김경종
23 KiB
text_image
Part 1 cohesive elements Part 2 all element-based surfaces
Figure 32.5.3–4 Default surface when cohesive elements share nodes with surrounding elements.
flowchart
graph LR
A["tie constraints"] --> B["Part 1"]
B --> C["cohesive elements"]
C --> D["Part 2"]
D --> E["all element-based surfaces"]
style A fill:#f9f,stroke:#333
style B fill:#ccf,stroke:#333
style C fill:#cfc,stroke:#333
style D fill:#fcc,stroke:#333
style E fill:#ffc,stroke:#333
Figure 32.5.3–5 Default surface when cohesive elements are tied to the surrounding elements.
flowchart
graph LR
A["contact interaction"] --> B["tie constraints"]
B --> C["cohesive elements"]
C --> D["all element-based surfaces"]
D --> E["Resulting surface"]
Figure 32.5.3–6 Default surface when cohesive elements are tied on one side and interact through contact on the other side.
Figure 32.5.3–7 shows the situation when the surfaces of the cohesive elements are also added to the default surface. Abaqus/Explicit generates a contact exclusion automatically so that the general contact algorithm avoids consideration of contact between the bottom surface of the cohesive elements and the top surface of Part 2 since these surfaces are tied together.
flowchart
graph LR
A["contact interaction"] --> B["tie constraints"]
B --> C["cohesive elements"]
C --> D["all element-based surfaces"]
style A fill:#f9f,stroke:#333
style B fill:#ccf,stroke:#333
style C fill:#cfc,stroke:#333
style D fill:#fcc,stroke:#333
Figure 32.5.3–7 Top and bottom faces of the cohesive element along with the default surface when cohesive elements are tied on one side and interact through contact on the other side.
Input File Usage: Use the following options to add the top and bottom faces of the cohesive elements to the default general contact surface (the cohesive elements are included in the element set COH_ELEMS):
*SURFACE, NAME=DEFAULT_PLUS_COH
, COH_ELEMS,
*CONTACT
*CONTACT INCLUSIONS
DEFAULT_PLUS_COH,
Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization:
Tools→Surface→Create: Name: default_plus_coh:
pick faces in viewport
Interaction module: Create Interaction: General contact (Explicit):
Included surface pairs: Selected surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of included pairs
• For general contact in Abaqus/Explicit, yet another approach for modeling contact between the surrounding structures involves activating contact only when the cohesive elements are completely degraded and deleted from the model (see “Maximum degradation and choice of element removal” in “Defining the constitutive response of cohesive elements using a traction-separation description,”
Section 32.5.6). For this approach the cohesive elements must share nodes with the neighboring element and the general contact definition must include surfaces on the top and bottom faces of the cohesive elements, as shown in Figure 32.5.3–8. Since each surface face of the cohesive elements directly opposes a surface face of a neighboring element, the general contact algorithm does not consider these faces active while both parent elements are active. However, if the cohesive element fails, the opposing surface faces become active.
Input File Usage: Use the following options to include the top and bottom faces of the cohesive elements in the general contact definition (the cohesive elements are included in the element set COH_ELEMS): *SURFACE, NAME=gc_surf , COH_ELEMS, *CONTACT *CONTACT INCLUSIONS gc_surf,
Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: gc_surf: pick faces in viewport Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: Selected surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of included pairs
flowchart
graph LR
A["Part 1: cohesive elements"] --> B["Part 2: all element-based surfaces and bottom and top faces of cohesive elements"]
B --> C["Final: single surface with shaded top face"]
Figure 32.5.3–8 Surfaces that are involved in general contact when cohesive elements are included in the surface definition and erosion is used.
The stable time increment for a cohesive element in Abaqus/Explicit is equal to the time, \Delta t . , required for a stress wave to travel across the constitutive thickness, T _ { c } , of the cohesive layer:
\Delta t = \frac {T _ {c}}{c},
where \begin{array} { r } { c = \sqrt { \frac { E _ { c } } { \rho _ { c } } } } \end{array} 1 is the wave speed and and represent the bulk stiffness and the density, respectively, E _ { c } \rho _ { c } of the adhesive material. In terms of the expression for the wave speed, the stable time increment can be written as
\Delta t = T _ {c} \sqrt {\frac {\rho_ {c}}{E _ {c}}}.
For cases in which the constitutive response is defined in terms of traction versus separation, the slope of the traction versus separation relationship is K _ { c } = E _ { c } / T _ { c } and the density is specified as mass per unit area rather than per unit volume: \bar { \rho } _ { c } = \rho _ { c } T _ { c } (see “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6, for further details on this issue). Therefore, for traction versus separation the expression for the time increment becomes
\Delta t = \sqrt {\frac {\bar {\rho} _ {c}}{K _ {c}}}.
