김경종
14 KiB
The effective outer diameter, D ; transverse fluid inertia coefficient, C _ { M } ; and transverse added-mass coefficient, C _ { A } , must be defined in the distributed load definition together with the distributed load type (distributed fluid inertia).
The fluid acceleration, \mathbf { a } _ { f n } , , is calculated according to the user-defined gravity wave and is further scaled by the amplitude curve, A _ { w } , , referred to by the distributed load definition.
Input File Usage: Use the following option to define distributed fluid inertia in a dynamic step:
*DLOAD
e l e m e n t n u m b e r o r s e t , \mathrm { F I } , M , D , C _ { M } , C _ { A } , A _ { w } ( t )
Specifying distributed fluid inertia loads in an eigenfrequency extraction step
The added mass contribution due to distributed fluid inertia loading is
\rho_ {w} \frac {\pi D ^ {2}}{4} C _ {A}
per unit length of the member in the directions transverse to the axis of the member only, where
\rho _ { w } is the mass density of the fluid (given in the fluid properties),
D is the effective outer diameter of the member, and
C _ { A } is the transverse added-mass coefficient.
Input File Usage: *D ADDED MASS
element number or set, FI, D, C _ { A }
Specifying concentrated fluid inertia loads in a direct-integration dynamic step using a concentrated load definition
Concentrated fluid inertia loading is automatically considered to be a follower force (for elements that have rotational degrees of freedom).
The inertia term is calculated as a force in the current direction of the outward normal to the exposed surface area:
\mathbf {F} _ {I} = A \rho_ {w} \left(K _ {t s} F _ {1 s} \mathbf {a} _ {f t} - L _ {t s} F _ {2 s} \mathbf {a} _ {p t}\right),
where
{ \bf { F } } _ { I } is the point force caused by fluid inertia;
A ( t ) is the amplitude curve referenced by the concentrated load definition multiplied by the userdefined magnitude factor, M;
\rho _ { w } is the mass density of the fluid (given in the fluid properties);
K _ { t s } is the tangential inertia coefficient;
F _ { 1 s } is the fluid acceleration shape factor (of dimension L ^ { 3 } ) ;
Lts L _ { t s } is the tangential added-mass coefficient;
F2s F _ { 2 s } is the structural acceleration shape factor (of dimension L ^ { 3 } ) ;
\mathbf { a } _ { f t } is the fluid acceleration in the direction of the outward normal to the exposed surface; and \mathbf { a } _ { p t } is the structural acceleration in the direction of the outward normal to the exposed surface (zero during static steps).
The tangential inertia coefficient, K _ { t s } ; the fluid acceleration shape factor, F _ { 1 s } ; the tangential added-mass coefficient, L _ { t s } ; and the structural acceleration shape factor, F _ { 2 s } , are given in the concentrated load definition together with the concentrated load type (transition section inertia).
The fluid acceleration, \mathbf { a } _ { f t } , is calculated according to the user-defined gravity wave and is further scaled by the amplitude curve, A _ { w } , referred to by the concentrated load definition.
Input File Usage: Use the following option to define transition section inertia in a dynamic step:
*CLOAD
n o d e ~ n u m b e r ~ o r ~ s e t , \mathrm { T S I } , \mathrm { M } , \mathrm { K } _ { t s } , \mathrm { F } _ { 1 s } , L _ { t s } , { F } _ { 2 s } , \mathrm { } A _ { w } ( t )
Specifying concentrated fluid inertia loads in a direct-integration dynamic step using a distributed load definition
You can apply concentrated fluid inertia loading at the ends of elements. These loads have the same effect as specifying a concentrated fluid added-inertia loading using a concentrated load definition with concentrated load type transition section inertia, except that the normal to the exposed area cannot be specified when a distributed load definition is used; the normal to the end of the element is defined by the tangent to the element.
The inertia loading can be applied to the first end (node) of the element or to the second end (node 2 or 3, as appropriate) of the element.
The loading is exactly the same as that described for the concentrated fluid inertia loading applied with a concentrated load definition. The “distributed” form of the loading is provided for convenience.
