May 25, 2023 at 5:07 pmkramerSubscriber
In the model below, I always get a solver pivot error although the end node of the beam has a fixed support applied to it. In SpaceClaim, Share Topology is set to "Merge" or "Share" (makes no difference). What is the reason for that? Do I still have to define some sort of connection between the beam and the solid?
Also, I would like to know how exactly the connection between solid and beam is established (since the beam has only one node in the intersection plane while the solid has many).
May 26, 2023 at 1:09 ampeteroznewmanSubscriber
Right click on the Connections folder and Insert a Fixed Joint. Select the flat face of the solid cylinder as the Reference side of the joint and select the vertex of the beam element that is touching that face as the Mobile side of the joint. The joint will allow the face and vertex to be connected in a way that transmits shear forces and bending moments from the solid to the beam.
May 26, 2023 at 6:07 amkramerSubscriber
thanks for your answer. When I select the end vertex of the beam, Body is set to multiple and the joint does not get a green check (selecting the vertex on the other end does work). I assume that is due to the shared topography? Should I disable it? That leaves me a bit confused since in this demo, topography sharing seems to work without extra steps: https://www.ansys.com/de-de/resource-center/video/beam-and-shell-modeling-with-ansys-mechanical
May 26, 2023 at 1:12 pmpeteroznewmanSubscriber
Yes kramer, go back to SpaceClaim and Unshare the geometry. The Joint needs a node at the vertex of the line body that is not shared with a node on the face of the solid.
Shared Topology works between beam and shell elements. It seems confusing why a beam and a solid element doesn’t work, so I will try to explain.
Nodes on beam and shell elements have 6 unknowns (x, y, x, Rx, Ry, Rz), three displacements and three rotations.
Nodes on solid elements have only 3 unknowns (x, y, z), three displacements. That means when a single node on a beam element is shared with solid elements, the beam behaves as if there is a spherical joint at that node because there is no rotational unknown on the solid elements to support rotational loads.
The same problem happens when a straight line at the edge of a surface is shared with a solid: a hinge would be created.
May 27, 2023 at 8:45 amkramerSubscriber
Ok, did that. Should I set behavior to rigid or deformable? Empirically, deformable seems to give more realistic results.
May 27, 2023 at 10:16 ampeteroznewmanSubscriber
Behavior = Rigid forces the solid to behave more like a beam element, since the cross-section of a beam can't change, it can only translate and rotate.
May 27, 2023 at 10:44 amkramerSubscriber
But rigid forces the solid cross section to move as one, right? Thus it would add artificial stiffness. I tried both rigid and deformable. The normal z-stress with deformable is very close to the analytical result (57.3 MPa for a force of 3 kN, a diameter of 20 mm and a distance of approx. 15 mm from load to end of solid), while the result with rigid is almost twice as high.
May 27, 2023 at 10:45 am
May 27, 2023 at 10:48 amkramerSubscriber
By the way, I get the following warning: "Joints are being used in the current analysis with Large Deflection turned Off. Thus, only linearized joint behavior will be considered. If finite rotation and large deflection effects are to be considered, please turn on Large Deflection."
But that should be ok, right?
May 27, 2023 at 2:55 pmpeteroznewmanSubscriber
Rigid elements often cause a stress concentration. That is why they should not be used in a region where accurate stress is needed. You can use deformable if it gives you a better result.
I expect the analytical equation does not account for large deflection.
It looks like there is a face on the solid cylinder where no force is applied. This makes the resultant force move from the center of the solid length. Did you account for that in the analytical result?
What is the analytical equation?
Where are you looking to evaluate the stress?
Is it at the plane where the solid meets the beam? It is recommended to transition from solid to beam at a different location from where you want to evaluate stress.
Is the beam cross-section the same as the solid?
Why are you switching from beam to solid elements?
What is the result if you just use beam elements?
- 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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- 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
- User manual
- 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
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.