October 29, 2017 at 9:06 pmpeteroznewmanSubscriber
If your model includes a threaded fastener, the simplest model is to use bonded contact to bond a smooth rod that represents a threaded fastener to a smooth hole that might represent a tapped hole or a threaded nut.
A more sophisticated treatment is where the smooth rod and hole have a thread geometry treatment applied in the frictional contact definition. This is more realistic than bonded contact for deformations on the surrounding parts since the stress builds up in the first few threads in a more representative way than the bonded contact which is less realistic. The smooth cylindrical hole had the contact geometry correction of Bolt Thread applied in the contact definition.
The image below shows two holes with a shoulder screw (hidden) tightened down on the outside face. This model is not intended to be a very accurate calculation of the stress in the treads. That is what a detailed model using actual thread geometry is for. This model distributes the force through the parts in a more realistic way than simple bonded contact.
It is recommended to have a mesh density of at least four elements per thread pitch.
Another post has an example of how to evaluate failure in the threads themselves.
July 16, 2019 at 12:47 amDerRepeater1Subscriber
I'm doing a same simulation using bolt threaded option of ansys, and the stress result is greater than the ultimate stress of the bolt's material.
Is the diameter of the cylindrical surface represents the thread of the bolt? When I set this option, is the thread actually will have a larger radius than the current face that leads to high penetration problem? The contact status is "closed" as I've checked it via contact tool.
July 16, 2019 at 1:17 ampeteroznewmanSubscriber
Make the diameter of the hole and the diameter of the fastener equal.
You must have a mesh density of at least four elements per thread pitch. It doesn't look like you have done that. If the thread pitch is 1 mm, then you must have a minimum of 4 elements per mm along the length of the fastener and the hole.
July 16, 2019 at 1:01 pmDerRepeater1Subscriber
The mesh density requirement is a big problem, I plan to split the bolt into 2 bodies, the threaded body is meshed with required density, the other will contain coarse mesh, then I set "bonded" contact between 2 bodies. Do you have any experience with this solution?
July 16, 2019 at 2:59 pmpeteroznewmanSubscriber
Look carefully at the original post and you will see that it is Frictional Contact, not Bonded Contact.
I know it seems weird to use frictional contact on a shaft and hole, it seems it would just slip out, but that is what the Contact Geometry Correcction = Bolt Thread does, it creates, under the hood, the pressure angle of the thread at the contact surfaces so that the two sides can push against each other when there is an axial load on the shaft.
- 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.