be applied in a similar way, using the Loads and Boundary Conditions form as follows.

Main Index

186

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Load/BoundaryConditions Create

Action: Object: Type:

Applied Heat

STEP 1: Change the settings to: Type:Element Uniform Option:Volumetric Generation

Element Uniform

Option: Volumetric Generation Analysis Type: Thermal Current Load Case: transient... Type:

Time Dependent

Existing Sets

New Set Name

tran_qvol

STEP 2: Click inside the New Set Name databox. Type in the name tran_qvol.

Target Element Type: 2D

STEP 3: Toggle the Target Element Type setting to 2D.

Input Data... . Select Application Region..

-Apply-

Main Index

STEP 4: Click on the Input Data button. The Input Data form will appear.

Chapter 7: Example Problems 187 Example 1 - Transient Thermal Analysis

Input Data Form Type:

Basic

Volumetric Heat Generation

* Time Function f:qvol_time

Time Dependent Fields qvol_time flux_time

Spatial Fields

OK

Reset

STEP 6: Click on OK.

Main Index

Cancel

STEP 5: Click on the qvol_time in the Time Dependent Fields listbox. The *Time Function databox will now include f:qvol_time. Note: The scale factor of the volumetric heating will be set to 1.0 by default if no data is input in the Volumetric Heat Generation databox.

188

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Next, click on Select Application Region located on the Loads and Boundary Conditions form. We want to apply an internal heat generation inside a section of the plate from x=0.0 m to x=0.4 m. This application region will be selected by graphical cursor using the FEM geometry filter.

Select Application Region Load/Boundary Conditions Geometry Filter Create Action: uu Geometry Object: Temp (Thermal) u FEM Type: Nodal

STEP 7: Click on FEM under the Geometry Filter. Use the mouse cursor to drag a rectangle covering the elements located between x=0.0 m and x=0.4 m. Release the mouse cursor. The first two columns of the elements will turn red indicating the selection. Also, a list of elements will appear in the Select 2D Elements databox.

Application Region Thermal Analysis Type: Select Load 2D Elements Current Case: 56 57 61 Default... 62 66 67 71 72 STEP 8: Click on Add.

Type: Static Add Remove Existing Sets Application Region

New Set Name

tempbc OK

STEP 9: Click on OK. Be sure to click on Apply located on the Load/Boundary Conditions form.

Note: A square yellow marker will appear on the center of the selected element indicating that a volumetric heating has been applied on this element.

Main Index

Chapter 7: Example Problems 189 Example 1 - Transient Thermal Analysis

Select Solution Type Now we are ready to set the analysis controls for transient thermal analysis. Click on the Analysis application. The Analysis form will appear. Analysis Action:

Analyze

Object:

Entire Model

Method:

STEP 1: Change the settings to: Action:Analyze Object:Entire Model Method:Full Run

Full Run

Code: MD Nastran Type: Thermal Available Jobs plate

Job Name STEP 2: Click inside the Job Name databox and change the j name to plate_tran.

plate_tran Job Description

STEP 3: Click on Solution Type. The Solution Type form will appear.

MSC.Nastran job created on 18-Apr-96 at 13:58:15

Solution Type Translation Parameters... Solution Type...

MD Nastran Solution Type Solution Type:

Direct Text Input... Subcase Create...

uu

STEADY STATE ANALYSIS

u

TRANSIENT ANALYSIS

STEP 4: Click on the TRANSIENT ANALYSIS.

Subcase Select... STEP 5: Click on Solution Parameters to specify the default initial temperature.

Main Index

190

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Specify the Default Initial Temperature For transient thermal analysis, we have to employ a starting temperature from which the solution evolves. If the initial temperature distribution is uniform, a default initial temperature is sufficient to specify the initial state. Otherwise, the Initial Temperature object in Loads and BCs application must be used to define initial nodal temperatures explicitly. See Initial Temperature, 75 for information.

Solution Parameters Transient Solution Parameters Print Out Singularities Data Deck Echo:

None

Maximum Printed Lines =

999999999

Maximum Run Time =

60

Default Init Temperature =

50.0

STEP 1: Click inside the Default Init Temperature databox and change the value to 50.0.

Radiation Parameters... View Factor Parameters...

OK

Defaults

Cancel

STEP 2: Click on OK. Be sure to click on OK located on the Solution Type form.

Define Time Steps We must now create a subcase. Click on Subcase Create located on the Analysis form. The Subcase Create form will appear.

Main Index

Chapter 7: Example Problems 191 Example 1 - Transient Thermal Analysis

Subcase Create

STEP 1: Within the Available Subcase listbox, highlight transient. The word transient will appear inside the Subcase Name databox.

Solution Sequence: 159 Available Subcases

STEP 2: Click on the Subcase Parameters button. The Subcase Parameters form will appear.

Default transient

STEP 3: Change the Initial Time Step to 10. Make sure the Number of Time Steps settings is 100. Thus, the total analysis time is 1000 seconds.

Subcase Name transient Subcase Parameters

Subcase Description

Initial Time Step = This is a default subcase.

10

Number of Time Steps = 100 Transient Nonlinear Iterations

Available Load Cases

Matrix Update Method: Adaptive

Default transient

Number of Bisections per Update = 2 Allowable Iterations per Time Step = 10

Subcase Options

Convergence Criteria

Subcase Parameters...

Temperature Error Temperature Tolerance = 1.0e-02

Output Requests... Load Error Direct Text Input...

Load Tolerance =

Select Superelements...

Work Error Work Tolerance =

Apply

Delete

1.0e-03

1.0e-06

Cancel Fixed Time Steps

STEP 4: Click on OK. Click on APPLY.

Exit on Failure to Converge OK

Main Index

Cancel

192

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Select a Transient Load Case Our last task on specifying analysis controls is to select the load case for the analysis. Click on Subcase Select located on the Analysis form. The Subcase Select form will appear. Subcase Select Subcases For Solution Sequence: Default transient

159 STEP 1: Click on transient within the Subcases for Solution Sequence: 159 listbox. The word transient will appear inside the Subcases Selected listbox.

Subcases Selected: Default transient

OK

STEP 2: Click on Default in the Subcases Selected listbox to remove the load case Default.

Cancel

Click on OK.

Perform a Transient Thermal Analysis To submit the job for MD Nastran thermal analysis, simply click on the Apply button on the Analysis form. It will take a while for the MD Nastran solver to perform a transient thermal analysis in the background. When the analysis is completed, the model is ready for result processing.

Main Index

Chapter 7: Example Problems 193 Example 1 - Transient Thermal Analysis

Read the Analysis Results into Database

Analysis Action:

Read Output2

Object:

Result Entities

Method:

Translate

STEP 1: Change the settings to: Action:Read Output2 Object:Result Entities Method:Translate

Code: MD Nastran Type:

Thermal

Available Jobs plate plate_tran

Job Name STEP 2: Make sure that the Job Name setting is plate_tran.

plate_tran Job Description MSC.Nastran job created on 18-Apr-96 at 13:58:15 Translation Parameters... Select Results File...

Apply

STEP 3: Click on the Select Results File button and double click on the file called plate_tran.op2.

STEP 4: Click on Apply.

Note: The heartbeat will change to the color blue, indicating that reading process is underway. When the heartbeat turns green again, the results are ready for postprocess.

Main Index

194

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Visualize the Transient Results (Contour Plot) We will create a contour plot of temperature distributions at time=700 sec using the Results Display form. Results Display Results Action: Object:

Create Quick Plot

Select Result Cases transient, Time=380. transient, Time=540. transient, Time=700.

STEP 1: Scroll down the vertical scroll bar of the Select Results Cases listbox, and click on transient, Time=700.

Select Fringe Result Heat Fluxes, Temperature Gradients, Temperatures,

Quantity:

STEP 2: Within the Select Fringe Result listbox, highlight Temperatures.

Magnitude

Select Deformation Result

Animate -Apply-

Main Index

STEP 3: Click on Apply.

Chapter 7: Example Problems 195 Example 1 - Transient Thermal Analysis

Visualize the Transient Results (XY Plot) Now we will apply XY plotting to visualize the temperature-time history of Nodes 49 to 54.

Results Action:

Create

Object: Method:

Graph Y vs X

-none- -none- -none- -noneSelect Result Case(s) transient, transient, Time=60. Time=60. transient, transient, Time=140. Time=140. transient, transient, Time=220. Time=220. transient, Time=380. transient, Time=540. transient, Time=700. Time=380. transient, Time=860. transient, transient, Time=860. Time=1020.

Y:

STEP 1: Set the Object setting to Graph.

STEP 4: Press the Target Entities icon to toggle the form to select target entities.

STEP 2: In the Select Result Case(s) listbox, click and drag mouse to select the time states from transient, Time=0. to transient, Time=1020.

Result

Select Y Result Boundary Heat Flux, Radiation Boundary Heat Flux, Total Heat Fluxes, Temperature Gradients, Temperatures, , STEP 3: Within the Select Y Result listbox, highlight Temperatures.

Position...((NON-LAYERED))

X:

Global Variable

Variable:

Main Index

Time

196

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Results Action:

Create

Object: Method:

-none-

Graph Y vs X

-none-

-none-

-none-

Target Entity: STEP 5: Select Nodes as the target entity.

Nodes Select Nodes

STEP 6: Click inside the Select Nodes databox. Use the mouse cursor to drag a rectangle covering nodes 49 to 54. A list of nodes, Node 49:54, will appear in the Node IDs databox.

Node 49:54

STEP 7: Click on Apply to create an XY plot.

Apply

Main Index

Reset

Chapter 7: Example Problems 197 Example 1 - Transient Thermal Analysis

Modify the XY Plot At this point, we will modify the Y scale of the XY plot and display grid lines in the Y direction by clicking on the XY Plot application. XY Plot Action:

Modify

Object:

Axis

STEP 1: Change the settings to: Action:Modify Object:Axis

Select Current XYWindow XYWindow1 XYWindow1

Active Axis uu

X

u

Y

STEP 2: Toggle the Active Axis setting to Y.

Options... Scale... Labels... Title... Tick Marks... Grid Lines...

Main Index

STEP 3: Click on Scale. The Axis Scale form will appear.

198

Patran Interface to MD Nastran Thermal Example 1 - Transient Thermal Analysis

Axis Scale Scale u

Linear

uu

Logarithmic

Assignment Method uu

Automatic

uu

Manual

uu

Semi-Automatic

u

Range

STEP 4: Toggle the Assignment Method to Range.

Enter Lower and Upper Values 45 70

STEP 5: Change the data under Enter Lower and Upper Values to 45 70.

Number of Primary Tick Marks 6

STEP 6: Change the data under Number of Primary Tick Marks to 6.

Reset Apply

Cancel

STEP 7: Click on Apply.

STEP 8: Click on Cancel.

Main Index

Chapter 7: Example Problems 199 Example 1 - Transient Thermal Analysis

Next, you must click on Grid Lines located on the XY Plot form. The Grid Lines form will appear. Grid Lines Display STEP 9: Click on Primary under the Display selection.

Primary Secondary Options u

Primary

uu

Secondary

uu

Both Color

Line Style:

?25

LongDash 1 1

50

Line Thickness

Reset Apply

Cancel

STEP 10: Click on Apply.

Main Index

200

Patran Interface to MD Nastran Thermal Example 2 - Free Convection on Printed Circuit Board

7.3

Example 2 - Free Convection on Printed Circuit Board Figure 7-1 Y

9.0 in 1.0 in

1.0 in 1.0 in

6.0 in 1.0 in 4.0 in

1.5 in 1.0 in 2.0 in 1.0 in

1.0 in X

4.0 in 5.5 in

q = 5.0 W/in2

Kpcb = 0.066 W/in-oC Kchip = 2.24 W/in-oC

0.25 in 0.1 in h = 0.02 W/in2-oC Tamb = 20.0 oC Figure 7-2

Printed Circuit Board Assembly

Problem Description Figure 7-2 depicts a printed circuit board (PCB) assembly which has three significant chip devices

mounted on it. Each chip is generating heat at a rate that is consistent with the application of a heat flux of 5.0 W/in2 over each device surface area. Heat is dissipated by thermal conduction within the chips and underlying board. Free convection to the ambient environment provides the ultimate heat sink. The ambient temperature for convection is assumed to be 20.0 oC, and a heat transfer coefficient of 0.02

Main Index

Chapter 7: Example Problems 201 Example 2 - Free Convection on Printed Circuit Board

W/in2-oC is used to apply convection to the entire assembly surface. We will analyze the printed circuit board to determine the device temperatures so that they can be compared to manufacturer allowables. Modeling This example demonstrates the modeling of a printed circuit board with multiple components. We will create surfaces for PCB and electronic devices, extrude the surfaces to generate 3D solids, specify properties, apply thermal loads and boundary conditions, and then perform a steady-state analysis.

Main Index

202

Patran Interface to MD Nastran Thermal Example 2 - Free Convection on Printed Circuit Board

Main Index

Chapter 7: Example Problems 203 Example 2 - Free Convection on Printed Circuit Board

Create the Surfaces of Printed Circuit Board and Electronic Components

Table 7-1

◆ Geometry

PCB Action:

Create

Object:

Surface

Method:

XYZ

Table 7-2 Surface ID List

1

Vector Coordinates List

<960>

Origin Coordinates List

[000]

-Apply-

Chip 1 Surface ID List

2

Vector Coordinates List

< 1 1.5 0 >

Origin Coordinates List

[110]

-Apply-

Chip 2 Surface ID List

3

Vector Coordinates List

<110>

Origin Coordinates List

[440]

-Apply-

Chip 3 Surface ID List

4

Vector Coordinates List

<110>

Origin Coordinates List

[ 5.5 2 0 ]

-Apply-

Main Index

204

Patran Interface to MD Nastran Thermal Example 2 - Free Convection on Printed Circuit Board

Extrude the Surfaces to Create Solids Create the PCB solid by extruding surface 1 by -0.1 inch in the Z direction. Extrude surfac direction by 0.25 inches.

