July 14, 2023 at 2:51 amFrank AstulleSubscriberHi everyone I tried to simulate a force inside a lifitng lug in a vessel. So I tried to do it with shell elements with a thickness of 6mm. So I`ve put 20000N in X and Y axes, and I believe that I get a singularity stress, because stress tends to infinity when when the mesh gets finer My question is ¿How I can determine the real strees in the shell of the vessel? And ¿how I can model a reinforcement pad with shell elements? I was thinking to split the shell and asign other thickness in the zone with reinforcement pad. How I can split the shell surface? I`ve tried to imprint face like a reinforcement plate but I can't asign another thickness in a imprinted face.
July 14, 2023 at 2:24 pmDave LoomanAnsys Employee
It's definitely a singularity at that location. Perhaps you should use solid elements for the lifting lug and the reinforcing pad.
July 15, 2023 at 4:48 ammjmiddleAnsys Employee
The real model has welds probably so has a taper at that corner. You can make small solid bodies with swept triangle shape to represent the welds, and use contact to connect to the solid.Or maybe an MPC bonded contact from edge-to-face can resolve the stress singularity, even without solid bodies to represent the welds, since the constraints will connect outward an additional layer of nodes.
If you want to specify a greater thickness to the shell just near the bond point, there are many ways to split the shell body or face. What CAD system does the geometry originate? You can draw a sketch line on the surface and split by that or split by a plane, or by two point selection on the boundary edges. Or you can split entirely in Mechanical using Virtual Topology. Right click on Model in the Outline to insert a Virtual Topology. This allows splitting and merging of faces and edges. If you split in the CAD Modeler you can split just the face so it is multiple faces in the same body, or you can split the body entirely, in which case, you can connect with shared topology if you use SpaceClaim or DesignModeler. In Mechanical you can, of course, set a different thickness on different bodies if you split the body entirely. If you split only the face, so as to have multiple faces in the same body, then you can right click in Mechanical on "Geometry > Insert > Thickness." This allows you to select faces and set different thicknesses for faces in the same body.
July 18, 2023 at 3:27 am
July 18, 2023 at 4:51 ammjmiddleAnsys Employee
I'm not entirely convinced it's a stress singularity. Based on the direction of the force, you could have high stress and deformation in that pattern. Is it steel with a yield stress around 250 MPa? It is over yield, but not excessively so. We verify stress singlarities by making smaller elements at the suspected location to see if the stress keeps going up. In non-singularities, the stress may go up but does so asymptotically, aproaching a constant value.
July 18, 2023 at 7:27 amErik KostsonAnsys Employee
Just to add to mjmiddle and to do a mesh refinement study to see if it is a singularity - see this post about this:
(see section on welds/shells)
All the best
- 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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- User manual
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- 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
- Defining rigid body and contact
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.