Input File Usage: Use the following option to define fluid inertia on the first end of the element in a dynamic step:
*DLOAD
e l e m e n t n u m b e r o r s e t , \mathrm { F I 1 } , M , K _ { t s } , F _ { 1 s } , L _ { t s } , F _ { 2 s } , A _ { w } ( t )
Use the following option to define fluid inertia on the second end of the element in a dynamic step:
*DLOAD
e l e m e n t n u m b e r o r s e t , \mathrm { F I 2 } , M , K _ { t s } , F _ { 1 s } , L _ { t s } , F _ { 2 s } , A _ { w } ( t )
Specifying concentrated fluid inertia effects in an eigenfrequency extraction step using a concentrated added mass definition
The added mass contribution due to concentrated fluid inertia loading in an eigenfrequency extraction step is
\rho_ {w} L _ {t s} F _ {2 s}
in the direction normal to the transition section area, where
\rho _ { w } is the mass density of the fluid (given in the fluid properties),
Lts L _ { t s } is the tangential added-mass coefficient, and
F _ { 2 s } is the structural acceleration shape factor (of dimension L ^ { 3 } ) .
Input File Usage: *C ADDED MASS
node number or set, TSI, L _ { t s } , F _ { 2 s }
direction cosines defining the outward normal of the exposed area
Specifying concentrated fluid inertia effects in an eigenfrequency extraction step using a distributed added mass definition
You can apply concentrated fluid inertia effects at the ends of elements. These loads have the same effect as specifying concentrated fluid inertia effects using a concentrated added mass definition with concentrated load type transition section inertia, but in this case the normal to the exposed area cannot be specified; the normal to the end of the element is defined by the tangent to the element.
The added mass can be applied to the first end (node) of the element or to the second end (node 2 or 3, as appropriate) of the element.
The effect is exactly the same as that described for the concentrated fluid inertia effects applied with a concentrated added mass definition. The “distributed” form of the loading is provided for convenience.
Input File Usage: Use the following option to define fluid inertia on the first end of the element in an eigenfrequency extraction step:
*D ADDED MASS
element number or set, FI1, \textit { L } _ { t s } , \textit { F } _ { 2 s }
Use the following option to define fluid inertia on the second end of the element in an eigenfrequency extraction step:
*D ADDED MASS
element number or set, FI2, \boldsymbol { L } _ { t s } , F _ { 2 s }
Applying non-Aqua loads to the structure
Concentrated and distributed load definitions can also be used to apply concentrated and distributed forces that are not associated with wind, waves, or steady current to the structure. See “Concentrated loads,” Section 34.4.2, and “Distributed loads,” Section 34.4.3.
Predefined fields
The following predefined fields can be specified for the structure (not the fluid) in an Abaqus/Aqua analysis, as described in “Predefined fields,” Section 34.6.1:
• Temperatures of nodes in the structure can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperaturedependent material properties, if any.
• The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any.
Material options
Any of the mechanical constitutive models in Abaqus can be used for modeling the structure in an Abaqus/Aqua analysis (see Part V, “Materials,” for details on the material models available in Abaqus/Standard).
Elements
The fluid loads in an Abaqus/Aqua analysis cannot be applied to all element types. Only the beam, pipe, elbow, truss, and rigid beam elements in Abaqus/Standard and linear beam and pipe elements in Abaqus/Explicit can be used to subject a structure to general Abaqus/Aqua loading. The only load that can be applied to two-dimensional rigid surfaces (R3D3 and R3D4 elements) is hydrostatic buoyancy; and this loading can be applied only in Abaqus/Standard. Current, wave, and wind loading have no effect on rigid surfaces.
Jack-up foundation analysis
Abaqus/Standard provides element types JOINT2D and JOINT3D, which can be used to model elasticplastic interaction between spud cans and the sea floor (see “Elastic-plastic joints,” Section 32.10.1).
Output
In addition to the usual output variables available in Abaqus/Standard (see “Abaqus/Standard output variable identifiers,” Section 4.2.1) and in Abaqus/Explicit (see “Abaqus/Explicit output variable identifiers,” Section 4.2.2), element section output variable ESF1 can be used to request output of the effective axial force in a beam subjected to pressure loading (see “Beam element library,” Section 29.3.8). The velocities and accelerations of the fluid cannot be output.
