3D Static Edge Crack SIF Study

Here is a study into the rate of convergence of Mode I stress intensity factor evaluated using contour integrals for an edge crack in a finite plate under uniaxial tension within Abaqus. Convergence is defined here as the relative error (calculated/theoretical) as a function of the mesh density (h is length of a side of the square/cube element). Results are compared for a variety of meshes and the final results are compared to the convergence rate for MXFEM, which can be downloaded from this website. Within Abaqus the domain is defined to be 1 x 1 x 4 with an edge crack of length 0.3. The same domain is used in MXFEM with plane strain elements. Several input files are available for download. Note that only 3D contour integrals are allowed within Abaqus, while 2D is used in MXFEM.

Downloadable Files

Abaqus Input Files: 10 Elements Per Unit Length (INP,CAE)
MXFEM Input File: 10 Elements Per Unit Length (m)


Note that only contour 3 from Abaqus is used to compare to MXFEM, which also used the third contour for the evaluation of the stress intensity factors.

Tutorial for Stress Intensity Factor Evaluation

Material Properties Used
Fracture Energy: 10e3
Maximum Principal Stress: 1e6
Poisson's Ratio: 0.33
Young's Modulus: 10e6

Requesting Contour Integral Evaluation

1. For a model with a predefined crack, double click on History Output Requests.
2. Enter SIF as name of History Output Request, Step is Loading, Click Continue.
3. Select Crack from Domain, then the Crack for which you want the SIFs evaluated.
4. Select the Frequency and Number of Contours to your liking. Here Last Increment and 3 were used.
5. Type was chosen as Stress Intensity Factors with Maximum Energy Release Rate as the Crack Initiation Criterion. Click Ok.
6. The stress intensity factor data can then be viewed from History Output in the Results screen.

Interpretation of Stress Intensity Factor Data
Here all of the values of the third contour have been averaged together to find a single Mode I stress intensity factor within Abaqus.

Discussion of Stress Intensity Factor Results
From the provided plot it is clear that the two-dimensional plane strain code converges to the theoretical stress intensity factor more quickly than the Abaqus model. This may be a result of the Abaqus model not being sufficiently long to simulate a plane strain condition. The main point of these results is simply to show that for accurate stress intensity factor calculations within Abaqus, a fine mesh around the crack tip is necessary, especially since stress intensity factor values are typically more accurate for two-dimensions1 than three-dimensions2.


1. Moes, N., Dolbow, J., Belytschko, T. (1999) "A finite element method for crack growth without remeshing," International Journal for Numerical Methods in Engineering, 46, 131-150.

2. Sukumar, N., Moes, N., Moran, B., Belytschko, T. (2000) "Extended finite element method for three-dimensional crack modelling," International Journal for Numerical Methods in Engineering, 48, 1549-1570.