May 27, 2021 at 1:23 pmfloatingstonesSubscriber
I'm doing the Static Structural analysis of a floating body. I performed load mapping from Aqwa to apply hydrodynamic pressures on a body and obtain stresses.
From what I've learned, there is no explicit boundary condition for restraining the body. Rather, Weak Springs are turned on in the Analysis Settings.
I understand that Ansys applies weak springs in strong spots of the body to ease rigid body motion. However, it does not fully prevent rigid body motion. For example, I get total deformations of 0.5 m up to 4 m, depending on the wave. Deformations are composed by the body deformation + rigid body motion. I see this motion from the animation of the results.
My questions are:
1) Does this present a problem? That is, should a proper static structural analysis of a floating body present ZERO rigid body motion, or a small amount is acceptable? If so, what is "acceptable"?
2) Is there a way where I can subtract the rigid body motion from the total deformation in order to only know structural deformations?
Any insights on this would be super helpful!May 27, 2021 at 2:02 pmErik KostsonAnsys EmployeeHi
Never looked into this (generally though one would want to have small reactions on the springs ansys adds)
Perhaps has some idea on how to do that.
May 27, 2021 at 2:44 pmMike PettitAnsys Employee
In the pressure mapping process we calculate and apply acceleration components that should balance the resultant forces on a structure due to the mapped hydrodynamic pressures. (These are basically the acceleration RAOs, applied to the structural reference frame.) This is why it is important for the total mass/inertia/CoG to be consistent between the hydrodynamic and structural models.
Ideally these accelerations would exactly balance the hydrodynamic pressures. However, naturally there is some numerical imprecision in the load mapping process, mostly because the hydrodynamic and structural meshes are not identical. Therefore we end up with some unbalanced rigid body acceleration which we need to remove using Weak Springs.
The forces on the Weak Springs boundary condition can be checked by right-clicking on Solution, then Insert > Probe > Force Reaction. The magnitude of the total spring reaction should be 'small' (maybe a few tenths of a percent) relative to the hydrodynamic forces acting on the structure and/or the weight of the structure.
Weak Springs should allow the Static Structural system to solve when it would otherwise complain about unconstrained motions. To cancel out the rigid body motion completely, you can also add Inertia Relief (under Analysis Settings). With this option you should find that the spring reactions drop to zero, but it is useful to try without Inertia Relief first to check that the spring reactions are not large.
Hope this helps!
June 8, 2021 at 11:43 amfloatingstonesSubscriber! You deserve an entire acknowledgment chapter on my thesis for all your help. Inertia Relief is really the solution for eliminating rigid body motions and thus, obtaining only the body deformations on the Total Deformation result. As you said, I'm first trying without Inertia Relief and checking reactions - if they are small, then I ensure that my modelling is okay.
Viewing 3 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
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- 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.