Linear buckling analysis of the shell

[Zhang]

Dear FEAP Users，
     I have been trying to use FEAP for linear buckling analysis of the shell, so as to calculate its buckling load. The geometric and physical parameters of the shell are as follows:
     H=2000mm, R=500mm, t=1mm, E=70000MPa, v =0.3, the boundary condition is clamped–clamped supports, and the compression load is 1MPa.
     FEAP can calculate its eigenvalues, but I don't know how to obtain the corresponding buckling load through the eigenvalues. The input file and the calculation results of eigenvalues are attached respectively.

Matrix: Eigenvalue                   
row/col     1           2           3           4           5           6
 1  -5.2751E+09  5.1169E+09  4.4137E+09  4.2952E+09 -4.2513E+09 -4.1328E+09
 2   1.7177E+08  1.7168E+08 -1.2035E+08  1.1218E+08  8.3460E+06 -9.6111E+04

     How can I calculate the buckling load of the shell through the data above? Of course, if there are any problems about the input file, please point them out.The problem has puzzled me for a long time, and I would be very grateful if you could answer it!

     Thanks for your support.

[Prof. S. Govindjee]

Your solution algorithm needs to be adjusted.  First solve for the in-plane stresses, then form the geometric tangent, then solve for the eigenvalues.
There were some other errors in your file which I have fixed (see the comments).

[Zhang]

According to the input file you modified, I recalculated the eigenvalues again. Here are the results of shell under the 40 elements.

 SUBSPACE: Current eigenvalues, iteration  25
        3.18503804D+04   3.82592597D+04   3.82592597D+04   7.92176686D+04
        7.92184636D+04   1.15715340D+05   1.28207836D+05   1.28207836D+05
        1.97111927D+05   1.97113944D+05   2.14913187D+05   2.17457334D+05
        2.17491606D+05   2.23736453D+05   2.24992593D+05   2.25172064D+05
        2.39837154D+05   2.40452789D+05   2.50346387D+05   2.61911983D+05
  SUBSPACE: Current residuals,   iteration  25
        1.29495943D-15   1.55552897D-15   1.29627414D-16   1.34199951D-16
        6.71006487D-16   1.96029411D-15   8.68770090D-16   2.82350279D-15
        7.88041148D-09   3.12076462D-08   1.43251185D-05   2.78371012D-06
        9.32812883D-05   9.25206820D-05   9.19578302D-06   3.90323335D-04
        1.80059628D-04   6.86403031D-04   8.42997980D-04   1.81707041D-02

1.As the above data show, Is the buckling load 3.18503804E+04 MPa?
2.When I increased the number of shell elements from 40 to 176, I found that the eigenvalues changed apparently. In other words, the results of eigenvalues are unstable. How can I obtain the stable eigenvalues ( buckling load ) ?
3.The following data is the results of shell under the 176 elements and I have attached its input file.

   SUBSPACE: Current eigenvalues, iteration  25
        4.07979300D-01   4.16258037D-01   4.42142250D-01   4.42147607D-01
        4.45398738D-01   4.45400507D-01   4.50431587D-01   4.59450138D-01
        4.78220053D-01   4.78311575D-01   5.09994947D-01   5.11203709D-01
        5.12252024D-01   5.14368554D-01   5.19938059D-01   5.20246885D-01
        5.30266270D-01   5.41071507D-01   5.65411865D-01   5.75674117D-01
  SUBSPACE: Current residuals,   iteration  25
        6.55948115D-08   5.46061503D-07   1.21272725D-06   8.09749784D-06
        6.32561628D-07   2.67493639D-06   1.20414227D-05   1.06855172D-05
        1.09074839D-05   7.97362584D-05   3.25227467D-05   2.46535822D-04
        3.02715976D-04   1.26529010D-03   1.30125007D-04   2.27510689D-04
        2.02327284D-03   1.16972042D-03   1.87545062D-03   4.45849720D-05

[Prof. R.L. Taylor]

First, you need to have a valid mesh to solve the problem.  It must not have rigid body modes, otherwise you are computing a value of zero (which is not zero due to numeriical roundoff).

Secondly, you need to understand what the fundamental buckling mode will be to have a sufficiently refined mesh to get an accurate solution.

Thirdly, the buckling mode will be the value of any applied load you use to compute the prebuckling forces times the eigenvalue you compute.

[Prof. S. Govindjee]

Convergence is probably the main issue.  Your original mesh was exceedingly coarse.  Perform a mesh refinement study; the value should converge.

[Zhang]

I got it, professor. Thank you very much for your help

[Prof. R.L. Taylor]

Linear buckling theory only works for certain shell problems.  For example probably not well for your shell that has end restraints that cause bending near the ends.  You need very fine mesh there and then the eigenproblem becomes numerically ill- conditioned.  Also, the post buckling response may have significant loss in load.

[Zhang]

Thank you for your reminder. I will notice.

[Zhang]

Dear Professors :
      I reset the size of the shell and the magnitude of the compression load, then start the linear buckling analysis. The basic parameters and input file of the shell are attached respectively.   
      However, When I run the program, the software flashed back and did not display the displacement graph. Is there any problem with my input file ?
      Secondly, I view the outcome file, the first-order eigenvalue is 1.61292786D-03. How can I calculate the first-order buckling load through the first-order eigenvalue ?

SUBSPACE: Current eigenvalues, iteration  25
        1.61292786D-03   1.61292786D-03   1.61824894D-03   1.63024382D-03
        1.64753667D-03   1.73237177D-03   1.73237177D-03   1.84065034D-03
        1.92481159D-03   2.11252474D-03   2.17983119D-03   2.17989550D-03
        2.27531134D-03   2.29483192D-03   2.39357803D-03   2.39424821D-03
        2.57570845D-03   2.57786481D-03   2.64855485D-03   2.75457523D-03

[Prof. S. Govindjee]

In your input you are applying nodal forces F_A = int_elements N_A(s) N_z(s) ds = 1.0e6 at each node on the ends of the tube.  So the total load is Applied_Load = N_edge_nodes*1.0e6.  If you multiply this by the lowest eigenvalue, that will then be the buckling load for your shell.

If you plan to perform such computations, I suggest you invest in a book on shell/plate buckling, say, the book by Brush.  Separately a good FEA book will help, maybe the Zienkiewicz and Taylor series or the book by T.J.R. Hughes which explicitly covers buckling.  It is important to understand the fundamentals as it will greatly help you perform meaningful analysis.

PS: The shell you have meshed is not the shell you are analyzing.  Your FEA mesh is a prismatic tube with an octogonal-like cross-section (not a perfect octogon).  Your PDF file shows a circular tube.