Plastic Collapse of a Beam

[Doodler3D]

All,

I’m working on a simple beam plastic collapse static analysis for some basic benchmarking in Ansys WB. The problem in question is a solid rod (φ = 0.85”, 16” long, σy = 60 ksi) fixed at both ends. A concentrated load acts at the center of the rod at is applied till solver divergence. A mesh size of 0.1” is sufficient for mesh convergence.

Hand Calcs: W[sub]collapse[/sub] = 3070 lbf

a) Beam model, Elastic-Perfectly Plastic Material: W[sub]collapse[/sub] = 3039 lbf

b) Beam model, Elastic-Plastic Material: W[sub]collapse[/sub] = 3125 lbf (At the onset of instability and first bisection, but the solution converges to the applied 5000 lbf load)

c) Brick model, Elastic-Perfectly Plastic Material: W[sub]collapse[/sub] = 3230 lbf

d) Brick model, Elastic-Plastic Material: W[sub]collapse[/sub] = 3421 lbf (At the onset of instability and first bisection, but the solution converges to the applied 5000 lbf load)

NL Material:

Q: Why does the solution continue bisection and converge while using an elastic plastic model? Is there a method to control this feature? The only warning in the log file at the first bisection is “The preconditioned conjugate gradient solver failed to converge, and therefore no solution was obtained. The equation solver is now being automatically switched to the sparse solver (EQSLV,SPARSE) to allow this analysis to continue". I do not get errors for excessive element deformation or large plastic strain increments typically associated with plastic collapse FEA.

Thank you

 

[FEA way]

Which software are you using ? Is geometric nonlinearity enabled ? Doesn't the documentation/knowledge base for your software say anything about how to approach warnings like this ?

 

[Doodler3D]

FEA way, I'm using Ansys, Yes, it's a full nonlinear solution. As far as I know, the error listed above is something to do with Sparse vs PCG solvers. I do not get errors associated with material nonlinearity while using an elastic plastic model (Multilinear isotropic hardening).

 

[centondollar]

Are you using displacement control or load control? Displacement control is preferable for significant nonlinearities (think "wavy", non-monotonous stiffness or stress-strain graphs), while load control will fail to converge in such cases. The iterative method is also of importance: Newton-Raphson cannot handle certain types of snap-through (displacement suddenly reduces compared to previous converged iteration of displacement), while the Arc-Length type methods can solve "almost anything" given proper parameters, element sizes and boundary conditions. Displacement control with arc-length method should be available in Ansys. Try those and see if the issue still persists.

As for the solution method applied to solve the system of nonlinear algebraic equations at each iteration of a load/displacement level, some of them are fast at the expense of a more narrow area of applicability. My advice is to read the Ansys documentation and try out all the equation system solver methods available.

 

[SSCon]

Bisecting occurs when the program can't obtain a solution and it tries again by cutting the load step in half. It's not a concern although it does mean the solution will take longer than necessary.

To avoid bisections you can simply apply the load more gradually. As in, if you applied a load of 10kN at 1s and the model bisected once and then successfully converged, you could use manual sub-stepping and and apply the load in 5kN increments.

 

[GregLocock]

An approach for the hand solution of that should use moment of plasticity method, 4*theta*s*mp=F*L/2*theta where mp is the first moment of area about the neutral axis, and s is the maximum tensile strength of the material. That's an upper bound.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[Doodler3D]

All, thank you for your inputs.

I was curious to know how ANSYS solved the BEAM models with a "close" plastic collapse load, as BEAM188/189 does not support multilinear isotropic material models (section b). I completely overlooked the element formulation conditions that are acceptable for BEAM elements.