Temperature dialog box (Nastran/Multiphysics/Samcef-Structural/Abaqus)

Type
Type	Temperature: Applies a temperature load to the selected geometry or nodes.Node ID Table: Lets you use varying temperature values at the nodes identified in the node ID table. For each node in the node ID table, the temperature magnitude is multiplied by a scale factor.Simcenter Nastran and MSC Nastran environment options:Through Thickness (Temperature and Gradient): Defines the temperature and gradient in the thickness direction for a 2D element.Through Thickness (Top and Bottom): Defines temperatures for additional membrane stress calculation at the lower and upper surface of 2D elements.On 1D elements: Lets you define temperature loads for certain types of 1D elements. Depending on the type of element, you can specify the temperature at each end as well as the gradient.Temperature – External Time Unassigned: Applies a temperature load from an imported results file. You can import results from Nastran, Simcenter 3D Thermal, Abaqus, or ANSYS. Simcenter 3D Multiphysics environment options:Temperature – Time Assigned: Defines a temperature load with a time-dependent field.Temperature – External Time Unassigned: Applies a temperature load from an imported results file. You can import results from Nastran, Simcenter 3D Thermal, Abaqus, or ANSYS. Temperature – External Time Assigned: Applies a time-dependent temperature load from an imported Simcenter 3D Thermal (.bun) file.Abaqus environment options:Temperature – External: Applies a temperature load from an Abaqus results (.fil) or output database (.odb) file.
Destination Folder
Load Container	Specifies the folder in the Simulation Navigator in which the boundary condition will be stored. The list includes the root container and existing folders that you created using the New Folder command. Examples of a root container include Load Container, Constraint Container, and Simulation Object Container.To view a hierarchical list of existing folders, click Folder Manager . To create a new folder, right-click any level of the hierarchy and choose New Folder.
Model Object/Model Objects
Group Reference	Appears when Type is set to Temperature, Through Thickness (Temperature and Gradient), Through Thickness (Top and Bottom), On 1D Elements, or Temperature –Time Assigned.Lets you apply the pressure load to a group.For more information, see Group Reference options.
Select Object	Lets you select the geometry or nodes on which to apply the load.
Stacked Smart Selector Methods	Opens the Smart Selector Methods dialog box where you can specify a progression of smart selection filters.For more information, see Smart Selector Methods dialog box.
Excluded	Appears when Type is set to Temperature, Node ID Table, Through Thickness (Temperature and Gradient), Through Thickness (Top and Bottom), On 1D Elements, or Temperature – Time Assigned.Lets you remove individual entities from within the selected object.
Magnitude
Appears when Type is set to Temperature, Node ID Table, Through Thickness (Temperature and Gradient), Through Thickness (Top and Bottom), Temperature Time Assigned, Temperatures – External Time Unassigned, or Temperature – External.
Temperature	Appears when Type is set to Temperature or Node ID Table.Sets the magnitude of the temperature load.For more information about defining a constant value, expression, or a field, see Additional magnitude options.
Temperature at Element Reference Plane	Appears when Type is set to Through Thickness (Temperature and Gradient).Sets the temperature at the element’s reference plane as defined by the Shell Offset value in the Mesh Associated Data dialog box (ZOFFS). This option corresponds to the TBAR field on the TEMPP1 bulk data entry.For more information about defining a constant value, expression, or a field, see Additional magnitude options.
Effective Linear Gradient	Appears when Type is set to Through Thickness (Temperature and Gradient).Sets the effective linear thermal gradient. This option corresponds to the TPRIME field on the TEMPP1 bulk data entry.For more information about defining a constant value, expression, or a field, see Additional magnitude options.
Temperature at Z1****Temperature at Z2	Appears when Type is set to Through Thickness (Temperature and Gradient) or Through Thickness (Top and Bottom).Sets the temperatures for an additional membrane stress calculation at points (Z1 and Z2) which you define in the PSHELL physical property table dialog box.These options correspond to the T1 and T2 fields on the TEMPP1 bulk data entry.For more information about defining a constant value, expression, or a field, see Additional magnitude options.
Specify Field	Appears when Type is set to Temperature – Time Assigned.Lets you select or define a field. One of the independent variables of your field must be time.
