김경종
26 KiB
The domain integral method
Using the divergence theorem, the contour integral can be expanded into an area integral in two dimensions or a volume integral in three dimensions, over a finite domain surrounding the crack. This domain integral method is used to evaluate contour integrals in Abaqus/Standard. The method is quite robust in the sense that accurate contour integral estimates are usually obtained even with quite coarse meshes. The method is robust because the integral is taken over a domain of elements surrounding the crack and because errors in local solution parameters have less effect on the evaluated quantities such as J , C _ { t } , the stress intensity factors, and the T-stress.
Requesting multiple contour integrals
Contour integrals at several different crack tips in two dimensions or along several different crack lines in three dimensions can be evaluated at any time by repeating the contour integral request as often as needed in the step definition. When you are using the conventional finite element method, you must specify the crack front and the direction of virtual crack extension (or the normal to the crack plane if this normal is constant) for each crack tip or crack line, as described below. When you are using XFEM, you do not need to specify the crack front or the virtual crack extension direction because they will be determined by Abaqus/Standard. However, you must set each crack name equal to the corresponding enriched feature, with each enriched feature consisting of only one crack. In addition, regardless of whether you are using either the conventional finite element method or XFEM, you must specify the number of contours to be calculated for each integral.
The J -integral
The J-integral is usually used in rate-independent quasi-static fracture analysis to characterize the energy release associated with crack growth. It can be related to the stress intensity factor if the material response is linear.
The J-integral is defined in terms of the energy release rate associated with crack advance. For a virtual crack advance \lambda ( s ) in the plane of a three-dimensional fracture, the energy release rate is given by
\bar {J} = \int_ {A} \lambda (s) \mathbf {n} \cdot \mathbf {H} \cdot \mathbf {q} d A,
where d A is a surface element along a vanishing small tubular surface enclosing the crack tip or crack line, is the outward normal to , and is the local direction of virtual crack extension. is given by
\mathbf {H} = \left(W \mathbf {I} - \pmb {\sigma} \cdot \frac {\partial \mathbf {u}}{\partial \mathbf {x}}\right).
For elastic material behavior W is the elastic strain energy; for elastic-plastic or elasto-viscoplastic material behavior W is defined as the elastic strain energy density plus the plastic dissipation, thus representing the strain energy in an “equivalent elastic material.” Therefore, the J-integral calculated is suitable only for monotonic loading of elastic-plastic materials.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=J
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: J-integral
Domain dependence
The J-integral should be independent of the domain used provided that the crack faces are parallel to each other, but J-integral estimates from different rings may vary because of the approximate nature of the finite element solution. Strong variation in these estimates, commonly called domain dependence or contour dependence, typically indicates an error in the contour integral definition. Gradual variation in these estimates may indicate that a finer mesh is needed or, if plasticity is included, that the contour integral domain does not completely include the plastic zone. If the “equivalent elastic material” is not a good representation of the elastic-plastic material, the contour integrals will be domain independent only if they completely include the plastic zone. Since it is not always possible to include the plastic zone in three dimensions, a finer mesh may be the only solution.
If the first contour integral is defined by specifying the nodes at the crack tip, the first few contours may be inaccurate. To check the accuracy of these contours, you can request more contours and determine the value of the contour integral that appears approximately constant from one contour to the next. The contour integral values that are not approximately equal to this constant should be discarded. In linear elastic problems the first and second contours typically should be ignored as inaccurate.
For some three-dimensional models with an open crack front, the J-integral estimates may be inaccurate from the node sets (or elements in the case with XFEM) at the crack front ends. The resolution difficulty is compounded by the skewness of the outmost layer of elements. This accuracy loss is confined only to the contour integrals at the front ends and has no effect on the accuracy of the contour integral values at the neighboring node sets (or elements in the case with XFEM) along the crack front.
