김경종
22 KiB
line
| Point | Pressure | Plastic Closure |
|---|---|---|
| A | 0 | 0 |
| D | 0 | 0 |
| F | 0 | 0 |
| N | 0 | 0 |
| E | 0 | 0 |
| C | 0 | 0 |
| B | 0 | 0 |
| P | 0 | 0 |
| M | 0 | 0 |
Figure 32.6.6–4 Elastic-plastic model.
Abaqus/Standard offers two alternatives to allow you to override this default method of determining the onset of yield as described below. If only a loading curve is provided, the unloading will be based on the curve , independent of the level of plasticity.
Defining the loading curve
To define the loading curve in piecewise linear form, you provide data points of pressure (or force, or force per unit length) versus closure (where closure represents the elastic plus the plastic closure), starting with point A. The last closure value given represents the closure at which the gasket is assumed crushed (point M in Figure 32.6.6–4); at this point, the maximum permanent deformation is reached. For negative closures the model gives zero pressure (or force).
To override the default method of determining the onset of yield, you can specify either a value for the decrease in slope other than the default value of 10% or the closure value at which onset of yield occurs. The specified value must correspond to a point on the loading curve at which the slope decreases.
Input File Usage:
Use the following option to define the loading curve and use the default method for determining the onset of yield:
*GASKET THICKNESS BEHAVIOR, TYPE=ELASTIC-PLASTIC, DIRECTION=LOADING
Use the following option to define the loading curve and specify a nondefault value for the decrease in slope that defines the onset of yield:
*GASKET THICKNESS BEHAVIOR, TYPE=ELASTIC-PLASTIC, DIRECTION=LOADING, SLOPE DROP=drop
Use the following option to define the loading curve and specify the closure value that defines the onset of yield:
*GASKET THICKNESS BEHAVIOR, TYPE=ELASTIC-PLASTIC, DIRECTION=LOADING, YIELD ONSET=closure_value
Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Type: Elastic-Plastic, Loading, Yield onset method: Relative slope drop drop or Yield onset method: Closure value closure_value
Defining the unloading curve
To define the unloading curves ( , , and so on), you provide data points of pressure (or force, or force per unit length) versus closure (elastic plus plastic) for each given plastic closure (closure at points D, F, and so on) in ascending values of closure. You can specify as many unloading curves as are necessary. If unloading occurs at a plastic closure for which an unloading curve is not specified, the unloading curve is interpolated from neighboring unloading curves. If no unloading curves are specified, unloading is assumed to follow a curve similar to the initial nonlinear elastic segment of the loading curve. The unloading curves are stored in normalized form so that they intersect the yield curve at a unit stress (or unit force) for a unit elastic closure, and the interpolation occurs between these normalized curves.
If the loading curve includes highly nonlinear behavior after the onset of yield, the interpolated unloading may give unreasonable behavior (such as the interpolated unloading path crossing over the user-defined loading curve). You should specify as many user-defined unloading curves as are needed to create regions for which interpolated unloading response is appropriate. For example, Figure 32.6.6–5 illustrates a loading curve that includes a sharp decrease in the hardening slope well after the onset of yield. In this case it is insufficient to specify only one unloading curve at the gasket crush point (the end of the loading data). If unloading were to take place from point C, the unloading path would cross over the loading path. At least one additional unloading curve is required, after the sharp decrease in hardening slope, to prevent the interpolated unloading path crossing the loading curve.
Input File Usage: *GASKET THICKNESS BEHAVIOR, TYPE=ELASTIC-PLASTIC, DIRECTION=UNLOADING
Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Type: Elastic-Plastic, Unloading, toggle on Include user-specified unloading curves
Defining the behavior for elements with an initial gap
For cases when the load in the gasket does not increase as soon as the gasket is compressed (see Figure 32.6.6–6), you can specify an initial gap as part of the gasket section property definition (see “Defining the gasket element’s initial geometry,” Section 32.6.4) and define the loading/unloading curves as if the initial gap were not present (the case of Figure 32.6.6–4). This method is convenient when many gasket elements refer to the same gasket behavior and the only difference is the initial gap.
