# Defining an imperfection based on static analysis data To define an imperfection based on the deformed geometry of a previous static analysis (“Unstable collapse and postbuckling analysis,” Section 6.2.4), specify the results file and step (and, optionally, the increment number) from a previous static analysis. (If the increment number is not specified, Abaqus will read data from the last increment available for the specified step in the results file.) Optionally, you can import modal data for a specified node set. Input File Usage: \*IMPERFECTION, FILE=results\_file, STEP=step, INC=inc, NSET=name # Defining an imperfection directly You can specify the imperfection directly as a table of node numbers and coordinate perturbations in the global coordinate system or, optionally, in a cylindrical or spherical coordinate system. Alternatively, you can read the imperfection data from a separate input file. Input File Usage: \*IMPERFECTION, SYSTEM=name, INPUT=input file If no input file is specified, Abaqus assumes that the data follow the option. # Imperfection sensitivity The response of some structures depends strongly on the imperfections in the original geometry, particularly if the buckling modes interact after buckling occurs. Hence, imperfections based on a single buckling mode tend to yield nonconservative results. By adjusting the magnitude of the scaling factors of the various buckling modes, the imperfection sensitivity of the structure can be assessed. Normally, a number of analyses should be conducted to investigate the sensitivity of a structure to imperfections. Structures with many closely spaced eigenmodes tend to be imperfection sensitive, and imperfections with shapes corresponding to the eigenmode for the lowest eigenvalue may not give the worst case. The imperfect structure will be easier to analyze if the imperfection is large. If the imperfection is small, the deformation will be quite small (relative to the imperfection) below the critical load. The response will grow quickly near the critical load, introducing a rapid change in behavior. On the other hand, if the imperfection is large, the postbuckling response will grow steadily before the critical load is reached. In this case the transition into postbuckled behavior will be smooth and relatively easy to analyze. # Input file template The following example illustrates a postbuckling analysis of a structure with an imperfection defined by a linear superposition of the buckling eigenmodes and involves two analysis runs with the same model definition. The initial analysis run performs an eigenvalue buckling analysis with Abaqus/Standard to establish the probable collapse modes and writes them to the results file. \*HEADING Initial analysis run to write the buckling modes to the results file \*NODE Data lines to define initial “perfect” geometry \*\* \*STEP \*BUCKLE Data lines to define the number of buckling eigenmodes \*CLOAD and/or \*DLOAD and/or \*DSLOAD and/or \*TEMPERATURE Data lines to specify the reference load, \*NODE FILE, GLOBAL=YES, LAST MODE=n U \*END STEP The second analysis run introduces the imperfection and performs a postbuckling analysis employing the modified Riks method in Abaqus/Standard. \*HEADING Second analysis run to define the imperfection and perform the postbuckling analysis \*NODE Data lines to define initial “perfect” geometry \*IMPERFECTION, FILE=results\_file, STEP=step Data lines specifying the mode number and its associated scale factor \*\* \*STEP, NLGEOM \*STATIC, RIKS Data line to define incrementation and stopping criteria \*CLOAD and/or \*DLOAD and/or \*DSLOAD and/or \*TEMPERATURE Data lines to specify reference loading, \*END STEP An alternative second analysis run introduces the imperfection and performs a postbuckling analysis with Abaqus/Explicit. \*HEADING Second analysis run to define the imperfection and perform the postbuckling analysis \*NODE Data lines to define initial “perfect” geometry \*IMPERFECTION, FILE=results\_file, STEP=step Data lines specifying the mode number and its associated scale factor \*\* \*STEP \*DYNAMIC, EXPLICIT Data line to define the time period of the step. \*CLOAD and/or \*DLOAD and/or \*DSLOAD and/or \*TEMPERATURE \*END STEP # 11.4 Fracture mechanics • “Fracture mechanics: overview,” Section 11.4.1 • “Contour integral evaluation,” Section 11.4.2 • “Crack propagation analysis,” Section 11.4.3 # 11.4.1 FRACTURE MECHANICS: OVERVIEW Abaqus/Standard provides the following methods for performing fracture mechanics studies: • Onset of cracking: The onset of cracking can be studied in quasi-static problems by using contour integrals (“Contour integral evaluation,” Section 11.4.2). The J-integral, the -integral (for creep), the stress intensity factors for both homogeneous materials and interfacial cracks, the crack propagation direction, and the T-stress are calculated by Abaqus/Standard. Contour integrals can be used in two- or three-dimensional problems. In these types of problems focused meshes are generally required and the propagation of a crack is not studied. • Crack propagation: The crack propagation capability allows quasi-static, including low-cycle fatigue, crack growth along predefined paths to be studied (“Crack propagation analysis,” Section 11.4.3). Cracks debond along user-defined surfaces. Several crack propagation criteria are available, and multiple cracks can be included in the analysis. Contour integrals can be requested in crack propagation problems. • Line spring elements: Part-through cracks in shells can be modeled inexpensively by using line spring elements in a static procedure, as explained in “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1. • Extended finite element