김경종
16 KiB
text_image
thickness direction 5 1 8 n 4 7 top face 2 3 4 1 6 3 bottom face 5 2 thickness direction z y x
Figure 32.5.4–1 Default thickness direction for three-dimensional cohesive elements.
text_image
y (z) x (r) 4 3 1 2 thickness direction
Figure 32.5.4–2 Default thickness direction for two-dimensional and axisymmetric cohesive elements.
use an orientation-based method as described below. The isoparametric direction choices for three-dimensional cohesive elements are shown in Figure 32.5.4–3.
text_image
F6 8 F5 F2 7 5 6 F4 F3 4 3 1 F1 2 3 2 1 Stack direction
Stack direction = 1 from face 6 to face 4
Stack direction = 2 from face 3 to face 5
Stack direction = 3 from face 1 to face 2
text_image
6 F5 3 F4 4 F2 5 F3 1 F1 2 3 Stack direction
Stack direction = 3 from face 1 to face 2
Figure 32.5.4–3 Stack directions for COH3D8 (left) and COH3D6 (right) elements.
Input File Usage:
Use the following option to define the element top and bottom faces based on the element’s isoparametric directions:
*COHESIVE SECTION, STACK DIRECTION=n
Abaqus/CAE Usage:
You cannot define the stack direction based on isoparametric directions in Abaqus/CAE. The stack direction will correspond to the default discussed above.
Setting the stack direction based on a user-defined orientation
You can also control the orientation of the stack direction through a user-defined local orientation (“Orientations,” Section 2.2.5). When you define an orientation for cohesive elements, you also specify an axis about which the local 1 and 2 material directions may be rotated. This axis also defines an approximate normal direction. The stack direction will be the element isoparametric direction that is closest to this approximate normal (see Figure 32.5.4–4).
text_image
Local cylindrical orientation cylor1: a = 0, 0, 0 b = 10, 0, 0 Cohesive section, stack direction based on cylor1 (10, 0, 0) Z Y Global a (0, 0, 0) x x' b ε₃ x' ε₂ ε₁ ABAQUS selects the isoparametric direction ε₃ that is closest to the 1st (i.e., x¹, or radial) axis, at the center.
Figure 32.5.4–4 Example illustrating the use of a cylindrical system to define the stack direction.
Input File Usage:
Use the following option to define the element thickness direction based on a user-defined orientation:
*COHESIVE SECTION, STACK DIRECTION=ORIENTATION, ORIENTATION=name
Abaqus/CAE Usage:
You cannot define the stack direction based on an orientation definition in Abaqus/CAE. The stack direction will correspond to the default discussed above.
Verifying the stack direction
The stack direction can be verified visually in Abaqus/CAE by using the stack direction query tool (see “Understanding the role of the Query toolset,” Section 71.1 of the Abaqus/CAE User’s Guide). For three-dimensional elements Abaqus/CAE colors the top face brown and the bottom face purple. For two-dimensional and axisymmetric elements, arrows indicate the orientation of the element. In addition, Abaqus/CAE highlights any element faces and edges that have inconsistent orientations.
Alternatively, the material axes can be plotted in the Visualization module of Abaqus/CAE to verify that the 3-axis points in the desired normal direction for three-dimensional elements; and if the element is oriented improperly, one of the in-plane axes (either the 1- or 2-axis) will point in the normal direction. For two-dimensional and axisymmetric elements, the stack direction is consistent with the 2-axis material direction.
Thickness direction computation for two-dimensional and axisymmetric elements
To compute the thickness direction for two-dimensional and axisymmetric elements, Abaqus forms a midsurface by averaging the coordinates of the node pairs forming the bottom and top surfaces of the element. This midsurface passes through the integration points of the element, as shown in Figure 32.5.4–5 for the default choice of the bottom and top surfaces. For each integration point Abaqus computes a tangent whose direction is defined by the sequence of nodes given on the bottom and top surfaces. The thickness direction is then obtained as the cross product of the out-of-plane and tangent directions.
text_image
midsurface n₁ 4 t₁ 3 n₂ t₂ 1 2
Figure 32.5.4–5 Thickness direction for a two-dimensional or axisymmetric element.
