김경종
252 lines
18 KiB
Markdown
252 lines
18 KiB
Markdown
<!-- source-page: 831 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
thickness direction
|
||
top face
|
||
cohesive element node
|
||
bottom face
|
||
midsurface
|
||
</details>
|
||
|
||
Figure 32.5.1–4 Spatial representation of a three-dimensional cohesive element.
|
||
|
||
direction quantifies the transverse shear behavior of the cohesive element. Stretching and shearing of the midsurface of the element (the surface halfway between the bottom and top faces) are associated with membrane strains in the cohesive element; however, it is assumed that the cohesive elements do not generate any stresses in a purely membrane response. Figure 32.5.1–5 shows the different deformation modes of a cohesive element.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
cohesive layer
|
||
through-thickness behavior
|
||
transverse shear
|
||
membrane stretch
|
||
membrane stretch
|
||
membrane shear
|
||
</details>
|
||
|
||
Figure 32.5.1–5 Deformation modes of a cohesive element.
|
||
|
||
# General issues related to modeling with cohesive elements
|
||
|
||
While using cohesive elements, you should be mindful of important issues that are specific to these elements. Such issues include special considerations associated with using cohesive elements in
|
||
|
||
<!-- source-page: 832 -->
|
||
|
||
conjunction with contact interactions, potential degradation of the stable time increment size in Abaqus/Explicit, and potential convergence problems in Abaqus/Standard. These issues are discussed in detail in “Modeling with cohesive elements,” Section 32.5.3. Cohesive elements are typically used to bond components together. “Modeling with cohesive elements,” Section 32.5.3, also discusses methods for connecting a cohesive layer to adjacent components.
|
||
|
||
# Procedures with which cohesive elements are allowed
|
||
|
||
Cohesive elements without pore pressure degrees of freedom can be used in all stress/displacement analysis types. Although they do not have any degrees of freedom other than displacement, they can be used in coupled procedures to bond together components made out of coupled temperature-displacement elements, and in Abaqus/Standard coupled pore pressure-displacement elements and/or piezoelectric elements, to simulate mechanical failure of interfaces. The response of the cohesive element in such coupled procedures is mechanical only (for example, no heat transfer occurs across the interface in a coupled temperature-displacement problem).
|
||
|
||
Cohesive elements with pore pressure degrees of freedom can be used in coupled pore fluid diffusion/stress analyses (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). The mechanical response of the coupled pore pressure–displacement element is the same as the equivalent displacement-only element, except that the gap fluid pressure is considered as a traction on open faces.
|
||
|
||
<!-- source-page: 833 -->
|
||
|
||
# 32.5.2 CHOOSING A COHESIVE ELEMENT
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit
|
||
|
||
# References
|
||
|
||
• “Cohesive elements: overview,” Section 32.5.1
|
||
• “Two-dimensional cohesive element library,” Section 32.5.9
|
||
• “Three-dimensional cohesive element library,” Section 32.5.10
|
||
• “Axisymmetric cohesive element library,” Section 32.5.11
|
||
|
||
# Overview
|
||
|
||
The Abaqus cohesive element library includes:
|
||
|
||
• elements for two-dimensional analyses;
|
||
• elements for three-dimensional analyses; and
|
||
• elements for axisymmetric analyses.
|
||
|
||
# Naming convention
|
||
|
||
The cohesive elements used in Abaqus are named as follows:
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
COH 3D 8 P
|
||
pore pressure (optional)
|
||
number of nodes
|
||
two-dimensional (2D), three-dimensional (3D), or axisymmetric (AX)
|
||
cohesive element
|
||
</details>
|
||
|
||
For example, COH2D4 is a 4-node, two-dimensional cohesive element. For pore pressure cohesive elements that model the transition from Darcy flow to Poiseuille flow, the first three letters for the elements’ names are changed to COD. For example, COD2D4P is the 4-node, two-dimensional pore pressure cohesive element with transitional modeling from Darcy flow to Poiseuille flow.
