김경종
24 KiB
Material options
Most material models that describe mechanical behavior are available for use in a dynamic analysis. The following material properties are not active during a dynamic analysis: thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity properties, and pore fluid flow properties.
Rate-dependent material properties (“Time domain viscoelasticity,” Section 22.7.1; “Hysteresis in elastomers,” Section 22.8.1; “Rate-dependent yield,” Section 23.2.3; and “Two-layer viscoplasticity,” Section 23.2.11) can be included in a dynamic analysis.
Elements
Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in Abaqus/Standard (including those with temperature, pressure, and electrical potential degrees of freedom) can be used in a dynamic analysis. Inertia effects are ignored in hydrostatic fluid elements, and the inertia of the fluid in pore pressure elements is not taken into account.
Output
In addition to the usual output variables available in Abaqus/Standard (see “Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables are provided specifically for implicit dynamic analysis:
Variables for a specified element set or for the entire model:
| XC | Current coordinates of the center of mass. |
| XCn | Coordinate n of the center of mass (n = 1, 2, 3). |
| UC | Displacement of the center of mass. |
| UCn | Displacement component n of the center of mass (n = 1, 2, 3). |
| URCn | Rotation component n of the center of mass. |
| VC | Equivalent rigid body velocity components. |
| VCn | Component n of the equivalent rigid body velocity (n = 1, 2, 3). |
| VRCn | Component n of the equivalent rigid body angular velocity (n = 1, 2, 3). |
| HC | Angular momentum about the center of mass. |
| HCn | Component n of the angular momentum about the center of mass (n = 1, 2, 3). |
| HO | Angular momentum about the origin. |
| HOn | Component n of the angular momentum about the origin (n = 1, 2, 3). |
| RI | Rotary inertia about the origin. |
| RIij | ij-component of the rotary inertia about the origin (i ≤ j ≤ 3). |
| MASS | Mass. |
| VOL | Current volume. |
Input file template
*HEADING
...
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
*AMPLITUDE, NAME=name
Data lines to define amplitude variations
**
*STEP (, NLGEOM)
Once NLGEOM is specified, it will be active in all subsequent steps.
*DYNAMIC
Data line to control automatic time incrementation
*BOUNDARY
Data lines to describe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD and/or *INCIDENT WAVE
Data lines to specify loads
*TEMPERATURE and/or *FIELD
Data lines to prescribe predefined fields
*CECHARGE and/or *DECHARGE (if electrical potential degrees of freedom are active)
Data lines to specify charges
*END STEP
Additional references
• Czekanski, A., N. El-Abbasi, and S. A. Meguid, “Optimal Time Integration Parameters for Elastodynamic Contact Problems,” Communications in Numerical Methods in Engineering, vol. 17, pp. 379–384, 2001.
• Hilber, H. M., T. J. R. Hughes, and R. L. Taylor, “Improved Numerical Dissipation for Time Integration Algorithms in Structural Dynamics,” Earthquake Engineering and Structural Dynamics, vol. 5, pp. 283–292, 1977.
6.3.3 EXPLICIT DYNAMIC ANALYSIS
Products: Abaqus/Explicit Abaqus/CAE
References
• “Defining an analysis,” Section 6.1.2
• *DYNAMIC
• “Configuring a dynamic, explicit 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
An explicit dynamic analysis:
• is computationally efficient for the analysis of large models with relatively short dynamic response times and for the analysis of extremely discontinuous events or processes;
• allows for the definition of very general contact conditions (“Contact interaction analysis: overview,” Section 36.1.1);
• uses a consistent, large-deformation theory—models can undergo large rotations and large deformation;
• can use a geometrically linear deformation theory—strains and rotations are assumed to be small (see “Defining an analysis,” Section 6.1.2);
• can be used to perform an adiabatic stress analysis if inelastic dissipation is expected to generate heat in the material (see “Adiabatic analysis,” Section 6.5.4);
• can be used to perform quasi-static analyses with complicated contact conditions; and
• allows for either automatic or fixed time incrementation to be used—by default, Abaqus/Explicit uses automatic time incrementation with the global time estimator.