It is quite common that the time increment of cohesive elements will be significantly less than that of the other elements in the model, unless you take some action to alter one or more of the factors influencing the time increment. This requires some judgement on your part. The following discussions provide some recommendations for controlling the time increment for the different methods of defining the material response. However, Abaqus/Standard may be preferable in some applications where it is necessary to model a thin, stiff cohesive layer without approximations.
Constitutive response defined in terms of a continuum or uniaxial stress-state approach
For constitutive response defined in terms of a continuum or uniaxial stress-state approach, the ratio of the stable time increment of the cohesive elements to that of the other elements is given by
\frac {\Delta t _ {c}}{\Delta t _ {e}} = (\frac {T _ {c}}{T _ {e}}) \sqrt {(\frac {\rho_ {c}}{\rho_ {e}}) (\frac {E _ {e}}{E _ {c}})},
where the subscripts \ " { } \mathbf { c } \overrightarrow { } \mathbf { \Gamma } and \ " e \ : ^ { \circ } stand for the cohesive elements and the surrounding elements, respectively. The thickness of the cohesive layer is often smaller than a characteristic length of the other elements in the model, so the quantity ( T _ { c } / T _ { e } ) is often small. The quantity under the radical will depend on the materials involved. For an epoxy adhesive between steel components, the quantity under
the radical is on the order of unity. The stable time increment of the cohesive element can be increased by artificially
• increasing the constitutive thickness, T _ { c } ;
• increasing the density, \rho _ { c } ,
• reducing the stiffness, E _ { c ; } ; or
• some combination of the above.
In many cases the most attractive option will be to increase the density, which is also referred to as mass scaling (“Mass scaling,” Section 11.6.1). However, if the thickness of the cohesive zone is very small, the mass scaling required to achieve a reasonable time increment may affect the results significantly. In such cases it may be necessary to artificially reduce the cohesive stiffness in addition to some mass scaling. This approach involves the use of a stiffness that is different from the measured stiffness of the interface; however, if the peak strength and the fracture energy remain unchanged, the global response will not be affected significantly in many cases.
Constitutive response defined in terms of traction versus separation
For constitutive response defined in terms of traction versus separation, the ratio of the stable time increment of the cohesive elements to that for the other elements is given by
\frac {\Delta t _ {c}}{\Delta t _ {e}} = \sqrt {(\frac {\bar {\rho} _ {c}}{\bar {\rho} _ {e}}) (\frac {K _ {e}}{K _ {c}})},
where the subscripts \ " { } \mathbf { c } \overrightarrow { } \mathbf { \Gamma } and \ " e \ : ^ { \circ } stand for the cohesive elements and the surrounding elements, respectively.
One way to ensure that the cohesive elements will have no adverse effect on the stable time increment is to choose material properties such that \Delta t _ { c } = \Delta t _ { e } , which implies
\frac {\bar {\rho} _ {c}}{\bar {\rho} _ {e}} = \frac {K _ {c}}{K _ {e}}.
This is accomplished if, for example, the cohesive element stiffness and density per unit area are chosen such that
K _ {c} = \frac {E _ {c}}{T _ {c}} = \frac {1}{1 0} \frac {E _ {e}}{T _ {e}} = 0. 1 K _ {e},
\bar {\rho} _ {c} = \rho_ {c} T _ {c} = \frac {1}{1 0} \rho_ {e} T _ {e} = 0. 1 \bar {\rho} _ {e},
where T _ { e } represents the characteristic length of the neighboring non-cohesive elements. By choosing K _ { c } = 0 . 1 K _ { e } , , the stiffness in the cohesive layer relative to the surrounding elements will be similar to the default stiffness used by penalty contact in Abaqus/Explicit (relative to the equivalent one-dimensional stiffness of the surrounding elements). This approach involves the use of a stiffness that is likely to
be different from the measured stiffness of the interface; however, if the peak strength and the fracture energy remain unchanged, the global response will not be affected significantly in many cases.
Convergence issues in Abaqus/Standard
In many problems cohesive elements are modeled as undergoing progressive damage leading to failure. The modeling of progressive damage involves softening in the material response, which is known to lead to convergence difficulties in an implicit solution procedure, such as in Abaqus/Standard. Convergence difficulties may also occur during unstable crack propagation, when the energy available is higher than the fracture toughness of the material. Several methods are available to help avoid these convergence problems.
