TAGGED: cfd, fluent, meshing, watertight-workflow
February 2, 2021 at 5:48 pmDanielOliveiraSubscriber
I'm trying to construct a mesh similar to the one in the image below, using the watertight meshing, since my structure has a complex geometry.
In previous versions I could perform mesh stretching using edge sizing with bias factor, however, I can not find any option like that.
Also, Is it possible to implement mesh grading in the vertical direction?
Could anyone help me?
Daniel OliveiraFebruary 3, 2021 at 6:41 amKeyur KanadeAnsys EmployeeWith watertight geometry, I assume you are using Fluent Meshing. nThere is no edge sizing with bias factor in Fluent Meshing. It is available in Ansys Meshing. Please go through help manual for more details nIn Fluent Meshing to get similar refinement, you may need to BOI. nPlease go through help manual for more details nnRegards,nKeyurnHow to access Ansys Online Help DocumentnHow to show full resolution imagenGuidelines on the Student CommunitynHow to use Google to search within Ansys Student CommunitynFebruary 3, 2021 at 11:04 amDanielOliveiraSubscriber,nAppreciate your help. nRegarding the stretching mesh, is it possible to do in fluent Meshing?nRegardsnDanielnFebruary 3, 2021 at 11:52 amDanielOliveiraSubscriberand how can you define different mesh sizes in different directions?.AppreciatenFebruary 3, 2021 at 12:06 pmKeyur KanadeAnsys EmployeeYou will need to define boi in different directions. nYou can find several posts on forum about boi. Also if you search boi ansys meshing on google, you can find some videos related to it. Same strategy will be used for Fluent Meshing. nRegards,nKeyurnHow to access Ansys Online Help DocumentnHow to show full resolution imagenGuidelines on the Student CommunitynHow to use Google to search within Ansys Student CommunitynFebruary 3, 2021 at 2:26 pmDanielOliveiraSubscriberSorry but I can not see how can I define a 3D mesh inFluent Meshing with different sizes in vertical and horizontal directions using BOI, can be more explicit?.Really appreciate your helpFebruary 3, 2021 at 4:41 pmRobAnsys EmployeeFluent Meshing doesn't have a stretched mesh option: it's also fully unstructured with options for a hex element core to the mesh. The mesh above is most likely a swept mesh from Ansys Meshing or ICEM CFD. nFebruary 4, 2021 at 2:41 pmFebruary 4, 2021 at 4:01 pmDanielOliveiraSubscriberI already find how to do it.nnReally appreciate your help.nBest RegardsnDaniel nFebruary 4, 2021 at 4:17 pmRobAnsys EmployeeMultibody parts are what you need, or share topology. nFebruary 5, 2021 at 12:44 amFebruary 5, 2021 at 9:39 amRobAnsys EmployeeFluent Meshing will give you a (mostly) low aspect ratio mesh with poly, tet and dependent on settings a hex core to the mesh. nThe refinement in the above image is adaption, and is found in the Fluent Solver. It's purpose is to allow us to refine a mesh based on the physics, so features like moving shocks or water free surface. However, in the above mesh I'd be fairly critical of the high aspect ratio in the direction of the waves: VOF is fairly sensitive to this so the results may not be good in that region. nIf you're using 2021R1 (and 2020R2) have a look in the adaption panel for the predefined criterion. We added one for VOF to help with phase break up; in your case 2 levels of refinement is probably sufficient. nFebruary 5, 2021 at 10:11 amDanielOliveiraSubscribernI already tried with poly-hexacore, however, I can not perform the swept meshing at the end of the NWT to decrease the overall total number of cells in the damping zone. Also, since I can not do any edge sizing in fluent meshing, to define the required aspect ratio (vertical/horizontal directions), and It also doesn't work with the body of influence technique, I need to use the adaption. Regarding the aspect ratio, I performed some convergence parametric studies using different values of CPL and CPH and I found 20CPH and 100CPL to be sufficiently accurate for wave generation and propagation with almost zero numerical wave damping, which are the same dimensions that I applied to this model. Therefore, I used 3 levels of refinement in order to increase the size of the cells away from the free surface level. nRegarding the predefined criterion for VOF, I also tried dynamic adaption, however, the computation looks faster applying this static refinement in the zone of interest. With dynamic VOF adaption, it is applied to the full domain, including the damping zone where it is not necessary. In this specific case, I'm working with a submerged structure, which will cause some breaking waves in extreme cases, however, the wave crest will not jump out of the refined zone. nI really appreciate your help. If you have any more advice for this type of application let me knownnBest RegardsnDanielFebruary 5, 2021 at 10:45 amRobAnsys EmployeeStatic adaption is faster as it's done once and not updated. However, if the region (flow feature) that needs the refinement moves you've refined the wrong part of the model. It's a trade off. nOne option to save on cell count is to run in 2d or with only 1 cell across a thin domain. We often do this for testing newer models or where we want to check settings before running a much larger model (ie 150M cells or more). nViewing 13 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
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
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.