flowchart
graph TD
A["Start A"] --> B["Start B"]
B --> C["Point C"]
C --> M["Point M"]
M --> P["Point P"]
P -->|gasket crush point| M
style A fill:#f9f,stroke:#333
style B fill:#f9f,stroke:#333
style C fill:#f9f,stroke:#333
style M fill:#f9f,stroke:#333
style P fill:#f9f,stroke:#333
note1["point where user-defined unloading response should be specified"] --> C
note2["interpolated unloading response"] --> C
note3["onset of yield"] --> B
note4["closure"] --> N
note5["pressure"] --> A
Figure 32.6.6–5 Elastic-plastic behavior with complex loading curve.
line
| Phase | Closure | Pressure |
|---|---|---|
| A | A | 0 |
| B | D | ~0.5 |
| C | F | ~0.7 |
| D | F | ~0.3 |
| E | N | ~0.8 |
| M | N | ~1.0 |
Figure 32.6.6–6 Elastic-plastic model with initial gap.
Numerical stabilization of the thickness-direction behavior
The damage and elastic-plastic models described above have zero stiffness at zero pressure. To overcome numerical problems caused by this zero stiffness, Abaqus/Standard automatically adds a small stiffness (by default, equal to 10−3 times the initial compressive stiffness) in the thickness direction of the gasket when the pressure obtained from the specified gasket thickness behavior is zero. This numerical stabilization ensures that the gasket element always returns to its stress-free thickness when it is totally unloaded. Hence, if the gasket surfaces are pulled apart, a small force will arise from the stabilization process. You can change the default stiffness.
Input File Usage: *GASKET THICKNESS BEHAVIOR, DIRECTION=LOADING, TENSILE STIFFNESS FACTOR=factor
Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Loading, Tensile stiffness factor: factor
Defining the transverse shear behavior of the gasket
You can define the elastic transverse shear stiffness of the gasket. Abaqus/Standard measures the relative displacement between the bottom and top of the gasket element along the local 2- or 3-directions to define the transverse shear in the gasket. Therefore, you should always define the elastic transverse stiffness as stress (or force, or force per unit length) per unit displacement. You can specify the stiffness as a function of temperature and field variables. The same stiffness is used for the shear in the 1–2 plane and the shear in the 1–3 plane. For each set of temperature and/or field variables, the first slope of the initial loading curve for the gasket’s thickness-direction behavior will be used to compute the transverse shear stiffness if the transverse shear behavior is not defined explicitly.
Input File Usage: *GASKET ELASTICITY, COMPONENT=TRANSVERSE SHEAR, DEPENDENCIES
Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Transverse Shear Elasticity
Choosing a unit system to define the transverse shear behavior
The transverse shear stiffness is defined with units of stress per unit displacement, force per unit displacement, or force per unit length per unit displacement. The unit system used to define the transverse shear behavior must be consistent with the unit system used for the thickness-direction behavior.
Providing the stiffness with units of stress per unit displacement
You can define the transverse shear stiffness in units of stress per unit displacement for all gasket element types. The stiffness will be used to compute transverse shear stresses, which are available for output or visualization.
Input File Usage: *GASKET ELASTICITY, COMPONENT=TRANSVERSE SHEAR, VARIABLE=STRESS
Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Transverse Shear Elasticity: Units: Stress
Providing the stiffness with other units
You can define the transverse shear stiffness in units of force (or force per unit length) per unit displacement only for link elements and three-dimensional line elements. This method is suited for cases where the gasket cross-section in the 1–2 or 1–3 plane varies greatly with deformation because it would be too expensive to model such a deformation mechanism with a full two- or three-dimensional model, as explained earlier.
When using two- or three-dimensional link elements, you must specify the stiffness in terms of units of force per unit displacement. Abaqus/Standard will use this stiffness to compute transverse shear forces, which are available for output or visualization. When using axisymmetric link elements and three-dimensional line elements, you must specify the stiffness in terms of units of force per unit length per unit displacement. Abaqus/Standard will use this stiffness to compute transverse shear forces per unit length, which are available for output or visualization.
Input File Usage: *GASKET ELASTICITY, COMPONENT=TRANSVERSE SHEAR, VARIABLE=FORCE
Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Transverse Shear Elasticity: Units: Force
Defining the membrane behavior of the gasket
You can define the linear elastic behavior of the gasket by giving Young’s modulus and Poisson’s ratio. These data can be provided as a function of temperature and/or field variables. If you do not specify the linear elastic behavior of the gasket, the gasket has no membrane stiffness. In this case you must ensure that the nodes of the elements are restrained adequately in the directions orthogonal to the thickness direction of the gasket.
