TAGGED: fracture, fracture-mechanics
February 11, 2021 at 10:24 amEd_GreenSubscriber
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.
EdFebruary 18, 2021 at 11:40 pmDavid WeedAnsys EmployeeHiArray,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.nViewing 1 reply thread
Ansys Innovation Space
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.