Table 7-3

◆ Geometry

PCB Action:

Create

Object:

Solid

Method:

Extrude

Table 7-4 Solid ID List

1

Translation Vector

< 0 0 -0.1 > If the Auto Execute is ON, you do not need to click on -Apply-

Auto Execute Surface List

Surface 1 -Apply-

Chips 1, 2, 3 Solid ID List

2

Translation Vector

<0 0 0.25>

Surface List

Surface 2:4 -Apply-

Main Index

You can use the Auto Execute instead of clicking on -Apply-

Chapter 7: Example Problems 205 Example 2 - Free Convection on Printed Circuit Board

Mesh the Solids You will now create the model’s finite elements. Table 7-5

◆Finite Elements

Action:

Create

Object:

Mesh

Type:

Solid

Global Edge Length

0.25 Hex8

Element Topology Solid List

Highlight

Solid 1:4 -ApplyTo obtain a clearer view, select the isometric view by clicking on the Iso 1 View icon

Main Index

206

Patran Interface to MD Nastran Thermal Example 2 - Free Convection on Printed Circuit Board

Specify Materials For this model we will assume that the PCB and chips are manufactured from isotropic materials having constant conductivities: Kpcb = 0.066 W/in-oCKchip = 2.24 W/in-oC PCB

◆ Materials Action:

Create

Object:

Isotropic

Method:

Manual Input

Table 7-6 Material Name

pcb

Input Properties... Thermal Conductivity =

0.066

-ApplyChips 1, 2, 3

◆ Materials Action:

Create

Object:

Isotropic

Method:

Manual Input

Table 7-7 Material Name

chip

Thermal Conductivity =

2.24

-Apply-

Main Index

Since we are preforming a steady-state analysis, specific heat and density are not required.

Chapter 7: Example Problems 207 Example 2 - Free Convection on Printed Circuit Board

Main Index

208

Patran Interface to MD Nastran Thermal Example 2 - Free Convection on Printed Circuit Board

Define Element Properties For a solid model element properties are used to assign the materials to the various parts of the model. PCB

◆ Properties Action:

Create 3D

Dimension:

Solid

Type:

Table 7-8 Property Set Name

pcb

Input Properties... Material Name

Select from Material Property Sets

m:pcb OK

Select Members

Solid 1 Add -Apply-

Chips 1, 2, 3 Property Set Name

chip

Input Properties... Material Name

Select from Material Property Sets

m:chip OK

Select Members

Solid 2:4 Add -Apply-

To verify that the correct material properties have been defined and assigned to the correct model locations, change th option to Show and create a scalar plot of the model’s materials. Table 7-9

◆ Properties Show

Action:

Table 7-10 Select Property

Material Name

Display Method

Scalar Plot

Select Groups

◆Current Viewport default group

-ApplyMain Index

Highlight

Highlight

Chapter 7: Example Problems 209 Example 2 - Free Convection on Printed Circuit Board

Merge the Common Nodes The duplicate nodes located at the PCB and chip interfaces must be merged. Merging establishes and simulates the physical connection between the PCB and chip components. In Patran equivalencing the model performs node merging.

◆ Finite Elements Action:

Equivalence

Object:

All

Method:

Tolerance Cube

Table 7-11 Equivalencing Tolerance0.005 -Apply-

Verify the Free Edges To check the equivalence process you should verify the element boundaries. If the model has been equivalenced properly you should see a wireframe rendering of your model where only the free edges are components of the wireframe image. Display the view to ensure that the model has no cracks between elements.

◆ Finite Elements Action:

Verify

Object:

Element

Test:

Boundaries

Table 7-12 Display Type -Apply-

Main Index

◆Free Edges

210

Patran Interface to MD Nastran Thermal Example 2 - Free Convection on Printed Circuit Board

Apply a Head Load on Each Device A heat flux will now be applied to the exposed plan form face of the chips.

◆ Load/Boundary Conditions Action:

Create

Object:

Applied Heat

Type:

Element Uniform

Table 7-13 Option:

Normal Fluxes

New Set Name

flux

Target Element Type:

3D

Input Data... Heat Flux

5 OK

Select Application Region Geometry Filter

◆Geometry

Select Solid Faces

Solid 2.6 3.6 4.6

Or select with mouse using the Select icon. Use the Free Face Select icon to help you pick the exposed chip faces.

Add OK -Apply-

Main Index

Chapter 7: Example Problems 211 Example 2 - Free Convection on Printed Circuit Board

Apply a Convection Boundary Condition on the PCB

.

The convection boundary condition will now be applied to the back side of the PCB (side opposite the chips).

Table 7-14

◆ Load/Boundary Conditions

Action:

Create

Object:

Convection

Type:

Element Uniform

Table 7-15 Option:

To Ambient

New Set Name

conv

Target Element Type:

3D

Input Data... Convection Coefficient

0.02

Ambient Temperature

20

OK Select Application Region Geometry Filter

◆Geometry

Select Solid Faces

Solid 1.6

Or select with mouse using the Select icon. Use the Free Face Select icon to help you pick the back face of the PCB.

Add OK -Apply-

Main Index

212

Patran Interface to MD Nastran Thermal Example 2 - Free Convection on Printed Circuit Board

Perform the Analysis

Table 7-16

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Table 7-17 Job Name

ex2

Solution Type...

◆ STEADY STATE ANALYSIS

Solution Type:

OK -Apply-

Read in the Analysis Results

Table 7-18

◆ Analysis

Action:

Read Output2

Object:

Result Entities

Method:

Translate

Table 7-19 Job Name

ex2

Select Results File... ex2.op2 OK -Apply-

Main Index

Highlight

Chapter 7: Example Problems 213 Example 2 - Free Convection on Printed Circuit Board

Display the Results

◆ Results Object:

Quick Plot

Table 7-20 Select Results Cases Select Fringe Result

Default, PW Linear: 100. % of Load

Highlight

Temperatures

Highlight

-ApplyDiscussion of Results The heat generated by the electronic devices is conducted to the printed circuit board, and then spread on the epoxy glas PCB. The cooling mechanism is provided by a free convection heat exchange between the backside of the PCB and th ambient fluid that is maintained at 20 oC. As a result, the largest electronic device has the highest temperature. Becaus of their identical size, the other two electronic chips possess nearly the same temperature distribution.

Main Index

214

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

7.4

Example 3 - Forced Air Convection on Printed Circuit Board Figure 7-3 Z

q = 20.0 W/in2

X

. m=

8.33E-3 lbm/sec

Tin = 20.0 oC

h = h(T) W/in2-oC

Air

9.0 in

X

Problem Description This is an extension of the previous analysis (Example 2). The geometry is unchanged; however, the applied heat flux is increased to 20.0 W/in2. In place of free convection to an ambient environment, an advective flow will traverse the surface. The coolant stream travels in the X-direction with the inlet located at X=0 and the outlet positioned at X=L=9.0 inches. The mass flow rate is constant at any X location with a value of 0.5 lbm/min (8.33E-03 lbm/sec). The inlet temperature is set at 20 oC. Associated with the advection flow which transports energy streamwise, is the heat transfer that takes place between the fluid stream and the PCB. In this problem, energy passes from the PCB into the fluid stream. The convection behavior for this transport is specified with a temperature dependent heat transfer coefficient. In the absence of any film node specification, the look up temperature for this heat transfer coefficient defaults to the average temperature between the PCB surface element and its ambient points, in this case, the nodal points in the advected fluid stream. Modeling We will model the previous PCB thermal analysis with forced air convection over the flat plate, using the Coupled Advection feature. The air temperature rises in the X direction as the fluid stream traverses the circuit board. The temperature dependency of the convection coefficient will be defined using a temperature dependent field.

Main Index

Chapter 7: Example Problems 215 Example 3 - Forced Air Convection on Printed Circuit Board

Create the Geometry

Table 7-21

◆ Geometry

Action:

Create

Object:

Surface

Method:

XYZ

Table 7-22 Vector Coordinates List < 9 6 0 > Origin Coordinates List

[000]

-ApplyVector Coordinates List

< 1 1.5 0 >

Origin Coordinates List

[110]

-ApplyVector Coordinates List

<110>

Origin Coordinates List

[440]

-ApplyVector Coordinates List

<110>

Origin Coordinates List

[ 5.5 2 0 ]

-Apply-

Main Index

216

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

Extrude the Solid

Table 7-23

◆ Geometry

Action:

Create

Object:

Solid

Method:

Extrude

Table 7-24 Translation Vector

< 0 0 -0.1> If the Auto Execute is ON, you do not need to click on -Apply-

Auto Execute Surface List

Surface 1 -Apply-

Translation Vector

< 0 0 0.25 >

Surface List

Surface 2:4 You can use the Auto Execute instead of clicking on -Apply-

-Apply-

Mesh the Solids

Table 7-25

◆ Finite Elements

Action:

Create

Object:

Mesh

Type:

Solid

Table 7-26 Global Edge Length

0.25

Element Topology Solid List

Solid 1:4 -Apply-

Main Index

Hex8

Highlight

Chapter 7: Example Problems 217 Example 3 - Forced Air Convection on Printed Circuit Board

Merge the Common Nodes

Table 7-27

◆ Finite Elements

Action:

Equivalence

Object:

All

Method:

Tolerance Cube

Table 7-28 Equivalencing Tolerance0.005 -Apply-

Verify the Element Boundaries

Table 7-29

◆ Finite Elements

Action:

Verify

Object:

Element Boundaries

Test: Display Type

-Apply-

Main Index

◆ Free Edges

218

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

Specify Materials

Table 7-30

◆ Materials

Table 7-31 Action:

Create

Object:

Isotropic

Method:

Manual Input

Table 7-32 Material Name

chip

Input Properties... Constitutive Model: Thermal Conductivity =

Solid properties 2.24

-ApplyMaterial Name

pcb

Constitutive Model: Thermal Conductivity =

-Apply-

Main Index

Solid properties 0.066

Chapter 7: Example Problems 219 Example 3 - Forced Air Convection on Printed Circuit Board

Define Element Properties

Table 7-33

◆ Properties Create

Action: Dimension:

3D

Type:

Solid

Table 7-34 Property Set Name

chip

Input Properties... Material Name

m:chip

Select from Material Property Sets

OK Select Members

Solid 2:4 Add -Apply-

Property Set Name

pcb

Input Properties... Material Name

m:pcb OK

Select Members

Solid 1 Add -Apply-

Main Index

Select from Material Property Sets

220

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

Define Temperature Dependent Field

Table 7-35

◆ Fields

Action:

Create

Object:

Material Property

Method:

Tabular Input

Table 7-36 Field Name

conv_temp

Active Independent Variables

Temperature (T)

Input Data... Input Scalar Data

Hit Enter Key T 0 100 200

OK -Apply-

Main Index

Value 0.2 0.3 0.35

Chapter 7: Example Problems 221 Example 3 - Forced Air Convection on Printed Circuit Board

Select Two Nodes to Create a Curve

Table 7-37

◆ Geometry

Action:

Create

Object:

Curve

Method:

Point With the mouse select the Node icon. Click on the nodes located at the center of the left edge and the center of the right edge.

Starting Point List

Node 938

Ending Point List

Node 1838

-Apply-

Define the Location of the Air Stream

Table 7-38

◆ Geometry

Action:

Transform

Object:

Curve

Method:

Translate

Table 7-39 Translation Vector

< 0 0 -1.0 >

Curve List

Curve 1 -Apply-

Main Index

222

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

Mesh the Air Stream Preferably, the mesh size should be the same on the air stream as on the PCB.

Table 7-40

◆ Finite Elements

Action:

Create

Object:

Mesh

Type:

Curve

Table 7-41 Global Edge Length

.25

Element Topology Curve List

Bar2 Curve 2

Highlight Curve 2 was the result of translating Curve 1

-ApplyNote: The identical mesh size is not required, but may provide the most accurate model. The Closest Approach metho select the nearest neighboring structure and fluid nodes.

Main Index

Chapter 7: Example Problems 223 Example 3 - Forced Air Convection on Printed Circuit Board

Specify the Materials Properties of Air

Table 7-42

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Table 7-43 Material Name

air

Input Properties... Constitutive Model:

Fluid properties

Thermal Conductivity =

6.66e-4

Specific Heat =

456.2

Density =

5.01e-5

Dynamic Viscosity =

1.03e-6

-Apply-

Main Index

224

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

Define Flow Tube Properties

Table 7-44

◆ Properties Create

Action: Dimension:

1D Flow Tube

Type:

Table 7-45 Property Set Name

flow_tube

Input Properties... Material Name

m:air

Diameter at Node 1

1.0 OK

Select Members

Curve 2 Add -Apply-

Main Index

Select from Material Property Sets

Chapter 7: Example Problems 225 Example 3 - Forced Air Convection on Printed Circuit Board

Action:

Create

Object:

Convection Element Uniform

Type:

Table 7-47 Option: New Set Name

Coupled Advection flow_by_plate

There are two application regions: • The Structure Region (Application Region 1) can be 1D, 2D, or 3D. In this case we have a 3D structure,

and the appropriate Target Element Type is 3D. • The Second Application Region must be 1D, which represents the airflow over the flat plate. In this case,

select the curve along the X direction. Patran will then couple the fluid to the structure locally by the Closest Approach method. Target Element Type:

3D

Region 2:

1D Input Data...

