김경종
270 lines
23 KiB
Markdown
270 lines
23 KiB
Markdown
<!-- source-page: 71 -->
|
||
|
||
$$
|
||
\mathbf {v} ^ {N} = \mathbf {v} ^ {g} + \omega \frac {(\mathbf {X} ^ {b} - \mathbf {X} ^ {a})}{| \mathbf {X} ^ {b} - \mathbf {X} ^ {a} |} \times (\mathbf {X} ^ {N} - \mathbf {X} ^ {a}).
|
||
$$
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=ROTATING VELOCITY
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Velocity for the Types for Selected Step
|
||
|
||
# Defining initial saturation for a porous medium
|
||
|
||
In Abaqus/Standard you can define the initial saturation, s, for elements in a coupled pore fluid diffusion/stress analysis (see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). If the porous material’s absorption/exsorption behavior under partially saturated flow conditions is not defined, the initial saturation is set to 1.0 by default.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=SATURATION
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Saturation for the Types for Selected Step
|
||
|
||
# Defining the initial values of solution-dependent state variables
|
||
|
||
You can define initial values of solution-dependent state variables (see “User subroutines: overview,” Section 18.1.1). The initial values can be defined directly or, in Abaqus/Standard, by user subroutine SDVINI. Values given directly will be applied uniformly over the element.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=SOLUTION
|
||
|
||
Abaqus/CAE Usage: Initial solution-dependent variables are not supported in Abaqus/CAE.
|
||
|
||
Defining the initial values of solution-dependent state variables for rebars
|
||
|
||
The initial values of solution-dependent variables can also be defined for rebars within elements. Rebars are discussed in “Defining rebar as an element property,” Section 2.2.4.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=SOLUTION, REBAR
|
||
|
||
Abaqus/CAE Usage: Initial solution-dependent state variables are not supported in Abaqus/CAE.
|
||
|
||
Defining the initial values of solution-dependent state variables in user subroutine SDVINI
|
||
|
||
For complicated cases in Abaqus/Standard user subroutine SDVINI can be used to define the initial values of solution-dependent state variables. In this case Abaqus/Standard will make a call to subroutine SDVINI at the start of the analysis for each material integration point in the model. You can then define all solution-dependent state variables at each point as functions of coordinates, element number, etc.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=SOLUTION, USER
|
||
|
||
Abaqus/CAE Usage: User subroutine SDVINI is not supported in Abaqus/CAE.
|
||
|
||
<!-- source-page: 72 -->
|
||
|
||
# Defining initial specific energy for equations of state
|
||
|
||
In Abaqus/Explicit you can specify the initial values of the specific energy for equations of state (see “Equation of state,” Section 25.2.1).
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY
|
||
|
||
Abaqus/CAE Usage: Initial specific energy is not supported in Abaqus/CAE.
|
||
|
||
# Defining spud can embedment or spud can preload
|
||
|
||
In Abaqus/Standard you can define an initial embedment of a spud can. Alternatively, you can define an initial vertical preload of a spud can (see “Elastic-plastic joints,” Section 32.10.1).
|
||
|
||
Input File Usage: Use one of the following options:
|
||
|
||
\*INITIAL CONDITIONS, TYPE=SPUD EMBEDMENT
|
||
|
||
\*INITIAL CONDITIONS, TYPE=SPUD PRELOAD
|
||
|
||
Abaqus/CAE Usage: Initial spud can embedment and preload are not supported in Abaqus/CAE.
|
||
|
||
# Defining initial stresses
|
||
|
||
You can define an initial stress field. Initial stresses can be defined directly or, in Abaqus/Standard, by user subroutine SIGINI. Stress values given directly will be applied uniformly over the element unless they are defined at each section point through the thickness in shell elements.
|
||
|
||
If a local coordinate system was defined (see “Orientations,” Section 2.2.5), stresses must be given in the local system.
|
||
|
||
In soils (porous medium) problems the initial effective stress should be given; see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1, for a discussion of defining initial conditions in porous media.
|
||
|
||
If the section properties of beam elements or shell elements are defined by a general section, the initial stress values are applied as initial section forces and moments. In the case of beams initial conditions can be specified only for the axial force, the bending moments, and the twisting moment. In the case of shells initial conditions can be specified only for the membrane forces, the bending moments, and the twisting moment. In both shells and beams initial conditions cannot be prescribed for the transverse shear forces.
|
||
|
||
Initial stress fields cannot be defined for spring elements. See “Springs,” Section 32.1.1, for a discussion of defining initial forces in spring elements.
|
||
|
||
Initial stress fields cannot be defined for elements using a fabric material. However, an initial stress and strain state can be introduced in a fabric material made of membrane elements by defining a reference mesh (see “Defining a reference mesh for membrane elements ” above).
