Figure 1 - "Quarter circular" superelement cube
Go back to text reference
Presented at the STRUCENG & FEMCAD Conference, Grenoble, France, 1990.
Note : Since being written the term "superelement" as described in this paper has been replaced by the term "crack-block".
G. Cook M.Sc.(Aero. Struc.), D.I.C., A.C.G.I.
C. Timbrell M.Eng., A.C.G.I.
P. Claydon M.Eng., A.C.G.I.
Zentech International Limited, 103 Mytchett Road, Camberley, Surrey,
GU16 6ES, U.K.
A method is presented for automatically generating meshes containing 3D crack fronts. Further, an adaptive meshing scheme is presented for automatically updating meshes during full 3D fatigue crack growth prediction.
Cracks are introduced into a valid mesh of the intact component by a mapping scheme which replaces standard 20 noded brick elements with "superelements". In the context of this paper, the term "superelement" refers to a set of 20 noded brick elements which models a quarter circular or through crack front using collapsed "quarter point node" brick elements. Replacement of elements in a mesh allows introduction of one or more distinct crack fronts, with more than one superelement permitted on each distinct crack front. A special mapping controls the crack size in each superelement and maintains original isoparametric surfaces thus creating a valid mesh for the cracked component. Following incremental fatigue crack growth prediction [1], all superelements are re-mapped to obtain a mesh with the new crack position. The mapping scheme allows non-planar crack growth in 3D geometries.
The procedure has been found to be flexible, efficient and a great time saver in 3D fatigue crack growth analyses. Good agreement with experimental fatigue crack growth data has been demonstrated using this meshing scheme [1].
Automatic, fatigue crack growth, mapping, mesh update, superelement, 3D.
Numerous publications deal with the calculation and prediction of fatigue crack growth, predominantly in 2D models or 2D planar cracks in 3D models e.g. [2-4]. As increased computing power becomes available at ever lowering costs the analysis of complex 3D non-planar cracks in 3D structures under arbitrary loading becomes more feasible. Historically the generation and updating of meshes for such analyses has been time consuming and difficult. A need existed for a general finite element meshing scheme for fast, easy and automatic generation and updating of meshes during full 3D fatigue crack growth.
This paper presents a general meshing scheme which meets these objectives. The scheme does not rely on a particular finite element package, and uses standard 20 noded isoparametric brick elements. It has been implemented in a software package, ZENCRACK [5], and tested using the MARC [6] and MENTAT [7] software packages.
The principle of the mesh generation scheme scheme is one of replacement of any 20 noded brick element in an uncracked mesh by "superelements" containing crack fronts. This automatically introduces cracks into a mesh and removes the necessity for the engineer to generate complex crack front meshes. The crack is allowed to grow through the superelements by re-mapping the nodes of the superelements to update the crack front and maintain the history of the crack surfaces. All superelements are stored in a library of standard 2x2x2 cubes, centred at the origin (e.g. Figure 1). Each superelement consists of standard 20 noded isoparametric brick elements and models either a quarter circular or through crack. The crack front region is modelled by collapsed 20 noded brick elements (singularity discussed later). Each superelement is refined to a different level at the crack front, allowing the user to choose a suitable superelement for a given problem. The superelements are compatible with standard brick elements on 3 sides for quarter circular and 2 sides for through crack superelements. The remaining "highly populated" faces can be left as free surfaces, symmetry surfaces, or connected to other compatible superelements. An example of two connected superelements incorporated into a mesh is shown in Figure 2.
To allow specification of an initial crack front and re-meshing of each superelement as the crack grows through it, a mapping scheme must be developed which allows control of the crack front and at the same time maintains the isoparametric surfaces on the highly populated faces of the superelements. To achieve this at present, the element face forming the initial crack plane for each superelement must be flat but not necessarily rectangular. The shape of the other five faces of the element is arbitrary. The mapping technique is described for a quarter circular crack superelement, but with very minor modifications is equally applicable to a through crack superelement.
It is assumed that a valid finite element mesh has been generated for the uncracked component, containing all necessary properties, loading and boundary conditions. This mesh can consist of any element type applicable to the finite element package being used, but only 20 noded brick elements can be replaced by a superelement.
There are 24 possible orientations for a crack front in each element to be replaced. To uniquely define the crack position and orientation requires an element number in the mesh and 2 corner node numbers forming an edge definition in the element. It is assumed that when travelling along that edge from node 1 to node 2 on the outside of the element that the crack lies on the face to the right hand side, such that node 1 will always be on the opening crack face (Figure 3).
It is required that the crack front coordinates in the mesh are known before mapping can take place. One method for defining the initial crack front is to use the ratios identified in Figure 3. The crack front nodal coordinates in the standard superelement are converted to an elliptic crack front with these ratios defining major and minor axes. The elliptic coordinates are mapped into the element space using the element shape functions, so that an initial set of crack front nodal coordinates are known. An alternative would be to explicitly define the required crack front positions in the element space.
