

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 JIntegral 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 wellposed, the Jint/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 xdirection should be in the direction of crack growth and the ydirection 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 Jint/SIF results for a mesh with tetrahedral elements. This is not available for 2D. For 2D cases, you either want a structured (hexahedral elements), fanshaped 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 JINT? 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.

 The topic ‘Solution Contours and Connection to Temperature, Material Properties, and Meshing.’ is closed to new replies.
 Preparing Solidworks Model for Thermal Desktop
 How to add Geometry to Ansys Rocky and not have the blocks merged into one?
 Exporting CGNS _ ICEM CFD
 SteadyState Thermal in case of Layered Sections
 Can somebody help me in Finding Stress intensity Factor of a crack …
 How to increase font size in ICEM CFD
 Advanced Turbogrid Topologies
 Why are the coordinates I specified and the coordinates outputted in the report
 NON MANIFOLD NODE WARNING
 PostProcessing in Aqwa: Getting Panel Pressure Time Response Series at Nodes

276

1

1

1

1
Â© 2024 Copyright ANSYS, Inc. All rights reserved.