김경종
24 KiB
cases; for a linear case stiffness proportional damping is exactly the same as defining a damping matrix equal to \beta _ { R } times the (elastic) material stiffness matrix. Other contributions to the stiffness matrix (e.g., hourglass, transverse shear, and drill stiffnesses) are not included when computing stiffness proportional damping. \beta _ { R } has units of (time).
Input File Usage: *DAMPING, BETA=
Abaqus/CAE Usage: Property module: material editor: Mechanical→Damping: Beta: \beta _ { R }
Defining variable stiffness proportional damping in Abaqus/Explicit
In Abaqus/Explicit you can define \beta _ { R } as a tabular function of temperature and/or field variables. Therefore, stiffness proportional damping can vary during an Abaqus/Explicit analysis.
Input File Usage: *DAMPING, BETA=TABULAR
Structural damping
Structural damping assumes that the damping forces are proportional to the forces caused by stressing of the structure and are opposed to the velocity. Therefore, this form of damping can be used only when the displacement and velocity are exactly 9 0 ^ { \circ } out of phase. Structural damping is best suited for frequency domain dynamic procedures (see “Damping in modal superposition procedures” below). The damping forces are then
F _ {D} ^ {N} = i s I ^ {N},
where F _ { D } ^ { N } are the damping forces, i = \sqrt { - 1 } , s is the user-defined structural damping factor, and I ^ { N } are the forces caused by stressing of the structure. The damping forces due to structural damping are intended to represent frictional effects (as distinct from viscous effects). Thus, structural damping is suggested for models involving materials that exhibit frictional behavior or where local frictional effects are present throughout the model, such as dry rubbing of joints in a multi-link structure.
Structural damping can be added to the model as mechanical dampers such as connector damping or as a complex stiffness on spring elements.
Structural damping can be used in steady-state dynamic procedures that allow for nondiagonal damping.
Input File Usage: Use the following option to define structural damping:
*DAMPING, STRUCTURAL=
Abaqus/CAE Usage: Property module: material editor: Mechanical→Damping: Structural:
Artificial damping in direct-integration dynamic analysis
In Abaqus/Standard the operators used for implicit direct time integration introduce some artificial damping in addition to Rayleigh damping. Damping associated with the Hilber-Hughes-Taylor and hybrid operators is usually controlled by the Hilber-Hughes-Taylor parameter \alpha , which is not the same as the \alpha _ { R } parameter controlling the mass proportional part of Rayleigh damping. The \beta and \gamma parameters of the Hilber-Hughes-Taylor and hybrid operators also affect numerical damping. The \alpha ,
\beta , and \gamma parameters are not available for the backward Euler operator. See “Implicit dynamic analysis using direct integration,” Section 6.3.2, for more information about this other form of damping.
Artificial damping in explicit dynamic analysis
Rayleigh damping is meant to reflect physical damping in the actual material. In Abaqus/Explicit a small amount of numerical damping is introduced by default in the form of bulk viscosity to control high frequency oscillations; see “Explicit dynamic analysis,” Section 6.3.3, for more information about this other form of damping.
Effects of damping on the stable time increment in Abaqus/Explicit
As the fraction of critical damping for the highest mode ( \xi _ { \mathrm { m a x } } ) increases, the stable time increment for Abaqus/Explicit decreases according to the equation
\Delta t \leq \frac {2}{\omega_ {\mathrm{max}}} (\sqrt {1 + \xi_ {\mathrm{max}} ^ {2}} - \xi_ {\mathrm{max}}),
where (by substituting \omega _ { \mathrm { m a x } } . , the frequency of the highest mode, into the equation for \xi _ { i } given previously)
\xi_ {\mathrm{max}} = \frac {\alpha_ {R}}{2 \omega_ {\mathrm{max}}} + \frac {\beta_ {R} \omega_ {\mathrm{max}}}{2}.
These equations indicate a tendency for stiffness proportional damping to have a greater effect on the stable time increment than mass proportional damping.
To illustrate the effect that damping has on the stable time increment, consider a cantilever in bending modeled with continuum elements. The lowest frequency is \omega _ { \mathrm { m i n } } = 1 rad/sec, while for the particular mesh chosen, the highest frequency is \omega _ { \mathrm { m a x } } = 1 0 0 0 \mathrm { r a d / s e c } . The lowest mode in this problem corresponds to the cantilever in bending, and the highest frequency is related to the dilation of a single element.
With no damping the stable time increment is
\Delta t = \frac {2}{\omega_ {\mathrm{max}}} = 2 \times 1 0 ^ {- 3} \mathrm{sec}.
