June 18, 2020 at 6:25 pmaaaaaSubscriber
I want to get the contact pressure between gear and shaft which are assembled by shrink fit, but when the mesh number increases, the solution (contact pressure) value also increases.
what is the problem where I can not reach the steady solution?
June 18, 2020 at 8:59 pmBhargava SistaAnsys Employee
Could you post a few images of the mesh and the contact settings? As the mesh density increases the contact stiffness increases which in turn may increase the contact pressure too but the % change must reduce as finer mesh is used.
June 19, 2020 at 12:29 pm
June 19, 2020 at 12:34 pm
June 19, 2020 at 1:01 pmWenlongAnsys Employee
Looks like the global mesh number is dominated by regions of the gear teeth, and your contact region mesh is still coarse. Can you try adding a mesh size control to the contact faces and only refine the mesh there?
June 19, 2020 at 9:52 pmaaaaaSubscriberHello Wenlong.
Thanks for your attention.
I tried this, but the problem still exists.
The contact pressure increased also.
June 23, 2020 at 8:46 pmBhargava SistaAnsys Employee
Can you set the pinball radius to 4e-2 mm? This is just to make sure that the contact algorithm detects the penetration and resolves the penetration properly. I picked a value slightly large than the offset value.
June 26, 2020 at 6:35 pmWenlongAnsys Employee
1) I noticed you defined an offset in the contact geometry modification. Why are you applying that? If you insert a positive offset, you are increasing the initial penetration. You can let your initial geometry determine the penetration amount.
2) What if your final version of mesh? Your current mesh looks way to coarse as a starting point of the convergence test.
3) When you output contact pressure, look for average value instead of maximum value to check for convergence, as stress concentration is likely to happen.
4) It makes more sense to compare contact pressure vs. the number of elements in contact instead of the total mesh because your other geometry takes the majority of the mesh number. To find the number of contacts, right click "solution information" --> Insert --> Contact.
5) Furthermore, if you want to test the model, I suggest you remove the teeth of the gear so it becomes a perfect hollow cylinder, and you can compare with analytical solution.
Please let me know if it helps.
FYI, these screenshots are taken from this video:
June 27, 2020 at 3:53 pmWenlongAnsys Employee
February 10, 2023 at 12:48 pmNing XingSubscriber
When we run an interference fit simulation by using two cylinders, what kind of Support needs to be set？
If any Support is not set, the Interface Pressure and Stress are well matched with analytical results, please see Fig.1, Fig,2 and Fig.3.
The Material of the two cylinders is Structural Steel. The inner and outer radius of the inner Cylinder is 25mm and 50mm. The inner and outer radius of the outer Cylinder is 49.8mm and 75mm. The interference fit is 0.2mm.
However, the Deformation is not right, please see Fig.4.
Thanks for your answering.
- 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
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.