Nonlinear Buckling Analysis after Pretensioning (Wrinkling Study – Patran/Nastran SOL 400)

[Nic0]

Hi everyone,

I'm trying to replicate a wrinkling experiment on solar sails described by Wong and Pellegrino, originally performed in Abaqus. Their simulation procedure involves three main steps:

1. A nonlinear static analysis to apply a pretensioning load.
2. A nonlinear buckling analysis to obtain an initial imperfection or deformed mesh shape.
3. A follow-up nonlinear analysis to apply further loads and study the onset of wrinkling based on the previous buckled shape.

I would like to perform the same simulation workflow in Patran/Nastran using SOL 400, but I’m struggling with one specific part:
How can I correctly pass the pretensioned state from the first step into a nonlinear buckling analysis in the second step?

Is there a way to use the deformed/stressed state from the nonlinear static solution as the starting point or preloaded state for the buckling computation?

Any advice, workflow steps, or examples would be greatly appreciated.

Thanks in advance!

 

[dmapguru]

SOL 400 uses the notion of STEPs in each SUBCASE to define events that occur in a sequence, sometimes called analysis chaining. In this context, the start of a STEP uses the deformed state at the end of a previous STEP, except of course for the very first STEP where the initial conditions are zero. So, to define your nonlinear static analysis with a pretension load which is then subject to a buckling analysis under some other loading, simply define 2 STEPs like this:

SOL 400
CEND

SUBCASE 1
STEP 1
ANALYSIS=NLSTATIC
NLSTEP=1
LOAD=1 $ preload
STEP 2
ANALYSIS=NLSTATIC
NLSTEP=2
LOAD=2 $ preload + buckling load
BEGIN BULK
...

At the end of STEP 1, the preload will be applied and the structure deforms and is stressed. As STEP 2 (in the same SUBCASE) is defined immediately after STEP 1, the initial condition for STEP 2 is the preloaded, deformed state from STEP 1. Be careful; at the end of STEP 1, the structure is under the load defined by LOAD=1 and will be deformed by it. In STEP 2, the LOAD=2 command should reference a set of loads which maintain the preload from STEP 1 and define the buckling load, otherwise the preload will be removed over the STEP 2 (unless that is what you wanted to happen of course).

Once you have the buckled shape, you can either use SOL 400 to define more steps to add more loads (more STEPs), using NLRESTART for efficiency (or run the whole sequence each time), or you could use the IMPERFECT command in a separate job to pick up the deformed geometry to use it for further studies. The difference between these 2 methods is the latter only updates the geometry (GRID point locations) of the model, there is no account for stress state with IMPERFECT; if this is needed, you must use SOL 400 with sequenced (chained) STEPs.

DG