Multiple analysis on the same model

[AmilcarPT]

Hi,

I am building a model of a nano structure on Abaqus. The geometry is a simple hexagonal truss that makes a thin bi-dimensional plate, simulating the molecular links of graphene.
In the same model, I want to make 4 diferent analysis, all static with diferent load cases and boundary conditions:
-an extension in the X direction, with a 0 displacement BC on one side, and a unitary displacement on the other.
-the same as above but in the Y direction
-another with both x and y boundary conditions.
-the last one with tangencial displacement on all the plate boundaries

Should i apply all this BC's on the model and propagate/ disable them through 4 diferent steps ? I've read that ABAQUS maintains the results from the previous steps.
What i wanted is that every one of these 4 steps were 4 diferent and independent analysis.

 

[akabarten]

Hi,

If your analysis is linear you can use *LOAD CASE.
See Abaqus documentation: Abaqus Analysis User's Manual, 6.1.4 Multiple load case analysis
If you have nonlinear analysis just define four separate jobs with one step each.

Regards,
Bartosz

VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[AmilcarPT]

Hi Bartosz,

From what I've been reading, if I use several LOAD CASE's in one model for the same job, the outputted results are linearly superimposed. And what i wanted was four separate analysis of one of each particular load case, and not the result of a linear combination of all 4 cases. Should i create 4 separate jobs with one independent step for each one (with its own boundary conditions and loads) ?

Thanks for the help!

 

[akabarten]

Hi,

the outputted results are linearly superimposed

For my understanding results from each load case is save separately in odb file.
You can do superimpose in pre-process after analysis if you want, it is just option.

Should i create 4 separate jobs with one independent step for each one

This will work independent on your type of analysis (linear static, nonlinear static, dynamic, ...) solver type (implicit, explicit) you are using.

Using "load case" can be done only with selected type of the analysis and only with Abaqus/Standard.
The advantage is faster calculation. With four separate analysis you have to invers stiffness matrix four time and this is the most time consuming part of calculation.
With "load case" you invers stiffness matrix only once and next use it with four different loads vector to get four different sets of displacements (results).

Regards,
Bartosz

VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[Mustaine3]

With changing BC I wouldn't use Load Cases and just define 4 linear pertubation steps in one analysis.

As mentioned, in nonlinear situation 4 separate analysis are needed.
If common preload setps existist, separate Restart analysis could be used.

 

[AmilcarPT]

Thanks bartosz, now I understand how to use the load cases. I think in my case, i'll use 4 diferent perturbation steps with one load case each, as the boundary conditions aren't common to all analysis, as Mustaine said (thanks!)

Should i create all the boundary conditions in the base step and then create a load case for each other perturbation step, where i supress, activate each of its boundary conditions ?