김경종
17 KiB
A local coordinate system (see “Transformed coordinate systems,” Section 2.1.5) cannot be used at a pre-tension node. It can be used at nodes located on pre-tension sections.
Applying the prescribed assembly load
The pre-tension load is transmitted across the pre-tension section by means of the pre-tension node.
Prescribing the pre-tension force
You can apply a concentrated load to the pre-tension node. This load is the self-equilibrating force carried across the pre-tension section, acting in the direction of the normal on the part of the fastener underlying the pre-tension section (the part that contains the elements that were used in the definition of the pretension section; see Figure 34.5.1–8).
Input File Usage: *CLOAD
Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step: select surface and if, necessary, datum axis: Method: Apply force
text_image
n pre-tension node underlying part
Figure 34.5.1–8 The prescribed assembly load is given at the pre-tension node and applied in direction .
Prescribing a tightening adjustment
You can prescribe a tightening adjustment of the pre-tension section by using a nonzero boundary condition at the pre-tension node (which corresponds to a prescribed change in the length of the component cut by the pre-tension section in the direction of the normal).
Input File Usage: *BOUNDARY
Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step: select surface and if, necessary, datum axis: Method: Adjust length
Controlling the pre-tension node during the analysis
You can maintain the initial adjustment of the pre-tension section by using a boundary condition fixing the degrees of freedom at their current values at the start of the step once an initial pre-tension is applied in the fastener; this technique enables the load across the pre-tension section to change according to the externally applied loads to maintain equilibrium. If the initial adjustment of a section is not maintained, the force in the fastener will remain constant.
When a pre-tension node is not controlled by a boundary condition, make sure that the components of the structure are kinematically constrained; otherwise, the structure could fall apart due to the presence of rigid body modes. Abaqus/Standard will issue a warning message if it does not find any boundary condition or load on a pre-tension node during the first step of the analysis.
Display of results
Abaqus/Standard automatically adjusts the length of the component at the pre-tension section to achieve the prescribed amount of pre-tension. This adjustment is done by moving the nodes of the underlying elements that lie on the pre-tension section relative to the same nodes when they appear in the other elements connected to the pre-tension section. As a result, the underlying elements will appear shrunk, even though they carry tensile stresses when a pre-tension is applied.
Limitations when using assembly loads
Assembly loads are subject to the following limitations:
• An assembly load cannot be specified within a substructure.
• If a submodeling analysis is performed (“Submodeling: overview,” Section 10.2.1), any pre-tension section should not cross regions where driven nodes are specified. In other words, a pre-tension section should appear either entirely in the region of the global model that is not part of a submodel or entirely in the region of the global model that is part of a submodel. In the latter case, a pre-tension section must also appear in the submodel when the submodel analysis is performed.
• Nodes of a pre-tension section should not be connected to other parts of the body through multi-point constraints (“General multi-point constraints,” Section 35.2.2). These nodes can be connected to other parts of the body through equations (“Linear constraint equations,” Section 35.2.1). However,
an equation connecting a node on the pre-tension section to a node located on the underlying side of the section introduces a constraint that spans across the pre-tension cut and, therefore, interacts directly with the application of the pre-tension load. On the other hand, an equation connecting a node on the pre-tension section to a node on the other side of the section does not influence the application of the pre-tension load.
Procedures
Any of the Abaqus/Standard procedures that use element types with displacement degrees of freedom can be used. Static analysis is the most likely procedure type to be used when prescribing the initial pre-tension (“Static stress analysis,” Section 6.2.2). Other analysis types such as coupled temperature-displacement (“Sequentially coupled thermal-stress analysis,” Section 16.1.2) or coupled thermal-electrical-structural (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4) can also be used. Once the initial pre-tension is applied, a static or dynamic analysis (“Dynamic analysis procedures: overview,” Section 6.3.1) may, for instance, be used to apply additional loads while maintaining the tightening adjustment.
Output
The total force across the pre-tension section is the sum of the reaction force at the pre-tension node plus any concentrated load specified at that node. The total force across the pre-tension section is available as output using the output variable identifier TF (see “Abaqus/Standard output variable identifiers,” Section 4.2.1). The forces are along the normal direction. The shear force across the pre-tension section is not available for output.
