김경종
12 KiB
Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Begin step: bstep, Begin increment: binc, End step: estep, and End increment: einc
Interpolation in time
When Abaqus reads temperature, field variable, or equivalent pressure stress data from a results file or temperatures from an output database file, it must obtain values of the field at the time points used by the analysis. Since data corresponding to these time points are usually not present in the results or output database files, Abaqus will interpolate linearly in time between the time points stored in the file to obtain values at the time points required by the analysis. Since the interpolation is linear, you must take care to provide sufficient data in the results or output database file to make this interpolation meaningful.
For the purpose of such interpolation the time period of the results being read in is determined as follows:
• The period starts at the time of the most recent increment written, of the relevant field, that precedes the beginning increment (either user-specified or default). For example if your results file contains temperature field data at increments 5, 10, and 15; and you specify a beginning increment number of 10 when reading these results; the results period starts with the time associated with increment 5 since that is the most recent increment that precedes the specified beginning increment of 10. You can ensure that the results starting time matches the beginning time of the beginning increment you specify by writing the results data with an increment frequency of 1.
• The period ends at the completion of the ending increment (either user-specified or default).
If the analysis requires data at a time point prior to the first increment for which data are available in the either of files, Abaqus will interpolate between the given initial condition data and the data of the first increment stored in the file.
Reading results for multiple fields
If data for multiple fields are being read in the same step and the time values corresponding to the starting step and increment or to the ending step and increment are different for different fields, Abaqus interpolates through the total time period from the earliest time point chosen in any file to the latest. For example, suppose the starting increment in the starting step in the temperature file begins at 3 sec and the ending increment in the ending step ends at 6 sec. During the same step we also read field variable data, for which the starting increment in the starting step begins at 2 sec and the ending increment in the ending step ends at 5 sec. In such a case the time period used for interpolation is from 2 sec to 6 sec.
Automatic adjustment of the time scale
It is convenient to set the period of the step equal to the time period of the files being read in. Otherwise, Abaqus will automatically scale the time period from the results or output database file to match the time period of the stress analysis. The scale factor is t ^ { \sigma } / t ^ { \theta } , where t ^ { \sigma } is the time period of the stress analysis and t ^ { \theta } is the total time period obtained from all results or output database files, as described above.
Obtaining results at a particular point in time
In Abaqus/Standard it is sometimes desirable to carry out a calculation corresponding to the field values at a particular point in time. For example, suppose that temperature data are available in the output file for increment 10 at time and increment 15 at time and that you wish to carry out a static analysis based on temperature values at . In this case Abaqus must interpolate linearly between the results at and to obtain the intermediate result at . To accomplish this task, you should specify an initial time increment of 4.5 and a time period of 5. for the static analysis step and read the temperature values from the output file starting at Step 1, Increment 1 and ending at Step 1, Increment 15. Specifying a starting increment of 1 instead of 10 ensures that is the entire time period stored in the output file, not just the period between increments 10 and 15; hence, the scale factor between the output file data and the static analysis is unity, and the initial time of 4.5 has the desired meaning.
Initial transients
To track initial transients accurately, Abaqus/Standard may automatically reduce the initial time increment for the step. If the user-specified suggested initial time increment is greater than the scaled value of the first time increment read from the Abaqus/Standard results file, Abaqus/Standard will use that scaled value.
Restrictions
The following restrictions exist:
• Temperatures and field variables cannot be read from a user-specified file in a modified Riks static analysis step (“Unstable collapse and postbuckling analysis,” Section 6.2.4).
• Temperature cannot be interpolated from a coupled thermal-electrical analysis.
• Equivalent pressure stress cannot be read from the results file if the model is defined in terms of an assembly of part instances.
• In Abaqus/Explicit field variables cannot be read from the output database file.
• Pressure stress cannot be read from the output database file.
• Elements that do not support interpolation for temperature mapping include the complete libraries of convective heat transfer elements, axisymmetric elements with nonlinear axisymmetric deformation, axisymmetric surface elements, truss elements, beam elements, link elements, hydrostatic fluid elements, solid infinite stress elements, and coupled thermal/electrical elements. Other specific elements that are not supported include: GKPS6, GKPE6, GKAX6, GK3D18, GK3D12M, GK3D4L, GK3D6L, GKPS4N, GKAX6N, GK3D18N, GK3D12MN, GK3D4LN, and GK3D6LN.
