March 17, 2022 at 11:13 pmzbath0316Subscriber
When it comes to the solution contours, should they converge to some level of accuracy? When I am calculating the J-Integral of the crack shown below, I get solution contours that vary very drastically (from negative to positive and positive to negative). I guess the real question here is how do I determine an accurate solution when the contours vary so much? I am also wondering if these contours are the result of low temperatures (perhaps at higher temperatures the material is easier to simulation, and therefore get a more proper solution). I am also wondering if there are additional material properties more necessary than the density, Young's Modulus and Poisson's Ratio. I am also wondering if a better meshing technique is needed. What is used is quad/tri with edge sizing by number of divisions (30). The two edges used are those of the crack.
The overall geometry:March 21, 2022 at 4:00 pmDavid WeedAnsys Employee
In general, if the FEA problem is well-posed, the J-int/SIF values should converge as the contours increase. Typically, the first contour result can be discarded as it tends to be the least accurate, since it is the contour which is closest to the stress singularity at the crack tip. In the case you've shown, there are a number of things at play that could be producing an oscillating result. First, check the position of the local crack tip coordinate system. It should be on the open side of the crack (not flush with the crack tip) and the x-direction should be in the direction of crack growth and the y-direction should be normal to the crack plane; hence, make sure that the local coordinate system is not directly scoped to the crack tip node, rather offset it slightly so that it is on the open side of the crack.
Also please confirm whether this is 2D or 3D; it appears to be 2D. Note that, for 3D cases, you can take advantage of the Unstructured Mesh Method (UMM), which can produce accurate J-int/SIF results for a mesh with tetrahedral elements. This is not available for 2D. For 2D cases, you either want a structured (hexahedral elements), fan-shaped mesh around the crack tip or, in lieu of a structured mesh, you want significant element refinement around this region. For instance, for a structured mesh, something like the following:
Note that the APDL command, KSCON, can also help in producing the type of mesh above; we have some Verification Manual examples which show usage of the KSCON command. If you're going to use an unstructured mesh for 2D cases, you'll need significant refinement of the elements around the crack tip region. I would also suggest refining the mesh, in a global sense, so that you accurately capture the stress field within the broader FEA model, as this will have an affect on the stresses seen around the crack tip as well. Regarding material models, if you are conducting a Linear Elastic Fracture Mechanics (LEFM) analysis, elastic properties are sufficient. I hope that this information is helpful to you.
May 11, 2022 at 5:00 pmzbath0316SubscriberI appreciate your help on the convergence. I got the solution to converge :). On another note, what if we are interested in the Plastic part of the fracture mechanics with a J-INT? What kind of material properties would be needed for plastic fracture besides the Young's Modulus and Poisson's ratio? I believe these only define the elastic region of crack propagation, and would like to know more about the plastic region as well.
Viewing 2 reply threads
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
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
- Conformal vs Non-Conformal Mesh
- inflation created stairstep mesh at some location
- Error in meshing
- Meshing Error
- How to resolve Mesh Failure
- How to get three elements across the wall thickness of a thin part
- Meaning of the symbol crossed out tick mark on a body in the tree outline indicate in Meshing
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.