The tightening adjustment of the pre-tension section is available as the displacement of the pretension node. The output of displacement is requested using output identifier U. Only the adjustment normal to the pre-tension section is output since there is no adjustment in any other direction.
The stress distribution across the pre-tension section is not available directly; however, the stresses in the underlying elements can be displayed readily. Alternatively, a tied contact pair can be inserted at the location of the pre-tension section to enable stress distribution output by means of output identifiers CPRESS and CSHEAR. See “Defining tied contact in Abaqus/Standard,” Section 36.3.7, for details on defining tied contact.
Input file template
*HEADING
Prescribed assembly load; example using continuum elements
...
*NODE
Optionally define the pre-tension node
*SURFACE, NAME=name
Data lines that specify the elements and their associated faces to define the pre-tension section
*PRE-TENSION SECTION, SURFACE=name, NODE=pre-tension_node
**
*STEP
** Application of the pre-tension across the section
*STATIC
Data line to control time incrementation
*CLOAD
pre-tension_node, 1, pre-tension_value
or
*BOUNDARY, AMPLITITUDE = amplitude
pre-tension_node, 1, 1, tightening adjustment
*END STEP
*STEP
** maintain the tightening adjustment and apply new loads
*STATIC or *DYNAMIC
Data line to control time incrementation
*BOUNDARY, FIXED
pre-tension_node, 1, 1
*BOUNDARY
Data lines to prescribe other boundary conditions
*CLOAD or *DLOAD
Data lines to prescribe other loading conditions
...
*END STEP
34.6 Predefined fields
• “Predefined fields,” Section 34.6.1
34.6.1 PREDEFINED FIELDS
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Prescribed conditions: overview,” Section 34.1.1
• *TEMPERATURE
• *FIELD
• *PRESSURE STRESS
• *MASS FLOW RATE
• “Defining a temperature field,” Section 16.11.9 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
This section describes how to specify the values of the following types of predefined fields during an analysis:
• temperature,
• field variables,
• equivalent pressure stress, and
• mass flow rate.
The procedures in which these fields can be used are outlined in “Prescribed conditions: overview,” Section 34.1.1.
Temperature, field variables, equivalent pressure stress, and mass flow rate are time-dependent, predefined (not solution-dependent) fields that exist over the spatial domain of the model. They can be defined:
• by entering the data directly,
• by reading an Abaqus results file generated during a previous analysis (usually an Abaqus/Standard heat transfer analysis), or
• in an Abaqus/Standard user subroutine.
Temperature can also be defined by reading an Abaqus output database file generated during a previous analysis. In Abaqus/Standard field variables can also be defined by reading an Abaqus output database file generated during a previous analysis.
Field variables can also be made solution dependent, which allows you to introduce additional nonlinearities in the Abaqus material models.
Predefined temperature
In stress/displacement analysis the temperature difference between a predefined temperature field and any initial temperatures (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) will create thermal strains if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The predefined temperature field also affects temperature-dependent material properties, if any. In Abaqus/Explicit temperature-dependent material properties may cause longer run times than constant properties.
You define the magnitude and time variation of temperature at the nodes, and Abaqus interpolates the temperatures to the material points.
Input File Usage: Use the following option to specify a predefined temperature field:
*TEMPERATURE
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step
Restrictions
Do not specify predefined temperature fields in a pure heat transfer analysis, a coupled thermal-electrical analysis, a fully coupled temperature-displacement analysis, or a fully coupled thermal-electricalstructural analysis; instead, specify a boundary condition (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1) to prescribe temperature degrees of freedom (11, 12, ...).
Predefined temperature fields cannot be specified in an adiabatic analysis step or in any mode-based dynamic analysis step.
To specify a predefined temperature field in a restart analysis, the corresponding predefined field must have been specified in the original analysis as either initial temperatures (see “Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) or a predefined temperature field.
Predefined field variables
The usage and treatment of predefined field variables is exactly analogous to that of temperature. You can prescribe the magnitude and time variation of the field at all of the nodes of the model, and Abaqus will interpolate the values to the material points.
When prescribing field variable values, you must specify the field variable number being defined; the default is field variable number 1. Field variables must be numbered consecutively starting from one. Repeat the field variable definition to define more than one field variable.