Including the effect of a residual stress field on J-integral evaluation
A residual stress field often occurs in a structure; for example, as a result of service loads that produce plasticity, a metal forming process in the absence of an anneal treatment, thermal effects, or swelling effects. When the residual stresses are significant, the standard definition of the J-integral as described above may lead to a path-dependent value. To ensure its path independence, the J-integral evaluation must include an additional term that accounts for the residual stress field. In Abaqus/Standard the problem with a residual stress field is treated as an initial strain problem. If the total strain is written as the sum of mechanical strain, \varepsilon ^ { m } , and initial strain, ; i.e.,
\varepsilon = \varepsilon^ {m} + \varepsilon^ {o},
a path-independent energy release rate in the presence of a residual stress field is given by
\bar {J} = \int_ {A} \lambda (s) \mathbf {n} \cdot (W \mathbf {I} - \pmb {\sigma} \cdot \frac {\partial \mathbf {u}}{\partial \mathbf {x}}) \cdot \mathbf {q} d A + \int_ {V} \pmb {\sigma}: \frac {\partial \pmb {\varepsilon} ^ {o}}{\partial \mathbf {x}} \cdot \mathbf {q} d V,
where V is the domain volume enclosing the crack tip or crack line, W is defined as the mechanical strain energy density only,
W = \int_ {0} ^ {\varepsilon^ {m}} \pmb {\sigma}: d \pmb {\varepsilon} ^ {m},
and \varepsilon ^ { \mathbf { o } } remains constant during the entire deformation.
The residual stress field can be specified by reading the stress data from a previous analysis step or by defining an initial condition (see “Defining initial stresses” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). You specify the step number from which the stress data in the last available increment of the specified step will be considered as residual stresses. If the step number is set equal to zero (default), the residual stress field is defined by the initial condition definition. When XFEM is used, the residual stress field can be defined only with an initial condition definition.
Input File Usage: *CONTOUR INTEGRAL, RESIDUAL STRESS STEP=n, TYPE=J
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Step for residual stress initialization values: step, Type: J-integral
The Ct -integral
The C _ { t } -integral is supported with the conventional finite element method; however, it is not supported with XFEM.
The -integral can be used for time-dependent creep behavior, where it characterizes creep crack deformation under certain creep conditions, including transient crack growth. C _ { t } is, for example, proportional to the rate of growth of the crack-tip/crack-line creep zone for a stationary crack under small-scale creep conditions. Under steady-state creep conditions, when creep dominates throughout the specimen, C _ { t } becomes path independent and is known as C ^ { * } . -integrals should be requested only in a quasi-static step.
The C _ { t } -integral is obtained by replacing the displacements with velocities and the strain energy density with the strain energy rate density in the J-integral expansion. The strain energy rate density is defined as
\dot {W} \stackrel {\mathrm{def}} {=} \int_ {0} ^ {\dot {\varepsilon}} \pmb {\sigma}: d \dot {\varepsilon}.
\dot { W } is not uniquely defined if multiple deformation mechanisms contribute to the strain rate. However, the creep mechanism will dominate within a zone surrounding a crack tip or crack line, so elastic and plastic contributions to \dot { W } are negligible. The size of that zone depends on the extent of creep relaxation: the zone is initially small but eventually encompasses the entire specimen when steady-state creep is reached. Abaqus/Standard considers only creep in the calculation of . Neglecting elastic and plastic strain rates, the strain energy density for the power law creep model with time hardening form in Abaqus/Standard is
\dot {W} = \frac {n}{n + 1} q \dot {\bar {\varepsilon}},
where n is the power law exponent, q is the equivalent Mises stress, and \dot { \bar { \varepsilon } } is the equivalent uniaxial strain rate.
For the hyperbolic-sine law an analytical expression of \dot { W } is not available. For this law \dot { W } is obtained by numerical integration; a five-point Gauss quadrature scheme gives reasonable accuracy in the range of realistic creep strain rates.
The domain integral method is used for -integrals as described above for J-integrals.
For user-defined creep laws the strain energy rate density must be defined in user subroutine CREEP.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=C
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Ct-integral
Domain dependence
Prior to steady state C _ { t } { \mathrm { - i n t e g r a l } } estimates will exhibit domain dependence, even if the finite element mesh is sufficiently refined, because of the assumption of creep dominance within the domain specified. These C _ { t } estimates should be extrapolated to zero radius to obtain an improved C _ { t } estimate corresponding to a contour shrunk onto the crack tip or crack line ( \mathrm { s e e } ^ { \ast } C _ { t } -integral evaluation,” Section 1.16.6 of the Abaqus Benchmarks Guide).