Explicit dynamic analysis
The explicit dynamics procedure performs a large number of small time increments efficiently. An explicit central-difference time integration rule is used; each increment is relatively inexpensive (compared to the direct-integration dynamic analysis procedure available in Abaqus/Standard) because there is no solution for a set of simultaneous equations. The explicit central-difference operator satisfies the dynamic equilibrium equations at the beginning of the increment, t; the accelerations calculated at time t are used to advance the velocity solution to time t + \Delta t / 2 and the displacement solution to time t + \Delta t .
Input File Usage: *DYNAMIC, EXPLICIT
Abaqus/CAE Usage: Step module: Create Step: General: Dynamic, Explicit
The explicit dynamics analysis procedure is based upon the implementation of an explicit integration rule together with the use of diagonal (“lumped”) element mass matrices. The equations of motion for the body are integrated using the explicit central-difference integration rule
\dot {u} _ {(i + \frac {1}{2})} ^ {N} = \dot {u} _ {(i - \frac {1}{2})} ^ {N} + \frac {\Delta t _ {(i + 1)} + \Delta t _ {(i)}}{2} \ddot {u} _ {(i)} ^ {N},
u _ {(i + 1)} ^ {N} = u _ {(i)} ^ {N} + \Delta t _ {(i + 1)} \dot {u} _ {(i + \frac {1}{2})} ^ {N},
where u ^ { N } is a degree of freedom (a displacement or rotation component) and the subscript i refers to the increment number in an explicit dynamics step. The central-difference integration operator is explicit in the sense that the kinematic state is advanced using known values of \dot { u } _ { ( i - 1 / 2 ) } ^ { N } and \ddot { u } _ { ( i ) } ^ { \dot { N } } from the previous increment.
The explicit integration rule is quite simple but by itself does not provide the computational efficiency associated with the explicit dynamics procedure. The key to the computational efficiency of the explicit procedure is the use of diagonal element mass matrices because the accelerations at the beginning of the increment are computed by
\ddot {u} _ {(i)} ^ {N} = (M ^ {N J}) ^ {- 1} (P _ {(i)} ^ {J} - I _ {(i)} ^ {J}),
where M ^ { N J } is the mass matrix, P ^ { J } is the applied load vector, and I ^ { J } is the internal force vector. A lumped mass matrix is used because its inverse is simple to compute and because the vector multiplication of the mass inverse by the inertial force requires only n operations, where n is the number of degrees of freedom in the model. The explicit procedure requires no iterations and no tangent stiffness matrix. The internal force vector, I ^ { J } , is assembled from contributions from the individual elements such that a global stiffness matrix need not be formed.
Nodal mass and inertia
The explicit integration scheme in Abaqus/Explicit requires nodal mass or inertia to exist at all activated degrees of freedom (see “Conventions,” Section 1.2.2) unless constraints are applied using boundary conditions. More precisely, a nonzero nodal mass must exist unless all activated translational degrees of freedom are constrained and nonzero rotary inertia must exist unless all activated rotational degrees of freedom are constrained. Nodes that are part of a rigid body do not require mass, but the entire rigid body must possess mass and inertia unless constraints are used. Nodes that belong to Eulerian elements also do not require mass, since the surrounding Eulerian elements may be void at some time during the simulation.
When degrees of freedom at a node are activated by elements with a nonzero mass density (e.g., solid, shell, beam) or mass and inertia elements, a nonzero nodal mass or inertia occurs naturally from the assemblage of lumped mass contributions.
When degrees of freedom at a node are activated by elements with no mass (e.g., spring, dashpot, or connector elements), care must be taken either to constrain the node or to add mass and inertia as appropriate.