Defining the values of a predefined field in a user subroutine
In Abaqus/Standard you can specify predefined temperatures, field variables, equivalent pressure stresses, or mass flow rates at the nodes in a user subroutine. Temperature values can be defined in user
subroutine UTEMP; field variable values, in user subroutine UFIELD; equivalent pressure stress values, in user subroutine UPRESS; and mass flow rates, in user subroutine UMASFL.
The user subroutine (UTEMP, UFIELD, UPRESS, or UMASFL) will be called for each specified node. Field values entered directly will be ignored. If a results or output database file has been specified in addition to the user subroutine, values read from the results or output database file will be passed into the user subroutine for possible modification.
Input File Usage: Use one of the following options:
*TEMPERATURE, USER
*FIELD, USER
*PRESSURE STRESS, USER
*MASS FLOW RATE, USER
Abaqus/CAE Usage: In Abaqus/CAE only predefined temperature fields are available.
Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: User-defined or From results or output database file and user-defined
Updating multiple predefined field variables
If multiple field variables are predefined, only one field variable at a time can be redefined in user subroutine UFIELD. There are situations in which the analysis requires a number of field variables that are predefined with respect to the solution but depend on each other. You can specify the number of field variables to be updated simultaneously at a point, n. Abaqus/Standard passes information about n field variables at each specified node into UFIELD.
You can update all or part of the field variables used in the analysis but must remember that the field variables are numbered consecutively from 1. If, for example, you have four field variables in the analysis and want to update the second and third variables simultaneously in subroutine UFIELD, you must specify n=3. In this case Abaqus/Standard passes information about the first three field variables into subroutine UFIELD, and you update only the second and third variables.
Input File Usage: *FIELD, USER, NUMBER=n
Abaqus/CAE Usage: Predefined field variables are not supported in Abaqus/CAE.
Defining solution-dependent field variables
In Abaqus/Standard solution-dependent field variables can be defined in user subroutine USDFLD. The values of predefined field variables or initial fields can be passed into user subroutine USDFLD and can be changed in that routine—see “Material data definition,” Section 21.1.2.
Changes to the field variables in USDFLD are local to the material point and do not affect the nodal values.
Data hierarchy
If both results or output database file input and direct data input are used in the same step, the direct data input will take precedence if both define the field at the same node. If user subroutine input is specified, the values given directly are ignored and the user subroutine modifies the values read from the results or output database file.
You can specify either one or several values of a predefined field at a node, depending on the element type that is used. You should note the following considerations when choosing the form of predefined field specification.
Use in a mass diffusion analysis
For solid elements only one value can be given at a node. Since only solid elements can be used in mass diffusion analysis, this is the only way to define equivalent pressure stresses at a node.
Use with beam and shell elements
The following possibilities exist for temperatures and field variable specification in beam and shell elements:
• For shell and beam elements with general cross-section definitions, the temperature and field variable magnitude at points in the section is defined by the value at the reference surface. Any gradient of these variables specified across the section is ignored.
• For shell and beam elements with cross-sections that require numerical integration, the temperature and field variable magnitudes at points in the section can be defined either from the value at the reference surface and the gradient or gradients across the section or by giving the values at a number of points across the section. The choice between these two methods is made in the section definition (see “Specifying temperature and field variables” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, and “Specifying temperature and field variables” in “Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6, for details).
See Part VI, “Elements,” for the details of use with each element type. The default, if only one value is given, is a constant magnitude across the section.
Temperature and field variable compatibility across elements
Abaqus assumes that the field definitions (including initial conditions) at all the nodes of any element are compatible with the field definition method chosen for the element. Cases may arise where the definition of a field changes from one element to the next (for example, when two adjacent shell elements have a different number of section points through the thickness or when the temperature and field variable magnitudes for one beam element are defined by giving the values at a number of points across the section while those for the abutting beam element are defined from the value at the reference surface and the gradient or gradients across the section). In these cases separate nodes should be used on the interface between such elements and multi-point constraints should be applied to make the displacements and rotations the same at corresponding nodes (see “General multi-point constraints,” Section 35.2.2); otherwise, the fields on the nodes at the interface will be used for each adjacent element with the field definition method chosen for the element.
Part VIII: Constraints
• Chapter 35, “Constraints”
35. Constraints
Overview 35.1
Multi-point constraints 35.2
Surface-based constraints 35.3
Embedded elements 35.4
Element end release 35.5
Overconstraint checks 35.6