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=STRESS
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step
|
||
|
||
<!-- source-page: 73 -->
|
||
|
||
# Defining initial stresses for rebars
|
||
|
||
Initial values of stress can also be defined for rebars within elements (see “Defining rebar as an element property,” Section 2.2.4).
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=STRESS, REBAR
|
||
|
||
Abaqus/CAE Usage: Initial stress for rebars is not supported in Abaqus/CAE.
|
||
|
||
# Defining initial stresses that vary through the thickness of shell elements
|
||
|
||
Initial values of stress can be defined at each section point through the thickness of shell elements.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=STRESS, SECTION POINTS
|
||
|
||
Abaqus/CAE Usage: Defining initial stress that varies through the thickness of shell elements is not supported in Abaqus/CAE.
|
||
|
||
# Defining initial stresses in user subroutine SIGINI
|
||
|
||
For complicated cases (such as elbow elements) in Abaqus/Standard the initial stress field can be defined by user subroutine SIGINI. In this case Abaqus/Standard will make a call to subroutine SIGINI at the start of the analysis for each material calculation point in the model. You can then define all active stress components at each point as functions of coordinates, element number, etc.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=STRESS, USER
|
||
|
||
Abaqus/CAE Usage: User subroutine SIGINI is not supported in Abaqus/CAE.
|
||
|
||
# Defining initial stresses using stress output from a user-specified output database file
|
||
|
||
You can define initial stresses using stress output variables from a particular step and increment in the output database (.odb) file of a previous Abaqus/Standard analysis.
|
||
|
||
In this case both the previous model and the current model must be defined consistently. The element numbering and element types must be the same in both models. If the models are defined in terms of an assembly of part instances, part instance naming must be the same.
|
||
|
||
The file extension is optional; however, only the output database file can be used.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=STRESS, FILE=file, STEP=step, INC=inc
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step; select region; Specification: From output database file
|
||
|
||
# Establishing equilibrium in Abaqus/Standard
|
||
|
||
When initial stresses are given in Abaqus/Standard (including prestressing in reinforced concrete or interpolation of an old solution onto a new mesh), the initial stress state may not be an exact equilibrium state for the finite element model. Therefore, an initial step should be included to allow Abaqus/Standard to check for equilibrium and iterate, if necessary, to achieve equilibrium.
|
||
|
||
<!-- source-page: 74 -->
|
||
|
||
In a soils analysis (that is, for models containing elements that include pore fluid pressure as a variable) the geostatic stress field procedure (“Geostatic stress state,” Section 6.8.2) should be used for the equilibrating step. Any initial loading (such as geostatic gravity loads) that contributes to the initial equilibrium should be included in this step definition. The initial time increment and the total time specified in this step should be the same. The initial stresses are applied in full at time zero; and if equilibrium can be achieved, this step will converge in one increment. Therefore, there is no benefit to incrementing.
|
||
|
||
To achieve equilibrium for all other analyses, a first step using the static procedure (“Static stress analysis,” Section 6.2.2) should be used. It is recommended that you specify the initial time increment to be equal to the total time specified in this step so that Abaqus/Standard will attempt to find equilibrium in one increment. By default, Abaqus/Standard ramps down the unbalanced stress over the first step. This allows Abaqus/Standard to use automatic incrementation if equilibrium cannot be found in one increment. This ramping is achieved in the following manner:
|
||
|
||
1. An additional set of artificial stresses is defined at each material point. These stresses are equal in magnitude to the initial stresses but are of opposite sign. The sum of the material point stresses and these artificial stresses creates zero internal forces at the beginning of the step.
|
||
2. The internal artificial stresses are ramped off linearly in time during the first step. Thus, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material will be the stress state in equilibrium.
|
||
|
||
You can force Abaqus/Standard to achieve equilibrium in one increment by using a step variation on the initial condition to resolve the unbalanced stress instead of ramping the stress down over the entire step. If Abaqus/Standard cannot achieve equilibrium in one increment, the analysis will terminate.
|
||
|
||
If the equilibrating step does not converge, it indicates that the initial stress state is so far from equilibrium with the applied loads that significantly large deformations would be generated. This is generally not the intention of an initial stress state; therefore, it suggests that you should recheck the specified initial stresses and loads.
|
||
|
||
Input File Usage: Use one of the following options to specify how the unbalanced stress should be resolved:
|
||
|
||
\*INITIAL CONDITIONS, TYPE=STRESS,
|
||
|
||
UNBALANCED STRESS=RAMP (default)
|
||
|
||
\*INITIAL CONDITIONS, TYPE=STRESS,
|
||
|
||
UNBALANCED STRESS=STEP
|
||
|
||
Abaqus/CAE Usage: Initial equilibrium stress is not supported in Abaqus/CAE.