*Temperature Function

f:conv_temp

Mass Flow Rate

8.33e-3

Select from Temperature Dependent Fields

OK Select Application Region Geometry Filter

◆Geometry

Select Solid Faces

Solid 1.6 Add For the Companion Region (the second one)

Active List Select Curves

Curve 2 Add OK -Apply-

Main Index

Highlight

226

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

Apply a Heat Flux on Each Device

Table 7-48

◆ Load/Boundary Conditions

Action:

Create

Object:

Applied Heat

Type:

Element Uniform

Table 7-49 Option:

Normal Fluxes

New Set Name

heat_flux

Target Element Type:

3D

Input Data... Heat Flux

20 OK

Select Application Region Geometry Filter

◆Geometry

Select Solid Faces:

Solid 2.6 3.6 4.6 Add OK

-Apply-

Main Index

With the mouse select the top surfaces of the three-chips

Chapter 7: Example Problems 227 Example 3 - Forced Air Convection on Printed Circuit Board

Define the Inlet Temperature of the Fluid

Table 7-50

◆ Load/Boundary Conditions

Action:

Create

Object:

Temp (Thermal)

Type:

Nodal

Table 7-51 New Set Name

inlet_temp

Input Data... Boundary Temperature

20

OK Select Application Region Geometry Filter

◆Geometry

Select Geometry Entities

Point 35

Add OK -Apply-

Main Index

Pick the initial point on the airstream curve

228

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

Define the Default Initial Temperature and Perform the Analysis

Table 7-52

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Table 7-53 Job Name

ex3

Solution Type... Solution Parameters... Data Deck Echo:

Sorted

Examine the input data in the F06 file

Default Init Temperature

100

Define the default initial temperature

OK OK -Apply-

Main Index

Chapter 7: Example Problems 229 Example 3 - Forced Air Convection on Printed Circuit Board

Read in the Analysis Results

Table 7-54

◆ Analysis

Action:

Read Output2

Object:

Result Entities

Method:

Translate

Table 7-55 Job Name

ex3

Select Results File... ex3.op2 OK -Apply-

Main Index

Highlight

230

Patran Interface to MD Nastran Thermal Example 3 - Forced Air Convection on Printed Circuit Board

Display the Results

Table 7-56

◆ Results Quick Plot

Object:

Table 7-57 Select Results Cases Select Fringe Result

Default, PW Linear: 100. % of Load Temperatures

-ApplyDiscussion of Results With the advection flow attached to the printed circuit board’s back surface, the resulting temperature pr significantly different behavior than in the prior example where free convection provided the heat transfe the printed circuit board and a surrounding fluid maintained at a constant temperature (20 oC). In this exam receives energy as it moves downstream along the PCB. Since the inlet flow is maintained at 20 oC, the ed coincides with X=0 is the coolest and the trailing edge (X=L) is necessarily warmer. Similarly, the most streamwise sense has the highest peak temperature.

Main Index

Chapter 7: Example Problems 231 Example 4 - Thermal Contact Resistance

7.5

Example 4 - Thermal Contact Resistance Figure 7-4 Y 5.0 in

2.0 in

2.0 in 5.0 in Kpwb = 0.6 W/in-oC Kchip = 1.34 W/in-oC 2.0 in

X

2.0 in q = 10.0 W/in2

Z

Contact Coefficient = 1.2 W/in2-oC

0.25 in 0.5 in

X T = 20.0 oC Problem Description The dimension of the chip is 2 x 2 inches with a thickness of 0.25 inches. The printed wiring board is 5 x 5 inches with a thickness of 0.5 inches. Thermal conductivity properties for the chip and wiring board are, respectively, 1.34 and 0.6 W/in-oC.

Main Index

232

Patran Interface to MD Nastran Thermal Example 4 - Thermal Contact Resistance

A heat flux of 10 W/in2 is imposed on the top of the chip component. A thermal conductance value of 1.2 W/in2-oC is applied between the chip and the printed wiring board. The bottom of the printed wiring board is held at a constant temperature of 20 oC. Modeling In this example we will model the contact resistance between two solids--in this case, the contact between an electronic component and a printed wiring board (PWB)--to determine the maximum temperature at the top of the chip and the temperature drop to the bottom of the wiring board. Creating the Geometry

Table 7-58

◆ Geometry

Action:

Create

Object:

Solid

Method:

XYZ

Table 7-59 Solid ID List

1

Vector Coordinates List

< 5 5 .5 >

Origin Coordinates List

[000]

-ApplySolid ID List

2

Vector Coordinates List

< 2 2 .25 >

Origin Coordinates List

[221]

-Apply-

Main Index

Chapter 7: Example Problems 233 Example 4 - Thermal Contact Resistance

Mesh the Solids

Table 7-60

◆Finite Elements

Action:

Create

Object:

Mesh

Type:

Solid

Table 7-61 Global Edge Length

0.25

Element Topology

Hex8

Solid List

Highlight

Solid 1:2 -ApplyTo obtain a clearer view, select the isometric view by clicking on the Iso 1 View icon.

Merge the Common Nodes

Table 7-62

◆ Finite Elements

Action:

Equivalence

Object:

All

Method:

Tolerance Cube

Table 7-63 Equivalencing Tolerance0.005 -Apply-

Main Index

234

Patran Interface to MD Nastran Thermal Example 4 - Thermal Contact Resistance

Specify Materials

Table 7-64

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Table 7-65 Material Name

pwb

Input Properties... Constitutive Model: Thermal Conductivity

Solid properties 0.6

-ApplyMaterial Name

chip Solid properties

Constitutive Model: Thermal Conductivity

-Apply-

Main Index

1.34

Chapter 7: Example Problems 235 Example 4 - Thermal Contact Resistance

Define Element Properties

Table 7-66

◆ Properties

Action:

Create

Dimension:

3D Solid

Type:

Table 7-67 Property Set Name

pwb

Input Properties... Material Name:

m:pwb

Select from Material Property Sets

OK Select Members

Solid 1 Add -Apply-

Property Set Name

chip

Input Properties... Material Name:

m:chip OK

Select Members

Solid 2 Add -Apply-

Main Index

Select from Material Property Sets

236

Patran Interface to MD Nastran Thermal Example 4 - Thermal Contact Resistance

Apply Coupled Convection Contact resistance is modeled in Patran using the Convection-Coupled menu operation (select the bottom chip surface and the top of the printed wiring board to specify the thermal conductance between the two surfaces). This technique enables you to apply a connection throu convection between two solid geometric faces without connecting the structures with finite elements. One advantage o method is that mesh sizes between the two regions need not be congruent. Patran will automatically find the ambient closest to the thermal contact area. (The same technique can be used to model thermal contacts directly from 2D to 1D ge entities, or even from solid faces to nodal ambient points.) However, this convenience is not intended as a replacemen responsible modeling practices. Table 7-68

◆ Load/Boundary Conditions

Action:

Create

Object:

Convection

Type:

Element Uniform

Table 7-69 Option:

Coupled

New Set Name

coup_conv

Target Element Type:

3D

Region 2:

3D

Select the Coupled Option before defining the Element Uniform Type

Input Data... Convection Coefficient:

1.2

OK Select Application Region Geometry Filter

◆Geometry

Select Solid Faces

Solid 2.5 Add For the Companion Region (the second one)

Active List Select Solid Faces

Solid 1.6 Add OK

-ApplyNote: Arrows should be pointing downward into the printed wiring board.

Main Index

Chapter 7: Example Problems 237 Example 4 - Thermal Contact Resistance

Apply a Heat Flux on the Top Surface of the Chip

Table 7-70

◆ Load/Boundary Conditions

Action:

Create

Object:

Applied Heat Element Uniform

Type:

Table 7-71 Option:

Normal Fluxes

New Set Name

heat_flux

Target Element Type:

3D

Input Data... Heat Flux

10 OK

Select Application Region Geometry Filter

◆Geometry

Select Solid Faces

Solid 2.6

Or select with mouse using the Select icon Using the mouse, select the Free Face of a Solid icon

Add OK -Apply-

Main Index

238

Patran Interface to MD Nastran Thermal Example 4 - Thermal Contact Resistance

Apply a Temperature Boundary Condition on the Back Side of the PWB

Table 7-72

◆ Load/Boundary Conditions

Action:

Create

Object:

Temp (Thermal) Nodal

Type:

Table 7-73 New Set Name

tempbc

Input Data... Boundary Temperature

20

OK Select Application Region Geometry Filter

◆Geometry

Select Geometry Entities

Solid 1.5

Or select with mouse using the Select icon Using the mouse, select the Surface or Face icon

Add OK -Apply-

Main Index

Chapter 7: Example Problems 239 Example 4 - Thermal Contact Resistance

Perform the Analysis

Table 7-74

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Table 7-75 Job Name

ex4

-Apply-

Read in the Analysis Results

Table 7-76

◆ Analysis

Action:

Read Output2

Object:

Result Entities

Method:

Translate

Table 7-77 Job Name

ex4

Select Results File... ex4.op2 OK -Apply-

Main Index

Highlight

240

Patran Interface to MD Nastran Thermal Example 4 - Thermal Contact Resistance

Display the Results

◆ Results Quick Plot

Object:

Table 7-78 Select Results Cases

Default, PW Linear: 100. % of Load

Highlight

Temperatures

Highlight

Select Fringe Result

-ApplyDiscussion of Results Due to the simple geometry, a hand calculation can be performed to provide an estimate of the maximum temperature at the chip surface: Layer Resistance ≅ Thickness / ( K * A cross section) Contact Resistance ≅ 1 / ( h * A contact) Material Chip Thermal Contact PWB (5x5) PWB (2x2) Total Resistance

Thermal Resistance (C/Watt) 0.046642 0.208333 0.03333 0.208333 0.2883 < R < 0.4633

For a total heat load of 40 W, the maximum temperature can be estimated as: Q = ∆T / Total Resistance Then, Tmax = 20.0 + 40.0 * (Total Resistance) or 31.53 oC < Tmax < 38.53 oC The finite element calculation determined the maximum temperature as 36.51 oC, which is rational considering the hand calculation and the approximation inherent in that solution.

Main Index

Chapter 7: Example Problems 241 Example 5 - Typical Avionics Flow

7.6

Example 5 - Typical Avionics Flow Figure 7-5 Y

X

Z

q = 20 W/in2

0.5 in

10.0 in 5.0 in

Aluminum Plate K = 4.0 W/in-oC

Tin = 20.0 oC

.

m=

DH = 0.5333 in h = 0.3

Air

0.8 in

8.333E-3 * 5 lbm/sec

0.4 in

0.5 in

W/in2-oC 1.0 in

K = 6.66E-4 W/in-oC Cp = 456.2 J/lbm-oC

ρ = 5.01E-5 lbm/in3 µ = 1.03E-6 lbm/in-sec

Problem Description Forced air convection is a very efficient method of removing heat in a limited space. In electronic packaging, forced air convection is used to remove heat in a compact heat exchanger. Modeling this problem within the Patran MD Nastran system requires building a structural model and a fluid model, and connecting them in an appropriate fashion. Patran can associate the structure nodes with the fluid nodes using a technique called the Closest Approach method. This method allows the analyst an option to specify non-coincident mesh sizes on the structure and the fluid nodes. However, it is recommended that you use an identical mesh size for a regular isoparametric rectangular mesh, as demonstrated in this example.

Main Index

242

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Modeling The compact heat exchanger dimensions are 0.5 inch high, 5.0 inches wide, and 10 inches long. The heat exchanger has a total of five rectangular ducts. Each duct has a dimension of 0.8 inch in width and 0.4 inch in height. The inlet temperature of the fluid is at 20 oC. The power density is applied to one side of the heatsink at 20 W/in2. The mass flow rate per channel is 0.5 lbm/min (0.008333 lbm/sec). The fluid properties of the air are evaluated at 25 oC.

Main Index

Chapter 7: Example Problems 243 Example 5 - Typical Avionics Flow

Main Index

244

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Create the Geometry

Table 7-79

◆ Geometry

Action:

Create

Object:

Curve

Method:

XYZ

Table 7-80 Curve ID List

1

Vector Coordinates List

<100>

Origin Coordinates List

[000]

-Apply-* Table 7-81

◆ Geometry

Action:

Transform

Object:

Curve

Method:

Translate

Table 7-82 Curve ID List

2

Translation Vector

< 0 0.5 0 > If the Auto Execute is ON you do not need to click on -Apply-

Auto Execute Curve List

Curve 1 -Apply-*

Table 7-83

◆ Geometry

Action:

Create

Object:

Curve

Method:

Point

Table 7-84 Curve ID List

3

Starting Point

Point 1

Main Index

Chapter 7: Example Problems 245 Example 5 - Typical Avionics Flow

Main Index

246

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Table 7-85

◆ Geometry

Action:

Create

Object:

Surface

Method:

Extrude

Table 7-86 Translation Vector

< 0 0 -10 >

Curve List

Curve 1:4 -ApplyUse Iso 4 View icon to obtain 3D view

Table 7-87

◆ Geometry

Action:

Create

Object:

Curve

Method:

XYZ

Table 7-88 Vector Coordinates List

< 0 0 -10 >

Origin Coordinates List

[ 0.5 0.25 0 ]

-ApplyTable 7-89

◆ Geometry

Action:

Transform

Object:

Surface

Method:

Translate

Table 7-90 Translation Vector

<100>

Repeat Count

4 Click on the Surface icon

Surface List

Surface 1 2 4 -Apply-

Main Index

Chapter 7: Example Problems 247 Example 5 - Typical Avionics Flow

Ending Point

Point 3 You can use the Auto Ex clicking on -Apply-

-ApplyCurve ID List

4

Starting Point

Point 2

Ending Point

Point 4 You can use the Auto Ex clicking on -Apply-

-Apply-

Main Index

Table 7-91 Translation Vector

<100>

Repeat Count

4

248

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Create Finite Elements Mesh Surfaces 1 to 16 to create QUAD4 elements with global edge length 0.25. Similarly, mesh Curves with Bar2 elements using a Global Edge Length of 0.25.

