September 30, 2023 at 12:15 am
September 30, 2023 at 10:58 ampeteroznewmanSubscriber
Mesh the rectangle with a single linear element and you will get straight edges.
September 30, 2023 at 1:31 pmjccubisinoSubscriber
Thank you Peter for your quick reply. I am afraid that if I proceed in the way suggested above, the precision of the results would be affected since the plate is in fact a 1500 x 500 mm stiffened plate. Could you please give me any other idea? Thank you.
September 30, 2023 at 3:09 pmpeteroznewmanSubscriber
What are the true boundary conditions and loads applied to it.
How is it possible that those loads and boundary conditions result in straight edges?
If the true deformation results in non-straight edges, why would you want to enforce a non-physical boundary condition?
September 30, 2023 at 8:30 pmjccubisinoSubscriber
Dear Peter, boundary conditions and loads are shown in pictures below (they are referred to the 2nd picture above). Boundary conditions are established by a regulatory body in ship structrural certification therefore I am not sure about the background to require straight edges but usually is because the panel is sorrounded by many other panels, therefore edges are assumed ideally straight.
I tried using simetric conditions in edges B3 a B4 but, in this case, edges can not be loaded. I hope this helps. Thank you in advance.
October 1, 2023 at 1:43 pmpeteroznewmanSubscriber
Use Constraint Equations.
First in geometry, split the surface to create a vertex where you need to control the side of the shape.
In Mechanical, create Remote Points at all the corners and sides that need to be controlled. Mesh with one linear element per body.
Next create Constraint Equations to force the mid point to stay halfway between the corners in the X and Y directions. For example, this equation forces B2 to be halfway between C2 and C3 in the X direction. I used a total of seven Constraint Equations.
Apply other loads and boundary conditions that are needed to deform the part.
The result is the sides remain straight and parallel.
Note that Constraint Equations add stiffness to the part compared with having no constraint equations. Observe below how much larger the deformation is under the same loads without the constraint equations.
October 3, 2023 at 1:58 amjccubisinoSubscriber
Thank you Peter for your help and your time. Your ideas are allways really appreciated.
- 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.