# ANSYS APDL Tutorial: Fracture Mechanics Simulation of A Cracked Plate

When it comes to general strength issues, we typically use stress to measure strength. However, for high-strength components with cracks, using stress to measure strength is incorrect. In such cases, new criteria are needed to examine strength.

Fracture Mechanics provides a method for calculating the strength of components with cracks and introduces concepts such as energy release rate, stress intensity factor, J integral, etc. to measure the strength of components with cracks. These concepts are used to determine if a component with a crack will further propagate under certain external loads or to determine the length of the crack required for it not to propagate further.

This article provides the most classic example of a crack on a flat plate subjected to tensile stress to examine the strength of the plate under this force.

## Case Description:

A long flat plate with a horizontal crack in the middle is subjected to uniform tensile forces at the top and bottom edges as shown in the figure below. The stress intensity factor of the crack is required. The material parameters, sizes and distribution of the applied forces are shown in the table below.

## Problem Analysis:

• This example comes from the ANSYS 15.0 APDL help, where the example is modeled using PLANE183, SOLID185, and SOLID186 and the stress intensity factor is examined. This article only uses the PLANE183 modeling part, partially rearranging the command sequence and deleting some unnecessary programs.
• For 2-D cracks, use the PLANE183 element recommended by ANSYS.
• Since it is a symmetrical problem, only one quarter is modeled and the crack tip is taken as the origin.
• When geometric modeling, the crack is represented by a straight line, and due to the high stress gradient at the crack tip, the grid around it needs to be carefully divided. Here, KSCON is used to indicate the crack tip and explain how to divide the grid around it.
• Set symmetrical boundary conditions and define the relevant parameters for calculating the crack with CINT.
• Extract the stress intensity factor in post-processing.

## Solution Process

### 1. Modeling

1.1 Creating element type
Enter the following command in the command window:
/PREP7
ET,1,PLANE183,,,2
The above command determines the use of PLANE183 to model a planar strain problem. PLANE183 is the recommended element for modeling cracked planar problems by ANSYS. For modeling cracks in 3D, ANSYS recommends using the SOLID186 element.

1.2 Inputting material properties
Enter the following commands in the command window:
MP,EX,1,30E6
MP,NUXY,1,0.3

The above commands define the material’s elastic modulus and Poisson’s ratio.

1.3 Creating a geometric model with cracks
Enter the following commands in the command window:

K,1
K,2,4
K,3,4,5
K,4,-1,5
K,5,-1

The above commands define several key points for a quarter model. The resulting output is shown in the figure below.

Enter the following commands in the command window:
L,1,2
L,2,3
LESIZE,2,,,4

The above commands draw two lines and set the second line to be divided into four equal parts.

Enter the following commands in the command window:
L,3,4
LESIZE,3,,,4

The above command draws another line shown in the figure below and sets the number of divisions to be four.

Enter the following commands in the command window:
L,4,5,
LESIZE,4,,,6,.2
L,5,1
ESIZE,,5

The above commands draw two more lines and set the size of the mesh to be used in each division.

KSCON,1,.15,0,8
AL,1,2,3,4,5

The above commands define a stress concentration key point and determine how to mesh around it. It specifies key point 1 as the stress concentration key point, sets the radius of the first row of elements around that key point to be 0.15, and sets the number of elements in the circumferential direction of the first row around that key point to be 8. The crack tip singularity keyword is 0, which is an important command for preparing meshing around the crack tip.

The second command is used to form a face enclosing the region bounded by the previously drawn lines. The resulting output is shown below.

1.4 Applying Boundary Conditions

In the command window, type:

DL,1,1,SYMM

DL,4,1,SYMM

The above commands define that symmetry boundary conditions are applied on edges 1 and 4. The “S” character will appear on these two edges after the command is executed, indicating that they are symmetric.

In the command window, type:

SFL,3,PRES,-.5641895

The above command is used to apply a uniformly distributed load upwards on edge 3. It is this load that causes the crack to continue to propagate. The result after running the command is shown in the figure.

In the command window, type:

AMESH,1

This command is used to mesh the model. The result is shown below.

Further zooming in on the crack tip:

It can be seen that there are 8 elements in the first circle around the crack tip.

In the command window, type:

ALLSEL,ALL

NSEL,S,LOC,X,0

NSEL,R,LOC,Y,0

D,ALL,UX,0

The above commands are used to constrain the crack tip so that it cannot move in the X direction.

1.5 Defining Crack Parameters

In the command window, type:

ALLSEL,ALL

NSEL,S,LOC,X,0

NSEL,R,LOC,Y,0

CM,CRACKTIP,NODE

The above commands are used to find the crack tip and define it as a component named CRACKTIP. After defining it, the component will have only one node, which is the crack tip node.

In the command window, type:

ALLSEL,ALL CINT,NEW,1
CINT,TYPE,SIFS
CINT,CTNC,CRACKTIP
CINT,SYMM,ON
CINT,NCON,6
CINT,NORM,0,2

The above commands first select all objects and then define a series of parameters to be used for calculating the crack parameters.

It first defines a new crack (NEW),

then specifies that the crack parameter to be calculated (TYPE) is the stress intensity factor (SIFS),

then indicates that the crack tip node (CTNC) is the component CRACKTIP defined earlier,

then indicates that the crack is symmetric (SYMM, ON),

then specifies that 6 equivalent points are used in the integration process,

and finally specifies that the crack coordinate system is the global coordinate system and the normal direction of the crack plane is the Y direction.

In the command window, type:

ALLSEL,ALL

FINISH

The above command is used to select all objects and exit the pre-processor.

### 2. Solution

Type the following commands in the command window:

/SOLU

ANTYPE,STATIC

SOLVE

FINI

These commands set the analysis type as static and exit the solver after the calculation is completed.

### 3. Post-processing

Type the following commands in the command window:

/POST1

*GET,K,CINT,1,CTIP,1,,5,,K1
*STATUS,K

These commands enter post-processing and extract the stress concentration factor at the crack tip, then display its value. The result is shown in the figure below.

It can be seen that the stress concentration factor at that point is 1.041.

After measuring the fracture toughness of the material, dividing it by the stress concentration factor gives the safety factor. This can be used to determine whether the crack will further propagate under the working stress for the cracked component.

Good Luck!