Including the effect of a residual stress field on -integral evaluation
An additional term is included to account for the residual stress field when calculating the C _ { t } { \mathrm { - i n t e g r a l } } _ { \mathrm { ; } } , as described in “Including the effect of a residual stress field on J-integral evaluation.”
Input File Usage: *CONTOUR INTEGRAL, RESIDUAL STRESS \operatorname { S T E P } { = } n , TYPE=C
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Step for residual stress initialization values: step, Type: Ct-integral
The stress intensity factors
The stress intensity factors K _ { I } , K _ { I I } , and K _ { I I I } are usually used in linear elastic fracture mechanics to characterize the local crack-tip/crack-line stress and displacement fields. They are related to the energy release rate (the J-integral) through
J = \frac {1}{8 \pi} \mathbf {K} ^ {T} \cdot \mathbf {B} ^ {- 1} \cdot \mathbf {K},
where \mathbf { K } = \lfloor K _ { I } , K _ { I I } , K _ { I I I } \rfloor ^ { T } are the stress intensity factors and is called the pre-logarithmic energy factor matrix. For homogeneous, isotropic materials is diagonal, and the above equation simplifies to
J = \frac {1}{\overline {{E}}} (K _ {I} ^ {2} + K _ {I I} ^ {2}) + \frac {1}{2 G} K _ {I I I} ^ {2},
where \bar { E } = E for plane stress and \bar { E } = E / ( 1 - \nu ^ { 2 } ) for plane strain, axisymmetry, and three dimensions. For an interfacial crack between two dissimilar isotropic materials,
J = \frac {1 - \beta^ {2}}{E ^ {*}} (K _ {I} ^ {2} + K _ {I I} ^ {2}) + \frac {1}{2 G ^ {*}} K _ {I I I} ^ {2},
where
\frac {1}{E ^ {*}} = \frac {1}{2} \left(\frac {1}{\bar {E} _ {1}} + \frac {1}{\bar {E} _ {2}}\right), \quad \frac {1}{G ^ {*}} = \frac {1}{2} \left(\frac {1}{G _ {1}} + \frac {1}{G _ {2}}\right);
\beta = \frac {G _ {1} (\kappa_ {2} - 1) - G _ {2} (\kappa_ {1} - 1)}{G _ {1} (\kappa_ {2} + 1) + G _ {2} (\kappa_ {1} + 1)};
for plane strain, axisymmetry, and three dimensions; and \kappa = ( 3 - \nu ) / ( 1 + \nu ) for plane stress. Unlike their analogues in a homogeneous material, K _ { I } and K _ { I I } are no longer the pure Mode I and Mode II stress intensity factors for an interfacial crack. They are simply the real and imaginary parts of a complex stress intensity factor.
Although the energy release rate is calculated directly in Abaqus/Standard, it is usually not straightforward to compute stress intensity factors from a known J-integral for mixed-mode problems. Abaqus/Standard provides an interaction integral method to compute the stress intensity factors directly for a crack under mixed-mode loading. This capability is available for linear isotropic and anisotropic materials. The theory is described in detail in “Stress intensity factor extraction,” Section 2.16.2 of the Abaqus Theory Guide.
In this case the J-integrals calculated from the stress intensity factors will also be output. These J-integral values may be slightly different from those estimated by requesting the J-integral directly, due to the different algorithms used for the calculations.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=K FACTORS
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Stress intensity factors
Domain dependence
The stress intensity factors have the same domain dependence features as the J-integral.
Including the effect of a residual stress field on stress intensity factor evaluation
An additional term is included to account for the residual stress field when calculating the stress intensity factors, as described in “Including the effect of a residual stress field on J-integral evaluation.”
Input File Usage: *CONTOUR INTEGRAL, RESIDUAL STRESS STEP=n, TYPE=K FACTORS
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Step for residual stress initialization values: step, Type: Stress intensity factors
The crack propagation direction
For homogeneous, isotropic elastic materials the direction of cracking initiation can be calculated using one of the following three criteria: the maximum tangential stress criterion, the maximum energy release rate criterion, or the K _ { I I } = 0 criterion. K _ { I I I } is not taken into account in any of these criteria.
