ABAQUS Civil Engineering - Geometric non-linear analysis eigenvalue error - Steel Framed Structure

[MannoEng]

Hello

Im a Civil Engineering student and im trying to use Abaqus to do a non-linear analysis of a 20-story building with steel frame structure, and for that im running tests with simple structures to validate my modeling method.

The structure im modeling is composed of beam elements for columns and beams and truss elements for the bracing system.

Im using "join+rotation" with UR2 and either UR1 or UR3 constrained depending on the direction of the beam connectors to simulate the connection between beams and columns and using "weld" to simulate the connection between two columns. Im also using a "cartesian+rotarion" with U1,U3 and UR2 constrained connector on all the nodes of a story to simulate the floor as a rigid diaphragm.

For the step im using static,general and so far for a linear analysis my model runs without any errors and gives me the results that i want, i used other software to validate everything too

Im currently having a problem that when i turn nlgeom on and run an analysis i keep getting multiple eigenvalue errors. I dont think this is a buckling problem as the sections im using are fairly robust and none of the elements are lengthy. The loads im applying arent very big either.

Apparently lagrange multipliers can cause eigenvalue errors depending on the situations and connector elements use lagrange multipliers, altho im not sure if that is whats causing the problem for me.

Any chance someone here knows whats causing these problems? Ive been having a really hard time looking for solutions for this problem.

When i submit the job my analysis does complete and the iterations converge, but due to the eigenvalues error im not sure if my results are correct.

 

[FEA way]

Negative eigenvalues are warnings, not errors. So there are no actual errors and the analysis completes ?

From the Knowledge Base:

Certain applications of connector elements. Negative eigenvalue warnings associated with connector elements are sometimes related to the ordering of the system equations and are spurious. If the iteration in which the warnings appear converges, check the magnitudes of the time average force and residual. If the time average force is physically reasonable and the solver controls have not been relaxed, the solution is likely acceptable.

 

[MannoEng]

Indeed the analysis completes, the iterations with negative eigenvalues all converge and the displacement results appear to make sense too, which leads me to think that the results might be correct but im not completely sure.
Ive tried increasing sections, lowering the loads and even adding small artifical damping to help the structure stabilize without affecting the end results too much but none of these seem to completely remove the negative eigenvalue warnings, only decrease them.
Would you say its fair to think that the results i get from the analysis are correct despite the warnings?

 

[FEA way]

What about the forces mentioned in the KB quote ? If you checked all the results carefully and everything looks good without doubts then the warnings likely can be ignored. You would probably have to model the joints differently to avoid them but a different modeling approach doesn’t seem to be necessary.

 

[SWComposites]

Be careful. For a linear buckling analysis, a negative eigenvalue simply means the loads are reversed, not that there is an error. So if reversed loads are possible, then those buckling loads must be considered in the analysis.

 

[MannoEng]

About the KB quote honestly im not too sure about how to check if the time average force is reasonable. I can see the time avg force at node in the message files but im not sure how to interpret this info. For example:

Wjat exactly do thoses values mean and how can i know if they are reasonable or not?

 

[MannoEng]

About reverse loads being possible, is there a way of knowing which load is the one that can cause buckling if reversed? The loads ive applied to this model are gravity loads due to the weight of the building, accidental loads that represent people and other objects inside the building and the wind load.
Is it correct to believe that if none of these loads can be "reversed" in a real life situation there shouldnt be any problems with the analysis?

 

[SWComposites]

It is reversing the entire set of applied loads. So probably not applicable unless wind loads are significantly greater than the gravity loads, in which case you should manually reverse the wind loads as appropriate.

 

[MannoEng]

I see, then onsidering that my final objective is a 20-story building or maybe even more depending on how my tests go the wind loads will be quite considerable.
If i want to test for this possibility then all i need to reverse the wind load as in adding a - in front of the load value to test how the structure reacts if the load is in the opposite directions?

 

[FEA way]

It's just a matter of making sure that the time average force values have a reasonable magnitude. So they shouldn't be on the mN level if it's a large steel structure or on the MN level if it's a tiny micromechanics device, for instance. Basically, they should correspond to the forces in the model.

 

[CHALLENGERSRT]

don't know if this is related...

but as far as "analysis" for roadway engineering specifically say in Revit

How would that go?? Is it beneficial to learn BIM for mechanical engineering??

How can i open up structures on revit and "Apply loads"

I'm still taking a BIM course of course...But i've heard i need to be versatile and learn about a lot more areas than what i may plan to work for.