Global stiffness matrix

An independent step is required for exporting assembled global stiffness matrix as well as mass matrix, etc.

An example: adding the following step into Abaqus input file jobfile.inp

** Output Global Stiffness Matrix
*Step, name=Global_Stiffness_Matrix
*MATRIX GENERATE, STIFFNESS
*MATRIX OUTPUT, STIFFNESS, FORMAT=MATRIX INPUT
*End Step

Run Abaqus through command:

$ abaqus -job jobfile

The outputs should include a binary file jobfile_X1.sim and a text file jobfile_STIF1.mtx. The binary file can be reread by Abaqus (see this post).

The text output would be a file jobfile_STIF1.mtx, which is a data file like:

Node1, Dof1, Node2, Dof2,  Stiffness value

  101,    1,   101,    1,  9.890109890109926e+01
  101,    2,   101,    1,  3.571428571428572e+01
  102,    1,   101,    1, -6.043956043956079e+01
  102,    2,   101,    1, -2.747252747252749e+00
  103,    1,   101,    1, -4.945054945054909e+01
  103,    2,   101,    1, -3.571428571428572e+01
  104,    1,   101,    1,  1.098901098901063e+01
  104,    2,   101,    1,  2.747252747252750e+00
  101,    2,   101,    2,  9.890109890109926e+01
......

Using a Python script with following functions, it is possible to convert the mtx file into a COO sparse matrix file following Matlab ASCII format:

def idx_conv(a,b):
    if b==3:
        return a*b
    else:
        return (a-1)*3 + b


def proc_mtx(fn_in,fn_out):
    fin = open(fn_in, 'r')
    fout = open(fn_out, 'w')
    for line in fin:
        line = line.split(',')
        v = float(line[4])
        i = idx_conv(int(line[0]),int(line[1]))
        j = idx_conv(int(line[2]),int(line[3]))
        fout.write('{0},{1},{2}\n'.format(i,j,v))
        if i!=j:
            fout.write('{0},{1},{2}\n'.format(j,i,v))
    fout.close()
    fin.close()

The output file will look like:

row, column,  value
  1,      1,  4.01340706825e-36
  2,      1,  5.60098743107e-37
  1,      2,  5.60098743107e-37
  3,      1, -5.22761524367e-37
  1,      3, -5.22761524367e-37
  4,      1, -2.07870246255e-37
  1,      4, -2.07870246255e-37
  5,      1, -3.62444662193e-38
  1,      5, -3.62444662193e-38
  6,      1, -3.18133224619e-37
  1,      6, -3.18133224619e-37
  7,      1, -6.63360514036e-37
  1,      7, -6.63360514036e-37

An alternative approach is to modify the line

*MATRIX OUTPUT, STIFFNESS, FORMAT=MATRIX INPUT

into

*MATRIX OUTPUT, STIFFNESS, FORMAT=COORDINATE

The output will be the same as the results generated from the Python script.

This works both for linear and nonlinear analysis. For the nonlinear case, the stiffness matrix is available only between steps since it requires an additional step to output.

Element stiffness matrix

The element stiffness matrix can also be output with a step as

*STEP, name=Test
*STATIC
*FILE FORMAT, ASCII
*ELEMENT MATRIX OUTPUT, ELSET=FRAME, FILE NAME=Stiffness, FREQUENCY=1, OUTPUT FILE=USER DEFINED, STIFFNESS=YES
*END STEP

The result file will be only Stiffness.mtx, which looks like:

**
** ELEMENT NUMBER 11 STEP NUMBER 2 INCREMENT NUMBER 1
** ELEMENT TYPE CPS4
*USER ELEMENT, NODES= 4, LINEAR
** ELEMENT NODES
** 101, 102, 103, 104
1, 2
*MATRIX,TYPE=STIFFNESS
98.901098901099 ,
35.714285714286 , 98.901098901099
-60.439560439561 , 2.7472527472527 , 98.901098901099
-2.7472527472527 , 10.989010989011 , -35.714285714286 , 98.901098901099
-49.450549450549 , -35.714285714286 , 10.989010989011 , 2.7472527472528
98.901098901099 ,
-35.714285714286 , -49.450549450549 , -2.7472527472527 , -60.439560439561
35.714285714286 , 98.901098901099
10.989010989011 , -2.7472527472527 , -49.450549450549 , 35.714285714286
-60.439560439561 , 2.7472527472528 , 98.901098901099
2.7472527472527 , -60.439560439561 , 35.714285714286 , -49.450549450549
-2.7472527472527 , 10.989010989011 , -35.714285714286 , 98.901098901099