Computing Fracture Mechanics Parameters in StressCheck

StressCheck has an advanced method implemented for the computation of Mode 1 and Mode 2 (K1 and K2) stress intensity factors (SIFs) in linear elastic fracture mechanics, for two- and three-dimensions. It also has the capability of computing the J-integral and the T-Stress for two- and three-dimensional problems. Note: StressCheck’s implementation supports the computation of fracture mechanics parameters for both 360 degree and 180 degree (i.e. symmetry plane) cracks.

The J-integral can be computed for linear and elastic-plastic solutions of isotropic materials and for linear solutions of orthotropic materials. For elastic-plastic solutions, the integration path should be selected in such a way that it does not cut through the plastic zone around the crack tip. The extraction of the separated J-integral for linear isotropic and orthotropic materials for Planar (J1 & J2) and 3D (J1, J2 & J3) is also available. For more details on fracture mechanics parameters, refer to Fracture Mechanics Analysis Overview.

To perform fracture mechanics extractions for a solved StressCheck model, select the Fracture tab in the Results dialog and specify the desired Fracture extraction options (Figure 1).

After specifying the Fracture extraction options, click on Accept to perform the extraction. After the extraction is completed, a graph will appear displaying the fracture extraction results.

Specifying the Solution ID(s) and Run(s)

To compute fracture mechanics parameters for a solved StressCheck model, select the Fracture tab in the Results dialog, and set the Object and Method combo-boxes of the C/A/O/M to the desired configuration (discussed in the following), click on the Solution ID in the scrolling listbox and enter the range of Run numbers for which you wish to compute fracture mechanics parameters. For example, you may enter Run: 8 to 8 if only Run number 8 is of interest. To compute an estimated convergence limit and relative error, at least three (3) Runs are required (e.g. Run: 1 to 3).

For more information on the importance of checking solution quality, refer to What Are the Key Quality Checks for FEA Solution Verification?.

Solution Run Wildcards

Entering a max Run number of “0” will automatically compute using the solution with the maximum DOF.

Specifying the Fracture Mechanics Object

If in 3D or Extrude reference, the fracture mechanics computation is only available for a selected element edge (set the Object combo-box of the C/A/O/M to to “Edge”, the default). If in the Planar reference, the fracture mechanics computation is available for a selected node (set the Object combo-box of the C/A/O/M to “Node”), a selected point (set the Object combo-box of the C/A/O/M to “Point”) or a selected crack object (set the Object combo-box of the C/A/O/M to “Crack”). The following are the resultant computation expectations for each object:

• Node/Point: Computes the SIF or J-integral at the selected node/point.
• Crack: Computes SIF’s at the A and B tips of the selected crack.
• Edge: Computes SIF or J-integral at the selected location on an element edge.

Specifying the Fracture Mechanics Method

The available fracture mechanics parameter methods are described in the following:

• SIF: the computation of Mode 1 and Mode 2 (K1 and K2) stress intensity factors (SIFs) via the Contour Integral Method (CIM) is performed. Additionally, the computation of T-stress is performed, which is an indication of the tendency the crack to turn.
• J-integral: the computation of the separated energy release rates (SERR) via the J-integral is performed. In Planar reference, this results in the path integral components J1/J2, and in the 3D/Extrude reference this results in the path/area integral components J1/J2/J3.

For more details on the fracture mechanics parameter methods, consult Numerical Simulation Series: Fracture Mechanics Parameters and Fracture Mechanics Analysis Overview.

Specifying the Display Format

You may input the precision with which you wish to display data values (“Format:” field, in C standard format). The default format is in scientific notation and any C language format specification can be used. For example, the number Pi (3.141592654…) will be displayed as: 3.141592654e+00 in format %16.9e or 3.14 in format %5.2f.

Specifying the Auxiliary/Independent Variable

Use the auxiliary variable input field (“Aux. Variable”) if you want to include a variable parameter in the
results. Switch the “Aux. Variable” toggle to “Indep. Var.” and enter a parameter name if you want the auxiliary variable to be the independent variable of the graph.

For example, if graphing the results of a Design Study analysis where one or more parameters is varied across a range of values.

Specifying the Integration Radius

To compute the SIF or J-integral, specify the radius (“Radius”) of the circle representing the integration path. Two integration radius options are available for the “Radius” field: click and drag (AUTO), or manual entry. The influence of the size of the integration radius on the results, such as for elliptical automeshed cracks, is generally very small if proper meshing is utilized. Typically, the integration radius should extend just outside the innermost layer of elements.

Note: if the Curve display is enabled, a dashed red circular path will appear after the computation providing feedback about the path of the integral.

Manual Entry

To do this, turn on the “Radius” toggle switch and specify a value such that the circle remains inside the solution domain. The value may be a constant, parameter or formula. Then select a location on a free edge of the crack front (3D/Extrude), or a crack tip point/node (Planar), to perform the fracture mechanics computation.

Click and Drag

Alternatively, you may turn off the switch in front of the radius (AUTO), bring the cursor to the node or point on the crack tip (free edge of crack front in 3D), click the left button of the mouse, and drag the cursor. A circle will appear which will grow in size as you are dragging the cursor, and the “Radius” field will automatically update with the current value of the circle radius. Once the circle is of the desired size, release the left button of the mouse to perform the computation.

The below animation shows a click and drag computation of the J-integral at a crack tip point in 2D (Planar):

Performing the Fracture Mechanics Computation

Assuming the integration radius is contained with the model domain, the Fracture Mechanics computation will be performed for the selected Solution ID(s), Run(s), integration radius, and element edge location (3D/Extrude) or point/node/crack (Planar), and a graph pane will be produced containing exportable details on the Fracture Mechanics computation. A new Fracture Mechanics computation may be performed at any time, resulting in a new graph pane.

When computing output function values from a sequence of at least 3 solutions, StressCheck performs an estimation of the true value of the selected function by projecting the results from the finite element solutions to an infinite number of degrees of freedom. The result of this projection is reported as the “Estimated Limit” together with the percent deviation from the value corresponding to the solution chosen having the highest number of degrees of freedom. The below shows a typical graph pane where the SIF was computed at a location on a selected element edge for an integration radius of 3e-3:

For an example of computing SIF’s along 3D crack front element edges, refer to StressCheck Demo: Part-Thru Crack SIFs for Stiffened Lug.

Note: for the fracture mechanics extraction to be valid the selected point should be related to the crack tip node either by associativity or having the same global coordinates. If the point or node does not correspond to a crack tip, the extraction will fail. In addition, if a crack tip object set contains multiple nodes, or points, the extraction will fail.