Input File Usage: *GASKET ELASTICITY, COMPONENT=MEMBRANE, DEPENDENCIES
Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Membrane Elasticity
Defining thermal expansion for the membrane and thickness-direction behaviors
You can define isotropic thermal expansion to specify the same coefficient of thermal expansion for the membrane and thickness-direction behaviors.
Alternatively, you can define orthotropic thermal expansion to specify three different coefficients of thermal expansion. The first coefficient will apply to the thermal expansion of the gasket in the thickness direction; the other two coefficients will apply to the expansion of the gasket in the local 2- and 3-directions, respectively.
The membrane thermal strains, \varepsilon ^ { t h } , are obtained as explained in “Thermal expansion,” Section 26.1.2. Abaqus/Standard computes the thermal closure for the thickness direction as
C ^ {t h} = \varepsilon^ {t h} * (\text { initial gap } + \text { initial void } - \text { initial thickness }),
so that the “mechanical” closure is obtained as
C ^ {m e c h} = C ^ {t o t a l} - C ^ {t h}.
You can specify the initial gap and initial void as part of the gasket section definition; the initial thickness is obtained directly from the nodal coordinates of the gasket elements, or you can specify it as part of the gasket section definition (see “Defining the gasket element’s initial geometry,” Section 32.6.4).
If user subroutine UEXPAN is used to define the thermal expansion of the gasket, the incremental thermal strains must be provided in the subroutine. The thermal closure will be obtained from the thermal strain in the thickness direction, as described above.
Input File Usage: Use either of the following options to define the thermal expansion directly:
*EXPANSION, TYPE=ISO
*EXPANSION, TYPE=ORTHO
Use either of the following options to define the thermal expansion in user subroutine UEXPAN:
*EXPANSION, TYPE=ISO, USER
*EXPANSION, TYPE=ORTHO, USER
Abaqus/CAE Usage: Property module: material editor: Mechanical→Expansion: Use user subroutine UEXPAN (optional)
Defining creep behavior for the thickness-direction behavior
You can define creep behavior in the thickness direction of the gasket only when the elastic-plastic model (see “Defining a nonlinear elastic-plastic model” above) is used. The creep closure rate will be obtained as
\dot {C} ^ {c r} = \dot {\varepsilon} ^ {c r} * (\text { initial thickness - initial gap - initial void }),
where is obtained as explained in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. You can specify the initial gap and initial void as part of the gasket section definition; the initial thickness is obtained directly from the nodal coordinates of the gasket elements, or you can specify it as part of the gasket section definition (see “Defining the gasket element’s initial geometry,” Section 32.6.4).
If user subroutine CREEP is used to define the rate-dependent thickness-direction response of the gasket, the compressive creep strain increment must be provided in the subroutine. The creep closure will be obtained from the creep strain, as described above.
Input File Usage: Use the following option to define the creep behavior directly:
*CREEP
Use the following option to define the creep behavior in user subroutine CREEP:
*CREEP, LAW=USER
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Creep:
Law: User-defined (optional)
Defining viscoelastic behavior for the thickness-direction behavior
You can define viscoelastic behavior in the thickness direction of the gasket only when the elasticdamage model (see “Defining a nonlinear elastic model with damage” above) is used. Only frequency domain viscoelastic behavior is supported. This behavior is useful for modeling the steady-state dynamic response of automotive components with gaskets about some pre-loaded base state, such as would be obtained at the end of a nonlinear sealing analysis, to determine the noise-vibration-harshness (NVH) characteristics of the system.
During the nonlinear sealing analysis step the frequency-domain viscoelastic behavior is ignored, and the material response is determined by the long-term elastic properties of the material. It is generally accepted (Zubeck and Marlow, 2002) that the dynamic stiffness and damping characteristics of automotive components such as gaskets and grommets vary with the frequency of excitation as well as the level of preload. These structural properties also depend on the geometry and the level of confinement of the gasket. This capability allows the direct specification of such dynamic properties as quantified by the effective storage and loss moduli in the thickness-direction, as tabular functions of the frequency of excitation and the level of preload. The preload is quantified by the amount of closure in the base state about which the steady-state dynamic response is desired.
