June 28, 2018 at 9:55 pmpeteroznewmanSubscriber
Fabricio wondered why his fastener model that consisted of a Head, Shaft and Nut had such a different value of peak stress depending on whether it was a 3-body multibody part or it was Boolean United into a single body. Below is the difference he was seeing.
The first image is the 3-body result. Note the peak is 821 MPa.
The second image is the 1-body part. Note the peak is 627 MPa.
Most of the difference is due to the setting Average Across Bodies set to No, which is the default.
If the Average Across Bodies is set to Yes, then there is little difference between the mulitbody part and the single body part. Note the peak goes down to 615 MPa.
It is understood that this model includes a stress singularity due to the sharp interior corner at the shaft, so comparing peak stress is somewhat pointless since any reduction in element size around the corner is going to result in a higher stress. The point of this post is to show that stress results on multibody parts should have Average Across Bodies set to Yes if they are all the same material.
Fabricio also asked how to get the full element display on the section view. It is by clicking the diamond shaped icon on the Section window.
Now here are the three section view:
It seems the elements are actually a little better quality in the 1-body mesh than the 3-body mesh above. I expect with a little work, the 3-body mesh could be made to look like the 1-body mesh.
Attached is an 18.2 archive.
June 29, 2018 at 12:04 amBhargava SistaAnsys Employee
That's a nice post with a good example! To further your point, I would like to add a few more notes:
- In FEA, forces and displacements are calculated at nodes and the stresses and strains are calculated at the integration points (internal to elements). The stresses are then either interpolated or copied to the nodal locations.
- Therefore, each node receives a stress value from each element it is connected to. An average of all these values is reported as the stress at that location. This is valid only when all these elements have the same material assignment.
- In a multi-body part, the bodies share nodes at the interface and they may have different material assignments. This is the reason the option to average across bodies is turned off by default. As stated in the above post, if all the bodies in the multi-body part have the same material assignment, this option can be manually turned ON.
Regarding the mesh, it might help to use multi-zone mesh method on the 3-body mesh to get a structured hex mesh as in the 1-body case. This is a common recommendation for modeling bolts.
P.S: You may want to mark the sentence "The point of this post..." in bold.
- 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.
- 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.