November 15, 2017 at 3:23 amTrungVNgSubscriber
I am trying to use beam element as the rivet connection between 2 sheet metal parts. I used the fix Join for this connection (picture below)
I would expect that the beam's nodes will be connected to the surrounding nodes of the circle similar to when I use the Circular Beam to connect the part (picture below)
However, beam's nodes do not connect to the surrounding nodes by the end nodes, but by the middle node (picture below).
This problem still persist even when I put 1 beam element. Have you get the similar problem? Why does it occur? and How can I fix it?
Thank you in advance!
November 15, 2017 at 5:17 ampeteroznewmanSubscriber
I don't see any problem, only a choice.
If you use a Beam connection, then you will get a beam element between the centers of the reference and mobile entities you selected.
If you use a Fixed Joint connection, then you will get a single coordinate system at the center of the reference entity, and connection elements to the reference and mobile entities.
If the connection between two parts can be abstracted to have all the forces pass through a single point, then a Fixed Joint is an adequate connection. A Fixed Joint is only appropriate when the two entities are relatively close to each other. Only the X, Y, Z force going through the joint coordinate system origin is available in the solution. The joint coordinate system origin can be edited to be placed between the two entities.
If there is a significant length between the two parts that are connected, and you want to include the bending of the shaft connecting them, then you need a Beam. The axial force and torque in the beam and the shear and moment at each end of the beam are available in the solution. There is no problem if the two entities are far apart.
April 23, 2019 at 4:09 pmtimescavengerSubscriber
"...The axial force and torque in the beam and the shear and moment at each end of the beam are available in the solution..."
OK, but how do you know which end is which? My guess: I is the reference entity and J the mobile entity?
In this page however, they say bending moments and shear forces in beam results refer to Y (I?) and Z (J?) perpendicular planes (being X the beam axis)? Which one is true? And still, how do you know where Y and Z (local) beam directions are?
April 25, 2019 at 11:39 ampeteroznewmanSubscriber
I saw your question, but I don't know the answers. The way I use beams, they are very short, so the results at the two ends are similar and I don't need to know which end is which. You could build a small model with a long beam and see if your guess is correct for how reference and mobile ends are mapped to I and J. The beam axis is the X axis and points from I to J. See plotting element triads below.
I also don't need to know which direction the two shear forces are pointing. I combine the two components into a net shear force by root sum of squares.
You can read the help about a BEAM188 and it says the X axis is the Beam axis. It will show you if you are building this in APDL, you define a third node K, to orient the beam and assign the Y and Z axes. Again, in APDL, there are two command LMESH and LATT to generate the K node automatically. In your small model, you can look at the ds.dat code in the Solution Information folder and see what was done in the APDL code that Mechanical generated.
Most simply, you can plot the Element Triads in the solution and see what direction Y and Z are pointing.
On the Solution Branch, Insert > Coordinate Systems > Elemental Triads and every element will get a triad glyph.
- 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.
- ANSYS Workbench Measuring within Design
- how to improve the inflation quality at sharp corners?
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- How to resolve Mesh Failure
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
- inflation created stairstep mesh at some location
© 2023 Copyright ANSYS, Inc. All rights reserved.