Input file template
*HEADING
...
*SURFACE SECTION, ELSET=aquaviz, AQUAVISUALIZATION=YES
*NSET, NSET=naquaviz, ELSET=aquaviz
*AQUA
Data lines defining the fluid properties and steady current velocity
*WAVE, TYPE=wave theory
Data lines defining gravity waves
**
*STEP (, NLGEOM)
Use the NLGEOM parameter to include nonlinear geometric effects
*DYNAMIC (or *STATIC or *DYNAMIC, EXPLICIT)
...
*CLOAD
Data lines defining concentrated buoyancy, fluid/wind drag, and fluid inertia loads
*DLOAD
Data lines defining distributed buoyancy, fluid/wind drag, and fluid inertia loads
*OUTPUT, FIELD, TIME INTERVAL=interval for field output
*NODE OUTPUT,NSET=naquaviz
U
*END STEP
**
*STEP
The NLGEOM parameter must have been included in the previous step to obtain the natural frequencies of the prestressed structure
*FREQUENCY
...
*C ADDED MASS
Data lines to define concentrated added-mass effects
*D ADDED MASS
Data lines to define distributed added-mass effects
*OUTPUT, FIELD, TIME INTERVAL=interval for field output
*NODE OUTPUT,NSET=naquaviz
U
*END STEP
6.12 Annealing
• “Annealing procedure,” Section 6.12.1
6.12.1 ANNEALING PROCEDURE
Products: Abaqus/Explicit Abaqus/CAE
References
• *ANNEAL
• “Configuring an annealing procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
The anneal procedure:
• is used to anneal a structure by setting all appropriate state variables and velocities to zero; and
• is intended only for metal plasticity and user-defined material models; it has no effect on other material models.
The annealing process
The anneal procedure is intended to simulate the relaxation of stresses and plastic strains that occurs as metals are heated to high temperatures. Physically, annealing is the process of heating a metal part to a high temperature to allow the microstructure to recrystallize, removing dislocations caused by cold working of the material. During the anneal procedure Abaqus/Explicit sets all appropriate state variables to zero. These variables include stresses, backstresses, plastic strains, and velocities. In the case of metal porous plasticity, the void volume fraction is also set to zero, such that the material becomes fully dense.
There is no time scale in an annealing step; therefore, time does not advance. The annealing process occurs instantaneously. No data are required for the anneal procedure.
Input File Usage: *ANNEAL
Abaqus/CAE Usage: Step module: Create Step: General: Anneal
Temperatures
Thermal strains are set to zero, and the temperature at all nodes in the model will be set to a uniform temperature or will be maintained at the current temperature during the anneal procedure. By default, the temperature at all nodes is maintained at the current temperature. You can specify a different final temperature, .
Input File Usage: *ANNEAL, TEMPERATURE=
Abaqus/CAE Usage: Step module: Create Step: General: Anneal: Post-anneal reference temperature: Value
Initial conditions
The initial state for the anneal step is the state of the model at the end of the last explicit dynamic analysis step.
Boundary conditions
It is not appropriate to specify new boundary conditions or to modify boundary conditions in an anneal procedure; all boundary conditions in effect prior to this procedure will remain fixed.
Loads
It is not meaningful to specify loads in an anneal procedure.
Predefined fields
It is not meaningful to specify predefined fields in an anneal procedure.
Material options
The annealing procedure is intended only for metal plasticity models (“Classical metal plasticity,” Section 23.2.1) and user-defined materials modeled with user subroutines VFABRIC and VUMAT. The metal plasticity models in Abaqus/Explicit include Mises, Johnson-Cook, Hill, and metal porous plasticity. Abaqus/Explicit also allows annealing of elastic materials (“Linear elastic behavior,” Section 22.2.1), including isotropic, orthotropic, and anisotropic elasticity. The annealing procedure has no effect on other material models.
Elements
All of the elements that are available in Abaqus/Explicit can be used in an anneal procedure. The elements are listed in Part VI, “Elements.”
Output
There is no output associated with an anneal step.
Input file template
*HEADING
...
**
*STEP
*DYNAMIC, EXPLICIT (,ADIABATIC) or
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT
Data line to specify the time period of the step