Using viscous regularization
Abaqus/Standard provides a viscous regularization capability that helps in improving the convergence for these kinds of problems. This capability is discussed in detail in “Using viscous regularization with cohesive elements, connector elements, and elements that can be used with the damage evolution models for ductile metals and fiber-reinforced composites in Abaqus/Standard” in “Section controls,” Section 27.1.4, and “Viscous regularization in Abaqus/Standard” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6.
Using automatic stabilization
Another approach to help convergence behavior is the use of automatic stabilization (see “Static stress analysis,” Section 6.2.2, and “Solving nonlinear problems,” Section 7.1.1, for further details), which is useful when a problem is unstable due to local instabilities. Generally, if sufficient viscous regularization is used (as measured by the viscosity coefficient—see “Viscous regularization in Abaqus/Standard” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6, for further details), the use of the automatic stabilization technique is not necessary. In problems where a small amount or no viscous regularization is used, automatic stabilization will improve the convergence characteristics.
Using nondefault solution controls
The use of nondefault solution controls (see “Commonly used control parameters,” Section 7.2.2, and “Convergence criteria for nonlinear problems,” Section 7.2.3, for further details) and activation of the line search technique (“Improving the efficiency of the solution by using the line search algorithm” in “Convergence criteria for nonlinear problems,” Section 7.2.3) may be useful in improving the solution efficiency.
32.5.4 DEFINING THE COHESIVE ELEMENT’S INITIAL GEOMETRY
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Cohesive elements: overview,” Section 32.5.1
• Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Guide
Overview
The initial geometry of a cohesive element is defined:
• by the nodal connectivity of the element and the position of these nodes;
• by the stack direction, which can be used to specify the top and the bottom faces of the cohesive element independent of the nodal connectivity; and
• by the magnitude of the initial constitutive thickness, which can either correspond to the geometric thickness implied by the nodal positions and stack direction or be specified directly.
Defining the element connectivity
The connectivity of a cohesive element is like that of a continuum element; however, it is useful to think of a cohesive element as being composed of two faces (a bottom and a top face) separated by the cohesive zone thickness. The element has nodes on its bottom face and corresponding nodes on its top face. Pore pressure cohesive elements include a third, middle face, which is used to model fluid flow within the element.
Three methods are available to define the element connectivity.
By directly defining the element’s complete connectivity
The complete connectivity of a cohesive element can be given directly (see “Defining cohesive elements” in “Element definition,” Section 2.2.1).
By defining the bottom-face element connectivity and an integer offset
Alternatively, you can specify the connectivity of the bottom face plus a positive integer offset (see “Defining cohesive elements” in “Element definition,” Section 2.2.1) that will be used to determine the remaining cohesive element nodes.
Input File Usage: *ELEMENT, OFFSET=n
Abaqus/CAE Usage: Element offsets are not supported in Abaqus/CAE.
Use with displacement cohesive elements
The integer offset will be used to define node numbers of the top face of the cohesive element. Abaqus will automatically position the nodes of the top face to be coincident with those of the bottom face unless the nodes of the top face have already been assigned coordinates directly with a node definition (“Node definition,” Section 2.1.1).
Use with pore pressure-displacement cohesive elements
When you define only the bottom face nodes, the integer offset will first be used to define the node numbers of the top face of the cohesive element, with the numbering of the top-face nodes offset from the bottom face node numbers. The integer offset will again be used to define the middle surface node numbers offset, with the numbering of the middle-face nodes offset from the top face node numbers. Abaqus will automatically position the nodes of the top and middle faces to be coincident with those of the bottom face unless the nodes of the top face have already been assigned coordinates directly with a node definition (“Node definition,” Section 2.1.1).
By defining the bottom- and top-face element connectivities and an integer offset
For pore pressure cohesive elements, you also can specify the connectivity of the bottom and top faces plus a positive integer offset (see “Defining cohesive elements” in “Element definition,” Section 2.2.1) that will be used to determine the middle face cohesive element nodes.
When you define the bottom and top face nodes, the integer offset will be used to define the node numbers of the middle face, with the numbering of the middle-face nodes offset from the bottom face node numbers. Abaqus will automatically position the nodes of the middle face to be halfway between those of the bottom and top faces unless the nodes of the middle face have already been assigned coordinates directly with a node definition (“Node definition,” Section 2.1.1).
Input File Usage: *ELEMENT, OFFSET=n
Abaqus/CAE Usage: Element offsets are not supported in Abaqus/CAE.
Specifying the out-of-plane thickness for two-dimensional elements
For two-dimensional cohesive elements the out-of-plane thickness is required. You specify this additional information in the cohesive section definition; the default value is 1.0.
