The Focused Mesh Contour Integral (FMCI) Crack Builder is an Abaqus/CAE plug-in to automatically create focused mesh partitions, meshes and contour integrals (including q-vectors) for conventional focused mesh contour integral fracture analysis.

Background

For many years Abaqus/Standard has included the ability to assess quasi-static, stationary crack fracture mechanics problems using contour integrals. While an XFEM-based contour integral method has been added in recent years, the conventional approach involves constructing a specific “focused” mesh configuration at the tip of the presumed crack. This configuration typically includes the following characteristics (some of which are illustrated in Figure 1):

• Two concentric tubular (circular in 2D) regions centered on and surrounding the crack tip;
  • The inner tube includes a single set of degenerate 2nd order hex elements
  • The outer tube is comprised of a series of concentric rings of 2nd order hex elements;
• Depending on the specifics of the problem the singularity at the crack tip may need to be handled via:
  • Biasing of the mid-side nodes of the degenerate crack tip elements to the quarter-point (or some other intermediate location) location toward the crack tip;
  • Specific types of crack tip element degeneracy including:
    • None
    • Collapsed to a single node
    • Collapsed to duplicate coincident nodes

Figure 1. Typical "focused mesh" for conventional contour integral method.

For 2D and simple 3D model geometries, the above tasks add some additional user effort but remain fairly manageable. For more complex 3D geometries the above tasks can become onerous, if not nearly impossible. This plug-in is intended to remove much of the burden in creating these focused mesh configurations for fracture mechanics problems. At present, the plug-in can properly handle cracks modeled as shown in the left-hand image in Figure 2 but not those that look like the right-hand image in that figure.

Figure 2. 2D schematic illustration of crack geometries the plug-in can (left) and cannot (right) support.

Plug-in Function

The starting state of an Abaqus/CAE model for use of this plug-in is a model assembly including at least two 3D geometry (i.e., not orphan mesh) part instances. One of these is the instance to be partitioned for focused meshing while the other is simply a 3D shell part geometry introduced to represent the geometry and location of the desired crack face/tip. (The concept is philosophically similar to that used for generating XFEM cracks in Abaqus/CAE.) Figure 3 illustrates a simple, typical case.

Figure 3. Assembly requirements for plug-in use. One instance is to be cut/partitioned, the other is used to define the crack geometry for partition generation.

Based on the user’s inputs, gathered by the plug-in GUI, the plug-in will perform the following operations:

1. Copy the current model to a new model and make a copy of the original part defining the crack instance;
   • The new model has the name of the original model with the string ‘-FMP’ appended to it;
   • The new “crack” part retains the original “crack” part’s name while the original “crack” part is renamed to include the suffix ‘-Original’.
2. Create the concentric tube partitions
   • Update the new “crack” part to add the concentric tube partitioning geometry as well as the crack surface
   • Partition the designated part instance with this new augmented “crack” part via the Merge/Cut Instances feature in Abaqus/CAE, creating both a new part with the suffix ‘–Partitioned’ appended to the original instance name and a corresponding update to the instance in the assembly.
   • The new partitioned instance is instantiated as an independent part instance to facilitate required subsequent seam definition & focused meshing operations.
3. Create a series of named assembly-level sets related to the new crack geometry to be referenced in subsequent operations.
4. Create the crack “seam” (allows coincident nodes on crack surface) then configure and generate the instance mesh;
   • Meshing includes both the two concentric tubular regions at the crack front and the remainder of the instance geometry
   • The inner tube is meshed with a single ring of degenerate (wedge-shaped) 2nd order hex elements (C3D20R);
   • The inner tube degeneracy includes any user-specified changes to mid-side node location and degeneracy type;
   • The outer tube is meshed with the user-specified number of contour rings (less the one included in the inner tube noted in c.) of 2nd order hex elements (C3D20R);
   • The remaining cells of the instance are meshed with 2nd order tetrahedral elements (C3D10);
   • Beyond the normal analysis warning/errors mesh verification, additional element quality checks are performed to ensure proper element type assignments and shape checks particularly for the degenerated wedge-shaped hexes at the crack tip.
5. Create the contour integral crack and contour integral history output requests;
   • The contour integral crack is defined to include a crack extension direction. One may use either the crack surface normal (for planar cracks) or so-called q vectors for this specification. If q vectors are specified, an orphan mesh version of the model must be created in order to define q vectors in Abaqus/CAE. The additional tasks of orphan mesh conversion and q-vector calculation and assignment are also handled by the plug-in.
   • When the contour integral crack extension direction is defined via the crack surface normal, the plug-in automatically defines the normal from the crack surface data.
   • The plug-in GUI allows for user specification of the analysis step in which the contour integral calculation will be performed. If no analysis steps are defined in the source model when the plug-in is invoked a default general static step (with NLGEOM=OFF) named ‘dummyStep’ will automatically be created for the final ‘-FMP’ model and the relevant contour integral history output requests added within that step.
   • The plug-in configures two contour integral history output requests: one for the J-integral and the other for the stress intensity factors. These requests auto-generate global coordinate location history output for each point on the crack front as well as the CPD (crack propagation direction output at hose locations as well.
6. Perform a mesh quality check for the newly partitioned and meshed instance.

