How can different results data be output to the Simcenter Nastran '.f06' and '.op2' files? For example, outputting stress data to one file and displacement data to the other, or outputting the same results data but for different element sets.
Solution
Outputting different results data to the Simcenter Nastran '.f06' and '.op2' files can be achieved using the Simcenter Nastran Case Control Command 'REPCASE'. Please review the information given within the Simcenter Nastran 2019.1 Quick Reference Guide for more detail.
However, in brief:
* the deck entry REPCASE delimits and identifies a repeated output subcase, e.g.:
REPCASE = n
* 'n' must be strictly increasing (i.e., must be greater than all previous subcase identification numbers)
* REPCASE defines a subcase that is used to make additional output requests for the previous real subcase. This command is required because multiple output requests for the same item are not permitted within the same subcase.
* REPCASE may only be used in statics (SOL 101) and normal modes (SOL 103) problems. However, in normal modes, only output for the first mode is obtained.
###
An example use of 'REPCASE' is shown below:
$*
$* Subcase 1 - Static Load 1
$*
SUBCASE 1
LABEL = Subcase - Static Loads 1
LOAD = 1
OUTPUT
STRESS (PRINT,REAL,VONMISES,CENTER) = 2
$*
$* Subcase 2 - Additional Output Request
$*
REPCASE = 2
STRESS (PLOT,REAL,VONMISES,CENTER) = ALL
###
Note that 'REPCASE' is not supported directly from within the Simcenter 3D user interface, but can be inserted into the analysis deck by way of 'user defined text'.
Notes