Using Beam Element as Rivet Connection

  • 665 Views
  • Last Post 25 April 2019
TrungVNg posted this 15 November 2017

Hello,

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!

Trung Nguyen

  • Liked by
  • SaisudheerM
Order By: Standard | Newest | Votes
peteroznewman posted this 15 November 2017

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.

Regards, Peter

  • Liked by
  • SaisudheerM
  • timescavenger
timescavenger posted this 23 April 2019

"...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?

peteroznewman posted this 25 April 2019

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.

  • Liked by
  • timescavenger
Close