|
||
|
||
<!-- source-page: 834 -->
|
||
|
||
<!-- source-page: 835 -->
|
||
|
||
# 32.5.3 MODELING WITH COHESIVE ELEMENTS
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Cohesive elements: overview,” Section 32.5.1
|
||
• “Choosing a cohesive element,” Section 32.5.2
|
||
• \*COHESIVE SECTION
|
||
• Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Guide
|
||
|
||
# Overview
|
||
|
||
# Cohesive elements:
|
||
|
||
• are used to model adhesives between two components, each of which may be deformable or rigid;
|
||
• are used to model interfacial debonding using a cohesive zone framework;
|
||
• are used to model gaskets and/or small adhesive patches;
|
||
• can be connected to the adjacent components by sharing nodes, by using mesh tie constraints, or by using MPCs type TIE or PIN; and
|
||
• may interact with other components via contact for gasket applications.
|
||
|
||
This section discusses the techniques that are available to discretize cohesive zones and assemble them in a model representing several components that are bonded to one another. It also discusses several common modeling issues related to cohesive elements.
|
||
|
||
# Discretizing cohesive zones using cohesive elements
|
||
|
||
The cohesive zone must be discretized with a single layer of cohesive elements through the thickness. If the cohesive zone represents an adhesive material with a finite thickness, the continuum macroscopic properties of this material can be used directly for modeling the constitutive response of the cohesive zone. Alternatively, if the cohesive zone represents an infinitesimally thin layer of adhesive at a bonded interface, it may be more relevant to define the response of the interface directly in terms of the traction at the interface versus the relative motion across the interface. Finally, if the cohesive zone represents a small adhesive patch or a gasket with no lateral constraint, a uniaxial stress state provides a good approximation to the state of these elements. Abaqus provides modeling capabilities for all the above cases. The details are discussed in later sections.
|
||
|
||
# Connecting cohesive elements to other components
|
||
|
||
At least one of either the top or the bottom face of the cohesive element must be constrained to another component. In most applications it is appropriate to have both faces of the cohesive elements tied to neighboring components. If only one face of the cohesive element is constrained and the other face
|
||
|
||
<!-- source-page: 836 -->
|
||
|
||
is free, the cohesive element exhibits one or (for three-dimensional elements) more singular modes of deformation due to the lack of membrane stiffness. The singular modes can propagate from one cohesive element to the adjacent one but can be suppressed by constraining the nodes on the side face at the end of a series of cohesive elements.
|
||
|
||
In some cases it may be convenient and appropriate to have cohesive elements share nodes with the elements on the surfaces of the adjacent components. More generally, when the mesh in the cohesive zone is not matched to the mesh of the adjacent components, cohesive elements can be tied to other components. When cohesive elements are used to model gaskets, it may be more appropriate to tie or share nodes on one side and define contact on the other side as discussed below. This will prevent the gaskets from being subjected to tensile stresses.
|
||
|
||
# Having cohesive elements share nodes with other elements
|
||
|
||
When the cohesive elements and their neighboring parts have matched meshes, it is straightforward to connect cohesive elements to other components in a model simply by sharing nodes (see Figure 32.5.3–1).
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
Part 1
|
||
pore pressure
|
||
cohesive elements
|
||
internally
|
||
generated nodes
|
||
Part 2
|
||
Explicitly
|
||
defined node
|
||
</details>
|
||
|
||
Figure 32.5.3–1 Cohesive elements sharing nodes with other Abaqus elements.
|
||
|
||
When these elements are used as adhesives or to model debonding, this method can be used to obtain initial results from a model—more accurate local results (in the decohesion zone) would typically be obtained with the cohesive zone more refined than the elements of the surrounding components. When these elements are used to model gaskets, this approach is suitable in situations when no frictional slip occurs between the gaskets and the surrounding components. The method of sharing nodes in gasket applications will lead to tensile stresses in the gasket should the parts connected to the gasket be pulled apart. Defining contact on one side of the cohesive elements will avoid such tensile stresses.
