Learning Forum

[kramer]

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).

[peteroznewman]

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.

[kramer]

Hi Peter,

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

[peteroznewman]

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.

[kramer]

Ok, did that. Should I set behavior to rigid or deformable? Empirically, deformable seems to give more realistic results.

[peteroznewman]

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.

[kramer]

 

 

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.

 

Deformable:

 

 

[kramer]

Rigid:

[kramer]

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?

[peteroznewman]

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?