June 29, 2021 at 5:46 amHaiquanSubscriber
I was performing a simple compression simulation for a metal spring. I found confused result in case 1 as shown below.
I applied displacement in case 1, due to insufficient constraint, the moment should be unbalanced and the spring should rotate, this should cause convergence issue unless I put a block to prevent such rotation. But simulation shown no rotation in spring and it converged! I checked the moment equilibrium carefully and found that the acting point of reaction force of displacement was not in the location where displacement was applied, it was near the middle of the spring as shown in the red arrow in case 1.
In case 2, I used a tool to apply displacement instead of applying it directly on spring, this was more realistic, the spring rotated. That is why I put a block to prevent such rotation. Deformation shape in case 2 matches the reality!
My question is why the acting point of reaction force of displacement is not in the location where displacement is applied?June 29, 2021 at 12:07 pmAkshay ManiyarAnsys Employee
In first case your model is not fully constraint, so solver would have created weak springs and tried to converge it. That is why you are not able to see any rotation in first case. You can try switching off weak springs and try running again. (analysis settings
June 29, 2021 at 12:11 pm1shanAnsys Employee"I checked the moment equilibrium carefully...... the middle of the spring as shown in the spring" - How did you arrive at this conclusion? You could simply insert a force/moment reaction probe and check if they balance out. When you apply a fixed displacement in Z, all nodes at the scoped geometric entity translate in Z together. This implies that the scoped faces cant rotate, because if they do then each node would have a different z displacement. In case 2 rotation is possible because there is no constraint which restricts this movement.
June 30, 2021 at 2:47 amHaiquanSubscriberThank you very much for your comment. I checked the week spring, it is turned off by default
Thank you very much for your comment. For the force and moment balance, they are balanced as shown below. Why I said the acting point of reaction force of displacement moved to center of the spring is based on this calculation: 169.89Nmm/31.798mm=5.3mm as shown below. The displacement reaction force is not at the location where displacement is applied(16mm), how Ansys still gets this balance result? This is what I feel confused.
Yes, I agree the scoped faces cannot rotate as this is displacement load. So If I donÔÇÖt introduce the tool, what should I do if I want to have a Z direction displacement, should I apply in an edge, or use remote displacement instead?
June 30, 2021 at 3:11 ampeteroznewmanSubscriberHello You should use a Remote Displacement on that face, leave 5 DOF Free and only apply the Z displacement.
July 3, 2021 at 8:05 amHaiquanSubscriberThank you very much for your comment. Remote displacement works well.
Viewing 5 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?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- 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.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.