Eigenvalues, nonlinear behavior

[user2705]

Dear,

Is there any way to obtain eigenvalues for a problem with nonlinear kinematic hardening?
I am running an example with a user element where I would like to compare eigenvalues before and after imposed loads.

I issue the command after the solution command due to the loads, but I obtain the same values.

Best regards and thanks in advance

[Prof. S. Govindjee]

Eigenvalues of what?  The global stiffness matrix?  An element matrix? A generalized (K,M) eigenproblem?

[user2705]

Dear Professor,

Eigenvalues of a generalized eigenproblem: frame structure on piles subjected to earthquake.

Best regards and thank you very much.

[Prof. S. Govindjee]

FEAP has SUBSpace and ARPAck methods available for solving the such problems on the global system matrices.  SUBSpace is built-in by default.  ARPAck is an add on that you can compile into the code.  The relevant routines are in the packages folder.  See the installation manual and the user manual for further details, but in short you would form the MASS matrix and the TANGent matrix, then compute the generalized eigenvalues with either the SUBSpace or ARPAck commands.

[user2705]

Dear professor,

Thank you for the reply.

I did use subspace command. However, the obtained periods are the same before and after the loads are imposed.
I tried issuing the subspace command after the loads are imposed, and also during the batch command for the loads, I always obtain the same values.

Code: [Select]

Code: [Select]


BATCh
TANGent
MASS
SUBSpace,,3
END

BATCh
  DT,,0.02
  TRANS NEWM
  LOOP,,500
    TIME
    LOOP,,100
TANG,,1     ! Solve problem
    NEXT iter
!PLOT MESH
!PLOT DEFO,50
    NEXT time
END

BATCh
MASS
SUBSpace,,3
END


or

Code: [Select]

BATCh
  DT,,0.02
  TRANS NEWM
  LOOP,,500
    TIME
    LOOP,,100
TANG,,1     ! Solve problem
         MASS
         SUBSpace,,3
    NEXT iter
!PLOT MESH
!PLOT DEFO,50
    NEXT time
END


Best regards

[Prof. S. Govindjee]

I am not sure what you are expecting to see since it is unclear what type of problem you are really solving.  Notwithstanding, You should use the tangent matrix from a converged time step and not within an iteration loop, so as you have it in your first solution algorithm and not your second one.

Also you do need to be careful if you are actually running a dynamical problem with Newmark.  If the problem is dynamical then the matrix that you are seeing from TANG is the dynamic stiffness matrix associated with whatever Newmark parameters you have selected (Kdyn = K + M/(beta dt^2)).  This will provide an effective shift your eigenvalues (you should be able to work it out by hand to see how to interpret the results); the modes shapes should be uneffected.  It is also possible to shift the tangent matrix; if you do this you should try out your work flow on a very basic problem where you know the correct answer.  In particular to convert the dynamic stiffness back to the stiffness you would (after converging) run, MASS then TANG,,,s  where s = 1/(beta*dt^2).

If you problem not dynamic, I would remove the NEWMark command and load your body quasi-statically.  One you have the stiffness you want, then issue MASS and SUBS to get your frequencies and modes.

I would also suggest thinking carefully about what you are trying to accomplish in computing such eigenvalues in a plasticity problem.  If you are interested in vibrational modes, it will be tricky due to elastic unloading and possible plastic loading.

[user2705]

Dear professor,

Thank you for the reply and for the help.
My problem is dynamic. I will try shifting the dynamic stiffness and see what is happening. 

Best regards