|
||
|
||
# Establishing equilibrium in Abaqus/Explicit
|
||
|
||
Abaqus/Explicit computes the initial acceleration at nodes taking into account the initial stresses, the loads, and the boundary conditions in the initial configuration. For an initially static problem, the specified boundary conditions, the initial stresses, and the initial loading should be consistent with a static equilibrium. Otherwise, the solution is likely to be noisy. The noise may be reduced by introducing a dummy step with a temporary viscous loading to attempt to reestablish a static
|
||
|
||
<!-- source-page: 75 -->
|
||
|
||
equilibrium. Alternatively, you can introduce an initial short step in which all degrees of freedom are fixed with boundary conditions (all initial loads should be included in this initial step); in a second step, release all but the actual boundary conditions.
|
||
|
||
# Defining elevation-dependent (geostatic) initial stresses
|
||
|
||
You can define elevation-dependent initial stresses. When a geostatic stress state is prescribed for a particular element set, the stress in the vertical direction (assumed to be the z-direction in three-dimensional and axisymmetric models and the y-direction in two-dimensional models) is assumed to vary (piecewise) linearly with this vertical coordinate.
|
||
|
||
For the vertical stress component, you must give two pairs of stress and elevation values to define the stress throughout the element set. For material points lying between the two elevations given, Abaqus will use linear interpolation to determine the initial stress; for points lying outside the two elevations given, Abaqus will use linear extrapolation. In addition, horizontal (lateral) stress components are given by entering one or two “coefficients of lateral stress,” which define the lateral direct stress components as the vertical stress at the point multiplied by the value of the coefficient. In axisymmetric cases only one value of the coefficient of lateral stress is used and, therefore, only one value need be entered.
|
||
|
||
Geostatic initial stresses are for use with continuum elements only. In Abaqus/Standard elevation-dependent initial stresses should be specified for beams and shells in user subroutine SIGINI, as explained earlier. In Abaqus/Explicit elevation-dependent initial stresses cannot be specified for beams and shells.
|
||
|
||
The geostatic stress state specified initially should be in equilibrium with the applied loads (such as gravity) and boundary conditions. An initial step should be included to allow Abaqus to check for equilibrium after this interpolation has been done; see the discussion above on establishing equilibrium when an initial stress field is applied.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Geostatic stress for the Types for Selected Step
|
||
|
||
# Defining initial temperatures
|
||
|
||
You can define initial temperatures at the nodes of either heat transfer or stress/displacement elements. The temperatures of stress/displacement elements can be changed during an analysis (see “Predefined fields,” Section 34.6.1).
|
||
|
||
The definition of initial temperature values must be compatible with the section definition of the element and with adjacent elements, as explained in “Predefined fields,” Section 34.6.1.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=TEMPERATURE
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step
|
||
|
||
<!-- source-page: 76 -->
|
||
|
||
Defining initial temperatures from a user-specified results or output database file
|
||
|
||
You can define initial temperatures as those values existing as nodal temperatures at a particular step and increment in the results or output database file of a previous Abaqus/Standard heat transfer analysis (see “Predefined fields,” Section 34.6.1).
|
||
|
||
The part (.prt) file from the previous analysis is required to read initial temperatures from the results or output database file (see “Defining an assembly,” Section 2.10.1). Both the previous model and the current model must be consistently defined in terms of an assembly of part instances; node numbering must be the same, and part instance naming must be the same.
|
||
|
||
The file extension is optional; however, if both results and output database files exist, the results file will be used.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=TEMPERATURE, FILE=file, STEP=step, INC=inc
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: 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, Step: step, and Increment: inc
|
||
|
||
Interpolating initial temperatures for dissimilar meshes from a user-specified results or output database file
|
||
|
||
When the mesh for the heat transfer analysis is different from the mesh for the subsequent stress/displacement analysis, Abaqus can interpolate the temperature values from the nodes in the undeformed heat transfer model to the current nodal temperatures. This technique can also be used in cases where the meshes match but the node number or part instance naming differs between the analyses. Only temperatures from an output database file can be used for the interpolation; Abaqus will look for the .odb extension automatically. The part (.prt) file from the previous analysis is required if that analysis model is defined in terms of an assembly of part instances (see “Defining an assembly,” Section 2.10.1).