Thickness direction computation for three-dimensional elements
To compute the thickness direction for three-dimensional elements, Abaqus forms a midsurface by averaging the coordinates of the node pairs forming the bottom and top surfaces of the element. This midsurface passes through the integration points of the element, as shown in Figure 32.5.4–6 for the default choice of the bottom and top surfaces. Abaqus computes the thickness direction as the normal to the midsurface at each integration point; the positive direction is obtained with the right-hand rule going around the nodes of the element on the bottom or top surface.
text_image
midsurface 8 5 n₁ n₄ 6 n₂ 7 n₃ 1 4 2 3
Figure 32.5.4–6 Thickness direction for a three-dimensional element.
Local directions at integration points
Abaqus computes default local directions at each integration point. The local directions are used for output of all quantities that describe the current deformation state of a cohesive element. Details of local directions are discussed separately below for cohesive elements with two versus three local directions.
Local directions for two-dimensional and axisymmetric cohesive elements
The local 2-direction for two-dimensional and axisymmetric cohesive elements corresponds to the thickness direction, which is computed as discussed above in “Element thickness direction definition.” The local 1-direction is defined such that the cross product between the local 1- and 2-directions gives the out-of-plane direction (see Figure 32.5.4–7). You cannot modify either local direction for these elements for a given stack orientation. Transverse shear behavior is defined in the 1–2 plane for these elements.
flowchart
graph TD
1 --> 2
2 --> 3
3 --> 4
1 -->|×| 2
2 -->|2| 3
3 -->|1| 4
Figure 32.5.4–7 Local directions for two-dimensional and axisymmetric cohesive elements.
Local directions for three-dimensional cohesive elements
The local 3-direction for three-dimensional cohesive elements corresponds to the thickness direction, which is computed as discussed above in “Element thickness direction definition” and cannot be modified for a given stack orientation. The local 1- and 2-directions are normal to the thickness direction and, by
default, are defined by the standard Abaqus convention for local directions on surfaces (“Conventions,” Section 1.2.2). The default local directions for a three-dimensional cohesive element are shown in Figure 32.5.4–8.
text_image
projection of x-axis onto surface 1 2 3 5 6 7 8 1 2 3 7 8
Figure 32.5.4–8 Local directions for three-dimensional cohesive elements.
Transverse shear behavior is defined in the local 1–3 and 2–3 planes for these elements. You can modify the local 1- and 2-directions for three-dimensional cohesive elements in the plane normal to the thickness direction by using a local orientation definition (“Orientations,” Section 2.2.5).
Input File Usage: *COHESIVE SECTION, ELSET=name, ORIENTATION=name
Abaqus/CAE Usage: Property module: Assign→Material Orientation: select region: select orientation
32.5.5 DEFINING THE CONSTITUTIVE RESPONSE OF COHESIVE ELEMENTS USING ACONTINUUM APPROACH
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Cohesive elements: overview,” Section 32.5.1
• “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6
• “Progressive damage and failure,” Section 24.1.1
• *COHESIVE SECTION
• *TRANSVERSE SHEAR STIFFNESS
• Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Guide
Overview
The features described in this section are used to model cohesive elements using a continuum approach, which assumes that the cohesive zone contains material of finite thickness that can be modeled using the conventional material models in Abaqus. If the cohesive zone is very thin and for all practical purposes may be considered to be of zero thickness, the constitutive response is commonly described in terms of a traction-separation law; this alternative approach is discussed in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6.
The constitutive response of cohesive elements modeled as a continuum:
• can be defined in terms of macroscopic material properties such as stiffness and strength using conventional material models;
• can be specified in terms of either a built-in material model or a user-defined material model;
• can include the effects of material damage and failure in Abaqus/Explicit; and
• can also include the effects of material damage and failure in a low-cycle fatigue analysis in Abaqus/Standard.
Behavior of cohesive elements with conventional material models
The implementation of the conventional material models (including user-defined models) in Abaqus for cohesive elements is based on certain assumptions regarding the state of the deformation in the cohesive layer. Two different classes of problems are considered: modeling of an adhesive layer of finite thickness and modeling of gaskets.
