Stress in Output File

[abaumann]

Hello,
I am a relatively new user, so I will apologize if this has already been covered in a previous post.  Presently, I am trying to compare the stresses in solid elements as determined by finite deformation theory to those determined by small deformation theory.  The stress portions of my output files for finite deformation have the following format:

   Elem.   11-Stress   22-Stress   33-Stress   12-Stress   23-Stress   13-Stress
   Matl.    1-Stress    2-Stress    3-Stress     1-Coord     2-Coord     3-Coord

If I am understanding this correctly, FEAP is first giving me the element number, followed by the component stresses.  Then, on the next line, the material number, followed by the three principal stresses and the cartesian coordinates of the respective element.  Now, when I switch to small deformation theory, the output files take on a different format:

 Elmt 1-coord  11-stress  22-stress  33-stress  12-stress  23-stress  31-stress
 matl 2-coord  11-strain  22-strain  33-strain  12-strain  23-strain  31-strain

This has me a little confused.  There are multiple (8 to be exact) lines each with the same element number.  Am I being given the stresses at the element's (8 noded hexahedral) nodes?  If so, how are the node positions defined with only 2 spatial coordinates?  Is there any way I can get this to display in the same manner as the finite deformation models?  Is there any particular reason why the format would change?  Everything between the two analyses is identical with the exception of one being finite and the other being small.  Also, as the element number increases, FEAP begins to print the element number as a string of asterisks:

 Elmt 1-coord  11-stress  22-stress  33-stress  12-stress  23-stress  31-stress
 matl 2-coord  11-strain  22-strain  33-strain  12-strain  23-strain  31-strain
 - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - -
****   -0.632  4.354E-03  2.484E-04  5.412E-03  7.696E-02  2.073E-03  5.709E-02
   1    4.968  1.770E-07 -1.788E-07  2.688E-07  1.334E-05  3.593E-07  9.895E-06

How can this be avoided?  I am using FEAP Release 8.1.a9.  Thank you for your time.  Again, I am still a bit of a novice, so any help or advice you can give me would be much appreciated.

[FEAP_Admin]

The coordinates reported are the coordinates where the stress are being computed.  These are generally the Gauss points but can be changed by user options (on the material cards).

In both cases you should get the 1,2, and 3 coordinate value of the point where the stresses are computed (it will be 1 and 2 coordinate value if you are doing a 2D problem).

However, ver81 has an omission and the 3-coordinate, while computed, is not printed for the displacement-form small strain element.  You can fix your code by editing the file program/elements/solid3d/sld3d1.f.  Search for 'isw.eq.4' and you will find the code that prints the output.  The variable that you need to add to the print is 'zn'.

[abaumann]

Hey, thanks for the tip!  Is there a quick way to get it to print stress in the element, though, and not the individual gauss points?  If not, does feap just average the gauss point stresses to calculate the element stress?

[Prof. R.L. Taylor]

Yes, FEAP when only single values are reported in solid elements they are averages of all the gauss point stresses in that element.  If more values are needed, a user must add the prints (for example in sld2d1 of the current release all the gauss point stresses are output).

[abaumann]

Alright, would I be correct in saying that there is no way to get a small deformation model to print like a finite deformation model without altering the source code?  I've been looking at it, and I'd rather not change the code if I don't have to.  Thanks again for all the advice!

[FEAP_Admin]

Yes you are correct.  You will need to edit the code if you want it to look exactly the same.

[abaumann]

Thank you!  Another question (and hopefully the last).  I have been using the Drucker-Lode plasticity model.  I recently noticed that the headers of my output files are (significantly?) different between finite and small deformation models.  The finite deformation headers look as I would expect them, listing the Drucker-Lode parameters:
    T h r e e   D i m e n s i o n a l   S o l i d   E l e m e n t

     M e c h a n i c a l   P r o p e r t i e s

     Logarithmic Stretch Stored Energy Function

          Modulus E        1.50000E+04
          Poisson ratio    0.30000
          Bulk Modulus     1.25000E+04
          Shear Modulus    5.76923E+03

          Density          0.00000E+00

          1-Gravity Load   0.00000E+00
          2-Gravity Load   0.00000E+00
          3-Gravity Load   0.00000E+00


        Drucker-Lode Yield function
          Yield stress in tension     :   6.15000E+01
          Yield stress in compression :   1.24500E+02
          Yield function radius       :   6.72227E+01
          Lode angle parameter        :   3.38710E-01
        Linear hardening parts
          Isotropic hardening (H_iso) :   1.50000E+02
          Kinematic hardening (H_kin) :   0.00000E+00


 *WARNING* Non-convex yield function


     C o n s t i t u t i v e    S t a r t

          State       : Elastic
          Formulation : Finite deformation.
          Element type: Displacement


However, for the small deformation models, there is no mention of the Prager-Lode material model, but rather Mises:
T h r e e   D i m e n s i o n a l   S o l i d   E l e m e n t

     M e c h a n i c a l   P r o p e r t i e s

          3-Dimensional Analysis

          Modulus E        1.50000E+04
          Poisson ratio    0.30000

     G a u s s   Q u a d r a t u r e
          Quadrature: Arrays  2
          Quadrature: Output  2

          Density          0.00000E+00

          1-Gravity Load   0.00000E+00
          2-Gravity Load   0.00000E+00
          3-Gravity Load   0.00000E+00


     M i s e s   P l a s t i c   P a r a m e t e r s

          Yield stress short      6.15000E+01
          Yield stress infin.     1.24500E+02
          Hardening exponent      0.00000E+00
        Linear hardening parts
          Isotropic hardening     7.50000E+02
          Kinematic hardening     0.00000E+00


     C o n s t i t u t i v e    S t a r t

          State       : Elastic
          Formulation : Small deformation.
          Element type: Displacement



Is the Prager-Lode material model only functional with finite deformation theory?  Does FEAP automatically revert to generalized plasticity (Mises) in cases of small deformation?  Thanks again for the help!

[Prof. R.L. Taylor]

Yes, Drucker-Lode is only programmed in finite deformation.