Scale Factor	Appears when Type is set to Temperature – Time Assigned.Applies a constant scale to the temperatures defined by the field.
File Type	Appears when Type is set to Temperature – External Time Unassigned or Temperature – External.Specifies the type of results file to import.Temperature – External Time Unassigned options:Nastran TemperaturesSimcenter 3D Thermal TemperaturesAbaqus TemperaturesANSYS TemperaturesTemperature – External options:ODB Temperatures: Specifies an Abaqus .odb output database file. FIL Temperatures: Specifies an Abaqus .fil result file.
Results File	Appears when Type is set to Temperature – External Time Unassigned, Temperature – External Time Assigned, or Temperature – External.Lets you select the results file to import.The software infers and stores the path to the file that you specify relative to the Simulation file. If the location of the file changes, the software uses the stored relative path information to try to locate the file. For more information, see Relative path support for external files.
End A/End B
Appear when Type is set to On 1D Elements.
Temperature at End A/Temperature at End B	Sets the temperature at ends A and B on the element’s neutral axis. These options correspond to the TA and TB fields on the TEMPRB bulk data entry.For more information about defining a constant value, expression, or a field, see Additional magnitude options.
Gradient in direction 1/Gradient in direction 2	Sets the effective linear gradient in directions 1 and 2 for CBAR, CBEAM, and CBEND elements. These options correspond to the TPij fields on the TEMPRB bulk data entry.For more information about defining a constant value, expression, or a field, see Additional magnitude options.
Temperature at SRP C, D, E, F	Sets the temperatures at the stress recovery points for CBAR, CBEAM, and CBEND elements. These options correspond to the Tij fields on the TEMPRB bulk data entry.For more information about defining a constant value, expression, or a field, see Additional magnitude options.
Scaling ID Table
Appears when Type is set to Node ID Table.
Specify Field	Lets you define temperature load magnitude on specific nodes in the node ID table.
Card Name	Displays the name of the solver card for the load.
Reading Temperature Parameters
Appears when type is set to Temperature – External.
Begin Step Number	Sets the step number that begins the history data to be read. If you enter no value, Abaqus begins reading temperature data from the first step available.
Begin Increment Number	Sets the increment number that begins the history data to be read. If you enter no value, Abaqus begins reading temperature data from the first increment available.
End Step Number	Sets the step number that ends the history data to be read. If you specify no value, the software sets End Step Number equal to Begin Step Number.
End Increment Number	Sets the increment number that ends the history data to be read. If you specify no value, the software sets End Increment Number to the last available increment of the end step specified in End Step Number.
Temperature Ramping – Starting Time	Sets the starting time measured relative to the total step time period after which the temperatures read from the results file are ramped to their initial condition values. The default value is 1.0, and no temperature ramping occurs. You can use Temperature Ramping – Starting Time to set a cyclic temperature history from a prior heat transfer analysis that is not cyclic.
Interpolation Method	Specifies the interpolation method:InterpolateSpecifies that the temperature field is to be interpolated between dissimilar meshes. Use this option to read temperatures from an output database file generated during a heat transfer analysis or generated during a global model analysis used with the submodeling capability. MidsideSpecifies that midside node temperatures in second-order elements are to be interpolated from corner node temperatures. Use this option to read temperatures from a results or an output database file generated during a heat transfer analysis using first-order elements.NoneSpecifies that the software does not perform an interpolation.
Absolute Exterior Tolerance	Appears when Interpolation Method is set to Interpolate. Sets the absolute value in model units by which nodes of the current model can lie outside the region of the model.
Exterior Tolerance	Appears when Interpolation Method is set to Interpolate. Sets the fraction of the average element size by which nodes of the current model can lie outside the region of the elements of the model.

How do I

Define a temperature load

Learn more

Temperature

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Temperature dialog box (Nastran/Multiphysics/Samcef-Structural/Abaqus), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });