April 11, 2022 at 5:41 pmcharlie_kcSubscriber
I have begun the modelling of a heat exchanger, using static structural analysis system. I've read online that hex mesh is preferred over tet, and so fortunately I have managed to apply hex mesh to the majority of the components (some required slicing to do so). However, my tubesheets and baffles [pictured] only appear to agree with the tet mesh ,which I am assuming is either to do with the thinness of the plates or the relatively uneven geometry (corners, holes etc).
Now my question is: is there any way to force these plates to adopt a hex mesh? And if not, will mixing tet and hex mesh across the various components greatly affect the accuracy of my solution?
Thank you in advance.April 12, 2022 at 8:00 amApril 12, 2022 at 9:15 amVigneswaran SridharanAnsys EmployeeHey Linear tetrahedral/triangular elements suffer from three issues:
ÔÇÉThey have one integration point and are constant strain elements ÔÇô so we need an extremely fine mesh to capture the strain gradient accurately.
ÔÇÉ It's difficult to distort the element without changing its volume so theyÔÇÖre prone to volumetric locking for nearly or fully incompressible materials and maybe overly stiff.
ÔÇÉIn the case of bending-dominated problems, linear elements are also prone to shear locking which introduces spurious shear stresses in the part and make it overly stiff regardless of how fine the mesh is created.
Linear hexahedral elements, or the 8-noded hex elements, do not suffer from the first two issues, so they seem like a good alternative to linear tetrahedral elements, hence the general recommendation!
While it is a valid suggestion, it's not always possible to generate a hexahedral mesh. The above limitations are resolved by introducing mid-side nodes which creates a 10-noded tet element that uses second-order polynomial for shape functions. If the geometry is a combination of sweepable and irregular shapes in such then the combination of brick, tetrahedral, pyramid, or wedge elements is used. Pyramid elements are used in the transition regions.
Look at this relevant video on "Understanding importance of 3D element shapes and order"
Rules & Guidelines ÔÇö Ansys Learning Forum
April 12, 2022 at 3:04 pmApril 12, 2022 at 3:17 pmAkshay ManiyarAnsys Employee
Yes, I can see the image now. Thank you.
About the parts which you have highlighted, have you tried to use multizone method on this parts? I guess, multizone method will be useful for this parts.
Thank you for the detailed answer and course link. If it is not meshing in hex then you can use quadratic tetrahedral elements, as it will be less stiff compared to linear tetrahedral elements. You can go through the course which has shared for more details about the various elements.
Ansys Learning Forum (Rules & Guidelines)
April 12, 2022 at 3:58 pmcharlie_kcSubscriberThank you very much for your detailed response. In order to add mid-surface nodes, does my component have to be a surface body as opposed to a solid body?
April 12, 2022 at 3:58 pmcharlie_kcSubscriberThank you very much for your detailed response. In order to add mid-surface nodes, does my component have to be a surface body as opposed to a solid body? Doing some research based off your video, it looks like it may be best to convert the components to shell (using mid surface) as opposed to solid bodies, since they are relatively thin in comparison to the other dimensions.
April 13, 2022 at 9:38 amVigneswaran SridharanAnsys EmployeeHey You could also use Shell/3D surface elements (Like Shell181, Shell281) with mid-surface extraction in SpaceClaim (Refer to Midsurface tutorial (spaceclaim.com)).
But, keep in mind you cannot generate a Midsurface unless the faces have a constant wall thickness. In SC, the Midsurface tool will not select the non-parallel faces.
Nodes on Shell elements have 6 Dof's. Hence MPC based bonded contact should be used to connect shell and solid elements.
Refer to this video for more info on understanding shell elements.
Rules & Guidelines ÔÇö Ansys Learning Forum
Viewing 7 reply threads
Ansys Innovation Space
- 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.Trending discussions
- How to calculate the residual stress on a coating by Vickers indentation?
- Solver Pivot Warning in Beam Element Model
- Errors – Reinforced Concrete Beam
- An Unknown error occurred during solution. Check the Solver Output…..
- 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
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Colors and Mesh Display
- Large deflection
Top Rated Tags