Nonlinear geometric instabilities using 3D solid elements

[sara.grbcic]

Dear FEAP admins,

I would like to model the problem of "Lateral buckling of a simply supported right-angle frame subjected to in-plane point moments" (Fig 1. attached, taken from ref. [1] ) using 3D geometrically non-linear solid elements integrated in FEAP, using a static and elastic analysis. The system of non-linear equations should be solved using the arc-length solution procedure due to the existence of bifurcation points. Due to symmetry of the problem only half of the problem is modelled. Please find the input file attached (Isolidhalfal.txt). The problem is modelled by applying an in-plane moment through 2 forces of the same intensity but opposite direction in the x-y plane, and a perturbation force in the z-direction. However, even by applying the loading as specified in [1] (and much much higher), when observing the deformed configuration, the non-linear buckling is not manifested.

However, in general, in order to detect buckling, i.e. the critical equilibrium state, we can either check is the determinant of the tangent stiffness matrix on the assembly level equal to zero or do we have a zero eigenvalue (in addition to the 6 rigid body modes) when performing the eigenvalue analysis on the assembly level.

My questions are the following:
1. How to obtain the value of the determinant of the stiffness matrix on the assembly level (not on the element level) in FEAP?
2. How to obtain the eigenvalues again on the assembly level (not on the element level) in FEAP?
3. Is it possible to apply follower load on this problem in order to keep the applied forces always perpendicular to the frame cross-section?

Thanks in advance.

Best regards,

Sara


Reference:

[1] G. Jelenic, M. Saje, A kinematically exact space finite strain beam model - finite element formulation by generalized virtual work principle, Comput. Methods Appl. Mech. Engrg. 120 (1995) 131-161

[Prof. R.L. Taylor]

What is the shape of the buckling mode you are trying to compute.  I seem to recall that it buckles out of the plane, thus, is really 3-d.  Also using 4-node solid elements will be very stiff so not good for beam type behavior.

It is bad practice to output huge number of files before the problem can be solved.  Also doing every iteration is not practical, why?

Can you talk to someone (your professor?) who can help you more.

Doing follower loads is hard with solid elements, one needs a direction to follow.  In addition, reactions at single points lead to large local deformations, which for non-linear material behavior may cause local non-physical behavior. 

[Prof. S. Govindjee]

It should be possible to use 3D elements and compute the frame from Jelenic and Saje.

Getting the global determinant is not particularly easy.  You will have to use TANG,,-1 to compute the
unfactored tangent and then use OUTP,TANG or OUTP,UTAN to get a file with the values.  You can then
read the matrix in to matlab or python etc. and compute the determinant. 

For the eigenvalues you and use TANG,,-1  followed by IDEN followed by SUBSpace or ARPack (if you have built the optional module).

For the follower load, add a 4-node element on the side of the frame and assign it to material 2.  For material 2, use PRESsure with the FOLLower option.  Note it is possible to use FEAP's eigensolver to detect the bifurcation point and then with ARCLength to perturb the solution onto the lowest eigen branch.  In this way you do not need to have the small transverse load out of the plane.

[Prof. S. Govindjee]

Also in Wrigger's book on non-linear finite elements he discusses arclength and the symbols and diagnostic quantities he mentions are the ones that FEAP computes and prints to the screen.

[Prof. S. Govindjee]

Here is link to the wiki page that shows how to branch switch:
http://feap.berkeley.edu/wiki/index.php?title=Branch_Switch