nonlinear buckling yielding very high eigenvalues

[jlkono]

The issue is that I am observing in the nonlinear buckling analysis, very high eingen values (close to 100) which appear to be very suspect. On the other hand, when analyzing linear static for shell von mises, I am observing compartively high stresses.

Any advice? Model upoaded.

The model is an internal assembly portion of a floating barge. The barge is sitting in drydock on docking blocks. The load in the analysis is represented by a pressure reaction on the shell bottom resulting from the docking block. Model constraints are around the perimeter of the structure and ends of primary and secondary framing. The girder tops are constrained at the web edge for the purpose of analyzing buckling of the webs. Deadweight is not input since the docking block pressures were predetermined for exerting on the barge.

[John_Holtz]

Hi @jlkono 

Note that the part files are missing, so we cannot view the model. Please zip the part files (.ipt) and attach them to the forum.

Out of curiosity, did you perform a linear buckling analysis? If so, what was the eigenvalue (buckling multiplier)? 

[jlkono]

thank you John. attached is the complete set of files. Yes, I had also run the linear buckling analysis which also was similarly high on the multiplier, but not exactly the same.

[jlkono]

Thank you John. Reply posted with new attachment.

[John_Holtz]

Hi @jlkono 

I am not entirely sure what the model represents compared to the full barge, but your constraints do not make sense to me. Just perform a linear static stress analysis and see if the displacements correspond to what you expect for the real barge.

Constraints an only be applied where the model is attached to the ground or where symmetry occurs.

1. I think your model is a portion of the full model, but there are no symmetry constraints applied. The "No translation" (Tx Ty Tz fixed) along the cut edges do not look correct.
2. I think the girder tops cannot be constrained at the web connection to limit the buckling calculation to the web area. There is nothing in real life holding the web. 

For static stress, you may be able to model a small portion of a complete assembly, put fake constraints at the boundaries, apply a load near the middle, and get reasonable results at the middle of the model. Buckling is a form of modal analysis, so the fake constraints are making the model much stiffer than real life. This increases the natural frequency and the buckling multiplier.

[jlkono]

Thank you John-

For certain I am not grasping the correct concept of constraining the assembly. Ultimately, for that modeled as shown, I want to examining buckling of the girders immediately above the red plate representing the docking block pressure and then in a subcase, the other red block below the bulkheads.

If I were to keep the structural model as is (albeit with extraneous structure) and remove all of my existing constraints, i am now at a loss as to how to resist the bottom pressure from the block and accomplish the tendency for buckling of the girders and bulkheads. Also, I am not understanding the application of symmetry and antisymmetry constraints.

[John_Holtz · Accepted solution]

Hi @jlkono 

I think the load should be gravity, and the constraints are the contact with the support pier and symmetry constraints (if you do not model the entire vessel). This schematic shows the model in simple terms.

1.  The physical vessel sitting on several piers.
2. The simplified engineering model. Although the piers are probably spaced uniformly, the stiffness of the vessel is probably not uniform along the length. In this situation, the maximum displacement may not be centered exactly between the piers. The "symmetry" lines shown in the image are where the maximum displacement occurs (the slope of the displacement is zero).
3. The portion of the vessel modeled. The constraints are the support by the pier and symmetry constraints on the two ends where the model is cut away. 

Note that the Y symmetry constraints on the left and right side are not a completely accurate way to setup the analysis, but I do not know how to do it more accurately. The problem with the two sets of Y symmetry constraints is that they prevent the model from getting longer or shorter in the Y direction. (The Y symmetry constraints prevent the nodes from moving in the Y direction.) The ideal constraints would be Y symmetry on the left side, and the nodes on the right side must translate the same Y displacement (either +Y if the vessel gets shorter, or -Y if the vessel expands due to the displacements). In other words, the nodes on both planes remain in a vertical plane, the plane on the left side does not move, but the plane on the right side can translate in the Y. This setup could be done with a multi-point constraint, but Inventor does not have that capability.

I suggest starting with a static stress test model to get a better understanding of the symmetry constraints. You can create a "full model" on several supports (just a simple block on several supports, nothing fancy), and then do a "symmetry" model on one support. The results should be the same.

[jlkono]

Thank  you John for that. I believe that I am also maybe too deep before grasping some important modeling understandings. I have attached a very simple part of a stiffened bulkhead. Both sides of the bulkhead are cut off from the wider portion. The load is to be compression top and bottom for examining buckling. I have not yet added the load or constraints. Let's say a load of about 5,000 lbs.

Any help on constraints is appreciated.