Matrix in ABAQUS
Matrices: Stiffness, Mass, Viscous Damping, Structural Damping, Load
- 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.
Extract Element matrices
It is simple and just edit the keywords in input file. As the *STEP in input file, adding the keywords in the last two lines after the definition of step.
** STEP: Step-1 ** *Step, name=Step-1, nlgeom=NO, perturbation *Frequency, eigensolver=Lanczos, acoustic coupling=on, normalization=displacement , , 10., , , *Element Matrix Output,Elset=SET-2, File Name=filename,Frequency=1,Output File=User Defined,Stiffness=Yes,Mass=Yes
Explanation: Elset, means the element set that you want to extract matrix from. File Name, you can name it as what you want and a .mxt file with this name will be generated in your file folder. In a nonlinear analysis, Dload=Yes can be used to extract the load vector from distributed loads on the element. The exact meanings are detailed in keyword *ELEMENT MATRIX OUTPUT in Abaqus Keywords Reference Guide.
Extract Global Matrices
It is also easy to extract global matrix. You need to add the following codes at the end of the input file or adding these lines before or between step definitions. The difference of the positions in input file between the three lies on the matrices after which step.
** *STEP *MATRIX GENERATE, STIFFNESS, MASS *MATRIX OUTPUT, STIFFNESS, MASS, FORMAT=MATRIX INPUT *END STEP
After completing the analysis, two .mtx files with the name jobname_STIF2 and jobname_MASS2 (2 is the location number of the this step, i.e. the second step) will be generated in your file folder. Open the jobname_STIF2 file and you will find texts as follows.
1,1, 1,1, 1.000000000000000e+36 1,5, 1,1, 9.283850055777577e-12 1,6, 1,1, -4.181074365176346e+04
The meaning of the five numbers in a line are respectively:
- Row node label
- Degree of freedom for row node
- Column node label
- Degree of freedom for column node
- Matrix entry
Note 1: It is noted that a step containing the mass matrix must be used to extract mass matrix. For example, the under a *Static step, the equation of structure is Kx=F and is not related to mass, and as such the mass matrix can not be extracted. In this example, a *Frequency step is defined.
All structural analyses apart from static will involve calculation and manipulation of the mass matrix.
Static case: Kx = f
Eigenvalue (modal or free vibration): Ma +Kx = 0
Dynamic (transient): Ma + Cv + Kx = f(t)
Note 2: This keyword is not available in Abaqus/Explicit and the analysis will be terminated.
Codes I often use in abaqus to extract matrices in dynamic implicit analysis
** *STEP *MATRIX GENERATE, STIFFNESS, MASS, STRUCTURAL DAMPING, VISCOUS DAMPING *MATRIX OUTPUT, STIFFNESS, MASS, STRUCTURAL DAMPING, VISCOUS DAMPING, FORMAT=COORDINATE *END STEP