Table 7-93

◆ Finite Elements

Action:

Create

Object:

Mesh

Type:

Surface

Table 7-94 Global Edge Length

.25

Element Topology

Quad 4

Surface List

Highlight

Surface 1:16 -Apply-

Table 7-95

◆ Finite Elements

Action:

Create

Object:

Mesh

Type:

Curve

Table 7-96 Global Edge Length

.25

Element Topology Curve List

Curve 5:9 -Apply-

Main Index

Bar 2

Highlight

Chapter 7: Example Problems 249 Example 5 - Typical Avionics Flow

Merge the Common Nodes

Table 7-97

◆ Finite Elements

Action:

Equivalence

Object:

All

Method:

Tolerance Cube

Equivalencing Tolerance -Apply-

Main Index

0.005

250

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Special Material Properties

Table 7-98

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Material Name

alum

Input Properties... Solid properties

Constitutive Model: Thermal Conductivity

4.0

-Apply-

Material Name

air

Constitutive Model:

Fluid properties

Thermal Conductivity

6.66e-4

Specific Heat

456.2

Density

5.01e-5

Dynamic Viscosity

1.03e-6

-Apply-

Main Index

Chapter 7: Example Problems 251 Example 5 - Typical Avionics Flow

Main Index

252

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Define Element Properties The thickness of the four side walls that separate fluid channels is 0.1 inch. The other walls have a thickness of 0.05 inch. For flow tube elements, the equivalent hydraulic diameter is: Dh = 4 * Cross-Sectional Area / Perimeter = 4 * 0.32 / 2.4 = 0.5333 inch. Table 7-99

◆ Properties

Action:

Create

Object:

2D

Type:

Shell

Table 7-100 Property Set Name

outside_walls

Input Properties... Material Name:

m:alum

Thickness

0.05

Select from Material Property Sets

OK Using mouse click on Front View icon to choose walls

Select Members

Surface 1:3 5 6 8 9 11 12 14:16 Add -Apply-

Property Set Name

inner_walls

Input Properties... Material Name:

m:alum

Thickness

0.1 OK

Select Members

Surface 4:13:3 Add -Apply-

Table 7-101

◆ Properties

Action:

Create

Object:

1D

Main Index

Select from Material Property Sets

Chapter 7: Example Problems 253 Example 5 - Typical Avionics Flow

Table 7-102 Property Set Name

air_flow

Input Properties... Material Name:

m:air

Diameter at Node 1

0.5333 OK

Select Members

Curve 5:9 Add -Apply-

Main Index

Select from Material Property Sets

254

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Apply a Heat Load on the Top Surface

Table 7-103

◆ Load/Boundary Conditions

Action:

Create

Object:

Applied Heat Element Uniform

Type:

Table 7-104 Option:

Normal Fluxes

New Set Name

flux

Target Element Type

2D

Input Data... Surface Option:

Top

Top Surf Heat Flux

20 OK

Select Application Region Geometry Filter

◆Geometry

Select Surfaces or Edges

Surface 2 6:15:3

Add OK -Apply-

Main Index

Or select with mouse using the Select icon

Chapter 7: Example Problems 255 Example 5 - Typical Avionics Flow

Define the Inlet Temperature of the Fluid

Table 7-105

◆ Load/Boundary Conditions

Action:

Create

Object:

Temp (Thermal) Nodal

Type: New Set Name

inlet_temp

Input Data... Boundary Temperature

20

OK Select Application Region

◆Geometry

Geometry Filter

Click on the Point or Vertex icon

Select Geometry Entities Add OK -Apply-

Main Index

Point 9 27:33:2

256

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Apply Coupled Advection

Five load sets, one for each channel, are defined for the fluid-structure coupling.

Table 7-106

◆ Load/Boundary Conditions

Action:

Create

Object:

Convection Element Uniform

Type:

Table 7-107 Option: New Set Name:

Coupled Advection conv1

Target Element Type:

2D

Region 2:

1D Input Data... Top

Surface Option: Top Surf Convection Coef

0.3

Mass Flow Rate

8.333e-3 OK

Select Application Region

◆Geometry

Geometry Filter

Change the view to Front View

Select Surfaces or Edges

Surface 1:4

For the Application Region

Add For the Companion Region (the second one)

Active List Select Curves

Curve 5 Add OK -Apply-

Do the same for the remaining four (4) channels.

Main Index

Chapter 7: Example Problems 257 Example 5 - Typical Avionics Flow

For the Companion Region

Active List Select Curves

Curve 6 Add OK -Apply-

New Set Name:

conv3

Select Application Region

◆Geometry

Geometry Filter

For the Application Region

Active List Select Surfaces or Edges

Surface 7:10

Add For the Companion Region

Active List Select Curves

Curve 7 Add OK -Apply-

New Set Name:

conv4

Select Application Region

◆Geometry

Geometry Filter

For the Application Region

Active List Select Surfaces or Edges

Surface 10:13

Add For the Companion Region

Active List Select Curves

Curve 8 Add OK -Apply-

Main Index

258

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

For the Companion Region

Active List Select Curves

Curve 9 Add OK -Apply-

Perform the Analysis Perform the analysis. Table 7-109

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Job Name

ex5 -Apply-

Main Index

Chapter 7: Example Problems 259 Example 5 - Typical Avionics Flow

Read in the Analysis Results

Table 7-110

◆ Analysis

Action:

Read Output2

Object:

Result Entities

Method:

Translate

Job Name

ex5

Select Results File... ex5.op2

Highlight

OK -Apply-

Display the Results Display the results.

◆ Results Quick Plot

Object:

Table 7-111 Select Results Cases Select Fringe Result

Default, PW Linear: 100. % of Load

Highlight

Temperatures

Highlight Change the view to Iso1 View

-Apply-

Main Index

260

Patran Interface to MD Nastran Thermal Example 5 - Typical Avionics Flow

Discussion of Results The heat flux is imposed on the top of the plate with power density of 20 W/in2. The heat is then spread throughout the aluminum heat sink, and is carried away by the forced air convection inside the channels. The inlet temperature is at 20 oC. There will be a temperature rise in the fluid due to the imposed surface heat flux. The maximum temperature, 101.2 oC, occurs near the exhaust of the module. The exit air temperature is at 71.82 oC. We can check the energy balance on the fluid as follows: Total heat = 20*5*10=1000 W The specific heat is 456.2 J/lbm-oC. The mass flow rate is 0.008333 * 5 = 0.04167 lbm/sec ∆T = 1000/(0.04167*456.2) = 52.6 oC Exit air temperature = 20 + 52.6 = 72.6 oC We can see the exit temperature (71.82oC) calculated by MD Nastran is very close to the hand calculation of 72.6 oC.

Main Index

Chapter 7: Example Problems 261 Example 6 - Radiation Enclosures

7.7

Example 6 - Radiation Enclosures

I

II

III

Cavity 1

Cavity 2

Aluminum Plate k = 204 W/m-oK

ε = 1.0

1 1/2 m

3m

Thickness = 0.001 m

q=2000 W/m2 2m

Y X

1m

Z

2m

3m

Problem Description Three plates are in radiative equilibrium with a zero-degree ambient environment. Each plate measures 2 m by 3 m, and are arranged as shown in the figure above. The center plate (II) has a heat flux applied to it with a magnitude of 2000 W/m2 in the central region, as illustrated. The emissivity of all surfaces is chosen as 1.0, representing perfect blackbodies. The plate thicknesses are all 0.001 m, and the material is aluminum. Temperature distribution for each plate will be determined. Modeling Each plate is meshed with sixteen QUAD8 elements. Two radiation cavities are defined. Cavity 1 includes all the elements on Plates I and II that view each other. These elements also communicate with zero-degree space. The second cavity is comprised of the elements on Plates II and III, which see each other, and they also communicate with zero-degree space. By defining two separate cavities, we have eliminated any of the shadowing calculations that would be required on a single-cavity model. The noncavity sides of Plates I and III are treated as adiabatic surfaces (i.e., perfectly insulated). The normal heat flux is applied to one side of the centermost four elements of Plate II, for a total heat load of 3000 W.

Main Index

262

Patran Interface to MD Nastran Thermal Example 6 - Radiation Enclosures

Create the Geometry

Table 7-112

◆ Geometry

Action:

Create

Object:

Surface

Method:

XYZ

Vector Coordinates List

<230>

Origin Coordinates List

[000]

-Apply-

Table 7-113

◆ Geometry

Action:

Transform

Object:

Surface

Method:

Translate

Translation Vector:

<002> If the Auto Execute is ON, you do not need to click on -Apply-

Auto Execute Surface List

Surface 1 -ApplyChange the view to Iso 2 View

Translation Vector:

<003>

Surface List

Surface 2 -Apply-

Main Index

You can use the Auto Execute instead of clicking on -Apply-

Chapter 7: Example Problems 263 Example 6 - Radiation Enclosures

Mesh the Plates Mesh the plates. Table 7-114

◆Finite Elements

Action:

Create

Object:

Mesh Seed Uniform

Type:

◆Number of Elements Number=

4

Curve List

Surface 1.1 1.2 2.1 2.2 3.1 3.2 -Apply-

Table 7-115

◆Finite Elements

Action:

Create

Object:

Mesh Surface

Type: Global Edge Length

1 Quad8

Element Topology

◆IsoMesh Surface List

Surface 1:3 -Apply-

Main Index

Highlight

264

Patran Interface to MD Nastran Thermal Example 6 - Radiation Enclosures

Specify Materials Specify the materials to be used. Table 7-116

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Material Name

alum

Input Properties... Solid properties

Constitutive Model

Thermal Conductivity -Apply-

Main Index

204

Chapter 7: Example Problems 265 Example 6 - Radiation Enclosures

Define Element Properties Define the element properties. Table 7-117

◆ Properties Create

Action:

2D

Dimension:

Shell

Type: Property Set Name

alum

Input Properties... Material Name

m:alum

Thickness

0.001 OK

Select Members

Surface 1:3 Add -Apply-

Main Index

Select from Material Property Sets

266

Patran Interface to MD Nastran Thermal Example 6 - Radiation Enclosures

Define Radiation Enclosures In this example, we are going to define two cavities for radiation exchange. In so doing, we explicitly eliminate the need for any shadowing calculations when performing the view factor calculations. This will save a lot of time in attaining a temperature solution within MD Nastran. Basically, to identify the TOP and BOTTOM surfaces appropriately, each independent surface within an enclosure will have a distinct SET NAME. Consistent use of the ENCLOSURE ID with each SET NAME ensures that the elements are included in the appropriate enclosure Table 7-118

◆ Load/Boundary Conditions

Action:

Create

Object:

Radiation Element Uniform

Type: Option:

Enclosures

New Set Name:

encl_1

Target Element Type:

2D

Select the Enclosures Option before defining the Element Uniform Type

Input Data... Surface Option:

Top

Enclosure ID

1

Top Surf Emissivity

1.0 First time must turn toggle OFF

Surface Can Shade

First time must turn toggle OFF

Surface Can Be Shaded OK Select Application Region Geometry Filter

◆Geometry

Select Surfaces or Edges

Surface 1

Add OK -ApplyNew Set Name: Input Data...

Main Index

encl_1a

Chapter 7: Example Problems 267 Example 6 - Radiation Enclosures

Main Index

268

Patran Interface to MD Nastran Thermal Example 6 - Radiation Enclosures

Select Application Region Geometry Filter

◆Geometry

Select Surfaces or Edges

Surface 2

Add OK -Apply-

New Set Name:

encl_2

Input Data... Surface Option:

Top

Enclosure ID

2

Top Surf Emissivity

1.0

OK Select Application Region Geometry Filter

◆Geometry

Select Surfaces or Edges

Surface 2

Add OK -Apply-

New Set Name:

encl_2a

Input Data... Surface Option:

Bottom

Enclosure ID

2

Bottom Surf Emissivity

1.0

OK Select Application Region Geometry Filter

◆Geometry

Select Surfaces or Edges

Surface 3

Add OK

Main Index

Chapter 7: Example Problems 269 Example 6 - Radiation Enclosures

Apply a Heat Flux

Table 7-119

◆ Load/Boundary Conditions

Action:

Create

Object:

Applied Heat Element Uniform

Type: Option:

Normal Fluxes

New Set Name

heat_flux

Target Element Type:

2D

Input Data... Surface Option:

Top

Top Surf Heat Flux

2000 OK

Select Application Region Geometry Filter

◆FEM

Select 2D Elements or Edges

Elm 22 23 26 27

Add OK -Apply-

Main Index

270

Patran Interface to MD Nastran Thermal Example 6 - Radiation Enclosures

Set Default Initial Temperature and Perform the Analysis Since radiation heat transfer, by definition, makes our problem highly nonlinear, we need to consider the Default Initial Temperature setting if we hope to achieve a converged solution with the MD Nastran thermal solver. Table 7-120

◆ Analysis

Action:

Analyze

Object:

Entire Model Full Run

Type: Job Name:

ex6

Solution Type.... Solution Parameters... Default Init Temperature=

500

Radiation Parameters.... Stefan-Boltzmann Constant: OK OK OK -Apply-

Main Index

5.6696E-8

Click on Stefan-Boltzmann Constant for list in various units

Chapter 7: Example Problems 271 Example 6 - Radiation Enclosures

Read in the Analysis Results

◆ Analysis Action:

Read Output2

Object:

Result Entities

Method:

Translate

Table 7-121 Job Name

ex6

Select Results File... ex6.op2

Highlight

OK -Apply-

Display the Results

◆ Results Quick Plot

Object:

Table 7-122 Select Results Cases Select Fringe Result

Default, PW Linear: 100. % of Load

Highlight

Temperatures

Highlight

-Apply-

Discussion of Results The center plate has the highest and the lowest temperature for the problem. Since the heat flux is applied to this plate, we expect the maximum temperature to occur here.