Stability
The explicit procedure integrates through time by using many small time increments. The centraldifference operator is conditionally stable, and the stability limit for the operator (with no damping) is given in terms of the highest frequency of the system as
\Delta t \leq \frac {2}{\omega_ {m a x}}.
With damping, the stable time increment is given by
\Delta t \leq \frac {2}{\omega_ {m a x}} (\sqrt {1 + \xi_ {m a x} ^ {2}} - \xi_ {m a x}),
where \xi _ { m a x } is the fraction of critical damping in the mode with the highest frequency. Contrary to our usual engineering intuition, introducing damping to the solution reduces the stable time increment. In Abaqus/Explicit a small amount of damping is introduced in the form of bulk viscosity to control high frequency oscillations. Physical forms of damping, such as dashpots or material damping, can also be introduced. Bulk viscosity and material damping are discussed below.
Estimating the stable time increment size
An approximation to the stability limit is often written as the smallest transit time of a dilatational wave across any of the elements in the mesh
\Delta t \approx \frac {L _ {m i n}}{c _ {d}},
where L _ { m i n } is the smallest element dimension in the mesh and c _ { d } is the dilatational wave speed in terms of \lambda _ { 0 } and \mu _ { 0 } , defined below.
In general, for beams, conventional shells, and membranes the element thickness or cross-sectional dimensions are not considered in determining the smallest element dimension; the stability limit is based upon the midplane or membrane dimensions only. When the transverse shear stiffness is defined for shell elements (see “Shell section behavior,” Section 29.6.4), the stable time increment will also be based on the transverse shear behavior.
This estimate for \Delta t is only approximate and in most cases is not a conservative (safe) estimate. In general, the actual stable time increment chosen by Abaqus/Explicit will be less than this estimate by a factor between 1 / { \sqrt { 2 } } and 1 in a two-dimensional model and between 1 / \sqrt { 3 } and 1 in a three-dimensional model. The time increment chosen by Abaqus/Explicit also accounts for any stiffness behavior in a model associated with penalty contact. For further discussion, see “Computational cost” below.
Stable time increment report
Abaqus/Explicit writes a report to the status (.sta) file during the data check phase of the analysis that contains an estimate of the minimum stable time increment and a listing of the elements with the smallest stable time increments and their values. The initial stable time increments listed do not include damping (bulk viscosity), mass scaling, or penalty contact effects.
This listing is provided because often a few elements have much smaller stability limits than the rest of the elements in the mesh. The stable time increment can be increased by modifying the mesh to increase the size of the controlling element or by using appropriate mass scaling.
Dilatational wave speed
The current dilatational wave speed, c _ { d } , , is determined in Abaqus/Explicit by calculating the effective hypoelastic material moduli from the material’s constitutive response. Effective Lamé’s constants, and \hat { G } = 2 \hat { \mu } , are determined in the following manner. Define \Delta p as the increment in the mean stress, \Delta \mathbf { S } as the increment in the deviatoric stress, \Delta \epsilon _ { v o l } as the increment of volumetric strain, and \Delta \mathbf { e } as the deviatoric strain increment. We assume a hypoelastic stress-strain rule of the form
\Delta p = (3 \hat {\lambda} + 2 \hat {\mu}) \Delta \epsilon_ {v o l},
\Delta \mathbf {S} = 2 \hat {\mu} \Delta \mathbf {e}.
The effective moduli can then be computed as
3 \hat {K} = 3 \hat {\lambda} + 2 \hat {\mu} = \frac {\Delta p}{\Delta \epsilon_ {v o l}},
2 \hat {\mu} = \frac {\Delta \mathbf {S} : \Delta \mathbf {e}}{\Delta \mathbf {e} : \Delta \mathbf {e}},
\hat {\lambda} + 2 \hat {\mu} = \frac {1}{3} (3 \hat {K} + 4 \hat {\mu}).