If we use stiffness proportional damping to create 1% of critical damping in the lowest mode, the damping factor is given by
\beta_ {R} = \frac {2 \times 0 . 0 1}{1} = 2 \times 1 0 ^ {- 2} \mathrm{sec}.
This corresponds to a critical damping factor in the highest mode of
\xi_ {\mathrm{max}} = \frac {\omega_ {\mathrm{max}} \beta_ {R}}{2} = 1 0.
The stable time increment with damping is, thus, reduced by a factor of
(\sqrt {1 + 1 0 ^ {2}} - 1 0) \approx 0. 0 5,
and becomes
\Delta t \approx (2 \times 1 0 ^ {- 3}) \times 0. 0 5
\approx 1 \times 1 0 ^ {- 4}.
Thus, introducing 1% critical damping in the lowest mode reduces the stable time increment by a factor of twenty.
However, if we use mass proportional damping to damp out the lowest mode with 1% of critical damping, the damping factor is given by
\alpha_ {R} = 2 \omega_ {\mathrm{min}} \xi = 2 \times 1 \times 1 0 ^ {- 2} = 2 \times 1 0 ^ {- 2} \mathrm{sec} ^ {- 1},
which corresponds to a critical damping factor in the highest mode of
\xi_ {\mathrm{max}} = \frac {\alpha_ {R}}{2 \omega_ {\mathrm{max}}} = \frac {2 \times 1 0 ^ {- 2}}{2 \times 1 0 0 0} = 1 0 ^ {- 5}.
The stable time increment with damping is reduced by a factor of
(\sqrt {1 + 1 0 ^ {- 1 0}} - 1 0 ^ {- 5}) \approx 0. 9 9 9 9 9,
which is almost negligible.
This example demonstrates that it is generally preferable to damp out low frequency response with mass proportional damping rather than stiffness proportional damping. However, mass proportional damping can significantly affect rigid body motion, so large \alpha _ { R } is often undesirable. To avoid a dramatic drop in the stable time increment, the stiffness proportional damping factor, \beta _ { R } , should be less than or of the same order of magnitude as the initial stable time increment without damping. With \beta _ { R } = 2 / \omega _ { \mathrm { m a x } } , the stable time increment is reduced by about 52%.
Damping in modal superposition procedures
Damping can be specified as part of the step definition for modal superposition procedures. “Damping in a linear dynamic analysis” in “Dynamic analysis procedures: overview,” Section 6.3.1, describes the availability of damping types, which depends on the procedure type and the architecture used to perform the analysis, and provides details on the following types of damping:
• Viscous modal damping (Rayleigh damping and fraction of critical damping)
• Structural modal damping
• Composite modal damping
Use with other material models
The \beta _ { R } factor applies to all elements that use a linear elastic material definition (“Linear elastic behavior,” Section 22.2.1) and to Abaqus/Standard beam and shell elements that use general sections. In the latter case, if a nonlinear beam section definition is provided, the \beta _ { R } factor is multiplied by the slope of the force-strain (or moment-curvature) relationship at zero strain or curvature. In addition, the \beta _ { R } factor applies to all Abaqus/Explicit elements that use a hyperelastic material definition (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1), a hyperfoam material definition (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2), or general shell sections (“Using a general shell section to define the section behavior,” Section 29.6.6).
In the case of a no tension elastic material the \beta _ { R } factor is not used in tension, while for a no compression elastic material the \beta _ { R } factor is not used in compression (see “No compression or no tension,” Section 22.2.2). In other words, these modified elasticity models exhibit damping only when they have stiffness.
Elements
The \alpha _ { R } factor is applied to all elements that have mass including point mass elements (discrete DASHPOTA elements in each global direction, each with one node fixed, can also be used to introduce this type of damping). For point mass and rotary inertia elements mass proportional or composite modal damping are defined as part of the point mass or rotary inertia definitions (“Point masses,” Section 30.1.1, and “Rotary inertia,” Section 30.2.1).
The \beta _ { R } factor is not available for spring elements: discrete dashpot elements should be used in parallel with spring elements instead.
The \beta _ { R } factor is also not applied to the transverse shear terms in Abaqus/Standard beams and shells.
The hybrid element stiffness matrix formulation is different than the corresponding non-hybrid formulation; therefore, the stiffness proportional damping is different for the same value of the \beta _ { R } factor in nonlinear dynamic analysis. In linear analyses Abaqus/Standard imposes equivalent stiffness proportional damping for hybrid and non-hybrid elements.