Main Index

272

Patran Interface to MD Nastran Thermal Example 6 - Radiation Enclosures

But what about the minimum temperature? Recall that our model includes a good deal of radiation exchange with a space environment. The outer plates (I and III) are insulated on their non-cavity sides. Therefore, only the cavity-facing side can “see” the space environment. The center plate with the heat flux load, however, can view space from both sides, allowing it to be twice as effective in loosing energy to space. This accounts for the minimum temperature condition on the edges of the plate. Additionally, plate I has a higher temperature than Plate III due to its relative location being closer to the center plate than Plate III.

Main Index

Chapter 7: Example Problems 273 Example 7 - Axisymmetric Flow in a Pipe

7.8

Example 7 - Axisymmetric Flow in a Pipe Figure 7-6

Z Region A

Fluid

Region B

q = qvol (z) = 1200 (1 - Z/5) Btu/hr-ft3

h = 3.0 Btu/hr-ft2-oF

5.0 ft

Tamb = 100 oF

X

1.5 ft 3.5 ft 3.9167 ft 4.75 ft Oil Flow

Nu = 0.023 Re0.8 Pr0.3333

Tin = 100 oF

Koil = 0.077 Btu/hr-ft-oF

KA = 0.2 Btu/hr-ft-oF

m = 2.88E6 lbm/hr

Cp oil = 0.44 Btu/lbm-oF

KB = 0.5 Btu/hr-ft-oF

µoil = 100.08 lbm/ft-hr

ρoil = 56.8 lbm/ft3

.

Problem Description In this example we will analyze an axisymmetric structure for its temperature distribution. We will use the MD Nastran CTRIAX6 axisymmetric element (in its 3 node configuration) as the heat conduction element. The basic geometry is detailed in the figure above. A section of pipe consisting of composite materials is divided into two different material regions. Region A is from radius 1.5 feet to 3.5 feet. Region B is from radius 3.5 feet to 4.75 feet. The overall pipe section is 5.0 feet long with an inside diameter of 3 feet and an outside diameter of 9.5 feet.

Main Index

274

Patran Interface to MD Nastran Thermal Example 7 - Axisymmetric Flow in a Pipe

Oil flows through the interior with an inlet temperature of 100 oF and a mass flow rate of 2.88E6 lbm/hr. The forced convection heat transfer coefficient between the oil and wall is calculated by MD Nastran using the following relationship: Nu = 0.023 Re0.8 Pr0.3333 Thermal conductivity properties for Region A and Region B are 0.2 and 0.5 Btu/hr-ft-oF. Volumetric internal heat generation occurs in the subregion of Region B (Specifically from radius 3.5 feet to 3.9167 feet), and varies based on Z location. The heat generation is 1200 * (1-Z/5) Btu/hr-ft3, where Z is given in units of feet. Free convection to an ambient temperature of 100 oF is applied to the exterior surface of the structure through a heat transfer coefficient of 3.0 Btu/hr-ft2-oF. Modeling We will apply a special modeling technique, FIELDS, to input the volumetric heating rate as a function of Z. Coupled Flow Tube is used to tie the structure to the fluid elements.

Main Index

Chapter 7: Example Problems 275 Example 7 - Axisymmetric Flow in a Pipe

Main Index

276

Patran Interface to MD Nastran Thermal Example 7 - Axisymmetric Flow in a Pipe

Create the Geometry

Table 7-123

◆ Geometry

Action:

Create

Object:

Curve

Method:

XYZ

Vector Coordinates List

<005>

Origin Coordinates List

[000] Select the Bottom View for working with axisymmetric geometries

-Apply-

Table 7-124

◆ Geometry

Action:

Create

Object:

Surface

Method:

XYZ

Surface ID List

1

Vector Coordinates List

<205>

Origin Coordinates List

[ 1.5 0 0 ]

-Apply-

Surface ID List

2

Vector Coordinates List

< .4167 0 5 >

Origin Coordinates List

[ 3.5 0 0 ]

-ApplySurface ID List

3

Vector Coordinates List

< .8333 0 5 >

Origin Coordinates List

[ 3.9167 0 0 ]

-Apply-

Main Index

Chapter 7: Example Problems 277 Example 7 - Axisymmetric Flow in a Pipe

Main Index

278

Patran Interface to MD Nastran Thermal Example 7 - Axisymmetric Flow in a Pipe

Mesh the Fluid Curve and the Pipe Surfaces

Table 7-125

◆Finite Elements

Action:

Create

Object:

Mesh Seed

Method:

One Way Bias

Number =

10 2.0

L2/L1 = Curve List

Curve 1 Surface 1.4 3.2 -Apply-

Table 7-126

◆Finite Elements

Action:

Create

Object:

Mesh Surface

Type:

0.25

Global Edge Length= Element Topology=

Tria3

Surface List

Surface 1:3 -Apply-

Table 7-127

◆Finite Elements

Action:

Create

Object:

Mesh

Type:

Curve 0.25

Global Edge Length = Element Topology =

Bar2

Curve List

Curve 1 -Apply-

Main Index

Chapter 7: Example Problems 279 Example 7 - Axisymmetric Flow in a Pipe

Remove Coincident Nodes

Table 7-128

◆ Finite Elements

Action:

Equivalence

Object:

All

Method:

Tolerance Cube

Equivalencing Tolerance -Apply-

Main Index

0.005

280

Patran Interface to MD Nastran Thermal Example 7 - Axisymmetric Flow in a Pipe

Specify Material Properties

Table 7-129

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Material Name

mat_a

Input Properties... Constitutive Model:

Solid Properties

Thermal Conductivity =

0.2

-Apply-

Material Name

mat_b

Constitutive Model:

Solid Properties

Thermal Conductivity =

0.5

-Apply-

Material Name

oil

Constitutive Model:

Fluid Properties

Thermal Conductivity =

0.077

Specific Heat =

0.44

Density =

56.8

Dynamic Viscosity =

100.08

-Apply-

Main Index

Chapter 7: Example Problems 281 Example 7 - Axisymmetric Flow in a Pipe

Define Element Properties

Table 7-130

◆ Properties Create

Action:

2D

Dimension:

Axisym Solid

Type: Property Set Name

pipe_a

Input Properties... Material Name:

m:mat_a

Select from Material Property Sets

OK Application Region Select Members

Surface 1 Add -Apply-

Property Set Name

pipe_b

Input Properties... Material Name:

m:mat_b OK

Application Region Select Members

Surface 2 3 Add -Apply-

Table 7-131

◆ Properties Create

Action: Dimension:

Flow Tube

Type: Property Set Name Input Properties...

Main Index

1D

oil

Select from Material Property Sets

282

Patran Interface to MD Nastran Thermal Example 7 - Axisymmetric Flow in a Pipe

Define a Spatial Field

Table 7-132

◆Fields

Action:

Create

Object:

Spatial

Method:

PCL Function

Field Name

qvol_z

Scalar Function (’X, ’Y, ’Z)

1200*(1.0-’Z/5.0)

-Apply-

Main Index

Chapter 7: Example Problems 283 Example 7 - Axisymmetric Flow in a Pipe

Apply a Volumetric Heat Load

Table 7-133

◆ Load/Boundary Conditions

Action:

Create

Object:

Applied Heat Element Uniform

Type: Option:

Volumetric Generation

New Set Name:

qvol

Target Element Type:

2D

Input Data... Volumetric Heat Generation

f:qvol_z

OK Select Application Region Geometry Filter

◆Geometry

Select Surfaces:

Surface 2 Add OK -Apply-

Main Index

Select from Spatial Fields

284

Patran Interface to MD Nastran Thermal Example 7 - Axisymmetric Flow in a Pipe

Apply Free Convection

Table 7-134

◆ Load/Boundary Conditions

Action:

Create

Object:

Convection Element Uniform

Type: Option:

To Ambient

New Set Name

conv

Target Element Type

2D

Input Data... Surface Option

edge

Edge Convection Coef

3.0

Ambient Temperature

100

OK Select Application Region

◆Geometry

Geometry Filter

Select the Edge icon

Select Surfaces or Edges Add OK -Apply-

Main Index

Surface 3.2

Chapter 7: Example Problems 285 Example 7 - Axisymmetric Flow in a Pipe

Define Inlet Temperatures of the Fluid

Table 7-135

◆ Load/Boundary Conditions

Action:

Create

Object:

Temp (Thermal) Nodal

Type: New Set Name

inlet_temp

Input Data... Boundary Temperature

100

OK Select Application Region Geometry Filter

◆Geometry

Select Geometry Entities

Point 1

Add OK -Apply-

Main Index

286

Patran Interface to MD Nastran Thermal Example 7 - Axisymmetric Flow in a Pipe

Main Index

Chapter 7: Example Problems 287 Example 7 - Axisymmetric Flow in a Pipe

Define Coupled Flow Tube Apply a fluid-structure coupling between the oil and the inner wall of the pipe. Table 7-136

◆ Load/Boundary Conditions

Action:

Create

Object:

Convection Element Uniform

Type: Option:

Coupled Flow Tube

New Set Name

coup_ftube

Target Element Type

10

Region 2

2D Input Data...

Form Type:

Advanced

Mass Flow Rate

2.88e6

Heat Transfer Coefficient

0.023

Formula Type Option

◆ h=k/d*coef*Re**Expr*Pr**Expp

Reynolds Exponent

0.8

Prandtl Exponent, Heat In

0.3333

OK Select Application Region Geometry Filter

◆Geometry

Select Curves

Curve 1 Add For the Companion Region (the second one)

Active List Select Surfaces or Edges

Surface 1.4 Be sure to click on the Edge icon while selecting the geometrical entity

Add OK -Apply-

Main Index

288

Patran Interface to MD Nastran Thermal Example 7 - Axisymmetric Flow in a Pipe

Perform the Analysis

Table 7-137

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Job Name

ex7 -Apply-

Read in the Analysis Results

Table 7-138

◆ Analysis

Action:

Read Output2

Object:

Result Entities

Method:

Translate

Job Name

ex7

Select Results File... ex7.op2 OK -Apply-

Main Index

Highlight

Chapter 7: Example Problems 289 Example 7 - Axisymmetric Flow in a Pipe

Display the Results

◆ Results Object:

Quick Plot

Table 7-139 Select Results Cases Select Fringe Result

Default, PW Linear: 100. % of Load

Highlight

Temperatures

Highlight

-ApplyDiscussion of Results The maximum temperature occurs near the internal heat generation region with a temperature of 842.3oF. The fluid temperature remains constant at 100 oF because of the massive flow rate at 2.88E6 lbm/hr. We can check the energy balance on this model as follows: Total heat = 2.91246E4 Btu/hr (from the OLOAD RESULTANT of the F06 file) Sum of the heat on the column under Free Convection = 2.5828E4 Btu/hr Sum of the heat on the column under Forced Convection = 3.297E3 Btu/hr Sum of the heat on the above two columns = 2.9125E4 Btu/hr, which is equal to the input heat of 2.91246E4 Btu/hr. An assumption of a 1-D fluid element is that temperature gradients within the fluid are only significant along the axial direction. With such a large diameter flow tube, this assumption is probably being misused in this particular problem. The application of the flow tube boundary convection relationship also implies fully developed flow, yet, over only a 5 foot section and with a 3 foot diameter, this is also a very crude approximation. In essence, what we are saying, is that this example serves to illustrate coupled convection in an axisymmetric environment, application of spatial heat loads, and use of convection correlation equations, rather than fluid physics.

Main Index

290

Patran Interface to MD Nastran Thermal Example 8 - Directional Heat Loads

7.9

Example 8 - Directional Heat Loads Figure 7-7

6.0 in

Radiation Boundary Condition View Factor = 1.0

1.5 in

q = qvec = 30

W/in2

Tamb = 20.0 oC

Aluminum Cylinder k = 3.96 W/in-oC

Y

α = ε = 0.8 Thickness = 0.0625 in

Z

X

Problem Description In this example we will apply a directional heat load on cylinder. We will orient the surface normal from the surface such that the normal vector (Right hand rule) will point away from the surface. This allows the incoming directional heat flux to see the normals, and project the correct energy by forming a dot product with this vector. A typical application of this directional heat load process is in an orbital heating environment. The dimension of the cylinder is 1.5 inch in diameter with a length of 6 inches. The material is aluminum with a thermal conductivity of 3.96 W/in-oC. The absorptivity and emissivity of the cylinder surface are

Main Index

Chapter 7: Example Problems 291 Example 8 - Directional Heat Loads

0.8. The directional heat load is 30 W/in2. The exterior surface of the cylinder looses heat by radiation to space. The radiation view factor is 1.0 and the ambient temperature is 20 oC. Modeling We will first calculate the temperature distribution based on the above boundary conditions. Subsequently in Example 9, we will create a spatial FEM field that defines the temperature load for a thermal stress analysis.

