1.2. Solving Fracture Mechanics Problems

A fracture analysis is a combination of stress analysis and fracture mechanics parameter calculation. The stress analysis is a standard linear elastic or nonlinear elastic plastic analysis.

Because high stress gradients exist in the region around the crack tip, the finite element modeling of a component containing a crack requires special attention in that region.

The 2-D and 3-D representations of the region around the crack tip and the terminology used is outlined in the following section. The edge or tip of the crack is referred to as a crack tip in a 2-D model and crack front in a 3-D model, as illustrated in Figure 1.5: Crack Tip and Crack Front.

Figure 1.5:  Crack Tip and Crack Front

Crack Tip and Crack Front

(a) 2-D models and (b) 3-D models


The following additional topics related to solving fracture problems are available :

1.2.1. Modeling the Crack-Tip Region

Stress and deformation fields around the crack tip generally have high gradients. The precise nature of these fields depends on the material, geometry, and other factors. To capture the rapidly varying stress and deformation fields, use a refined mesh in the region around the crack tip. For linear elastic problems, the displacements near the crack tip (or crack front) vary as , where r is the distance from the crack tip. The stresses and strains are singular at the crack tip, varying as . To produce this singularity in stresses and strains, the crack tip mesh should have certain characteristics:

  • The crack faces should be coincident.

  • The elements around the crack tip (or crack front) should be quadratic, with the midside nodes placed at the quarter points. (Such elements are called singular elements.)

Figure 1.6: Singular Element Examples shows examples of singular elements for 2-D and 3-D fracture models.

Figure 1.6:  Singular Element Examples

Singular Element Examples

(a) 2-D models and (b) 3-D models


The following additional topics for modeling the crack-tip region are available:

1.2.1.1. Modeling 2-D Linear Elastic Fracture Problems

The recommended element type for a 2-D fracture model is PLANE183, the 8-node quadratic solid. The first row of elements around the crack tip should be singular, as illustrated in Figure 1.6: Singular Element Examples (a).

The PREP7 preprocessor's KSCON command (Main Menu> Preprocessor> Meshing> Size Cntrls> Concentrat KPs> Create), which assigns element division sizes around a keypoint, is particularly useful in a fracture model. It automatically generates singular elements around the specified keypoint. Other fields on the command allow you to control the radius of the first row of elements, the number of elements in the circumferential direction, and more. Figure 1.7: Fracture Specimen and 2-D FE Model shows a fracture model generated with the help of KSCON.

Figure 1.7:  Fracture Specimen and 2-D FE Model

Fracture Specimen and 2-D FE Model

Take advantage of symmetry where possible. In many cases, you need to model only one half of the crack region, with symmetry or antisymmetry boundary conditions, as shown below.

Figure 1.8:  Using Symmetry to Your Advantage

Using Symmetry to Your Advantage

For reasonable results, the first row of elements around the crack tip should have a radius of approximately a / 8 or smaller, where a is the crack length. In the circumferential direction, roughly one element every 30° or 40° is recommended.

The crack-tip elements should not be distorted and should take the shape of isosceles triangles.

1.2.1.2. Modeling 3-D Linear Elastic Fracture Problems

The recommended element type for 3-D models is SOLID186, the 20-node brick element. As shown in Figure 1.6: Singular Element Examples (b), the first row of elements around the crack front should be singular elements. Notice that the element is wedge-shaped, with the KLPO face collapsed into the line KO.

Generating a 3-D fracture model is considerably more involved than a 2-D model. The KSCON command is not available for 3-D modeling. You must verify that the crack front is along edge KO of the elements.

Element size recommendations are the same as for 2-D models. In addition, aspect ratios should not exceed approximately 4 to 1 in all directions.

For curved crack fronts, the element size along the crack front depends on the amount of local curvature. A general guideline is to have at least one element every 15° to 30° along a circular crack front.

All element edges should be straight, including the edge on the crack front.

1.2.2. Calculating Fracture Parameters

You can evaluate various fracture parameters. Most are calculated during the solution phase of the analysis (CINT), the results stored to the .rst results file for postprocessing.

Stress-intensity factors can also be calculated during (POST1) postprocessing (KCALC).

For more information, see Evaluation of Fracture Mechanics Parameters.

1.2.3. Postprocessing Fracture Parameters

To print or display various fracture parameters during postprocessing, issue the PRCINT or PLCINT command, respectively.


Release 18.2 - © ANSYS, Inc. All rights reserved.