Input File Usage: *COHESIVE SECTION
first data line
out-of-plane thickness
Abaqus/CAE Usage: Property module: cohesive section editor: toggle on Out-of-plane thickness:
and specify the out-of-plane thickness
Specifying the constitutive thickness
You can specify the constitutive thickness of the cohesive element directly or allow Abaqus to compute it based on nodal coordinates such that the constitutive thickness is equal to the geometric thickness. The default behavior depends on the nature of the application.
If the geometric thickness of the cohesive element is very small compared to its surface dimensions, the thickness computed from the nodal coordinates may be inaccurate. In such cases you can specify a constant thickness directly when defining the section properties of these elements.
The characteristic element length of a cohesive element is equal to its constitutive thickness. The characteristic element length is often useful in defining the evolution of damage in materials (see “Mesh dependency” in “Progressive damage and failure,” Section 24.1.1).
When the cohesive element response is based on a continuum approach
When the response of the cohesive elements is based on a continuum approach, by default the constitutive thickness of the element is computed by Abaqus based on the nodal coordinates. You can override this default by specifying the constitutive thickness directly.
Input File Usage: Use the following option to have Abaqus compute the thickness based on the nodal coordinates:
*COHESIVE SECTION, RESPONSE=CONTINUUM, THICKNESS=GEOMETRY (default)
Use the following option to specify the thickness directly:
*COHESIVE SECTION, RESPONSE=CONTINUUM,THICKNESS=SPECIFIED
thickness (1.0 by default)
Abaqus/CAE Usage: Property module: cohesive section editor: Response: Continuum: Initial thickness: Use nodal coordinates, Specify: thickness, or Use analysis default
When the cohesive element response is based on a traction-separation approach
When the response of the cohesive elements is based on a traction-separation approach, Abaqus assumes by default that the constitutive thickness is equal to one. This default value is motivated by the fact that the geometric thickness of cohesive elements is often equal to (or very close to) zero for the kinds of applications in which a traction-separation-based constitutive response is appropriate. This default choice ensures that nominal strains are equal to the relative separation displacements (see “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6, for further details). You can override this default by specifying another value or specifying that the constitutive thickness should be equal to the geometric thickness.
Input File Usage: Use the following option to specify the thickness directly:
*COHESIVE SECTION, RESPONSE=TRACTION SEPARATION, THICKNESS=SPECIFIED (default)
thickness (1.0 by default)
Use the following option to have Abaqus compute the thickness based on the nodal coordinates:
*COHESIVE SECTION, RESPONSE=TRACTION SEPARATION, THICKNESS=GEOMETRY
Abaqus/CAE Usage: Property module: cohesive section editor: Response: Traction Separation: Initial thickness: Specify: thickness, Use analysis default, or Use nodal coordinates
When the cohesive element response is based on a uniaxial stress state
When the response of the cohesive elements is based on a uniaxial stress state, there is no default method for computing the constitutive thickness. You must indicate your choice of the method of determining the constitutive thickness.
Input File Usage: Use the following option to specify the thickness:
*COHESIVE SECTION, RESPONSE=GASKET, THICKNESS=SPECIFIED
thickness (1.0 by default)
Use the following option to have Abaqus compute the thickness based on the nodal coordinates:
*COHESIVE SECTION, RESPONSE=GASKET, THICKNESS=GEOMETRY
Abaqus/CAE Usage: Property module: cohesive section editor: Response: Gasket: Initial thickness: Specify: thickness or Use nodal coordinates
Element thickness direction definition
It is important to define the orientation of cohesive elements correctly, since the behavior of the elements is different in the thickness and in-plane directions. By default, the top and bottom faces of cohesive elements are as shown in Figure 32.5.4–1 for three-dimensional cohesive elements and Figure 32.5.4–2 for two-dimensional and axisymmetric cohesive elements. Options for overriding the default orientation of cohesive elements are discussed below along with an explanation of how the local thickness direction and in-plane direction vectors are established.
Setting the stack direction equal to an isoparametric direction
The “stack direction” refers to the isoparametric direction along which the top and bottom faces of a cohesive element are stacked. By default, the top and bottom faces are stacked along the third isoparametric direction in three-dimensional cohesive elements and along the second isoparametric direction in two-dimensional and axisymmetric cohesive elements. You can choose to stack the top and bottom faces along an alternate isoparametric direction for most element types (the COH3D6 element can have only the third isoparametric direction as the stack direction). The choice of the isoparametric direction depends on the element connectivity. For a mesh-independent specification,