Plug-in Usage

Use of the plug-in is straightforward. To start, invoke the plug-in by selecting the “Build FMCI Crack Model” option from the Plug-ins menu in the Abaqus/CAE environment. This selection instantiates the plug-in dialog box entitled “Create Focused Mesh Contour Integral Crack” and shown in Figure 4.

Figure 4. Focused Mesh Contour Integral plug-in GUI.

For all the details of plug-in usage and limitations select the “Help” button from the plug-in dialog to launch the HTML user’s guide.

Plug-in Download & Installation

The attached zip archive contains all the files necessary to install and run the Focused Mesh Contour Integral Crack Builder plug-in for Abaqus/CAE (6.14-1 and higher). To install the plug-in, save the FMCI_Crack_Builder folder to one of the following directories:

 abaqus_dir\\abaqus_plugins where abaqus_dir is the Abaqus parent directory

home_dir\\abaqus_plugins where home_dir is your home directory

current_dir\\abaqus_plugins where current_dir is the current directory

 Note that if the abaqus_plugins directory does not exist in the desired path, it must be created. The plugin_dir directory can also be used, where plugin_dir is a directory specified in the abaqus_v6.env file by the environment variable plugin_central_dir. You can store plug-ins in a central location that can be accessed by all users at your site if the directory to which plugin_central_dir refers is mounted on a file system that all users can access. For example:

 plugin_central_dir = r'\\\\fileServer\\sharedDirectory'

***NOTE:

BY DOWNLOADING THIS FILE (“DOWNLOAD”) YOU AGREE TO THE FOLLOWING TERMS:

THIS DOWNLOAD IS MADE AVAILABLE ON AN "AS IS" BASIS WITHOUT WARRANTY OF ANY KIND, WHETHER EXPRESS OR IMPLIED, ORAL OR WRITTEN, INCLUDING, WITHOUT LIMITATION, ANY IMPLIED WARRANTIES OF MERCHANTABILITY, FITNESS FOR A PARTICULAR PURPOSE, TITLE OR NON-INFRINGEMENT.

DASSAULT SYSTEMES SIMULIA CORP., ANY OF IT AFFILIATES (COLLECTIVELY “DS:”), AND ITS LICENSORS SHALL HAVE NO LIABILITY FOR DIRECT, INDIRECT, INCIDENTAL, CONSEQUENTIAL OR PUNITIVE DAMAGES, INCLUDING WITHOUT LIMITATION CLAIMS FOR LOST PROFITS, BUSINESS INTERRUPTION AND LOSS OF DATA, THAT IN ANY WAY RELATE TO THIS DOWNLOAD, WHETHER OR NOT DS HAS BEEN ADVISED OF THE POSSIBILITY OF SUCH DAMAGES AND NOTWITHSTANDING THE FAILURE OF THE ESSENTIAL PURPOSE OF ANY REMEDY.

YOUR USE OF THIS DOWNLOAD SHALL BE AT YOUR SOLE RISK. NO SUPPORT OF ANY KIND OF THE DOWNLOAD IS PROVIDED BY DS.