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=TEMPERATURE, INTERPOLATE, FILE=file, STEP=step, INC=inc
|
||
|
||
Abaqus/CAE Usage: 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, Mesh compatibility: Incompatible
|
||
|
||
Interpolating initial temperatures for dissimilar meshes with user-specified regions
|
||
|
||
When regions of elements in the heat transfer analysis are close or touching, the dissimilar mesh interpolation capability can result in an ambiguous temperature association. For example, consider a node in the current model that lies on or close to a boundary between two adjacent parts in the heat transfer model, and consider a case where temperatures in these parts are different. When interpolating, Abaqus will identify a corresponding parent element at the boundary for this node from the heat transfer
|
||
|
||
<!-- source-page: 77 -->
|
||
|
||
analysis. This parent element identification is done using a tolerance-based search method. Hence, in this example the parent element might be found in either of the adjacent parts, resulting in an ambiguous temperature definition at the node. You can eliminate this ambiguity by specifying the source regions from which temperatures are to be interpolated. The source region refers to the heat transfer analysis and is specified by an element set. The target region refers to the current analysis and is specified by a node set.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=TEMPERATURE, INTERPOLATE, FILE=file, STEP=step, INC=inc, DRIVING ELSETS
|
||
|
||
Abaqus/CAE Usage: You cannot specify the regions where temperatures are to be interpolated in Abaqus/CAE.
|
||
|
||
Interpolating initial temperatures for meshes that differ only in element order from a user-specified results or output database file
|
||
|
||
If the only difference in the meshes is the element order (first-order elements in the heat transfer model and second-order elements in the stress/displacement model), in Abaqus/Standard you can indicate that midside node temperatures in second-order elements are to be interpolated from corner node temperatures read from the results or output database file of the previous heat transfer analysis using first-order elements. You must ensure that the corner node temperatures are not defined using a mixture of direct data input and reading from the results or output database file, since midside node temperatures that give unrealistic temperature fields may result. In practice, the capability for calculating midside node temperatures is most useful when temperatures generated by a heat transfer analysis are read from the results or output database file for the whole mesh during the stress analysis. Once the midside node capability is activated, the capability will remain active for the rest of the analysis, including for any predefined temperature fields defined to change temperatures during the analysis. The general interpolation and midside node capabilities are mutually exclusive.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=TEMPERATURE, MIDSIDE, FILE=file, STEP=step, INC=inc
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: 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, Step: step, Increment: inc, Mesh compatibility: Compatible, and toggle on Interpolate midside nodes
|
||
|
||
# Defining initial velocities for specified degrees of freedom
|
||
|
||
You can define initial velocities for specified degrees of freedom. When initial velocities are given for dynamic analysis, they should be consistent with all of the constraints on the model, especially timedependent boundary conditions. Abaqus will ensure that they are consistent with boundary conditions and with multi-point and equation constraints but will not check for consistency with internal constraints such as incompressibility of the material. In case of conflict, boundary conditions take precedence over initial conditions.
|
||
|
||
<!-- source-page: 78 -->
|
||
|
||
Initial velocities must be defined in global directions, regardless of the use of local transformations (“Transformed coordinate systems,” Section 2.1.5).
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=VELOCITY
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Velocity for the Types for Selected Step
|
||
|
||
# Defining initial volume fractions for Eulerian elements
|
||
|
||
You can define initial volume fractions to create material within Eulerian elements in Abaqus/Explicit. By default, these elements are filled with void. See “Initial conditions” in “Eulerian analysis,” Section 14.1.1, for a description of strategies for initializing Eulerian materials.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=VOLUME FRACTION
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Material Assignment for the Types for Selected Step
|
||
|
||
# Reading the input data from an external file
|
||
|
||
The input data for an initial conditions definition can be contained in a separate file. See “Input syntax rules,” Section 1.2.1, for the syntax of such file names.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, INPUT=file\_name
|
||
|
||
Abaqus/CAE Usage: Initial conditions cannot be read from a separate file in Abaqus/CAE.
|
||
|
||
# Consistency with kinematic constraints
|
||
|
||
Abaqus does not ensure that initial conditions are consistent with multi-point or equation constraints for nodal quantities other than velocity (see “General multi-point constraints,” Section 35.2.2, and “Linear constraint equations,” Section 35.2.1). Initial conditions on nodal quantities such as temperature in heat transfer analysis, pore pressure in soils analysis, or acoustic pressure in acoustic analysis must be prescribed to be consistent with any multi-point constraint or equation constraint governing these quantities.
|
||
|
||
# Spatial interpolation method
|
||
|
||
When you define initial conditions using a method that interpolates between dissimilar meshes, Abaqus operates by interpolating results from nodes in the old mesh to nodes in the new mesh. For each node:
|
||
|
||
1. The element (in the old mesh) in which the node lies is found, and the node’s location in that element is obtained. (This procedure assumes that all nodes in the new mesh lie within the bounds of the old mesh: warning messages are issued if this is not so.)
|
||
2. The initial condition values are then interpolated from the nodes of the element (in the old mesh) to the new node.
|
||
|
||
Elements that do not support spatial interpolation include the complete libraries of convective heat transfer elements, axisymmetric elements with nonlinear axisymmetric deformation, axisymmetric
|
||
|
||
<!-- source-page: 79 -->
|
||
|
||
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.
|
||
|
||
<!-- source-page: 80 -->
|