## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Fracture Stress Intensity Fracture Discrepancy

• Ed_Green
Subscriber

Hi there,

As part of one of my projects, I am trying to model a crack within a plate in-order to evaluate the effectiveness of crack propagation retarding techniques. I have followed two instructional videos in order to help me generate a zero volume crack in a thin plate.

One of these makes the geometry from two bodies in SpaceClaim and joins them using the share tool to crate the crack and the other uses two frozen bodies joined by a bonded normal Lagrange contact.

After applying a 10mPa load to the plate (figure1), the values for SIFS vary by a factor of (almost exactly) 100% between the two methods at 186 and 92 MPa mm^0.5. Other fracture parameters (J-integral) also vary by 100%. I do not understand why there is a discrepancy between these values and would appreciate some insight from an expert.

I am positive that I have set the model up the same (thickness/force) between the two and have had my colleague verify this for me. Figure 1 shows the SpaceClaim method (left) and the Design Modler method (right). Figure 2 is the boundary conditions (left) and contact method for the Design Modler method (right)

In order to determine which was true, I analytically calculated the applied stress intensity factor for this plate (thickness = 0.2m, crack = 0.05m). This analytical value agrees with the SpaceClaim method (188MPa / mm^0.5).

My question is, why is there a discrepancy between the two methods, and am I correct in thinking that the design modeler method will always be a factor of 1/2 the true value. I want to continue with Design Modeler as it is much easier to parameterise the geometries that I want to add to the model later.

Ed

• David Weed
Ansys Employee
HiArray,nThe discrepancy is most likely due to the presence of contact elements at the crack tip; usage of these elements within the fracture zone is not supported. It seems that the solver is calculating one half of the domain integral value at the crack tip (perhaps it's being truncated by the contact elements). In general, you should use either shared topology or a mesh connection to join surfaces where the fracture parameters are being calculated. DesignModeler also has a shared topology feature. You can pick multiple surfaces, right click on them and choose Form a new part and the shared topology field should be set to Automatic, which will function the same as SpaceClaim's feature.n