Errors - Reinforced Concrete Beam

  • 288 Views
  • Last Post 19 July 2018
Joseph Lim posted this 19 July 2018

Dear all,

Attached are two errors that I encounter when modelling the beam using the Finite Element Method (FEM). May I ask for some suggestions and help with those problems?

The first error is regarding the converge on a solution for the nonlinear problem. May I know why will this happen and how to solve it?

The second error is regarding an internal solution magnitude limit was exceeded. Is that mean that the load applied to the beam was too large or exceed the ultimate load? 

Thank you in advance.

 

Regards,

Joseph 

Attached Files

SandeepMedikonda posted this 19 July 2018

Hi Joseph,

In finite element analyses, all the components are expected to be fully constrained to ensure that the applied forces and the internal forces will balance each other out. The reaction force always follows stiffness and constraints, if there is neither of them to resist an applied force, it results in rigid body motion.

When a model is not fully constrained in Static structural analysis, the solver throws out pivoting error, or errors related to a certain degree of freedom (DOF) exceeding limits. Four ways for identifying the unconstrained body are:

1. If the message appears under the WB messages, right click on the message > Go to Object will take you to the part under Geometry Tree.

2. Identify the node based on the node number provided in the error message. In case the node number is not available in the mesh, it must be an internal node created by Mechanical for features such as remote points, or bolt pretension.

3. Perform a modal analysis on the assembly to identify if there are any 0 Hz (or near zero) modes. If such modes are identified, plot the mode shapes for those modes to identify which parts are free floating.

4. Turn on the Newton-Raphson residuals under Solution information prior to running the model and check the contours for residuals, typically when a part is not constrained, the residuals are distributed all over the problematic part.

Possible Solutions:

  • Once you identify the part, check how is the part supposed to be held in place in the actual physical application.
  • If the internal forces are expected to be self-balancing due to symmetry (e.g., free thermal expansion of parts), then use weak springs (turn it ON under Analysis Settings) or inertial relief for linear models (small deformation, linear materials, linear contacts).

In case the part is to be held in place by contacts:

Linear contacts (bonded and no separation):

  • make sure that there are no initial gaps or penetrations between the parts.
  • If there are any, manually define pinball radius so that it is larger than the gap/penetration. Also, use MPC formulation if there are no other MPC based constraints in the vicinity.
  • Mesh in the contact region is fine enough.

Nonlinear contacts (frictionless, frictional and rough):

  • Change the contact type to Bonded to see if that fixes the issue. If it does, proceed to the following steps. If not, check if the steps listed under linear contacts resolve the issue. If yes, then proceed with the following steps. • If gap is negligibly small, consider using the Interface Treatment Option "Adjust to Touch" to close the gap.
  • Use a small amount of friction so that part will not slide away during loading.
  • In case of force or pressure loading, use smaller initial timestep, increase a pinball radius.
  • If the issue persists, define contact stabilization damping (use a small value such as 5e-2).
  • Mesh in the contact region is fine enough.
  • In case of internal nodes such a bolt pretension, make sure that there is no conflicting constraint equation based definition (e.g., scoped surface sharing bolt pretension and symmetry conditions).

Close