Main Index

292

Patran Interface to MD Nastran Thermal Example 8 - Directional Heat Loads

Create the Geometry Table 7-140

◆ Geometry

Action:

Create

Object:

Point

Method:

XYZ

Point ID List

1

Refer Coordinate Frame

Coord 0

Point Coordinates List

[ 0.75 0 0 ]

-Apply-

Table 7-141

◆ Geometry

Action:

Create

Object:

Curve

Method:

Revolve

Curve ID List

1

Total Angle

360.0 If the Auto Execute is ON, you do not need to click on -Apply-

Auto Execute Point List

Point 1 -Apply-

Table 7-142

◆ Geometry

Action:

Create

Object:

Surface

Method:

Extrude

Translation Vector

< 0 0 -6 >

Curve List

Curve 1 Click on Iso1 View icon to obtain 3D view of the cylinder

Main Index

Chapter 7: Example Problems 293 Example 8 - Directional Heat Loads

The surface normal direction is important in this problem, because the incoming heat flux vector will form a dot product with the normal vector for the surface generating the correct projected surface area for application of the heat load. Therefore, when we created the cylinder using geometry, we should verify that the normal vector points outward. This is accomplished by using: Table 7-143

◆ Geometry

Action:

Show

Object:

Surface

Info:

Normal If the Auto Execute is ON, you do not need to click on -Apply-

Auto Execute Surface List

Surface 1

With the mouse draw a box around Surface 1 Change the view to Front View

-ApplySelect Surface 1 to make sure that the normal vector indicated by the red arrow points outward from the cylinder. If the normal vector is pointing inward, then you can reverse the surface normal by using the following command: Table 7-144

◆ Geometry

Action:

Edit

Object:

Surface

Method:

Reverse If the Auto Execute is ON, you do not need to click on -Apply-

Auto Execute Surface List

Surface 1 -Apply-

Main Index

294

Patran Interface to MD Nastran Thermal Example 8 - Directional Heat Loads

Create Finite Elements

Table 7-145

◆Finite Elements

Action:

Create

Object:

Mesh

Method:

Surface

Global Edge Length

0.1 Quad4

Element Topology Surface List

Highlight

Surface 1 -ApplyChange the view to Iso1

Remove Coincident Nodes

Table 7-146

◆ Finite Elements

Action:

Equivalence

Object:

All

Method:

Tolerance Cube

Equivalencing Tolerance -Apply-

Main Index

0.005

Chapter 7: Example Problems 295 Example 8 - Directional Heat Loads

Specify Material Properties

Table 7-147

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Material Name

alum

Input Properties... Solid properties

Constitutive Model Thermal Conductivity -Apply-

Main Index

3.96

296

Patran Interface to MD Nastran Thermal Example 8 - Directional Heat Loads

Define Element Properties

Table 7-148

◆ Properties Create

Action:

2D

Dimension:

Shell

Type: Property Set Name

alum

Input Properties... Material Name

m:alum

Thickness

0.0625 OK

Select Members

Surface 1 Add -Apply-

Main Index

Select from Material Property Sets

Chapter 7: Example Problems 297 Example 8 - Directional Heat Loads

Apply a Directional Heat Load

Table 7-149

◆ Load/Boundary Conditions

Action:

Create

Object:

Applied Heat Element Uniform

Type: Option:

Directional Fluxes New Set Name

vector_flux 2D

Target Element Type: Input Data... Surface Option:

Top

Top Surf Absorptivity

0.8

Top Surf Heat Flux

30

Incident Thermal Vector

< -1 0 0 >

OK Select Application Region Geometry Filter

◆Geometry

Select Surfaces or Edges

Surface 1

Add OK -Apply-

Main Index

Select the Directional Fluxes Option before defining the Element Uniform Type

298

Patran Interface to MD Nastran Thermal Example 8 - Directional Heat Loads

Apply a Radiation Boundary Condition

Table 7-150

◆ Load/Boundary Conditions

Action:

Create

Object:

Radiation Element Uniform

Type: Option:

Ambient Space

New Set Name:

rad_space

Target Element Type:

2D

Input Data... Surface Option:

Top

Top Surf Emissivity

0.8

Top Surf Absorptivity

0.8

Ambient Temperature

20

View Factor

1.0 OK

Select Application Region Geometry Filter

◆Geometry

Select Surfaces or Edges

Surface 1

Add OK -Apply-

Main Index

Chapter 7: Example Problems 299 Example 8 - Directional Heat Loads

Specify Radiation Parameters and Perform the Analysis

Table 7-151

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Job Name

ex8 Solution Type...

STEADY STATE ANALYSIS Solution Parameters... Radiation Parameters... Absolute Temperature Scale:

273.15

Click on Absolute Temperature Scale for list in various units

Stefan-Boltzmann Constant:

3.6580E-11

Click on Stefan-Boltzmann Constant for list in various units

OK OK OK -Apply-

Main Index

300

Patran Interface to MD Nastran Thermal Example 8 - Directional Heat Loads

Read in the Analysis Results

Table 7-152

◆ Analysis

Action:

Read Output2

Object:

Result Entities

Method:

Translate

Job Name

ex8

Select Results File...

Highlight

ex8.op2

OK -Apply-

Display the Results

◆ Results Quick Plot

Object:

Table 7-153 Select Results Cases Select Fringe Result

Default, PW Linear: 100. % of Load

Highlight

Temperatures

Highlight

-ApplyNote:

Continue with Step 1 of Example 9 to perform a structural analysis.

Discussion of Results Example 8 demonstrates an aluminum cylinder in radiative equilibrium. The heat source is directional (light source oriented), and the radiation boundary condition is equal for all directions. The cylinder’s maximum temperature (~473 oC) is attained on the side subject to the solar heat load. The minimum

Main Index

Chapter 7: Example Problems 301 Example 8 - Directional Heat Loads

temperature (~424 oC) occurs in the shadow region. The high conductivity of the cylinder helps to equilibrate the temperatures. If the conductivity were very low, the maximum temperature would approach 740 oC with the minimum approximately 20 oC.

Main Index

302

Patran Interface to MD Nastran Thermal Example 9 - Thermal Stress Analysis from Directional Heat Loads

7.10

Example 9 - Thermal Stress Analysis from Directional Heat Loads Figure 7-8

6.0 in

Aluminum Cylinder

1.5 in

E = 1.0E7 lb/in2

ν = 0.34 α = 1.3E-5 in/in-oC

Y Thickness = 0.0625 in

Z

X

Problem Description This example demonstrates how to apply the thermal results of Example 8 to perform a stress analysis. We will create the temperature loading for the stress run by using the Create-Spatial-FEM command under the Fields Application. You can also use the include punch file option to get the thermal load. The diameter of the cylinder is 1.5 inch with a length of 6 inches. The material is aluminum. The heat transfer problem solved in Example 8 resulted in a temperature solution which we would now like to apply to a thermal stress analysis.

Main Index

Chapter 7: Example Problems 303 Example 9 - Thermal Stress Analysis from Directional Heat Loads

Modeling We will first apply the Create-Spatial-FEM command to define the temperature load for a thermal stress analysis. Initially, the structure is stress-free at a temperature of 0 oC. The cylinder is clamped on both ends for the thermal stress calculation. Create a Spatial FEM Field Based on the Temperature Profile

Table 7-154

◆Fields

Action:

Create

Object:

Spatial

Method:

FEM

Field Name

tempload

FEM Field Definition

◆Continuous

Field Type

◆Scalar

Mesh/Results Group Filter

◆Current Viewport

Select Group

default_group -Apply-

Change the Analysis Type to Structural

Table 7-155 Preferences Analysis...

Analysis Type:

Structural OK

Main Index

Highlight

304

Patran Interface to MD Nastran Thermal Example 9 - Thermal Stress Analysis from Directional Heat Loads

Specify the Structural Materials

Table 7-156

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Material Name

alum_st

Input Properties... Linear Elastic

Constitutive Model Elastic Modulus =

1.0e7

Poisson Ratio =

0.34

Thermal Expan. Coeff =

1.3e-5

Reference Temperature

0.0

-Apply-

Main Index

Chapter 7: Example Problems 305 Example 9 - Thermal Stress Analysis from Directional Heat Loads

Assign Element Properties

Table 7-157

◆ Properties Create

Action:

2D

Dimension:

Shell

Type: Property Set Name

alum_st

Input Properties... Material Name

m:alum_st

Thickness

0.0625

Select from Material Pro

OK Select Members

Surface 1 Add -Apply-

Create a New Load Case

We will create a new load case consisting of the structural thermal loading and apply the fi conditions on the ends of the cylinder.

Table 7-158

◆ Load Cases Create

Action: Load Case Name Load Case Type: -Apply-

Main Index

struct_load Static

306

Patran Interface to MD Nastran Thermal Example 9 - Thermal Stress Analysis from Directional Heat Loads

Apply the Clamped Boundary Conditions

Table 7-159

◆ Load/Boundary Conditions

Action:

Create

Object:

Displacement Nodal

Type: Analysis Type:

Structural struct_load

Current Load Case: New Set Name:

Switch to Structural from Thermal

clamp_bc

Input Data... Load/BC Set Scale Factor

1.0

Translations

< 0., 0., 0. >

Rotations

< 0., 0., 0. >

OK Select Application Region

◆Geometry

Geometry Filter

Click on the Curve or Edge icon

Select Geometry Entities Add OK -Apply-

Main Index

Curve 1 Surface 1.3

Chapter 7: Example Problems 307 Example 9 - Thermal Stress Analysis from Directional Heat Loads

Define a Temperature Load

Table 7-160

◆ Load/Boundary Conditions

Action:

Create

Object:

Temperature Nodal

Type:

Structural

Analysis Type:

struct_load

Current Load Case: New Set Name

temp_load

Input Data... Load/BC Set Scale Factor

1.0

Temperature

f:tempload

Select from Spatial Fields

OK Select Application Region

◆Geometry

Geometry Filter

Click on the Surface or Face icon

Select Geometry Entities Add OK -Apply-

Main Index

Surface 1

308

Patran Interface to MD Nastran Thermal Example 9 - Thermal Stress Analysis from Directional Heat Loads

Perform the Analysis

Table 7-161

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Job Name

ex9 Subcase Select

Subcases For Solution Sequence: 101

struct_load

Highlight

Subcases Selected:

struct_load

Click on default to remove

OK -Apply-

Read in the Analysis Results

◆ Analysis Action:

Read Output2

Object:

Result Entities

Method:

Translate

Table 7-162 Job Name Select Results File... OK -Apply-

Main Index

ex9 ex9.op2

Highlight

Chapter 7: Example Problems 309 Example 9 - Thermal Stress Analysis from Directional Heat Loads

Display the Results

◆ Results Object:

Quick Plot

Table 7-163 Select Results Cases Select Fringe Result

struct_load, Static Subcase Stress Tensor

Position:

At Z1

Quantity:

von Mises

Select Deformation Result

Displacements, Translational

-Apply-

Discussion of Results For output we plot the von Mises stress for the fixed end cylinder undergoing the directional thermal load. Peak stresses occur near the fixed end points (recall the points are fixed in X, Y, and Z directions). Thermal expansion causes growth in the axial and radial directions with a circumferential variation due to the directional nature of the thermal load. Near the cylinder mid-plane, in an axial sense, we find the maximum stress at the location which is normal to the directional load vector. The minimum is on the opposite side of the cylinder in the shadow.

Main Index

310

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

7.11

Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate Figure 7-9 Y

KGe = 1.524 W/in-oC

1.0 in

Ksolder = 1.27 W/in-oC EGe = 1.885E7 lb/in2 GGe = 0.933E7 lb/in2 αGe = 5.8E-6 in/in-oC

1.0 in

X

Z

ESolder = 1.3E7 lb/in2 νSolder = 0.4 αSolder = 2.47E-5 in/in-oC

T = -30.0 oC

Ge: 0.025 in X

Solder: 0.05 in

Tref = -30 oC

T = 70.0 oC

Problem Description In this example we will perform the thermal stress analysis of a bi-metallic strip. We will build the entire model from geometric construction so that we can apply loads directly on the geometry. The dimension of the bi-metallic strip is one inch by one inch. The thickness for the solder type material is 0.05 inch, and the thickness of the Ge material is 0.025 inch. Thus the assembly thickness is 0.075 inch. The top surface temperature boundary condition is -30 oC, and the bottom surface temperature boundary condition is 70 oC. We will determine the temperature distribution by running a steady-state thermal analysis. Modeling Prior to the development of the Patran MD Nastran Heat Transfer interface, one would request: TEMP(PUNCH)=all in the MD Nastran Case Control section of the thermal run. The temperature load is then created and saved inside the punch file. In the subsequent thermal stress analysis one can access this file by defining TEMP(LOAD)=1

Main Index

Chapter 7: Example Problems 311 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

in the Case Control section of the ensuing stress analysis run. However, using Patran you can use the Create-Spatial-FEM command after you have postprocessed the thermal result in the viewport. We will use this technique to apply a thermal load for the stress analysis. Also, we will analyze the thermal stress analysis for the free-free expansion by enforcing a minimum number of constraints to fix-rigid body motion.

