July 30, 2019 at 5:40 pmedoardoSubscriber
I have a problem in simulating a flexible pivot (see the image below). The top plate is fixed, while the bottom plate has a force applied on the edge in -y direction. I need a solution to make the bottom plate rigid (as you can see I get an unrealistic result). I was thinking of splitting the body in 2 pieces, is that possible? In that case, what condition do I need to apply between the 2 parts? Any other possible solution?
I hope my question makes at least a little bit of sense. Forgive me for my lack of knowledge, I'm new to Ansys (using 16.0). If you need any more files/infos let me know. Thanks in advance
July 31, 2019 at 1:22 ampeteroznewmanSubscriber
The best version of this model would be built by having the three surface bodies to represent the flexures. The fixed body doesn't need to exist. Just fix the ends of the flexures where they would connect to the fixed body. The moving body can be a rigid body. Just make it so by changing the setting under the Details for that solid body. Use three fixed joints to fix the end of each flexure to the rigid body.
Make sure you turn on Large Deflection under the Analysis settings.
July 31, 2019 at 7:43 amedoardoSubscriber
thank you for your prompt answer. I have a few more issues.
1) After defining the moving body as rigid, I wasn't able to apply a force on it (I could instead apply a force on the flexure). Instead I applied a remote force with success. Is there any difference between them?
2) Now it seems that I can't mesh the rigid bodies ( I tried with "Full Mesh" on Rigid Body Behavior but Ansys couldn't solve the model). Is there a way around?
Thank you in advance.
August 1, 2019 at 6:35 amedoardoSubscriber
sorry for being redundant: does anyone know how to solve some of my issues? Thank you
August 1, 2019 at 3:13 pmpeteroznewmanSubscriber
August 8, 2019 at 8:35 amedoardoSubscriber
thank you again for your answer.
I'm having trouble changing the solid bodies to surface! Where can I do that? Is the fillet going to be preserved? (I need to modify it to see how the deformation of the model changes).
August 8, 2019 at 11:52 ampeteroznewmanSubscriber
No, the fillet would not be preserved if you choose to use midsurface. In fact, you have to delete them to perform the midsurface operation. You can do that in SpaceClaim under the Prepare tab.
Fillets the size of one wall thickness are not going to change the deformation significantly but if you want to study very large fillets, then you will need to keep the solid body.
August 8, 2019 at 1:36 pmedoardoSubscriber
August 8, 2019 at 4:53 pmpeteroznewmanSubscriber
It's a Warning not an Error, and you can ignore most of these kinds of warnings. It look okay.
September 10, 2019 at 8:40 amedoardoSubscriber
Sorry for bumping this thread, but I have a new question related to it. My purpose here is applying a fixed remote displacement to the bottom plate (let's say 20mm in direction -y, while others dofs are let free). While I mantain this value constant, I wanna increase the thickness of the leafs, to get to the point that the material won't yield.
The problem is that as I enlarge the leafs, the maximum stress value won't change. How is that possible? I was expecting it to get lower, as I increase the thickness of the leafs. Any ideas?
September 10, 2019 at 11:30 ampeteroznewmanSubscriber
Did you try double the thickness of the leaf? I would expect the stress to increase with thickness since you have a fixed displacement.
Is this the model that has the solid elements with the blend radius at the bottom or the shell model?
Please attach the archive if you want me (or anyone else) to take a closer look.
September 10, 2019 at 12:44 pmedoardoSubscriber
I made some changes in the geometry and forgot to update the leafs to shell model, it works as you said. Thank you for pointing out the thickness matter: it makes sense that if I increase the thickness, the structure is more rigid and so I should expect an higher stress under the same displacement. The problem is that I'm used to think with forces rather than displacements
- You must be logged in to reply to this topic.
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
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- 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.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.