|
||
|
||
<!-- source-page: 837 -->
|
||
|
||
# Connecting cohesive elements to other components by using surface-based tie constraints
|
||
|
||
If the two neighboring parts do not have matched meshes, such as when the discretization level in the cohesive layer is different (typically finer) from the discretization level in the surrounding structures, the top and/or bottom surfaces of the cohesive layer can be tied to the surrounding structures using a tie constraint (“Mesh tie constraints,” Section 35.3.1). Figure 32.5.3–2 shows an example in which a finer discretization is used for the cohesive layer than for the neighboring parts.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
tie constraints
|
||
Part 1
|
||
cohesive elements
|
||
Part 2
|
||
</details>
|
||
|
||
Figure 32.5.3–2 Independent meshes with tie constraints.
|
||
|
||
# Contact interactions between cohesive elements and other components
|
||
|
||
For some applications involving gaskets it is appropriate to define contact on one side of the cohesive element (see Figure 32.5.3–3). Contact can be defined with either the general contact algorithm in Abaqus/Explicit (“Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1) or the contact pair algorithm in Abaqus/Standard (“Defining contact pairs in Abaqus/Standard,” Section 36.3.1) or Abaqus/Explicit (“Defining contact pairs in Abaqus/Explicit,” Section 36.5.1). If pure master-slave contact is used, typically the surface of the cohesive elements should be the slave surface and the surface of the neighboring part should be the master surface. This choice of master and slave is based on the cohesive zone typically being composed of softer materials and having a finer discretization. The second consideration also suggests that mismatched meshes will often be used in analyses involving cohesive elements. If mismatched meshes are used, the pressure distribution
|
||
|
||
<!-- source-page: 838 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
Part 1
|
||
contact interaction
|
||
tie constraints
|
||
cohesive elements
|
||
Part 2
|
||
</details>
|
||
|
||
Figure 32.5.3–3 Contact interaction on one side of a cohesive zone.
|
||
|
||
on the cohesive elements may not be predicted accurately; submodeling (“Submodeling: overview,” Section 10.2.1) may be required to obtain accurate local results.
|
||
|
||
# Using cohesive elements in large-displacement analyses
|
||
|
||
Cohesive elements can be used in large-displacement analyses. The assembly containing the cohesive elements can undergo finite displacement as well as finite rotation.
|
||
|
||
# Selecting the broad class of the constitutive response of cohesive elements
|
||
|
||
As discussed earlier, cohesive elements can be used to model finite-thickness adhesives, negligibly thin adhesive layers for debonding applications, as well as gaskets and/or small adhesive patches. You must choose one of these broad classes of applications when you define the section properties of cohesive elements. The detailed implications of each choice are discussed in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5, and “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6.
|
||
|
||
Input File Usage: Use the following option to model a finite-thickness adhesive layer using a continuum-based constitutive response:
|
||
|
||
$\mathrm { * C O H E S I V E ~ S E C T I O N , R E S P O N S E { = } C O N T I N U U M }$
|
||
|
||
<!-- source-page: 839 -->
|
||
|
||
Use the following option to model a negligibly (geometrically) thin layer of adhesive using a traction-separation-based response:
|
||
|
||
\*COHESIVE SECTION, RESPONSE=TRACTION SEPARATION
|
||
|
||
Use the following option to use cohesive elements as gaskets and/or small adhesive patches:
|
||
|
||
\*COHESIVE SECTION, RESPONSE=GASKET
|
||
|
||
Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Continuum, Traction Separation, or Gasket
|
||
|
||
# Assigning a material behavior to a cohesive element
|
||
|
||
You assign the name of a material definition to a particular element set. The constitutive behavior for this element set is defined entirely by the constitutive thickness of the cohesive layer (discussed in “Specifying the constitutive thickness” in “Defining the cohesive element’s initial geometry,” Section 32.5.4) and the material properties referring to the same name.