In Abaqus/Standard composite modal damping cannot be used with or within substructures. Rayleigh damping can be introduced for substructures. When Rayleigh damping is used within a substructure, \alpha _ { R } and \beta _ { R } are averaged over the substructure to define single values of \alpha _ { R } and \beta _ { R } for the substructure. These are weighted averages, using the mass as the weighting factor for \alpha _ { R } and the volume as the weighting factor for \beta _ { R } . These averaged damping values can be superseded by providing them directly in a second damping definition. See “Using substructures,” Section 10.1.1.
26.1.2 THERMAL EXPANSION
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
References
• “Material library: overview,” Section 21.1.1
• “UEXPAN,” Section 1.1.30 of the Abaqus User Subroutines Reference Guide
• *EXPANSION
• “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Guide
• “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Guide
Overview
Thermal expansion effects:
• can be defined by specifying thermal expansion coefficients so that Abaqus can compute thermal strains and, in Abaqus/CFD, buoyancy forces;
• can be isotropic, orthotropic, or fully anisotropic;
• are defined as total expansion from a reference temperature;
• can be specified as a function of temperature and/or field variables;
• can be defined with a distribution for solid continuum elements in Abaqus/Standard; and
• in Abaqus/Standard can be specified directly in user subroutine UEXPAN (if the thermal strains are complicated functions of field variables and state variables).
Defining thermal expansion coefficients
Thermal expansion is a material property included in a material definition (see “Material data definition,” Section 21.1.2) except when it refers to the expansion of a gasket whose material properties are not defined as part of a material definition. In that case expansion must be used in conjunction with the gasket behavior definition (see “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6).
In an Abaqus/Standard analysis a spatially varying thermal expansion can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include default values for the thermal expansion. If a distribution is used, no dependencies on temperature and/or field variables for the thermal expansion can be defined.
In an Abaqus/CFD analysis the thermal expansion coefficient, , can be defined for computation of thermal strains in solid materials and the volumetric thermal expansion coefficient, , can be defined for computation of buoyancy forces in fluid materials. See “Computation of thermal strains,” and “Computation of buoyancy forces in Abaqus/CFD” below, for a detailed description of each of these coefficients.
| Input File Usage: | Use the following options to define thermal expansion for most materials:*MATERIAL*EXPANSIONUse the following options to define thermal expansion for gaskets whose constitutive response is defined directly as gasket behavior:*GASKET BEHAVIOR*EXPANSION |
| Abaqus/CAE Usage: | Use the following option in conjunction with other material behaviors, including gasket behavior, to include thermal expansion effects:Property module: material editor: Mechanical→Expansion |
Computation of thermal strains
Abaqus requires thermal expansion coefficients, , that define the total thermal expansion from a reference temperature, \theta ^ { 0 } , as shown in Figure 26.1.2–1.
line
| θ | ε₁ᵗʰ | ε₂ᵗʰ |
|---|---|---|
| θ⁰ | 0 | 0 |
| θ¹ | α₁ | α₁' |
| θ² | α₂ | α₂' |
Figure 26.1.2–1 Definition of the thermal expansion coefficient.
They generate thermal strains according to the formula
\varepsilon^ {t h} = \alpha (\theta , f _ {\beta}) (\theta - \theta^ {0}) - \alpha (\theta^ {I}, f _ {\beta} ^ {I}) (\theta^ {I} - \theta^ {0}),
where
| $\alpha(\theta, f_{\beta})$ | is the thermal expansion coefficient; |
| $\theta$ | is the current temperature; |
| $\theta^{I}$ | is the initial temperature; |
| $f_{\beta}$ | are the current values of the predefined field variables; |
| $f_{\beta}^{I}$ | are the initial values of the field variables; and |
| $\theta^{0}$ | is the reference temperature for the thermal expansion coefficient. |
The second term in the above equation represents the strain due to the difference between the initial temperature, \theta ^ { I } , and the reference temperature, \theta ^ { 0 } . This term is necessary to enforce the assumption that there is no initial thermal strain for cases in which the reference temperature does not equal the initial temperature.
Defining the reference temperature
If the coefficient of thermal expansion, , is not a function of temperature or field variables, the value of the reference temperature, \theta ^ { 0 } , is not needed. If is a function of temperature or field variables, you can define \theta ^ { 0 } .
