I want to extract the element stiffness matrices of an Abaqus modal analysis, so as to post-processing it, in a simpler way, with Matlab. I add the following lines to the end of my Input file to get the output result file which contains the values of the stiffness matrices:
*ELEMENT MATRIX OUTPUT,ELSET=m,STIFFNESS=YES,MASS=YES,OUTPUTFILE=USER
whit this lines, the *.dat file is created, but the file is not in an organized and appropriate format which the stiffness values could be easily extracted. for instance, here are some lines of the result *.dat file:
*MATRIX,TYPE=STIFFNESS
1 ,
2, 3
are you have another approach for this in which for every arbitrary element number the Matlab extract the matrices in the simpler manner? besides *.dat file, is there another file format could be created with the input file ( for example Excel )?
This way you can extract the global stiffness matrix:
*Step, name=Step-1, nlgeom=NO
*MATRIX GENERATE, STIFFNESS
*MATRIX OUTPUT, STIFFNESS, FORMAT=COORDINATE
*LOAD CASE, NAME=LC1
*Cload
l2-1,2,-0.01
*END LOAD CASE
*End Step
The output is a *.mtx file looking like this:
1 1 1.000000000000000e+36
1 3 -5.494505494505494e-01
3 1 -5.494505494505494e-01
...
This format you can load into matlab and recreate the matrix using sparse.
Write following lines before *step in .inp file
For mass matrix:
*STEP, name=exportmatrix
*MATRIX GENERATE, MASS
*MATRIX OUTPUT, MASS, FORMAT=MATRIX INPUT
*END STEP
** STEP: Step-1
For stiffness matrix:
*STEP, name=exportmatrix
*MATRIX GENERATE, STIFFNESS
*MATRIX OUTPUT, STIFFNESS, FORMAT=MATRIX INPUT
*END STEP
**
** STEP: Step-1 (#The above 4 lines need to be added before STEP #)
Hello Julian,
Thank you for your answer. I am able to exactly obtain the stiffness matrix from the steps that you suggested. However, I do not understand the format in which it is written.
How can one use Matlab in order to get a global stiffness matrix from this? I would be extremely grateful if you could help me out!
Hope this may be useful for reading stiffness matrix to MATLAB:
function [matlab_stiffness_matrix] = import_stiffness_matrix_modified(mtx_file)
abaqus_stiffness_matrix = dlmread(mtx_file);
% If number of Dof are 6
matlab_nodes(:,1) = 6*(abaqus_stiffness_matrix(:,1)-1)+ ...
abaqus_stiffness_matrix(:,2);
matlab_nodes(:,2) = 6*(abaqus_stiffness_matrix(:,3)-1)+ ...
abaqus_stiffness_matrix(:,4);
stiffness_values = [abaqus_stiffness_matrix(:,5); ...
abaqus_stiffness_matrix(:,5)];
[matlab_matrix_indices, abaqus_stiffness_value_index] = unique( ...
[matlab_nodes; matlab_nodes(:,2) matlab_nodes(:,1)], 'rows');
matlab_stiffness_matrix = accumarray( matlab_matrix_indices, ...
stiffness_values(abaqus_stiffness_value_index), [], @max, [], true);
The format is a sparse matrix.First column indicates the column index, second the row index and the last one the values at that position. Matlab can handle sparse matrices. If you read in the file and receive those three vectors you can use the command sparse (i,j,v).
Please note, that the result is the GLOBAL stiffness matrix.
Hi Nima Geran malek ,
There are four (4) formats that you can extract the global stiffness matrix. Base on the format selected you can write a simple code to read it into MATLAB.
FORMAT=MATRIX INPUT (default) to specify that the output use the matrix input text format that is consistent with the format used by the matrix definition technique in Abaqus/Standard.
FORMAT=LABELS to specify that the output use the standard labeling format.
FORMAT=COORDINATE to specify that the output use the common mathematical coordinate format.
FORMAT=DMIG to specify that the output use the NASTRAN DMIG-s format.
Regards.
- Badges
- Science topic
- Similar topics
- Mathematics
- Algebra
- Matrix