The maximum tangential stress criterion
Using either the condition \partial \sigma _ { \theta \theta } / \partial \theta = 0 \mathrm { o r } \tau _ { r \theta } = 0 (where r and are polar coordinates centered at the crack tip in a plane orthogonal to the crack line), we can obtain
\hat {\theta} = \cos^ {- 1} \left(\frac {3 K _ {I I} ^ {2} + \sqrt {K _ {I} ^ {4} + 8 K _ {I} ^ {2} K _ {I I} ^ {2}}}{K _ {I} ^ {2} + 9 K _ {I I} ^ {2}}\right),
where the crack propagation angle \hat { \theta } is measured with respect to the crack plane and \hat { \theta } = 0 represents the crack propagation in the “straight-ahead” direction. \hat { \theta } < 0 \mathrm { i f } K _ { I I } > 0 , while \hat { \theta } > 0 \mathrm { ~ i f ~ } K _ { I I } < 0 . The crack propagation angle is measured from to ; i.e., it is measured about the direction , or counterclockwise measured from in Figure 11.4.2–1.
The crack propagation angle \ddot { \theta } will be output.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=K FACTORS, DIRECTION=MTS
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Stress intensity factors, Crack initiation criterion: Maximum tangential stress
The maximum energy release rate criterion
This criterion postulates that a crack initially propagates in the direction that maximizes the energy release rate.
The crack propagation angle \hat { \theta } will be output.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=K FACTORS, DIRECTION=MERR
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Stress intensity factors, Crack initiation criterion: Maximum energy release rate
The K _ { I I } = 0 criterion
This criterion assumes that a crack initially propagates in the direction that makes K _ { I I } = 0 .
The crack propagation angle \hat { \theta } will be output.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=K FACTORS, DIRECTION=KII0
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Stress intensity factors, Crack initiation criterion: K11=0
The T -stress
The T-stress component represents a stress parallel to the crack faces at the crack tip. Its magnitude can alter not only the size and shape of the plastic zone but also the stress triaxiality ahead of the crack tip. It is, therefore, a useful indicator of whether measures of the strength of the crack-tip singularity (such as the J-integral or the stress intensity factors) are useful in characterizing a crack under a particular loading. In a linear elastic analysis the T-stress should be calculated using loads equal to the loads in the elastic-plastic analysis. See “T -stress extraction,” Section 2.16.3 of the Abaqus Theory Guide, for more information.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=T-STRESS
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: T-stress
Domain dependence
In general, the T-stress has larger domain dependence or contour dependence than the J-integral and the stress intensity factors. Numerical tests suggest that the estimates from the first two rings of elements abutting the crack tip or crack line generally do not provide accurate results. Sufficient contours extending from the crack tip or crack line should be chosen so that the T-stress can be determined to be independent of the number of contours, within engineering accuracy. Particularly for axisymmetric models, the closer the crack tip is to the symmetry axis, the more refined the mesh in the domain should be to achieve path independence of the contour integral.
Including the effect of a residual stress field on T -stress evaluation
An additional term is included to account for the residual stress field when calculating the T -stress, as described in “Including the effect of a residual stress field on J-integral evaluation.”
Input File Usage: *CONTOUR INTEGRAL, RESIDUAL STRESS STEP=n, TYPE=T-STRESS
Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Step for residual stress initialization values: step, Type: T-stress
Defining the data required for a contour integral with the conventional finite element method
To request contour integral output with the conventional finite element method, you must define the crack front and specify the virtual crack extension direction.
Defining the crack front
You must specify the crack front; i.e., the region that defines the first contour. Abaqus/Standard uses this region and one layer of elements surrounding it to compute the first contour integral. An additional layer of elements is used to compute each subsequent contour.
The crack front can be equivalent to the crack tip in two dimensions or the crack line in three dimensions; or it can be a larger region surrounding the crack tip or crack line, in which case it must include the crack tip or crack line.
If blunted crack tips are modeled, the crack front should include all the nodes going from one crack face to the other that would collapse onto the crack tip if the radius of the blunted tip were reduced to zero. Otherwise, the contour integral value will depend on the path until the contour region reaches the parallel crack faces.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n
Specify the crack front node set name on the data line; the format depends on the method you use to specify the virtual crack extension direction.