Input File Usage: *EXPANSION, ZERO=
Abaqus/CAE Usage: Property module: material editor: Mechanical→Expansion:
Reference temperature: \theta ^ { 0 }
Computation of buoyancy forces in Abaqus/CFD
Buoyancy forces driving natural convection in Abaqus/CFD fluids are computed using the Boussinesq approximation
(\rho - \rho^ {I}) g \approx - \rho^ {I} \beta (\theta - \theta^ {0}) g,
where
| $\rho$ | is the density; |
| $\rho^{I}$ | is the initial density; |
| $g$ | is the acceleration due to gravity; |
| $\theta$ | is the temperature; |
| $\theta^{0}$ | is the reference temperature, and; |
| $\beta$ | is the volumetric thermal expansion coefficient. |
The volumetric thermal expansion coefficient, , is defined as
\beta (\theta) = \frac {- 1}{\rho} \left(\frac {\delta \rho}{\delta \theta}\right) _ {p}
and is related to the thermal expansion coefficient, , by the expression
\beta = 3 \alpha .
Converting thermal expansion coefficients from differential form to total form
Total thermal expansion coefficients are commonly available in tables of material properties. However, sometimes you are given thermal expansion data in differential form:
d \varepsilon^ {t h} = \alpha^ {\prime} (\theta) d \theta ;
that is, the tangent to the strain-temperature curve is provided (see Figure 26.1.2–1). To convert to the total thermal expansion form required by Abaqus, this relationship must be integrated from a suitably chosen reference temperature, \theta ^ { 0 } :
\varepsilon^ {t h} = \int_ {\theta^ {0}} ^ {\theta} \alpha^ {\prime} d \theta \Rightarrow \alpha (\theta) = \frac {1}{\theta - \theta^ {0}} \int_ {\theta^ {0}} ^ {\theta} \alpha^ {\prime} d \theta .
For example, suppose \alpha ^ { \prime } is a series of constant values: \alpha _ { 1 } ^ { \prime } between \theta ^ { 0 } and \theta ^ { 1 } ; \alpha _ { 2 } ^ { \prime } between \theta ^ { 1 } and \theta ^ { 2 } ; \alpha _ { 3 } ^ { \prime } between \theta ^ { 2 } and \theta ^ { 3 } ; ; etc. Then,
\varepsilon_ {1} ^ {t h} = \alpha_ {1} ^ {\prime} (\theta^ {1} - \theta^ {0})
\varepsilon_ {2} ^ {t h} = \varepsilon_ {1} ^ {t h} + \alpha_ {2} ^ {\prime} (\theta^ {2} - \theta^ {1})
\varepsilon_ {3} ^ {t h} = \varepsilon_ {2} ^ {t h} + \alpha_ {3} ^ {\prime} (\theta^ {3} - \theta^ {2}).
The corresponding total expansion coefficients required by Abaqus are then obtained as
\alpha_ {1} = \varepsilon_ {1} ^ {t h} / (\theta^ {1} - \theta^ {0})
\alpha_ {2} = \varepsilon_ {2} ^ {t h} / (\theta^ {2} - \theta^ {0})
\alpha_ {3} = \varepsilon_ {3} ^ {t h} / (\theta^ {3} - \theta^ {0}).
Defining increments of thermal strain in user subroutine UEXPAN
Increments of thermal strain can be specified in Abaqus/Standard user subroutine UEXPAN as functions of temperature and/or predefined field variables. User subroutine UEXPAN must be used if the thermal strain increments depend on state variables.
Input File Usage: *EXPANSION, USER
Abaqus/CAE Usage: Property module: material editor: Mechanical→Expansion:
Use user subroutine UEXPAN
Defining the initial temperature and field variable values
If the coefficient of thermal expansion, \alpha , is a function of temperature or field variables, the initial temperature and initial field variable values, \theta ^ { I } and f _ { \beta } ^ { I } , are given as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1.
Element removal and reactivation
If an element has been removed and subsequently reactivated in Abaqus/Standard (“Element and contact pair removal and reactivation,” Section 11.2.1), \bar { \theta } ^ { I } and f _ { \beta } ^ { I } in the equation for the thermal strains represent temperature and field variable values as they were at the moment of reactivation.
Defining directionally dependent thermal expansion
Isotropic or orthotropic thermal expansion can be defined in Abaqus. In addition, fully anisotropic thermal expansion can be defined in Abaqus/Standard.
Orthotropic and anisotropic thermal expansion can be used only with materials where the material directions are defined with local orientations (see “Orientations,” Section 2.2.5).
