Inital stress as a predefined field

[PeteTranc]

I am trying to define a stress field as a initial condition. My procedure
Analysis 1 - Job-1:

Step-1: load "elasto-plastic deformation"​

Step-2: unload "residual stress visible"​

Created a set of all elements:​

*Elset, elset=Set-all, instance=Part-1-1, generate​

1, 100, 1​

Analysis 2 - Job-2: (copy of Analysis 1)

Perscribe initial condition - stress as: (in Job-2.inp)​

*Initial Conditions, type=stress, file=Job-1, step=2​

Set-all​

I have also tried to define initial stress as initial state eg:

Analysis 3 - Job-3: (copy of Analysis 1)

Abaqus CAE-Predefined fields-Initial state (Initial step), Job name: Job-1 Step:last Frame:last​

Results: in the Analysis 2 there are no initial stresses. In the Analysis 3 there are initial stresses, but I have lost the possibility to manipulate the nodes and elements in the .inp file, which is crucial for my goal.

Any sugestions?

 

[ISC214]

PeteTranc,

Does the data or message file contain any warning that may give a clue why you don't see any initial stresses in Analysis-2?

I am actually struggling with the same problem. In my case, I am using beam elements (B21). I did a static analysis to reach to the residual stress field that I want (using subroutine SIGINI). Then created another analysis (explicit/dynamic) and tried to initialize the stresses using the odb of the first analysis. Unfortunately, Abaqus says this procedure can be used only with continuum elements and initial stresses will be ignored. When I check the second analysis there is no initial stress (seems similar to what you have?).

I am currently looking for a workaround. It would be nice if someone can point the right direction.

Thanks in advance...

 

[PeteTranc]

I have finaly came up with a solution. The problem was in my argument to define initial stress to a defined set of elements Set-all. Abaqus seems to do that automatically (if meshes are the same), therefore leaving the argument blank successfully applies the initial stress imported from a external .odb. E.g:

Analysis 2 - Job-2: (copy of Analysis 1)
Perscribe initial condition - stress as: (in Job-2.inp)
*Initial Conditions, type=stress, file=Job-1, step=2

ISC214: I also recieve a message in the .dat file explaining that only continuum elements can be used in conjuction with initial stress, others will be ignored. Before predefined field -> mechanical -> stress I described the initial stress concentration as predefined field -> other -> Initial State (see Analysis 3), but I presume that this is somewhat similar to inital stress, therefore not applicable to non-continuum elements.