In general the element crack plane will be at an arbitrary orientation to the x-y plane. To assist in the mapping (and history tracking) of the crack plane, each element is rotated so that its initial crack plane is parallel to the x-y plane. Nodes are readily mapped from the unit superelement to this "x-y position" before being rotated to the required space in the mesh.
Consider mapping a point L in the crack plane of the unit superelement to L' in the crack plane of the element in the "x-y position" (Figure 4). In the 2x2 crack plane of the standard superelement the crack front coordinates and coordinates of point L are known. In the crack plane in the "x-y position" the coordinates of the crack front nodes are known, as are the coordinates of the 8 nodes defining the plane (via the element shape functions). The point L' is calculated using the following steps:
Since the shape functions for the element reduce to a parabolic variation along an element edge, the assumed parabola is consistent with the shape functions along the two edges extending from point A'.
It is noted that this mapping can fail in the extreme case of a highly elliptic crack front in a superelement. This can be avoided by sensible choice of element geometry in the initial uncracked mesh.
Having found the mapped point L', it is now possible to give it an associated out of plane position. This technique is adopted for tracking crack history. The initial crack plane is split into triangular facets, based on the number of nodes along the crack front. As new crack fronts are defined, so the number of facets increases and the history of the free crack surface is approximated by these planar triangular facets. Having mapped point L to point L', location of the appropriate facet allows calculation of the out of plane position. It is noted that facets on the edge of the element crack plane must be extended beyond the crack plane boundary to cater for the possibility of convex boundaries. If this was not done, it would be possible to obtain a region in the crack plane with no associated triangular facet.
Mapping a general point P from the standard superelement can be achieved using a shape function approach, as shown in Figure 5. If P lies at (xp,yp,zp) in the 2x2x2 superelement, then define points L, M and U at (xp,yp,+1), (xp,yp,0) and (xp,yp,-1) respectively. Points M and U map to M' and U' in the x-y position using the element shape functions. Point L maps to L' using the previously described crack plane mapping. Point P' is found using eqn. 1.
XP' = - 0.5 zp ( 1 - zp ) XL' + ( 1 - zp2 ) XM' + 0.5 zp ( 1 + zp ) XU'........Eqn (1)
It is noted that very large amounts of out of plane crack growth will cause difficulty in this mapping. This can be avoided as far as possible by choosing a deep initial element to be replaced by the superelement.
Once all nodes of all superelements have been mapped into position in the mesh an automatic merge process eliminates surplus nodes and connects superelements to one another and to the remainder of the mesh (without merging crack faces together). This is done by rejecting a node from each coincident pair and updating element connectivities, thus avoiding the need for nodal tying constraints.
Automatic transfer of displacement boundary conditions and loading to the new mesh can be made as simple or complex as is seen fit. The minimum requirement is an ability to impose symmetry constraints on all nodes of a highly populated superelement face (except on free crack faces). This can be done by examining the constraints applied to the initial mesh and by the use of some simple rules for updating boundary conditions. For example, if all four corner nodes on an element face in the initial mesh are fixed in the same direction, then all nodes on the face in the new mesh must be fixed in that direction. Transfer of loading is more complex but can be handled in a similar fashion if sets of rules are laid down. As a simplification, loading can be forbidden on any element to be replaced by a superelement. In many cases this is acceptable as loading is often remote from the crack itself.
In a full crack growth analysis the above merging and transfer processes need to be carried out only once. Updating the mesh simply requires re-mapping of the nodes of the superelements once the new crack front positions have been defined.
Having generated a new mesh, its suitability for analysis should be considered. In the case of a linear elastic model, a r-1/2 stress and strain field exists at the crack front. In a 3D finite element model this singularity can be obtained by using collapsed standard 20 noded isoparametric brick elements, provided that certain constraints are placed on the nodes of the collapsed elements [8]. The positioning of quarter point nodes and other nodes in the collapsed elements is carried out after all nodes have been mapped.
In the standard 2x2x2 superelement, all midside nodes are correctly positioned. When mapping this superelement geometry into a mesh it is possible for midside nodes to move away from their ideal midside positions. Nodes which are considered to have moved too far from the midside point can be corrected on a parabolic arc length basis.
In order to help evaluate mesh quality in the new mesh, several element distortion parameters can be been defined and automatically calculated. The analysis can be terminated if these parameters fall outside user defined limits.
Figure 1 - "Quarter circular" superelement cube
Go back to text reference
Figure 2 - Two brick elements replaced by superelements
Go back to text reference
Figure 3 - Crack position in an element
Go back to text reference
Figure 4 - Mapping a point in the crack plane
Go back to text reference
Figure 5 - Mapping a general point
Point P in the 2x2x2 standard superelement maps to point P'
Go back to text reference