For shell elements defined by a shell cross-section that requires numerical integration (see “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5), the effective moduli for the section are computed by integrating the effective moduli at the section points through the thickness. These effective moduli represent the element stiffness and determine the current dilatational wave speed in the element as
c _ {d} = \sqrt {\frac {\hat {\lambda} + 2 \hat {\mu}}{\rho}},
where \rho is the density of the material.
In an isotropic, elastic material the effective Lamé’s constants can be defined in terms of Young’s modulus, E, and Poisson’s ratio, , by
\hat {\lambda} = \lambda_ {0} = \frac {E \nu}{(1 + \nu) (1 - 2 \nu)}
and
\hat {\mu} = \mu_ {0} = \frac {E}{2 (1 + \nu)}.
Time incrementation
The time increment used in an analysis must be smaller than the stability limit of the central-difference operator. Failure to use a small enough time increment will result in an unstable solution. When the solution becomes unstable, the time history response of solution variables such as displacements will usually oscillate with increasing amplitudes. The total energy balance will also change significantly.
If the model contains only one material type, the initial time increment is directly proportional to the size of the smallest element in the mesh. If the mesh contains uniform size elements but contains multiple material descriptions, the element with the highest wave speed will determine the initial time increment.
In nonlinear problems—those with large deformations and/or nonlinear material response—the highest frequency of the model will continually change, which consequently changes the stability limit. Abaqus/Explicit has two strategies for time incrementation control: fully automatic time incrementation (where the code accounts for changes in the stability limit) and fixed time incrementation.
Scaling the time increment
To reduce the chance of a solution going unstable, you can adjust the stable time increment computed by Abaqus/Explicit by a constant scaling factor. This factor can be used to scale the default global time estimate, the element-by-element estimate, or the fixed time increment based on the initial element-byelement estimate; it cannot be used to scale a fixed time increment specified directly by you.
Input File Usage: Use the following option to scale the stable time increment based on the global time estimate:
*DYNAMIC, EXPLICIT, SCALE FACTOR=f
Use the following option to scale the stable time increment based on the element-by-element estimate:
*DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT, SCALE FACTOR=f
Use the following option to scale the stable time increment based on the fixed time increment on the initial element-by-element estimate:
*DYNAMIC, EXPLICIT, FIXED TIME INCREMENTATION, SCALE FACTOR=f
Abaqus/CAE Usage: Step module: Create Step: General: Dynamic, Explicit: Incrementation: Time scaling factor: f
Automatic time incrementation
The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user intervention. Two types of estimates are used to determine the stability limit: element by element and global. An analysis always starts by using the element-by-element estimation method and may switch to the global estimation method under certain circumstances, as explained below.
Element-by-element estimation
In an analysis Abaqus/Explicit initially uses a stability limit based on the highest element frequency in the whole model. This element-by-element estimate is determined using the current dilatational wave speed in each element.
The element-by-element estimate is conservative; it will give a smaller stable time increment than the true stability limit that is based upon the maximum frequency of the entire model. In general, constraints such as boundary conditions and kinematic contact have the effect of compressing the eigenvalue spectrum, and the element-by-element estimates do not take this into account.
The concept of the stable time increment as the time required to propagate a dilatational wave across the smallest element dimension is useful for interpreting how the explicit procedure chooses the time increment when element-by-element stability estimation controls the time increment. As the step proceeds, the global stability estimate, if used, will make the time increment less sensitive to element size.
Input File Usage: *DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT
Abaqus/CAE Usage: Step module: Create Step: General: Dynamic, Explicit: Incrementation: Stable increment estimator: Element-by-element
Global estimation
The stability limit will be determined by the global estimator as the step proceeds unless the element-byelement estimation method is specified, fixed time incrementation is specified, or one of the conditions explained below prevents the use of global estimation. The switch to the global estimation method occurs once the algorithm determines that the accuracy of the global estimation method is acceptable.
The adaptive, global estimation algorithm determines the maximum frequency of the entire model using the current dilatational wave speed. This algorithm continuously updates the estimate for the maximum frequency. The global estimator will usually allow time increments that exceed the elementby-element values.