In determining the dynamic response of the gasket, the long-term elastic response is assumed to be defined by the nonlinear elastic model with damage. The steady-state dynamic response is assumed to be a perturbation about a base state defined by this elastic damage behavior at a certain value of closure. The viscoelastic response can be specified using two approaches, as discussed below.
Direct specification of the properties
The first approach involves direct (tabular) specification of the thickness-direction loss and storage moduli as functions of excitation frequency at different levels of closure.
Input File Usage: *VISCOELASTIC, TYPE=TRACTION, PRELOAD=UNIAXIAL
Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Viscoelastic:
Domain: Frequency and Frequency: Tabular
Specification of properties in terms of ratios
The second approach allows the specification of the ratio of both the thickness-direction storage and the loss moduli to the long-term thickness-direction elastic modulus. These ratios can be specified as tabular functions of the excitation frequency but are assumed to be independent of the amount of closure. The actual storage or loss modulus at any given level of closure is computed by multiplying the appropriate ratio with the long-term elastic modulus at the current value of closure (of the base state). See “Frequency domain viscoelasticity,” Section 22.7.2, for a summary of the second approach in the
context of continuum material viscoelastic properties (the approach used here is just a one-dimensional specialization of the more general approach presented there).
Input File Usage: *VISCOELASTIC, TYPE=TRACTION
Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Viscoelastic:
Domain: Frequency and Frequency: Tabular
Defining the contact area for average contact pressure output
When the thickness-direction behavior of the gasket is defined in terms of force or force per unit length versus closure, Abaqus/Standard will provide the thickness-direction force or force per unit length as output variable S11. In this case you can define either a contact width or contact area versus closure curve that will be used to obtain the average “contact” pressure at each integration point as output variable CS11. This average pressure considers the changing contact area that occurs as a result of the deformation of a gasket, as shown in Figure 32.6.6–1. The closure used for input of this curve corresponds to the total mechanical closure, defined as the sum of the elastic, plastic, and creep closures.
When two- and three-dimensional link gasket elements are used, you should specify the contact area versus mechanical closure in tabular form. When axisymmetric link and three-dimensional line elements are used, you should specify the contact width versus mechanical closure in tabular form. A typical curve is shown in Figure 32.6.6–7.
line
| mechanical closure | area |
|---|---|
| 0 | 0 |
| 1 | 1 |
| 2 | 2 |
| 3 | 3 |
| 4 | 4 |
Figure 32.6.6–7 Specification of contact area versus mechanical closure for output of average pressure.
You must specify the area at zero closure, then the area at increasing closures. The area is constant when the mechanical closure is negative and is extrapolated from the slope computed from the last two user-specified data points if the closure reaches values that are greater than the last user-specified closure. Area versus closure curves can be provided as a function of temperature and field variables.
Input File Usage: *GASKET CONTACT AREA, DEPENDENCIES
Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Units: Force, Suboptions→Contact Area
Specific output for directly defined gasket behavior
Output variable E is usually used in Abaqus/Standard to output strain. For gasket elements with behavior defined by a gasket behavior model this output variable has thickness-direction and transverse shear components with units of displacement and membrane strains. Output variable NE is used to output an effective strain. The effective strain components are computed as follows:
NE11 = E11/(initial thickness - initial gap) for perturbation steps; otherwise
NE11 = max(0, (E11 - initial gap)/(initial thickness - initial gap)); and
NE22 = E22;
NE33 = E33;
NE12 = E12/(initial thickness);
NE13 = E13/(initial thickness);
NE23 = E23.
The output variables THE, PE, or CE can also be used for gasket elements to output generalized thermal strains, plastic strains, or creep strains, respectively.
For all stress/strain output variables the 11-component refers to the through-thickness direction; the 22-, 33- and 23-components refer to two direct and one shear membrane component, respectively; the remaining 12- and 13-components refer to the transverse shear components. For details about these definitions, see “Gasket elements: overview,” Section 32.6.1.
The output of the elastic strain energy (output variable ALLSE) also contains the energy due to damage or change in elasticity as a function of plasticity. Therefore, this energy is usually not fully recoverable.
Additional reference
• Zubeck, M. W., and R. S. Marlow, “Local-Global Finite Element Analysis for Cam Cover Noise Reduction,” Society of Automotive Engineering, Inc., no. SAE 2003–01–1725, 2003.