|
||
|
||
The constitutive behavior of the cohesive elements can be defined either in terms of a material model provided in Abaqus or a user-defined material model (see “User-defined mechanical material behavior,” Section 26.7.1). When cohesive elements are used in applications involving a finite-thickness adhesive, any available material model in Abaqus, including material models for progressive damage, can be used. For applications involving gasket and/or small finite-thickness adhesive patches, any material model that can be used with one-dimensional elements (such as beams, trusses, and rebars), including material models for progressive damage, can be used. For further details, see “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5. For applications in which the behavior of cohesive elements is defined directly in terms of traction versus separation, the response can be defined only in terms of a linear elastic relation (between the traction and the separation) along with progressive damage (see “Defining the constitutive response of cohesive elements using a tractionseparation description,” Section 32.5.6).
|
||
|
||
To define the constitutive behavior of cohesive elements, you assign the name of a material model to a particular element set through the section definition. The actual material model for a user-defined material model is defined in user subroutine UMAT in Abaqus/Standard or VUMAT in Abaqus/Explicit.
|
||
|
||
Input File Usage: \*COHESIVE SECTION, ELSET=name, MATERIAL=name
|
||
|
||
Abaqus/CAE Usage: Property module: cohesive section editor: Material: name
|
||
|
||
# Using cohesive elements in coupled pore fluid diffusion/stress analyses
|
||
|
||
Cohesive elements with, or without, pore pressure degrees of freedom can be used in coupled pore fluid diffusion/stress analyses. Cohesive elements without pore pressure degrees of freedom will only contribute mechanically, and surfaces exposed when cohesive elements open will be impermeable to fluid flow.
|
||
|
||
Cohesive elements with pore pressure degrees of freedom provide a more general response, including the ability to model tangential flow and leakage flow from the gap into the adjacent material.
|
||
|
||
<!-- source-page: 840 -->
|
||
|
||
These elements have additional pore pressure nodes in the gap interior, and you can choose to define these nodes explicitly or have them generated automatically by Abaqus/Standard.
|
||
|
||
In a typical use you will have these gap interior nodes generated for you for the majority of cohesive elements in the model. You invoke automatic node generation as discussed in “By defining the bottomface element connectivity and an integer offset” in “Defining the cohesive element’s initial geometry,” Section 32.5.4.
|
||
|
||
# Defining contact between surrounding components
|
||
|
||
Cohesive elements are used to bond two different components. Often the cohesive elements completely degrade in tension and/or shear as a result of the deformation. Subsequently, the components that are initially bonded together by cohesive elements may come into contact with each other. Approaches for modeling this kind of contact include the following:
|
||
|
||
• In certain situations this kind of contact can be handled by the cohesive element itself. By default, cohesive elements retain their resistance to compression even if their resistance to other deformation modes is completely degraded. As a result, the cohesive elements resist interpenetration of the surrounding components even after the cohesive element has completely degraded in tension and/or shear. This approach works best when the top and the bottom faces of the cohesive element do not displace tangentially by a significant amount relative to each other during the deformation. In other words, to model the situation described above, the deformation of the cohesive elements should be limited to “small sliding.”
|
||
|
||
• Another possible approach is to define contact between the surfaces of the surrounding components that could potentially come into contact and to delete the cohesive elements once they are completely damaged. Thus, contact is modeled throughout the analysis. This approach is not recommended if the geometric thickness of the cohesive elements in the model is very small or zero (the geometric thickness of the cohesive elements may be different from the constitutive thickness you specify while defining the section properties of the cohesive elements—see “Specifying the constitutive thickness” in “Defining the cohesive element’s initial geometry,” Section 32.5.4) because contact will effectively cause nonphysical resistance to compression of the cohesive layer while the cohesive elements are still active. If frictional contact is modeled, there may also be nonphysical shearing forces.
|
||
|
||
This is the behavior that will occur by default with the general contact algorithm in Abaqus/Explicit. Figure 32.5.3–4, Figure 32.5.3–5, and Figure 32.5.3–6 show the default surface for general contact. This surface:
|
||
|
||
– is insensitive to whether the cohesive elements and neighboring elements share nodes, are tied together, or are not connected; and
|
||
– does not include faces of cohesive elements.
|