Abaqus/Explicit monitors the effectiveness of the global estimation algorithm. If the cost for computing the global time estimate is more than its benefit, the code will turn off the global estimation algorithm and simply use the element-by-element estimates to save computation time.
Conditions that will prevent the use of the global time estimator
The global estimation algorithm will not be used when any of the following capabilities are included in the model:
• Fluid elements
• Infinite elements
• Dashpots
• Thick shells (thickness to characteristic length ratio larger than 0.92)
• Thick beams (thickness to length ratio larger than 1.0)
• The JWL equation of state
• Material damping
• Nonisotropic elastic materials with temperature and field variable dependency
• Distortion control
• Adaptive meshing
• Subcycling
“Improved” stable time increment for three-dimensional continuum elements and elements with plane stress formulations
For three-dimensional continuum elements and elements with plane stress formulations (shell, membrane, and two-dimensional plane stress elements) an “improved” estimate of the element characteristic length is used by default. This “improved” method usually results in a larger element stable time increment than a more traditional method. For analyses using variable mass scaling, the total mass added to achieve a given stable time increment will be less with the improved estimate.
Input File Usage: Use the following option to activate the “improved” element time estimation method:
*DYNAMIC, EXPLICIT, IMPROVED DT METHOD=YES
Use the following option to deactivate the “improved” element time estimation method:
*DYNAMIC, EXPLICIT, IMPROVED DT METHOD=NO
Abaqus/CAE Usage: The ability to deactivate the “improved” element time estimation method is not supported in Abaqus/CAE.
Fixed time incrementation
A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size is determined either by the initial element-by-element stability estimate for the step or by a user-specified time increment.
Fixed time incrementation may be useful when a more accurate representation of the higher mode response of a problem is required. In this case a time increment size smaller than the element-by-element
estimates may be used. The element-by-element estimate can be obtained simply by running a data check analysis (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2).
When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response is stable during the step. You should ensure that a valid response has been obtained by carefully checking the energy history and other response variables.
Basing the fixed time increment size on the initial element-by-element stability limit
You can use time increments the size of the initial element-by-element stability limit throughout a step. The dilatational wave speed in each element at the beginning of the step is used to compute the fixed time increment size.
Input File Usage: *DYNAMIC, EXPLICIT, FIXED TIME INCREMENTATION
Abaqus/CAE Usage: Step module: Create Step: General: Dynamic, Explicit: Incrementation: Type: Fixed: Use element-by-element time increment estimator
Specifying the fixed time increment size directly
Alternatively, you can specify a time increment size directly.
Input File Usage: *DYNAMIC, EXPLICIT, DIRECT USER CONTROL
Abaqus/CAE Usage: Step module: Create Step: General: Dynamic, Explicit: Incrementation: Type: Fixed: User-defined time increment
Advantages of the explicit method
The use of small increments (dictated by the stability limit) is advantageous because it allows the solution to proceed without iterations and without requiring tangent stiffness matrices to be formed. It also simplifies the treatment of contact.
The explicit dynamics procedure is ideally suited for analyzing high-speed dynamic events, but many of the advantages of the explicit procedure also apply to the analysis of slower (quasi-static) processes. A good example is sheet metal forming, where contact dominates the solution and local instabilities may form due to wrinkling of the sheet.
The results in an explicit dynamics analysis are not automatically checked for accuracy as they are in Abaqus/Standard (Abaqus/Standard uses the half-increment residual). In most cases this is not of concern because the stability condition imposes a small time increment such that the solution changes only slightly in any one time increment, which simplifies the incremental calculations. While the analysis may take an extremely large number of increments, each increment is relatively inexpensive, often resulting in an economical solution. It is not uncommon for Abaqus/Explicit to take over 105 increments for an analysis. The method is, therefore, computationally attractive for problems where the total dynamic response time that must be modeled is only a few orders of magnitude longer than the stability limit; for example, wave propagation studies or some “event and response” applications.