Learning Forum

[BenediktaSchmidt]

Hi,

I want to study a compressed beam in Ansys Mechanical APDL. To model the beam I used shell elements.

But, in order to run the analysis, I need to prevent rigid body motions of the beam. How can I do it? Which constraints should I use?

[peteroznewman]

What do you mean by a "compressed beam"?
When a beam experiences a bending moment, one side goes into tension and the opposite side goes into compression. Is that what you mean?
There are multiple ways to apply a bending moment to a beam. You can do a cantilever beam with an end load, you can do three or four point bending, you can apply a pure moment. You have to say how you want to load your beam first, since the supports that prevent rigid body motion will change depending on the load you want to apply.

[BenediktaSchmidt]

I want to simulate a beam compressed by both sides (on the web and on the flanges). The problem itself doesn't need any constraint, because it is auto-equilibrated, but to run analysis on Ansys I need to prevent the rigid body motion (translations ad rotations). I hope I was clear enough :) .

[peteroznewman]

Select all the edges on the -X and use a Remote Displacement, Behavior = Deformable, then set all six DOF to 0.0 to hold one end fixed without adding any stiffness and have no forces at the -X end. Only apply forces at the +X end.
Another approach is to have no constraints and turn on Inertia Relief, then you can have equal and opposite forces.
A final approach is to have equal and opposite forces but pick just three vertices on the flange. The bottom vertex at the left end can have 0,0,0 for X,Y,Z. The bottom vertex at the right end can have Y and Z set to zero displacement then finally pick a top node at the left end and set Z = 0.

[BenediktaSchmidt]

I already tried by picking just three vertices on the flange. By doing this I notice that the reaction forces at the fixed boundary conditions (i.e. the supports) are very close to zero, and I think that means that the choice of the boundary conditions was correct. Although this I'm not sure if by proceeding with this method it's possible to run a non-linear analysis (or an eigenvalue analysis), because I keep receiving the warning that the solution does not converge and I've read on the internet that a limitation of the 3-2-1 method is that it is not applicable to non-linear geometry cases. Is that true?

[peteroznewman]

The 3-2-1 method can be used in a large displacement nonlinear solution for a shell element model. The problem for solid elements would be the stress singularity that is created by selecting three points. But in a case with reaction forces that are very close to zero, that would not be a problem.
An eigenvalue analysis will run with a 3-2-1 method of constraint.
There are many reasons a nonlinear solution fails to converge. You have to look at why it failed to converge. What is the specific error message near the end of the Solution Output text listing?