For two-dimensional cases only one crack front node set (the crack front at the crack tip) must be specified. For three-dimensional cases you must repeat the data line to specify the crack front for each node (or cluster of focused nodes) along the crack line in order from one end of the crack to the other, including the midside nodes of second-order elements; it is not permissible to skip nodes along the crack line.
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front
Defining the crack tip or crack line
By default, Abaqus/Standard defines the crack tip as the first node specified for the crack front and the crack line as the sequence of first nodes specified for the crack front. The first node is the node with the smallest node number, unless the node set is generated as unsorted. Alternatively, you can specify the crack-tip node or crack-line nodes directly. This specification plays a critical role for a three-dimensional crack with a blunt crack tip.
Abaqus/CAE cannot determine the crack tip or crack line automatically based on the specified crack front. However, if you select a point to define the crack front in two dimensions, the same point defines the crack tip; likewise, if you select edges to define the crack front in three dimensions, the same edges define the crack line. For all other cases you must define the crack tip or crack line directly.
Input File Usage: Use the following option to specify the crack-tip nodes directly:
*CONTOUR INTEGRAL, CONTOURS=n, CRACK TIP NODES
Specify the crack front node set name and the crack tip node number or node set name on the data line; the format depends on the method you use to specify the virtual crack extension direction.
Repeat the data line for three-dimensional cases.
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front, then select the crack tip (in two dimensions) or crack line (in three dimensions)
Defining a closed-loop crack line
Sometimes a crack line may form a closed loop (for example, when modeling a full penny-shaped crack without invoking symmetry conditions). In such cases the finite element mesh in the crack-tip region can be created with or without seams; i.e., linear constraint equations (“Linear constraint equations,” Section 35.2.1) or multi-point constraints (“General multi-point constraints,” Section 35.2.2) may or may not be used to tie two layers of nodes together.
If a crack line forms a closed loop, the starting node set of the crack front can be chosen arbitrarily and the other node sets defining the crack front must go around the crack front sequentially. The last node set defining the crack front must be the same as the first node set. If a closed loop is formed by creating coincident nodes that are then tied together by linear constraint equations and multi-point constraints, the node sets must be specified in order starting from one of the node sets involved in the constraint equation or multi-point constraint and terminating with the other node set.
Specifying the virtual crack extension direction
You must specify the direction of virtual crack extension at each crack tip in two dimensions or at each node along the crack line in three dimensions by specifying either the normal to the crack plane, , or the virtual crack extension direction, .
If the virtual crack extension direction is specified to point into the material (parallel to the crack faces), the J-integral values calculated will be positive. Negative J-integral values are obtained when the virtual crack extension direction is specified in the opposite direction.
Specifying the normal to the crack plane
The virtual crack extension direction can be defined by specifying the normal, , to the crack plane. In this case Abaqus/Standard will calculate a virtual crack extension direction, , that is orthogonal to the crack front tangent, , and the normal, . As shown in Figure 11.4.2–1, for a three-dimensional crack; for a two-dimensional crack, we simply have q _ { x } = - n _ { y } and q _ { y } \ = \ n _ { x } . Specifying the normal implies that the crack plane is flat since only one value of can be given per contour integral.
Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, NORMAL -direction cosine (or ), -direction cosine (or ), -direction cosine (or blank) crack front node set name (2D) or names (3D)
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front: Specify crack extension direction using: Normal to crack plane
Specifying the virtual crack extension direction
Alternatively, the virtual crack extension direction, , can be specified directly. In three dimensions the virtual crack extension direction, , will be corrected to be orthogonal to any normal defined at a node or in other cases to the tangent to the crack line itself. The tangent, , to the crack line at a particular point is obtained by parabolic interpolation through the crack front for which the virtual crack extension
text_image
Crack front node set. See section A-A below. 1/4 point nodes crack plane Crack front node set Section A-A
Figure 11.4.2–1 Typical focused mesh for fracture mechanics evaluation.
vector is defined and the nearest node sets on either side of this region. Abaqus/Standard will normalize the virtual crack extension direction, .
Input File Usage:
*CONTOUR INTEGRAL, CONTOURS=n
crack front node set name, -direction cosine (or ), -direction
cosine (or ), -direction cosine (or blank)