Displacement from subcases

[lingdeer]

Hi, I have a very stupid question about Nastran structural analysis.

I have one solution with different subcases. Is the displacement obtained from each subcase relative to the original mesh? Or relative to the previous subcase?

Thanks!!!

 

[Naffoussi]

Dear lingdeer,

In Nastran you can define the same output results for all subcases, or specific output for each subcase.
Here is an example of requesting the same output for all subcases:

CEND
DISPLACEMENT(PLOT) = ALL
SPC = 1
SUBCASE 1
SUBTITLE = TITLE1
LOAD = 1
SUBCASE 2
SUBTITLE = TITLE2
LOAD = 2
BEGIN BULK

Requesting different output for each subcase:

CEND

SPC = 1 $the same boundary conditions for all subcases
SUBCASE 1
DISPLACEMENT(PLOT) = ALL $request displacement results only for subcase1
SUBTITLE = TITLE1
LOAD = 1
SUBCASE 2
SPCFORCE(PLOT) = ALL $request spcforces only for subcase2
SUBTITLE = TITLE2
LOAD = 2
BEGIN BULK

To learn more about how defining an analysis and setting the outputs refers to the Quick Reference Guide. You can find it in the Nastran directory.

Hope this help,
SN

Seif Eddine Naffoussi, Stress Engineer

http://www.Innovamech.com

33650 Martillac – France

 

[nlgyro]

It depends on what kind of an analysis you are doing.

For a SOL 101, nastran treats every subcase as a separate analysis, and the displacements that you obtain would be with reference to the un-deformed configuration.

For a SOL 106, having multiple subcases would mean that the deformed configurations from the previous subcase would be the starting point for the next subcase ( i.e. updated structural stiffness is passed b/w subcases)