Main Index

312

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Create the Model

Table 7-164

◆ Geometry

Action:

Create

Object:

Surface

Method:

XYZ

Vector Coordinates List

<110>

Origin Coordinates List

[000]

-Apply-

Table 7-165

◆ Geometry

Action:

Create

Object:

Solid

Method:

Extrude

Translation Vector

< 0 0 0.05 > If the Auto Execute is ON, you do not need to click on -Apply-

Auto Execute Surface List

Surface 1 -ApplyClick on the Solid Face icon

Translation Vector

< 0 0 0.025 >

Surface List

Solid 1.6 -Apply-

Main Index

You can use the Auto Execute instead of clicking on -Apply-

Chapter 7: Example Problems 313 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Mesh the Solids

Table 7-166

◆Finite Elements

Action:

Create

Object:

Mesh Seed

Type:

Uniform

Number =

4

Curve List

Solid 1.1.1 1.2.1 1.2.3 1.1.3

Click on the four (4) corners of Solid 1. Hold the shift key down while you click

-ApplyNumber =

2

Curve List

Solid 2.1.1 2.2.1 2.2.3 2.1.3

Click on the four (4) corners of Solid 2. Hold the shift key down while you click

-Apply-

Table 7-167

◆Finite Elements

Action:

Create

Object:

Mesh

Type:

Solid 0.1

Global Edge Length= Element Topology=

Hex8

Solid List

Solid 1 2 -Apply-

Main Index

Highlight

314

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Remove Coincident Nodes

Table 7-168

◆ Finite Elements

Action:

Equivalence

Object:

All

Method:

Tolerance Cube

Equivalencing Tolerance

0.005

-Apply-

Specify Thermal Material Properties

Table 7-169

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Material Name

Ge

Input Properties... Solid properties

Constitutive Model Thermal Conductivity

1.524

-ApplyMaterial Name

Solder Solid properties

Constitutive Model Thermal Conductivity -Apply-

Main Index

1.27

Chapter 7: Example Problems 315 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Define Element Properties

Table 7-170

◆ Properties Create

Action:

3D

Dimension:

Solid

Type: Property Set Name

Ge

Input Properties... Material Name

m:Ge

Select from Material Property Sets

OK Change the view to Bottom View

Select Members

Solid 2 Add -Apply-

Property Set Name

Solder

Input Properties... Material Name

m:Solder OK

Select Members

Solid 1 Add -Apply-

Main Index

Select from Material Property Sets

316

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Main Index

Chapter 7: Example Problems 317 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Apply Temperature Boundary Conditions Table 7-171

◆ Load/Boundary Conditions

Action:

Create

Object:

Temp (Thermal) Nodal

Type:

Thermal

Analysis Type: New Set Name

temp_bottom

Input Data... Boundary Temperature

70

OK Select Application Region

◆Geometry

Geometry Filter

Click on the Surface or Face icon

Select Geometry Entities

Surface 1

Click on bottom surface

Add OK -Apply-

New Set Name

temp_top

Input Data... Boundary Temperature

-30

OK Select Application Region

◆Geometry

Geometry Filter

Click on the Surface icon

Select Geometry Entities Add OK -ApplyMain Index

Solid 2.6

318

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Perform the Thermal Analysis

Table 7-172

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Job Name

ex10 -Apply-

Read in the Analysis Results

◆ Analysis Action:

Read Output2

Object:

Result Entities

Method:

Translate

Table 7-173 Job Name

ex10

Select Results File... ex10.op2 OK -Apply-

Main Index

Highlight

Chapter 7: Example Problems 319 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Display the Results

◆ Results Object:

Quick Plot

Table 7-174 Select Results Cases

Default, PW Linear: 100. % of Load Temperatures

Select Fringe Result

-ApplyDefine a Spatial FEM Field Based on the Temperature Profile

◆Fields Action:

Create

Object:

Spatial

Method:

FEM

Table 7-175 Field Name

t_load

FEM Field Definition

◆Continuous

Field Type

◆Scalar

Mesh/Results Group Filter

◆Current Viewport

Select Group

default_group -Apply-

Main Index

Highlight

320

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Change the Analysis Type to Structural

Table 7-176 Preferences Analysis...

Analysis Type:

Structural OK

Main Index

Chapter 7: Example Problems 321 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Specify Structural Material Properties

Table 7-177

◆ Materials

Action:

Create

Object:

Isotropic

Method:

Manual Input

Material Name

Solder_st

Input Properties... Linear Elastic

Constitutive Model Elastic Modulus =

1.3e7

Poisson Ratio =

0.4

Thermal Expan. Coeff =

2.47e-5

Reference Temperature

-30.0

-ApplyMaterial Name

Ge_st Linear Elastic

Constitutive Model Elastic Modulus =

1.885e7

Shear Modulus =

0.933e7

Thermal Expan. Coeff =

5.8e-6

Reference Temperature

-30.0

-Apply-

Main Index

322

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Assign Element Properties

Table 7-178

◆ Properties Create

Action:

3D

Dimension:

Solid

Type: Property Set Name

Ge_st Standard Formulation

Options: Input Properties... Material Name

m:Ge_st

Select from Material Property Sets

OK Select Members

Solid 2 Add -Apply-

Property Set Name

Solder_st Standard Formulation

Options: Input Properties... Material Name

m:Solder_st OK

Select Members

Solid 1 Add -Apply-

Main Index

Select from Material Property Sets

Chapter 7: Example Problems 323 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Create a New Load Case

Table 7-179

◆ Load Cases Create

Action: Load Case Name Load Case Type: -Apply-

Main Index

struct_load Static

324

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Define a Temperature Load

Table 7-180

◆ Load/Boundary Conditions

Action:

Create

Object:

Temperature Nodal

Type:

Structural

Analysis Type:

struct_load

Current Load Case: New Set Name

Switch to Structural from Thermal

temp_load

Input Data... Load/BC Set Scale Factor

1.0

Temperature

f:t_load

Select from Spatial Fields

OK Select Application Region

◆Geometry

Geometry Filter

Click on the Solid icon

Select Geometry Entities Add OK -Apply-

Main Index

Solid 1 2

Chapter 7: Example Problems 325 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Main Index

326

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Apply Constraints

Apply constraints on the four corner points of the top surface. Table 7-181

◆ Load/Boundary Conditions

Action:

Create

Object:

Displacement Nodal

Type:

Structural

Analysis Type New Set Name:

fix_x

Input Data... Load/BC Set Scale Factor

1.0

Translations

< 0., , >

OK Select Application Region

◆Geometry

Geometry Filter

Click on the Point icon

Select Geometry Entities

Point 9 10

Add OK -Apply-

New Set Name:

fix_y

Input Data... Load/BC Set Scale Factor

1.0

Translations

< , 0., >

OK Select Application Region Geometry Filter

◆Geometry

Select Geometry Entities

Point 11

Add OK -ApplyMain Index

Chapter 7: Example Problems 327 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

New Set Name:

fix_z

Input Data... Load/BC Set Scale Factor

1.0

Translations

< , , 0.>

OK Select Application Region Geometry Filter

◆Geometry

Select Geometry Entities

Point 9:12

Add OK -Apply-

Perform the Structural Analysis

Table 7-182

◆ Analysis

Action:

Analyze

Object:

Entire Model

Method:

Full Run

Job Name

ex10_st Subcase Select

Subcases For Solution Sequence: 101

struct_load

Highlight

Subcases Selected:

struct_load

Click on Default to remove

OK -Apply-

Main Index

328

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Read in the Analysis Results

Table 7-183

◆ Analysis

Action:

Read Output2

Object:

Result Entities

Method:

Translate

Job Name

ex10_st

Select Results File... ex10_st.op2

Highlight

OK -Apply-

Display the Results

◆ Results Quick Plot

Object:

Table 7-184 Select Results Cases Select Fringe Result

struct_load, Static Subcase Stress Tensor von Mises

Quantity: Select Deformation Result

Displacements, Translational

-ApplyDiscussion of Results The reference or zero stress state for the assembly is initialized at -30 oC. The thermal coefficient of expansion for the solder is approximately four times that of Ge. When the temperature gradient

Main Index

Chapter 7: Example Problems 329 Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

associated with the temperature boundary conditions is applied, the solder layer wants to grow significantly more than the Ge layer due not only to the higher coefficient of thermal expansion, but also because of the higher temperature relative to TREF. The Ge layer ends up with a more complex stress pattern due to its four corner points being constrained, the distribution of temperature through the layer, and the growth enforced by the solder layer. The free surface of the solder layer exhibits the low stress levels.

Main Index

330

Patran Interface to MD Nastran Thermal Example 10 - Thermal Stress Analysis of a Bi-Metallic Plate

Main Index

A

Files

J

Main Index

Files

332

332 Files

1.1

Files The Patran MD Nastran Preference uses or creates several files.The following table outlines each file and its uses. In the file name definition, jobname will be replaced with the jobname assigned by the user. Description

*.db

This is the Patran database. During an analyze pass, model data is read from this database and, during a Read Results pass, model and/or results data is written into it. This file typically resides in the current directory.

jobname.jbr

These are small files used to pass certain information between Patran and the independent translation programs during translation. There should never be a need to directly alter these files. These files typically reside in the current directory.

jobname.bdf

This is the MD Nastran input file created by the interface. This file typically resides in the current directory.

msc_v#_sol#.alt

These are a series of MD Nastran alters that are read during forward translation. These alters instruct MD Nastran to write information to the OUTPUT2 file that the results translation will be looking for. The forward translator searches the Patran file path for these files, but they typically reside in the /alters directory. If these files do not meet specific needs, edit them accordingly. However, the naming convention of msc_v# _sol#<solution #>.alt must be preserved. Either place the edited file back into the /alters directory or in any directory on the Patran file path, which takes precedence over the /alters directory. If these files are not used, remove them from the Patran file path, rename them, or delete them altogether.

jobname.op2

This is the NASTRAN OUTPUT2 file, which is read by the Read Results pass. This file typically resides in the current directory.

jobname.flat

This file may be generated during a Read Results pass. If the results translation cannot write data directly into the specified Patran database, it will create this jobname.flat file. This file typically resides in the current directory.

jobname.msg.xx

These message files contain any diagnostic output from the translation, either forward or reverse. This file typically resides in the current directory.

MscNastranExecute

This is a UNIX script file, which is called on to submit MD Nastran after translation is complete. This file might need customizing with site specific data, such as, host machine name and MD Nastran executable commands. This file contains many comments and should be easy to edit. Patran searches its file path to find this file, but it typically resides in the /bin/exe directory. Either use the general copy in /bin/exe, or place a local copy in a directory on the file path, which takes precedence over the /bin/exe directory.

Main Index

B

Error Messages

J

Main Index

Error Messages

334

334 Error Messages

2.1

Error Messages There are many error or warning messages that may be generated by the Patran MD Nastran Interface. The following table outlines some of these. Description

Unable to open a new message file " ". Translation If the translation tries to open a message file and cannot, it messages will be written to standard output. will write messages to Standard Output. On most systems, the translator automatically writes dmessages to standard output and never tries to create a separate message file. Unable to open the specified OUTPUT2 file " ".

The OUTPUT2 file was not found. Check the OUTPUT2 file specification in the translation control file.

The specified OUTPUT2 file " " is not in standard binary format and cannot be translated.

The OUTPUT2 file is not in standard binary format. Check the OUTPUT2 file specification in the translation control file.

Group " " does not exist in the database. Model data will not be translated.

The name of a nonexistent group was specified in the translator control file. No model data will be translated from the OUTPUT2 file.

Needed file specification missing! The full name of The translation control file must be specified as the first the job file must be specified as the first command- on-line argument to the translator. line argument to this program. Unable to open the specified database " ". Writing the OUTPUT2 information to the PCL command file " ". Unable to open either the specified database " or a PCL command file, " ". Unable to open the NASTRAN input file " Unable to open the specified database, "

If the translator cannot communicate directly to the specified database. It will write the results and/or model data to a PCL session file. ",

". ".

The naspat3 translator is unable to open any output file. Check file specification and directory protection. The translator was unable to open a file to where the input file information will be written. The forward Patran MD Nastran translator was unable to open the specified Patran database.

Alter file of the name " " could not be found. No OUPUT2 alter will be written to the NASTRAN input file.

The OUTPUT2 DMAP alter file, for this type of analysis, could not be found. Correct the search path to include the necessary directory if you want the alter files to be written to the input file.

No property regions are defined in the database. No elements or element properties can be translated.

Elements referenced by an element property region in the Patran database will not get translated by the forward Patran MD Nastran translator. If no element regions are defined, no elements will be translated.

Main Index

C

Main Index

Supported Commands

J

File Management Statements

336

J

Executive Control Statements

337

J

Case Control Commands

J

Bulk Data Entries

339

338

336 File Management Statements

3.1

File Management Statements The following MD Nastran File Management statement is supported. Description

ASSIGN

Main Index

An ASSIGN command is used to assign a particular name (job name + user specified MD Nastran results suffix) to the NASTRAN OUTPUT2 file to be created during the analysis.

