How to confirm that Abaqus is incorporating the prescribed geometric imperfections?

[Scard]

Dear All,

I created a certain shell-element based model of a frame structure using Abaqus 6.10.3 software.

The approach that I adopted to incorporate initial geometric imperfections was via the scaling of the first buckling modes.
Thus, I:
(i) Performed a buckling analysis of the model recording the nodal displacements of each buckling mode (Command: *NODE FILE, Global=Yes / U)
(ii) Created a second analysis with two steps named Equilibrium and Riks:
(ii.i) Previous to the following steps, geometric imperfections were incorporated based on the scaling of the first buckling mode (Command: *IMPERFECTION, FILE=<Name of the Buckling job>, STEP=1 / 1,1.32)
(ii.ii) On the first step - Equilibrium, a negligible load (1N) was applied and a static non-linear analysis was carried on. This step was created with the sole purpose of incorporating geometric imperfections and residual stresses (RS not included yet) to allow the structure to find a new equilibrium (situation where an uneven residual stresses distribution is considered)
(ii.iii) On the second step - Riks, a non-linear failure analysis based on the Riks methodology was carried on.

Since my model was built in [mm], I reckon I am considering an imperfect shape equal to the first buckling mode w/a maximum value of displacement of 1.32 mm.

MY QUESTION IS: How can I confirm if that was in fact the imperfect shape adopted in the analysis? When I check the displacement values after the first iteration of the step 1, the maximum displacement of the model has a magnitude of 10^-2 mms (instead of the expected 1.32 mms).... So I am concerned about what Abaqus is in fact assuming...

Thankful in advance.
/sc

 

[ktantheta]

You can tell that the initial imperfections have been incorporated by simply looking at your model in the ODB file before doing anything (ie. don't plot the deformed shape of your model or contours yet). When you open up your ODB file in the visualization module, take a close look at the model that it's displaying. Try very high scale of imperfection so you'll see what I mean. Alternatively, run a model with no imperfections, inquiry a few specific nodes and note their initial coordinates. Then, when you add the imperfections, pick those nodes again and inquiry their initial coordinates again. You will see that the initial coordinates are different because of the initial imperfection. In my models, I've been using solid tet elements, but I'm sure it's the same with shell elements.

 

[Scard]

Thanks for your answer.

Using a high scale factor I was finally able to see the deformed shape. I was surprised to realise that geometric imperfections were already incorporated on step 0 of the analysis.

Btw, did you ever have problems obtaining the descendent part of the force-displacement curve while performing a Riks analysis (and be aware that no warning messages were issues)?

Anyway, I appreciated your help a lot.
/sc