November 15, 2022 at 10:46 amEddie2324Subscriber
Hello, I am facing an issue about hexa solid mesh, I tried to use sweep method first but the bodies are not sweepable, after that I tried to use multizone method but it failed too and I succed to mesh my geometry with hex dominant method. It seems not bad at all when I checked the outer faces but I have really bad elements in inside of body. I see 1000+ aspect ratio in mesh metric graph but when I tried to check it it shows nothing all blank. Beside that I have another bad elements in inside of mesh but even tough my max mesh metrics are terrible, I still have pretty good aspect ratio and other criterias in avarage( avarage is 1.8 for aspect ratio and 0.9 for element quality).
I could not find a way to solve it, I tried to change element size, mesh defarture, and adaptive sizing but nothing worked I even split to geometry to a lot of simple cubical shapes, I tried to mesh this simple cubical parts but even tough I still have this massive invisible aspect ratios and skewness as well.
Should I try to solve the problem, will it effect the precision of my solution? I am going to do structural analysis with a brittle cast iron material I am thinking its going to be a lineer analaysis.
November 15, 2022 at 12:14 pmpeteroznewmanSubscriber
The average mesh quality is not important. The element with the worst quality is the problem. Poor element quality will affect the accuracy of the solution
I usually succeed when I split the solids into small cubical shapes. Since this failed for you, I recommend you apply a Tet mesh to the complete solid. Tet elements should fill the volume and the minimum element quality should be acceptable. If it is not, then there are defects in the geometry that need to be fixed.
November 16, 2022 at 4:27 amEddie2324Subscriber
Thank you for your answer, I wondering did I something wrong while doing splitting operations, without split there is none sweepable body but now I have few bodies but still something feels wrong because when I checked sweepable bodies I saw one body is ok for a sweep but its mirror simetric(splitted with the same way) its not sweepable, I have few examples like that and you can see one in the picture. The body in the left is sweepable but body in the right its not, they only have slightly different wides and thats all. What possibly went wrong here? Do you have any tip for splitting? Since I am not used to do this kind of splitting operations of mesh I might did something wrong.
November 17, 2022 at 1:13 pmpeteroznewmanSubscriber
The number of edges on the end faces have to be equal, and the side faces have to have no splits. In SpaceClaim, go to the Repair tab and eliminate Extra Edges and Extra Points.
November 17, 2022 at 2:40 pmEddie2324Subscriber
I changed share topology to none from shared, after doing that %90 of my bodies became sweepable. Idk why but sharing topology cuased the problem I guess. The software defined bonded contact for every part I splitted, since there is a lot of splitted part it is not possible to define contacts one by one for me. I checked penetration gap etc. from connection tool after solved the model, it seems there is no penetration(really really small number such as 7.e-9) and no gap between parts so it seemed okay to me but can I trust the software about making connections or do I have to use shared topology? Normally there is no assembly, it is one big solid casting part but it defined connections because I turned off share topology, as far as I know bonded contact will act same as shared topology for implicit static analysis, please correct me if I am wrong. Thanks
November 18, 2022 at 12:28 ampeteroznewmanSubscriber
Bonded contact is okay to hold parts together as long as the contact is not near any high stress areas. Shared topology is prefered when there is high stress. If Shared topology with split solids is not working, don't split the solid and use Quadratic Tet Mesh on that body.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- How to calculate the residual stress on a coating by Vickers indentation?
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.