Orthotropic thermal expansion in Abaqus/Explicit is allowed only with anisotropic elasticity (including orthotropic elasticity) and anisotropic yield (see “Anisotropic yield/creep,” Section 23.2.6).
Only isotropic thermal expansion is allowed in Abaqus/CFD, for adiabatic stress analysis, and with the hyperelastic and hyperfoam material models.
Isotropic expansion
If the thermal expansion coefficient is defined directly, only one value of is needed at each temperature. If user subroutine UEXPAN is used, only one isotropic thermal strain increment ( \Delta \varepsilon = \Delta \varepsilon _ { 1 1 } = \Delta \varepsilon _ { 2 2 } = \Delta \varepsilon _ { 3 3 } ) must be defined.
| Input File Usage: | Use the following option to define the thermal expansion coefficient directly:*EXPANSION, TYPE=ISOUse the following option to define the thermal expansion with user subroutine UEXPAN:*EXPANSION, TYPE=ISO, USER |
| Abaqus/CAE Usage: | Use the following input to define the thermal expansion coefficient directly:Property module: material editor: Mechanical→Expansion: Type: IsotropicUse the following input to define the thermal expansion with user subroutine UEXPAN:Property module: material editor: Mechanical→Expansion: Type: Isotropic, Use user subroutine UEXPAN |
Orthotropic expansion
If the thermal expansion coefficients are defined directly, the three expansion coefficients in the principal material directions ( \alpha _ { 1 1 } , \alpha _ { 2 2 } , and \alpha _ { 3 3 } ) should be given as functions of temperature. If user subroutine UEXPAN is used, the three components of thermal strain increment in the principal material directions ( \Delta \varepsilon _ { 1 1 } , \Delta \varepsilon _ { 2 2 } , and \Delta \varepsilon _ { 3 3 } ) must be defined.
Input File Usage: Use the following option to define the thermal expansion coefficient directly: *EXPANSION, TYPE=ORTHO
Use the following option to define the thermal expansion with user subroutine UEXPAN:
*EXPANSION, TYPE=ORTHO, USER
Abaqus/CAE Usage: Use the following input to define the thermal expansion coefficient directly:
Property module: material editor: Mechanical→Expansion:
Type: Orthotropic
Use the following input to define the thermal expansion with user subroutine UEXPAN:
Property module: material editor: Mechanical→Expansion: Type:
Orthotropic, Use user subroutine UEXPAN
Anisotropic expansion
If the thermal expansion coefficients are defined directly, all six components of \alpha \ ( \alpha _ { 1 1 } , \ \alpha _ { 2 2 } , \ \alpha _ { 3 3 } , \alpha _ { 1 2 } , \alpha _ { 1 3 } , \alpha _ { 2 3 } ) must be given as functions of temperature. If user subroutine UEXPAN is used, all six components of the thermal strain increment ( \Delta \varepsilon _ { 1 1 } , \Delta \varepsilon _ { 2 2 } , \Delta \varepsilon _ { 3 3 } , \Delta \varepsilon _ { 1 2 } , \Delta \varepsilon _ { 1 3 } , \Delta \varepsilon _ { 2 3 } ) must be defined.
In an Abaqus/Standard analysis if a distribution is used to define the thermal expansion, the number of expansion coefficients given for each element in the distribution, which is determined by the associated distribution table (“Distribution definition,” Section 2.8.1), must be consistent with the level of anisotropy specified for the expansion behavior. For example, if orthotropic behavior is specified, three expansion coefficients must be defined for each element in the distribution.
Input File Usage: Use the following option to define the thermal expansion coefficient directly:
*EXPANSION, TYPE=ANISO
Use the following option to define the thermal expansion with user subroutine UEXPAN:
*EXPANSION, TYPE=ANISO, USER
Abaqus/CAE Usage: Use the following input to define the thermal expansion coefficient directly:
Property module: material editor: Mechanical→Expansion:
Type: Anisotropic
Use the following input to define the thermal expansion with user subroutine UEXPAN:
Property module: material editor: Mechanical→Expansion: Type:
Anisotropic, Use user subroutine UEXPAN
Thermal stress
When a structure is not free to expand, a change in temperature will cause stress. For example, consider a single two-node truss of length L that is completely restrained at both ends. The cross-sectional area; the Young’s modulus, E; and the thermal expansion coefficient, , are all constant. The stress in this one-dimensional problem can then be calculated from Hooke’s Law as \sigma _ { x } = E ( \varepsilon _ { x } - \varepsilon _ { x } ^ { t h } ) , where \varepsilon _ { x }