337 Executive Control Statements

3.2

Executive Control Statements The following MD Nastran Executive Control statements are supported. Description

SOL

Specifies the solution sequence or main subDMAP to be executed. (p. 113)

TIME

Sets the maximum CPU and I/O time.(p. 114), (p. 117)

Main Index

338 Case Control Commands

3.3

Case Control Commands The following MD Nastran Case Control commands are supported. Description

DLOAD

Selects a dynamic load or an acoustic source to be applied in a transient or frequency response problem. (p. 66)

ECHO

Controls echo (i.e., printout) of the Bulk Data. (p. 114), (p. 117)

ENTHALPY

Requests form of enthalpy vector output in transient heat transfer analysis (SOL 159). (p. 130)

FLUX

Requests the form and type of gradient and flux output in heat transfer analysis. (p. 130)

HDOT

Requests form of rate of change of enthalpy vector output in transient heat transfer analysis (SOL 159). (p. 130)

IC

Selects the initial conditions for direct transient analysis (SOLs 27, 69, 99, 109, 129, and 159). (p. 75)

LOAD

Selects an external static load set. (p. 66)

MAXLINES

Sets the maximum number of output lines. (p. 114), (p. 117)

MPC

Selects a multipoint constraint set. (p. 50)

NLPARM

Selects the parameters used for nonlinear static analysis. (p. 123), (p. 133)

OLOAD

Requests the form and type of applied load vector output. (p. 130)

SPC

Selects a single-point constraint set to be applied. (p. 73)

SPCFORCES

Requests the form and type of single-point force of constraint vector output. (p. 130)

SUBCASE

Delimits and identifies a subcase. (p. 121), (p. 135)

SUBTITLE

Defines a subtitle that will appear on the second heading line of each page of printer output. (p. 121)

TEMPERATURE

Selects the temperature set to be used in either material property calculations or thermal loading in heat transfer and structural analysis. (p. 75)

THERMAL

Requests the form and type of temperature output. (p. 130)

TITLE

Defines a character string that will appear on the first heading line of each page of MD Nastran printer output. (p. 106)

TSTEPNL

Selects integration and output time steps for nonlinear transient problems. (p. 128), (p. 133)

Main Index

339 Bulk Data Entries

3.4

Bulk Data Entries The following MD Nastran Bulk Data entries are supported. Description

CBAR

Defines a simple beam element. (p. 60)

CBEAM

Defines a beam element. (p. 62)

CBEND

Defines a curved beam, curved pipe, or elbow element. (p. 61) (p. 62)

CDAMP1

Defines a scalar damper element. (p. 60)

CELAS1

Defines a scalar spring element. (p. 60)

CHBDYG

Defines a boundary condition surface element without reference to a property entry. (p. 71)

CHBDYP

Defines a boundary condition surface element with reference to a PHBDY entry. (p. 63), (p. 71)

CHEXA

Defines the connections of the six-sided solid element with eight to twenty grid points. (p. 65)

CONROD

Defines a rod element without reference to a property entry.(p. 110)

CONV

Specifies a free convection boundary condition for heat transfer analysis through connection to a surface element (CHBDYi entry). (p. 81), (p. 85), (p. 90)

CONVM

Specifies a forced convection boundary condition for heat transfer analysis through connection to a surface element (CHBDYi entry). (p. 82), (p. 87), (p. 90)

CORD2C

Defines a cylindrical coordinate system using the coordinates of three points. (p. 51)

CORD2R

Defines a rectangular coordinate system using the coordinates of three points. (p. 51)

CORD2S

Defines a spherical coordinate system using the coordinates of three points. (p. 51)

CPENTA

Defines the connections of a five-sided solid element with six to fifteen grid points. (p. 65)

CQUAD4

Defines an isoparametric membrane-bending or plane strain quadrilateral plate element. (p. 64)

CQUAD8

Defines a curved quadrilateral shell or plane strain element with eight grid points. (p. 64)

CROD

Defines a tension-compression-torsion element. (p. 60)

CTETRA

Defines the connections of the four-sided solid element with four to ten grid points. (p. 65)

CTRIA3

Defines an isoparametric membrane-bending or plane strain triangular plate element.

CTRIA6

Defines a curved triangular shell element or plane strain with six grid points. (p. 64)

CTRIAX6

Defines an isoparametric and axisymmetric triangular cross section ring element with midside grid points. (p. 65)

CTUBE

Defines a tension-compression-torsion tube element. (p. 63)

DLOAD

Defines a dynamic loading condition for frequency response or transient response problems as a linear combination of load sets defined via RLOAD1 or RLOAD2 entries for frequency response or TLOAD1 or TLOAD2 entries for transient response. (p. 66)

(p. 64)

Main Index

340 Bulk Data Entries

Description INCLUDE

Inserts an external file into the input file. The INCLUDE statement may appear anywhere within the input data file. (p. 109)

MAT4

Defines the constant or temperature dependent thermal material properties for conductivity, heat capacity, density, dynamic viscosity, heat generation, reference enthalpy and latent heat associated with a single phase change. (p. 53)

MAT5

Defines the thermal material properties for anisotropic materials. (p. 53)

MATT4

Specifies table references for temperature-dependent MAT4 material properties. (p. 53)

MATT5

Specifies temperature-dependent material properties on MAT5 entry fields via TABLEMi entries. (p. 53)

MPC

Defines a multipoint constraint equation of the form. (p. 50)

NLPARM

Defines a set of parameters for nonlinear static analysis iteration strategy. (p. 123), (p. 133)

PARAM,AUT OSPC

AUTOSPC specifies the action to take when singularities exist in the stiffness matrix [Kgg]. AUTOSPC = YES means that singularities will be constrained automatically. AUTOSPC = NO means that singularities will not be constrained. (p. 114)

PARAM,PRG PST

Controls the printout of singularities. See AUTOSPC. Default = YES. (p. 117)

PARAM,SIG MA

The radiant heat flux is proportional to SIGMA*(Tgrid + TABS)4, where SIGMA is the Stefan-Boltzmann constant. Default = 0.0. (p. 115)

PARAM,TAB S

TABS is used to convert units of the temperature input (oF or oC) to the absolute temperature (°R or °K). Default = 0.0. (p. 115)

PBAR

Defines the properties of a simple beam element (CBAR entry). (p. 60)

PBEAM

Defines the properties of a beam element (CBEAM entry). This element may be used to model tapered beams. (p. 62)

PBEND

Defines the properties of a curved beam, curved pipe, or elbow element (CBEND entry). (p. 61) (p. 62)

PCONV

Specifies the free convection boundary condition properties of a boundary condition surface element used for heat transfer analysis. (p. 81), (p. 85), (p. 90)

PCONVM

Specifies the forced convection boundary condition properties of a boundary condition surface element used for heat transfer analysis. (p. 82), (p. 87), (p. 90)

PDAMP

Specifies the damping value of a scalar damper element using defined CDAMP1 or CDAMP3 entries. (p. 60)

PELAS

Specifies the stiffness, damping coefficient, and stress coefficient of a scalar elastic (spring) element (CELAS1 or CELAS3 entry). (p. 60)

PHBDY

Referenced by CHBDYP entries to give auxiliary geometric information for boundary condition surface elements. (p. 63), (p. 71)

PROD

Defines the properties of a rod element (CROD entry). (p. 60)

Main Index

341 Bulk Data Entries

Description PSHELL

Defines the membrane, bending, transverse shear, and coupling properties of thin shell elements. (p. 64)

PSOLID

Defines the properties of solid elements (CHEXA, CPENTA, and CTETRA entries). (p. 65)

PTUBE

Defines the properties of a thin-walled cylindrical tube element (CTUBE entry). (p. 63)

QBDY2

Defines grid point heat flux into CHBDYi elements. (p. 76)

QBDY3

Defines a uniform heat flux load for a boundary surface. (p. 76)

QHBDY

Defines a uniform heat flux load into a set of grid points. (p. 79)

QVECT

Defines thermal vector flux from a distant source into a face of one or more CHBDYi boundary condition surface elements. (p. 77)

QVOL

Defines a rate of volumetric heat addition in a conduction element. (p. 56), (p. 80)

RADBC

Specifies a CHBDYi element face for application of radiation boundary conditions. (p. 96),

RADCAV

Identifies the characteristics of each radiant enclosure. (p. 98), (p. 115), (p. 115)

RADM

Defines the radiation properties of a boundary element for heat transfer analysis. (p. 77), (p. 96), (p. 97), (p. 98)

RADMT

Specifies table references for temperature dependent RADM entry radiation boundary properties. (p. 71), (p. 77), (p. 96), (p. 97), (p. 98)

RADSET

Specifies which radiation cavities are to be included for radiation enclosure analysis.

(p. 97)

(p. 98)

SLOAD

Defines concentrated static loads on scalar or grid points. (p. 79)

SPC

Defines a set of single point constraints and enforced displacements. (p. 73)

SPOINT

Defines scalar points. (p. 81), (p. 82), (p. 96)

TABLED1

Defines a tabular function for use in generating frequency-dependent and time-dependent dynamic loads. (p. 71)

TABLEM1

Defines a tabular function for use in generating temperature-dependent material properties. (p. 53), (p. 71)

TEMP

Defines temperature at grid points for determination of thermal loading, temperaturedependent material properties, or stress recovery. (p. 75)

TEMPBC

Defines the temperature boundary conditions for heat transfer analysis. Applies to steady state and transient conditions. (p. 73)

TEMPD

Defines a temperature value for all grid points of the structural model which have not been given a temperature on a TEMP entry. (p. 114), (p. 117)

TLOAD1

Defines a time-dependent dynamic load or enforced motion of the form. (p. 66), (p. 71)

TSTEPNL

Defines parametric controls and data for nonlinear transient structural or heat transfer analysis. TSTEPNL is intended for SOLs 129, 159, and 99. (p. 128), (p. 133)

Main Index

342 Bulk Data Entries

Description VIEW

Defines radiation cavity and shadowing for radiation view factor calculations. (p. 98)

VIEW3D

Defines parameters to control and/or request the Gaussian Integration method of view factor calculation for a specified cavity. (p. 115)

Main Index

MSC.Fatigue Quick Start Guide

Index Patran Interface to MD Nastran Thermal

A Pa tra n Int erf ac e to M

case control, 119, 133, 338 conductivity, 5 contour plots, 41, 138, 151 convergence criteria, 14, 125, 127, 129 coordinate frames, 47, 51, 110, 145 analysis coordinate frames, 47 reference coordinate frames, 47

film node, 69, 82, 85, 87, 90, 93, 95 finite element mesh, 26, 46, 47 finite element properties, 30, 46, 49, 57, 58 0D, 58, 59 1D, 58, 59 2D, 58, 60 2D axisymmetric solid elements, 65 2D shell elements, 64 3D, 58, 60 3D solid elements, 65 beam and rod elements-general section, 60 capacitors, 60 conductors, 60 curved general section beam, 61 curved pipe section beam, 62 flow tube, 63 pipe section rod, 63 tapered section beam, 62 forced convection, 8 formats, 110 free convection, 8

D

G

absolute temperature, 10, 115 alter file, 109 ambient temperature, 8, 82, 84, 85, 89, 91 analysis, 105, 108 analysis form, 106 applied linear loads, 143, 147 Attach XDB, 139

B bulk data entry, 109, 110, 111, 119, 339 bulk data file, 162

C

database (Patran), 22, 138, 143 delete XY window, 158 direct text input, 119, 133

E elements, 145 enthalpies, 144, 148 error messages, 334 executive control, 119, 337

F file management statements, 119, 336 files, 332 film coefficient(see also heat transfer coefficient), 8

Main Index

GEOM1, 144 GEOM2, 145 geometry creation, 25 geometry import, 46 grid points, 48

H heat flows, 143, 148 heat flux, 8, 143, 148, 152 heat generation, 7, 8, 56 heat transfer coefficient, 7, 8, 9, 82, 83, 84, 86, 89, 90, 92, 93, 94 heats of constraint, 143, 147

344 Patran Interface to MD Nastran Thermal

I

P

INCLUDE files, 110 input file, 162 input file reader, 112, 119

Prandtl number, 8, 9, 56, 85, 90, 95

K Kirchhoff’s Identity, 10

L load cases, 101, 104 load tolerance, 14, 125, 127, 129

M material properties, 5, 29, 46, 52 absorptivity, 9, 10, 77, 78, 79, 96, 97 anisotropic, 55, 56 conductivity, 5, 56 consistent units, 6 density, 5, 56 dynamic viscosity, 6, 56 emissivity, 9, 10, 96, 97, 98 enthalpy, 6, 56 heat capacitance, 5, 56 isotropic, 54, 55, 56 latent heat, 6, 56 orthotropic, 54, 56 specific heat, 5, 56 MSC.Nastran version, 110 Patran Analysis Manager, 107 multi-point constraints, 47, 50

N node points, 47 nodes, 47, 110, 144 numbering options, 110, 111

O OEF1, 143 OPG1, 143 OQG1, 143 OUGV1, 143 output requests, 130, 132, 133, 143, 144, 147 OUTPUT2, 41, 109, 138, 139, 141, 143, 144

Main Index

R radiation ambient nodes, 68, 97 ambient space, 68, 96 enclosures, 68, 98 rate of change of enthalpies, 144, 148 read input file, 162 results, 141 results postprocessing, 41, 150 Reynolds number, 8, 9, 56, 85, 88, 90, 95

S steady-state analysis (SOL 153), 11, 40, 113 initial conditions, 12 Newton-Raphson iteration, 11 radiation parameters, 114, 115 solution parameters, 114, 127 subcase parameters, 123, 125, 127 view factor parameters, 114, 116 Stefan-Boltzmann constant, 10, 115 subcase, 104, 107, 121, 123, 135 SUPG, 9, 56

T temperature gradients, 143, 148, 152 temperature tolerance, 14, 124, 127, 129 thermal analysis loads and boundary conditions, 7 steady-state analysis, 11 transient analysis, 13 units, 6, 7

INDEX 345

thermal loads and BCs, 7, 46, 66 advection, forced convection, 8, 68 basic convection, 8, 37, 68 consistent units, 7 contact, 68 control nodes, 69, 76, 79, 80 convection coupled, 85 convection coupled advection, 90 convection coupled flow tube, 87 convection flow tube to ambient, 82 convection to ambient, 81 directional heat flux, 8, 68, 77, 79 directional heat flux-function of time, 78, 79 flow tubes, 82, 87, 90 initial temperatures, 75 nodal source, 8, 68, 79 normal heat flux, 7, 34, 68, 76 radiation enclosures, 10, 68, 98 radiation to ambient nodes, 97 radiation to space, 9, 68, 96 spatial dependence, 71 surface area, 71 temperature boundary conditions, 7, 32, 68, 73 temperature dependence, 71 time dependence, 71 two application regions, 70, 85, 87, 90, 97 volumetric heat generation, 8, 54, 56, 68, 80 tolerances, 109 transient analysis (SOL 159), 13, 113 initial conditions, 13 initial time step, 13, 128 solution parameters, 117 subcase parameters, 128 translation parameters, 109, 110

U undo feature, 27

V view factors, 10, 97, 115, 117

Main Index

W work tolerance, 14, 124, 127, 129

X XY plots, 138, 153, 156

346 Patran Interface to MD Nastran Thermal

Main Index