THERMO-STRUCTURAL ANALYSIS SECTION 15 THERMO-STRUCTURAL ANALYSIS

TABLE OF CONTENTS Section Page 15.0 Thermo-structural Analysis Overview…………………………………………………………………………………………………………….. 15-3 Free Thermal Expansion ………………………………………………………………………………………….. 15-4 Restrained Thermal Growth ……………………………………………………………..……………………….. 15-5 Thermal Strains And Stresses ………………………………………………………………………………….... 15-6 Differential Thermal Expansion ………………………….……………………………………………………….. 15-7 Temperature Loads And Conditions …………………………………………………………………………….. 15-8 Procedure …………………………………………………………………………………………………………... 15-9 Material Properties ……………………………………………..………………………………………………….. 15-10 Specifying The Temperatures ………………………………………………………...………………………….. 15-11 Using Previous Msc.Marc Analysis Results …………………………………………………………………….. 15-12 Temperature Distributions From Spatial Fields ……………………………………………………………….. 15-14 Creating Fields – Fem Fields …………………………………………………………………………………….. 15-15 Creating Temperature Loads …………………………………………………………………………………….. 15-16

OVERVIEW Free Thermal Expansion versus Restrained Thermal Growth How to Setup the Initial Temperature and the Temperature Load for a Structural Static MSC.Marc Analysis in the MSC.Patran Marc Preference Using Previous MSC.Marc Thermal Results A Walk-Thru on MSC.Patran forms that would reduce the Required Temperature Loads and Initial Conditions Free Thermal Expansion versus Restrained Thermal Growth Basic Equations Governing the Problem Required Data in MSC.Marc Differential Thermal Expansion The Physics of the Problem How to Setup the MSC.Marc Steady –State Thermal Analysis

FREE THERMAL EXPANSION Temperature changes in a structure cause thermal expansion strains Uniform Thermal Expansion or Contraction And No BCs Restringing Growth = Free Thermal Expansion No Thermal Stresses

RESTRAINED THERMAL GROWTH Non-Uniform (Differential) Thermal Expansion or Contraction And / Or BCs Restringing Growth = Mechanical Strains Mechanical Thermal Stresses

THERMAL STRAINS AND STRESSES How do we discriminate stresses due to thermal expansion out from total ones? If etotal = ethermal then we have free expansion s = 0 If etotal = 0 then emechanical = - ethermal s = -EaDT (for a 1-D problem)

DIFFERENTIAL THERMAL EXPANSION Differential Thermal Expansion occurs when: The temperature distribution is nonuniform The constituent materials have different a values Since aaluminum > asteel differential thermal expansion will occur under uniform temperature increase. Similar behavior occurs when temperature distribution is non-uniform. This differential expansion leads to mechanical stresses

TEMPERATURE LOADS AND CONDITIONS The initial and final temperature values may also be defined under MSC.Patran Load and Boundary Condition (LBC) menu Uniform values may be entered as a constant on the LBC Input Data form The initial temperature represents the “stress-free” temperature of the structure. Default=0 Note: Initial Temperature LBC’s for either thermal or structural analysis must be created with Load/BCs’ Analysis Type set to Thermal

PROCEDURE MSC.Marc will calculate the stress due to differential thermal expansion provided the user: Supplies the coefficient of thermal expansion (cte) values Supplies the initial and final temperature values Runs the analysis as a “general” step Non-Linear steps are always general steps.

MATERIAL PROPERTIES Usually a = f(T), described with a tabular material property field. This field is then referenced on the material property form

SPECIFYING THE TEMPERATURES Temperature Load Scalar Plot Temperatures may come from a steady-state or transient temperature profile Temperature distributions may be specified in one of two ways: From a previous MSC.Marc thermal analysis Post file (thermjobname.t16) As an LBC through a PATRAN spatial FEM field Example of final Temperature load created in MSC.Patran Loads/BCs form using Spatial FEM field

USING PREVIOUS MSC.MARC ANALYSIS RESULTS The final temperature distribution maybe specified as the result of a previous MSC.Marc thermal analysis Temperature from a MSC.Marc thermal analysis Done by specifying the jobname.t16 (or jobname.t19) of a given load step and increment Found on the Read Temperature form under Analysis - Step Create - Solution Parameters (shown in next slide)

USING PREVIOUS MSC.MARC ANALYSIS RESULTS (CONT.) For transient thermal results MSC.Marc will perform linear interpolation in the time domain If the structural analysis reads the temperatures directly from a previous thermal analysis’ post (t16) file, the mesh of the thermal analysis must match the mesh of the structural analysis since node-to- node results mapping is performed.

TEMPERATURE DISTRIBUTIONS FROM SPATIAL FIELDS Temperature distributions may be specified through a PATRAN spatial field Results from a different thermal analysis code can be used to create a spatial FEM field Any kind of temperature data that can be used to create a spatial field can be used to specify the distribution Any results that can be used to create a fringe plot can be used to create a FEM field Temperature data from a table can be used to create a tabular special field

CREATING FIELDS – FEM FIELDS FEM Fields are generally used to map results from one analysis to a different analysis as a Load/Boundary Condition FEM Fields are created from data associated with finite element mesh Two types of FEM Fields are available, continuous and discrete Discrete FEM Fields define data for a list of nodes or elements, no interpolation/extrapolation is available Continuous FEM Fields use interpolation to define arbitrary points within the defined region. Therefore, continuous FEM fields allow the thermal model mesh to be different than the structural model mesh

CREATING TEMPERATURE LOADS If a continuous FEM field is used and the thermal and structural meshes are different you must: Import (or keep if using the same db) the mesh from the thermal analysis to do the fringe plot and create the FEM field Keep the thermal model mesh in the structural model db as long as the FEM field is active Use separate groups for the thermal mesh and structural mesh and perform the analysis using Object: Current Group Create Initial Temperature as a Thermal Type of Load.

CREATING TEMPERATURE LOADS (CONT.) Change the Analysis type to Structural. Create a structural load case and include the Initial Temperature Use the continuous FEM field to create a Temperature Load as a Structural Type of load. Create or use all other needed structural loads and boundary conditions.

CREATING TEMPERATURE LOADS (CONT.) More details on the appropriate procedure to create FEM Fields: Display desired results or loads on mesh. Field data is defined by graphical display Assign unique name to field Select continuous for field definition, and select type of field Select the group with results or loads displayed on it. Make sure display matches field type selected Choose proper extrapolation option If mapping of 2D field onto 3D region is required Select reference coordinate system Define axis normal to 2D plane Coordinate system must be specified for 2D to 3D mapping, also.