Limit Load Analysis in Ansys

[csbarone]

I'm new to using Ansys and trying to run a elastic perfectly plastic (EPP) limit load model. I'm coming from using Abaqus where a I would create a static structural run ramp the pressure have output written for each increment so I could visuals results up to failure. I'm trying to do the same in Ansys and having trouble. Any assistance would be appreciated. I've currently created and applied a material with bilinear isotropic hardening (yield strength set to strength limit and tangent modulus to 0), in a transient and static analysis. Both fail as expected but I can not visualize any results.

 

[rickfischer51]

Are running MAPDL or Workbench?

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[rb1957]

that's curious, isn't it ? a limit load NL FEA ??

why not "just" do a linear elastic analysis ?? I mean, you don't want to see any yielding ...

Quando Omni Flunkus Moritati

 

[rickfischer51]

Sounds like ASME BPVC Section VIII Division 2, Part 5, paragraph 5.2 Protection Against Plastic Collapse. Three methods are offered; Elastic, Limit-Load and Elastic Plastic. In the limit-load method, you apply a factored load to a model with an EPP material model, and if the solution converges, you pass. Looks like csbarone is skipping the factored load and just ramping it up until it collapses.

The three methods are listed in order of increasing complexity, increasing accuracy, and decreasing conservativeness. If the design doesnt pass with the elastic method, try the next one. I work on a device that only sees vacuum load, but we use BPVC anyway for lack anything better. If we use elastic method, the walls get too thick, and distortion occurs from welding heat. If we use limit load method, we can pass with a wall thickness that is easier to fabricate.

csbarone: in MAPDL use NSUBST or DELTIM commands to control substeps and determine where you will have results to save. Use the OUTRES command to odetermine which results get saved. Use the SET command on POST1 to load a result set for plotting. In Workbench go to Analysis Settings in the tree. set Auto Time Stepping to ON. Then set Define By to Time or Substeps (this is analagous to DELTIM and NSUBST in MAPDL). Then scroll down to Output Controls and use Store Results At to control which times to save.



Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[rb1957]

i thought NL FEA didn't like perfectly pastic materials ? that the discontinuity at the yield point was too much for the codes to work with. for "protection against plastic collapse" is the point to show that
1) the structure doesn't go plastic (under anticipated loading), or
2) if it did go plastic (under some elevated loading), then it wouldn't collapse

Quando Omni Flunkus Moritati

 

[rickfischer51]

If you take a EPP bar and apply a tensile force, FEA goes ape. But if you have a complex structure and localized areas go perfectly plastic, the load may transfer to the elastic areas and the solution will converge. When the solution doesnt converge, it usually means the structure is unstable and has collapsed.

The goal of protection against plastic collapse is #2.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[inline6]

try using a small non zero number for hardening slope

 

[rickfischer51]

In this case, the tangent modulus should be zero. If the structure is stable, the load will transfer to the non-plastic portion of the structure and the solution will converge. In the case of the BPVC, it specifies a zero tangent modulus and says "The limit load is the load that causes structural instability. This point is indicated by the inability to achieve an equilibrium solution for a small increase in load (i.e. the solution will not converge)."

Rick Fischer
Principal Engineer
Argonne National Laboratory