June 18, 2019 at 1:19 pmJonathan974Subscriber
I would like to realize an analysis of a beam's response under a 4 point bending test in order to get the curve : Force VS Deflection on a node. It would be a non linear curve I guess.
The beam is composed by 4 materials as shows the picture (2FaceSheets-1Core-2FaceSheets-16Composite)
Unfortunately when I solve the project after have applying my boundaries conditions (I've applied 2 nodal forces and fixed translations on edges of the beam), I get this result :
Maybe this is due to connections between each layers ( I've automatically created contacts area ).
Would it be more coherent to work with ACP system components instead of a static structure ? Using 2D orthotropic propertie for each materials is that correct to get a non linear solution ?
Thank you in advance for your help,
Project is joined,
June 19, 2019 at 2:53 ampeteroznewmanSubscriber
1) Don't use Nodal Force to push down on this beam. The elements are quadratic, which means pushing each node down with an equal force does not result in a uniform pressure along the line of nodes. You can use a nodal displacement instead, but it is better to slice the geometry to get an edge where it is needed.
2) You don't have small enough elements, though you may be limited by the Student license limit of 32,000 nodes.
3) Use Symmetry to solve 1/4 of the problem by slicing the model in half about two plane through the center.
4) Don't use Contact to connect the layers. Use Shared Topology
5) Use SOLSH190 for bending thin layers of material, but you must define the Mesh Control as Sweep and select a Source face to define the through thickness direction and then set Solid Shell as the type of element.
6) Use more than one element through the thickness of the sandwich core layer, which is thicker than all the thin layers.
7) Under Analysis Settings, Change to Auto Time Stepping and set the Initial and Minimum Substeps to 10. Turn on Large Deflection.
Even with all those changes, it is still possible that local buckling of the face sheet is the failure mode and that can be an accurate result, but you will need much smaller elements to see that clearly.
June 19, 2019 at 7:26 amJonathan974Subscriber
Thank you for your answer, I'll try to deal with it.
The core is actually a honeycomb panel, do I need to use specified elements to deal with ?
I let you know results asap,
Thanks ! J.
June 25, 2019 at 2:23 pmJonathan974Subscriber
Hello, I update this topic with a new model,
So I re worked it with ACP, problem is solved but results are not coherent. When I turn off the large deflection option I've got a linear solution (F=k*x) but I would obtain a non linear solution just as F=A*(1-exp(-B*x)) and I am obtaining a kind of simply exponential model which goes to infinity with the large deflection option. So I guess this is not a model problem's (this is a simple 4 points test bending)
Maybe I need to edit a limit before break of something like that ? Or maybe I need to precise non-linearity of materials I use into Engineering Data ?
Here is my modeling plies :
Thank you !
- 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.