Modeling onset and propagating of crack using ABAQUS
Modeling cracks in finite element software is done in several ways. In general, these methods can be divided into two categories: traditional methods and modern methods.
The traditional method is to include two methods:
- Surface-based cohesive behavior
- Virtual crack closure technique
In traditional methods, simulating onset and propagating of cracks, need to design meshing of model regarding to crack propagation probability. If the model is also considered to simulate opening and propagating of crack, it would be far more complex and harder. In this method crack opening direction should be predicted and elements faces should be in this direction. Also at the crack tip, singularity for the elements should be defined.
The new method, called the Extended Finite Element Method or XFEM many complexities and limitations of methods by using enriched elements have been fixed.
In this example we will investigate opening and propagating of crack in a steel plate using XFEM method. Sheet dimensions are 6*3 units and at the beginning there is a 1.5 unit long crack in the middle of it. Sheet is under longitudinal and transverse forces at two ends, making the crack to open and propagate.
Part / Sketch
First in part module, make 2D part and name it “Plate”. Using dimensions command to make it 6*3. We will come back to part module again later.
In property modules, we define the desired material. Submit your material as defined in the previous examples.
E = 200 GPa
ν = 0.3
It is very important to have enough knowledge about failure criteria when you want to simulate it. But, here we only want to learn how to model crack in ABAQUS. One of the common failure criteria is the amount of maximum stress. In this example we will use these criteria. We consider 84 MPa for the start of cracking. Complete Maxps Damage and Damage Evolution settings according to the figure.
Do Damage Evolution settings from suboptions.
In assembly module assemble an instance of “Plate”. Location of initial cracks in the piece is done in the Assembly module. Therefore it is necessary to return again to the Part module to create the crack initial geometry.
Create a new Part and name it “Crack”. Draw a horizontal line of length 1.5 units. Now in the tree diagram you may see Plate and Crack in the branch of Part.
Returned to the Assembly module and add crack to model. Note that more than once the parts are not assembled. To check this, there should not be more than two instances under assembly branch.
If parts have been assembled correctly, you should resemble the following figure.
In Step module define a Static General step and turn Nlgeom on.
To define crack, in interaction module follow the following path:
Special / Crack / Create
Create a crack with arbitrary name. Choose XFEM in create crack window. We will talk about XFEM and its methods in another post. In comparison with other crack modeling methods, XFEM is a new way that for the first time introduced in ABAQUS version 6.9. This concept adds some new characteristics to elements such as ability to divide and make them enriched.
In the Edit crack window choose the whole sheet as the Region and the crack lane in front of the crack location. It is possible to define interaction properties for crack edges but in this example we do not need it. Enriched region and initial crack are shown by green crosses.
Please enter the Load module. Unlike the previous examples in this example instead of applying force on the part we will apply movement. First it is better to define some sets for the part special areas. Execute the following command from the main menu.
Tools / Set / Create
Name the set upper and choose Geometry type. Choose the upper edge of the part. In a same manner make another set and name it lower for lower part edge.
Click on Create boundary condition button. Select Displacement / Rotation and select upper using sets button from prompt area.
Enter -0.00135 and +0.00081 for longitudinal and transverse displacements like the figure. Similarly, for lower enter values of +0.00135 and -0.00081.
In mesh module, mesh the plate in 0.1 unit size. In Assign Element Type check the family of plate elements to be Plane strain. Part crack does not need mesh.
In Job module, define the model and click submit.
To view the results of run click results and get into the Visualization module. In order to see better results and see how crack propagates increase scale from common options. The following animation shows crack opening trend and the Mises stress.
It is possible to adjust the number of frames in the Field Output options in step module.