How to Generate hex mesh with high quality and lower acceptable number of elements in ANSYS Meshing?
December 10, 2019 at 10:57 pmMohamed AbdulazimSubscriber
I am trying to generate a structured mesh with improved orthogonality for a rectangular channel with tilted perforated baffles as a heat transfer case. I use ANSYS meshing for that case, but the resulted mesh elements are very high in number, about 6000000 or higher, and the resulted mesh elements are tetrahedrons, also when I export it to the fluent, the program recorded error message mentioning that the memory run out and the mission aborted automatically. Moreover, when I tried to modify the shape by slicing option in the design modeler in the hope of making hex mesh, the resulted mesh has a very low orthogonality quality about lower than 0.003 and the aspect ratio is too high about 1200. I am really depressed about this situation. Any help will be appreciated. Thanks in advance.
December 11, 2019 at 1:07 ampeteroznewmanSubscriber
I suggest you delete all the holes in all the baffles. That will make it possible to have an all Hex mesh.
I understand removing the holes changes the flow slightly compared with having holes, but at least you will get a result that is a good approximation to the original baffles. When you have a better computer, you can put the holes back in. Another way to approximate the holes is to make the solid body without holes slightly porous to account for the flow that goes through the baffle.
Another observation is there are at least five sets of double baffles. You could slice out one segment with an upper and lower baffle to make the geometry edits to make a good hex mesh. When that is working, you can make four more copies in a pattern or use Periodic Symmetry to rebuild the full length model.
December 11, 2019 at 10:51 amRobAnsys Employee
The other observation is that we can include baffles in Fluent as thin walls: no need to model them as a solid body. That may effect the flow around the baffle tips, but will have the benefit of significantly reducing the cell count.
December 11, 2019 at 11:52 amMohamed AbdulazimSubscriberThank you very much, Peter,for your kind reply. You suggested making a slice for one set of upper and lower Baffles, how could I do that in order to reach a fully developed flow condition for reaching a constant local heat transfer coefficient, as you know. In other words, what is the exact position for slicing? When I make periodic symmetry, Do you think that the variations from the beginning of the channel to the end of it would be sensible for the solver and can be seen in the contours or the pattern will be similar for each set of the Baffles and variation couldn't be seen .
December 11, 2019 at 11:59 amMohamed AbdulazimSubscriberThank you very much for your kind help,rwoolhou . I'm going to try this method, it's a good idea.
December 11, 2019 at 12:58 pmpeteroznewmanSubscriber
If you are interested in a fully developed flow condition, Periodic Symmetry delivers that solution. A pair of baffles occurs at a repeating pitch length, that is the important parameter. It doesn't matter where you slice out the periodic section. If you slice it at 25% between the upper and lower baffles on the input side, you will have 75% on the output side. Keep it simple and just slice halfway between the baffles. In any case, the Periodic BC will make the inlet flow conditions identical with the outlet flow conditions. I'm not sure how that works with a Thermal model. Maybe rwoolhou can comment.
If you are interested in seeing how the flow develops, then you can't use Periodic Symmetry.
December 11, 2019 at 4:24 pmRobAnsys Employee
Thanks Peter. There are a few limitations for thermal periodic flow (relating to solids, and what temperature/heat flux boundaries you can use) but they're simple enough to set up. The issues are all covered in the section of the Heat Transfer chapter of the User's Guide outlining the periodic boundary.
Slitting mid way is a good idea: don't split over the baffle as that may break the rules and always makes it more complicated than it needs to be.
- 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.
- how to improve the inflation quality at sharp corners?
- ANSYS Workbench Measuring within Design
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
- How to resolve Mesh Failure
- inflation created stairstep mesh at some location
© 2023 Copyright ANSYS, Inc. All rights reserved.