Request Output of the MCT State Variables

Use a text editor to request output for the MCT state variables.

Solution-dependent MCT state variables track the history of certain quantities computed in the Helius PFA User-Defined Material Subroutine. These MCT state variables are not written to the output database file unless explicitly requested in the Abaqus input file. To request MCT state variable output, add the identifying key 'SDV' to the list of output variables requested in the *ELEMENT OUTPUT keyword statement. For example, the following *ELEMENT OUTPUT keyword statement requests that stresses (S), strains (E), and MCT state variables (SDV) be written in the output database file (note that the stresses (S) and strains (E) are not necessary for an analysis, but are included here for demonstrative purposes):

*ELEMENT OUTPUT	
S,E,SDV

It should be emphasized that the number of MCT state variables written to the output file depends on the number of state variables requested by the *DEPVAR statement (refer to the flow chart in the Request MCT State Variable Output for Composite Materials section).

When requesting output, consider the number and location of the section points where the output variables are calculated. In an element containing multiple material layers, the default section points correspond to the top and bottom surface of the element. Thus, the output variables are not available for any of the internal material layers. To view the output variables for each of the material layers within an element, you must explicitly list the section points where the output variables should be computed. As an example, consider a 4 ply composite plate with 3 section points per ply, for a total of 12 section points as shown in the image below. By default, the output variables are only computed for section points 1 and 12 corresponding to the top and bottom surfaces of the element. To view results for each material layer of the element, it is most practical to request that outputs be computed at the mid-surface of each material layer (i.e., section points 2, 5, 8, 11). To request specific section points for the calculation of output variables, add a data line immediately after the *ELEMENT OUTPUT keyword statement. This data line lists the specific section points where the output variables will be computed. For example, the following *ELEMENT OUTPUT keyword statement requests calculation of stress (S), strain (E) and the MCT state variables (SDV) at section points 2, 5, 8 and 11.

*ELEMENT OUTPUT
2,5,8,11	
S,E,SDV

Be aware that Abaqus allows only 16 quantities to be entered on the section point data line of the *ELEMENT OUTPUT keyword statement. For elements containing large numbers of material layers, more than one *ELEMENT OUTPUT keyword statement is required to request all of the desired section points. For example, consider an element with 24 material layers. The following pair of *ELEMENT OUTPUT keyword statements is used to request output at the mid-surface of each of the 24 material layers.

*ELEMENT OUTPUT
2,5,8,11,14,17,20,23,26,29,32,35,38,41,44,47
S,E,SDV
*ELEMENT OUTPUT
50,53,56,59,62,65,68,71
S,E,SDV