method (XFEM): XFEM models a crack as an enriched feature by adding degrees of freedom in elements with special displacement functions (“Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1). XFEM does not require the mesh to match the geometry of the discontinuities. It can be used to simulate initiation and propagation of a discrete crack along an arbitrary, solution-dependent path without the requirement of remeshing. XFEM can also be used to perform contour integral evaluation without the need to refine the mesh around the crack tip. # 11.4.2 CONTOUR INTEGRAL EVALUATION Products: Abaqus/Standard Abaqus/CAE # References • “Fracture mechanics: overview,” Section 11.4.1 • \*CONTOUR INTEGRAL • “Using contour integrals to model fracture mechanics,” Section 31.2 of the Abaqus/CAE User’s Guide # Overview Abaqus/Standard offers the evaluation of several parameters for fracture mechanics studies based on either the conventional finite element method or the extended finite element method (XFEM, see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1): • the J-integral, which is widely accepted as a quasi-static fracture mechanics parameter for linear material response and, with limitations, for nonlinear material response; • the -integral, which has an equivalent role to the J-integral in the context of time-dependent creep behavior (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) in a quasi-static step (“Quasi-static analysis,” Section 6.2.5); • the stress intensity factors, which are used in linear elastic fracture mechanics to measure the strength of the local crack-tip fields; • the crack propagation direction—i.e., the angle at which a preexisting crack will propagate; and • the T-stress, which represents a stress parallel to the crack faces and is used as an indicator of the extent to which parameters like the J-integral are useful characterizations of the deformation field around the crack. # Contour integrals: • are output quantities—they do not affect the results; • can be requested only in general analysis steps; • can be used only with two-dimensional quadrilateral elements or three-dimensional brick elements when used with the conventional finite element method; • can be evaluated without requiring a detailed refined mesh around the crack tips when used with XFEM; and • are currently available only for first-order or second-order tetrahedron and first-order brick elements with isotropic elastic material when used with XFEM. # Contour integral evaluation Abaqus/Standard offers two different ways to evaluate the contour integral. The first approach is based on the conventional finite element method, which typically requires you to conform the mesh to the cracked geometry, to explicitly define the crack front, and to specify the virtual crack extension direction. Detailed focused meshes are generally required, and obtaining accurate contour integral results for a crack in a three-dimensional curved surface can be quite cumbersome. The extended finite element method (XFEM) alleviates these shortcomings. XFEM does not require the mesh to match the cracked geometry. The presence of a crack is ensured by the special enriched functions in conjunction with additional degrees of freedom. This approach also removes the requirement for explicitly defining the crack front or specifying the virtual crack extension direction when evaluating the contour integral. The data required for the contour integral are determined automatically based on the level set signed distance functions at the nodes in an element (see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1). Several contour integral evaluations are possible at each location along a crack. In a finite element model each evaluation can be thought of as the virtual motion of a block of material surrounding the crack tip (in two dimensions) or surrounding each node along the crack line (in three dimensions). Each block is defined by contours, where each contour is a ring of elements completely surrounding the crack tip or the nodes along the crack line from one crack face to the opposite crack face. These rings of elements are defined recursively to surround all previous contours. Abaqus/Standard automatically finds the elements that form each ring from the regions defined as the crack tip or crack line. Each contour provides an evaluation of the contour integral. The possible number of evaluations is the number of such rings of elements. You must specify the number of contours to be used in calculating contour integrals. In addition, you must specify the type of contour integral to be calculated, as described below. By default, Abaqus/Standard calculates the J-integral. You can assign a name to a crack that is used to identify the contour integral values in the data file and in the output database file. The name is also used by Abaqus/CAE to request contour integral output. If you are using the conventional finite element method and do not specify a crack name, by default Abaqus/Standard generates crack numbers that follow the order in which the cracks are defined. If you are using XFEM, you must set the crack name equal to the name assigned to the enriched feature. Input File Usage: Use the follow option to evaluate the contour integral with the conventional finite element method: \*CONTOUR INTEGRAL, CRACK NAME=crack name, CONTOURS=n, TYPE=integral\_type Use the following option to evaluate the contour integral with XFEM: \*CONTOUR INTEGRAL, CRACK NAME=crack name, XFEM, CONTOURS=n, TYPE=integral\_type Abaqus/CAE Usage: Interaction module: Special→Crack→Create: Name: crack name, Type: Contour integral or XFEM Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: integral\_type