Modeling of damage with cohesive elements for these classes of problems can be carried out in both Abaqus/Standard and Abaqus/Explicit (see “Progressive damage and failure,” Section 24.1.1, for details regarding the damage models). You may need to alter the damage model for an adhesive material to
account for the fact that the failure of an adhesive bond may occur at the interface between the adhesive and the adherend rather than within the adhesive material.
When used with conventional material models in Abaqus, cohesive elements use true stress and strain measures. When used with a material model that is based on a traction-separation description (see “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6, for details on this approach), cohesive elements use nominal stress and strain measures.
The frequency characteristics of cohesive elements are accounted for by the algorithms to automatically choose the time increment in Abaqus/Explicit (“Explicit dynamic analysis,” Section 6.3.3). In many applications involving adhesives or gaskets cohesive elements may be quite thin compared to the other elements, which tends to decrease the stable time increment. See “Stable time increment in Abaqus/Explicit” in “Modeling with cohesive elements,” Section 32.5.3, for further discussion on this topic, including suggestions on how to avoid significant reductions in the stable time increment when using cohesive elements.
Modeling of an adhesive layer of finite thickness
For adhesive layers with finite thickness it is assumed that the cohesive layer is subjected to only one direct component of strain, which is the through-thickness strain, and to two transverse shear strain components (one transverse shear strain component for two-dimensional problems). The other two direct components of the strain (the direct membrane strains) and the in-plane (membrane) shear strain are assumed to be zero for the constitutive calculations. More specifically, the through-thickness and the transverse shear strains are computed from the element kinematics. However, the membrane strains are not computed based on the element kinematics; they are simply assumed to be zero for the constitutive calculations. These assumptions are appropriate in situations where a relatively thin and compliant layer of adhesive bonds two relatively rigid (compared to the adhesive) parts. The above kinematic assumptions are approximately correct everywhere inside the cohesive layer except around its outer edges.
An additional linear elastic transverse shear behavior can be defined to provide more stability to cohesive elements, particularly after damage has occurred. The transverse shear behavior is assumed to be independent of the regular material response and does not undergo any damage.
Input File Usage: Use the following options (the second option is needed only to define uncoupled transverse shear 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 }
*TRANSVERSE SHEAR STIFFNESS
Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Continuum
Transverse shear behavior is not supported in Abaqus/CAE for cohesive sections.
Modeling of gaskets and/or small adhesive patches
The modeling of gaskets and/or small adhesive patches involves situations where there are no lateral constraints on the cohesive layer. Hence, the layers are free to expand in the lateral direction in a stress-
free manner. Application areas include individual spot welds and gaskets. The constitutive calculations assume only one direct stress component, which is the through-thickness normal stress. All other stress components, including the transverse shear stress components, are assumed to be zero.
The gasket modeling capability that is offered with this option has some advantages compared to the family of gasket elements in Abaqus/Standard. The cohesive elements are fully nonlinear (the element kinematics properly account for finite strains as well as finite rotations), can contribute mass and damping in a dynamic analysis, and are available in Abaqus/Explicit. The gasket response modeled in the above manner is similar to modeling using the special-purpose gasket elements in Abaqus/Standard with thickness-direction behavior only (see “Including gasket elements in a model,” Section 32.6.3).
Uncoupled, linear-elastic transverse shear behavior, if desired, can be defined. The transverse shear behavior may either define the response of the gasket and/or adhesive patch or provide stability after damage has occurred in the response in the thickness direction. There is no damage associated with the transverse shear response.
Input File Usage: Use the following options (the second option is needed only to define uncoupled transverse shear response):
*COHESIVE SECTION, RESPONSE=GASKET *TRANSVERSE SHEAR STIFFNESS
Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Gasket
Transverse shear behavior is not supported in Abaqus/CAE for cohesive sections.
Output
All standard output variables in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2) are available for cohesive elements that are used with conventional material models. The stresses due to the additional transverse shear response are reported separately using the output variables TSHR13 and (in three dimensions) TSHR23. These stresses are not added to the usual material point stresses reported using the output variable S.