November 11, 2020 at 12:18 pmChristijaaanSubscriberHi, ndoes anybody know if there is a function which enables the determination of the inner volume change delta_v of a shell structure due to an inner static load (static mechanic case). I was thinking about a function which has an output like displacement of a surface in normal direction - > apply on the surface areas of the inner elements - >This values times the surface area itself gives a volume change. A math integration over the whole area of interest should give the volume change... Is there an area function as described above available? Or is there an easier way to do all this? nThanks in advance to everybody und greetingsn
November 18, 2020 at 3:48 pmHuiLiuAnsys EmployeeThere is no direct way of output what you are looking for. If there is no volume (solid element) inside of the shell structure, there is nothing to output. For the workflow that you described, you can check out the ARNODE(N) and NORMNX/Y/Z(N1,N2,N3) get functions, which get the area of node and normal directions defined by 3 nodes. For a full list of get functions, see thislinkfrom APDL user's guide. Hope this can make your calculation easier.n
November 19, 2020 at 7:20 amChristijaaanSubscriberthat sounds as to be a nice feature for my problem. Thank you very much. Will try it out. nFurthermore...nDo you have any suggestion for an APDL function which gets the displacement of a node / surface in normal direction? I did it ones for selected nodes by placing user defined coordinate systems within every single node and orientate the z-axis by normal in click-point in the really near surrounding (as near as possible). Last step was to define a solution (one for every single node) which gets the diplacement in local z-direction. That felt like a work around... isn't there any function which makes it easier?n
November 23, 2020 at 7:58 amChristijaaanSubscriberDoes nobody alse have an idea? When I first thought about that problem, I was pretty sure that there was a standard solution available ...n
November 24, 2020 at 1:37 ampeteroznewmanSubscribernThere is a FLUID221 quadratic tetrahedral element. If your shell mesh was quadratic triangles, you could fill the volume with FLUID221 elements that shared the outer surface nodes with the shell elements.nThe volume of the FLUID221 element is an output result quantity: VOLU.nFor a completely different approach that does not require meshing the volume, read this discussion:nThis approach uses an element called HSFLD242 but you don't mesh the volume, you just need a node on the inside and have a named selection to all the element faces that enclose the volume.n
November 24, 2020 at 10:22 amChristijaaanSubscribernThank you so much. Both ways seem really worth a try. Really cool!n
- The topic ‘Determination of the volume change of a shell-structure due to an inner load’ is closed to new replies.
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.
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- 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
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.