The field variable can be a real field (such as an electromagnetic field) generated by a previous simulation (Abaqus or another analysis code). It can also be an artificial field that you define to modify certain material properties during the course of an analysis. For example, suppose that you wish to vary Young’s modulus linearly between 3 0 \times 1 0 ^ { 6 } and 3 5 \times 1 0 ^ { 6 } during the response. The linear elastic material definition shown in Table 34.6.1–1 could be used.
Table 34.6.1–1 Sample material definition.
| Number of field variable dependencies: 1 | ||
| Young's modulus | Poisson's ratio | Value of field variable 1 |
| 30.E6 | 0.3 | 1.0 |
| 35.E6 | 0.3 | 2.0 |
Define an initial condition to specify the initial value of field variable 1 as 1.0 for a node set. Then, define a predefined field variable in the analysis step to specify the value of field variable 1 as 2.0 for the node set. Young’s modulus will vary smoothly over the course of the step as the field variable’s value is ramped from 1.0 to 2.0 at all nodes in the node set.
Field variables can also be used to vary real properties in space by making the properties depend on field variables, as above, and by assigning different field variable values to different nodes.
Making properties depend on field variables will increase the computer time required, since Abaqus must perform the necessary table look-ups.
In an Abaqus/Standard stress/displacement analysis the difference between a predefined field variable and its initial value (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) will create volumetric strains analogous to thermal strains if a field expansion coefficient (for the corresponding field variable) is given for the material (“Thermal expansion,” Section 26.1.2).
Input File Usage: Use the following option to specify a predefined field variable: *FIELD, VARIABLE=n
Abaqus/CAE Usage: Predefined field variables are not supported in Abaqus/CAE.
Restrictions
To specify a predefined field variable in a restart analysis, the corresponding predefined field must have been specified in the original analysis as either an initial field variable value (see “Defining initial values of predefined field variables” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) or a predefined field variable.
Predefined pressure stress
You can apply equivalent pressure stress as a predefined field in a mass diffusion analysis. The usage and treatment of pressure stresses is analogous to that of temperatures and field variables. In Abaqus equivalent pressure stresses are positive when they are compressive.
Input File Usage: Use the following option to specify a predefined equivalent pressure stress field: *PRESSURE STRESS
Abaqus/CAE Usage: Predefined equivalent pressure stress is not supported in Abaqus/CAE.
Restrictions
Predefined equivalent pressure stress fields can be specified only in a mass diffusion procedure (see “Mass diffusion analysis,” Section 6.9.1).
To specify a predefined equivalent pressure stress field in a restart analysis, the corresponding predefined field must have been specified in the original analysis as either initial pressure stresses (see “Defining initial pressure stress in a mass diffusion analysis” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) or a predefined equivalent pressure stress field.
Predefined mass flow rate
You can specify the mass flow rate per unit area (or through the entire section for one-dimensional elements) for forced convection/diffusion elements in a heat transfer analysis. The usage and treatment of mass flow rate is analogous to that of temperatures and field variables.
Input File Usage: Use the following option to specify a predefined mass flow rate field:
*MASS FLOW RATE
Abaqus/CAE Usage: Predefined mass flow rate is not supported in Abaqus/CAE.
Restrictions
A predefined mass flow rate field can be specified only with forced convection/diffusion elements in a heat transfer procedure (see “Uncoupled heat transfer analysis,” Section 6.5.2).
To specify a predefined mass flow rate field in a restart analysis, the corresponding predefined field must have been specified in the original analysis by using either initial mass flow rates (see “Defining initial mass flow rates in forced convection heat transfer elements” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) or a predefined mass flow rate field.
Reading initial values of a field from a user-specified results file
An Abaqus/Standard results file can be used to specify initial values of
• temperature (see “Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1);
• field variables (see “Defining initial values of predefined field variables” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1); and
• pressure stress (see “Defining initial pressure stress in a mass diffusion analysis” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1).
Field variable values must be read from the temperature record (see “Reading field values from a userspecified results file” below). The part (.prt) file from the original analysis is also required when reading data from the results file.
If the zero increment results were requested as output to the Abaqus/Standard results file (see “Obtaining results at the beginning of a step” in “Output,” Section 4.1.1), you can define initial values of prescribed fields as those existing at the beginning of a step (the zero increment) in the previous heat