I have 2 models where the first model is a subpart of the second one. The components of the subpart have the same mesh and geometry in both the models. I have performed stress analysis on the first model and I need the stress field data of a part-instance after the analysis to be given as input in the form of a predefined field(or something similar where the stress exists before the loads) to the same part-instance in my second model. The instance in the second model is undeformed. I only want the stress field as input. Can you please advise me with the relevant resources and methods necessary to achieve this?
It depends on what you want to achieve. If you want to investigate the behaviour of the smaller model in more detail then look up "Submodelling" in the manual.
If you are interested in simulating something like a coupon cut out from a pre-stressed part, then you can use "Initial Conditions" to define the stresses based on the other model, check the manual it is very straightforward to map from the .odb file.
Just understand what you are doing and consider that a stressed part has stresses because of the loads and constraints (be their external or internal for example residual stresses due to forming). If you load your larger model in a purely elastic way then map over the stresses to the smaller part, the first thing that will happen is it will equilibrate the stresses, so you will end up with an unstressed (but deformed part) unless you apply boundary conditions (and possibly loads) to retain the stress.
David Sziroczak , in my situation I need to perform, say as an example, my first model contains a slab geometry part on which I apply loads and temperature, but at the end of the analysis there are no loads but the deformation and stress exist.
The second model is like the slab part is sandwiched between two other parts.Now I want the stress distribution after the first model analysis to exist as an initial condition in the slab of second model.
I used INITIAL CONDITIONS method input as:
INITIAL CONDITIONS,TYPE=STRESS,FILE=stressonly,STEP=2,INC=10
but I am getting the deformations as well. I ran a job without any loads hoping that I would get the first model's stress distribution in the second model without deformation.But it was not the case.
Can you help me how to input only stress?
Dear Manoj Gembali
To be honest, I cant recognized what you said, in Abaqus simulations, we have some options to get to your goal.
If you want stress distributions during the second analysis, in the other word in the current simulation (during it) stress values must be considered:
For this purpose just do the first analysis, after that while you are in the second analysis, add the "first.odb" file in the load module, initial condition section.
On the other wise, if you need stress distributions just for the start of your analysis, it is so easy to manage it, you can create two steps so that at the first of the second step you will have field values that come from the first step.
Manoj Gembali ok I've posted an answer here, but somehow it disappeared, so here it is again.
What you describe is how things should work. The aim of the Abaqus solver is to find equilibrium (static or dynamic) conditions and you pay good money for this feature! As such when you apply stresses to a model, the solver will calculate the strains until the deformations, stresses, internal forces, external forces, constraints, etc. are in equilibrium. Think about it, you can't just apply stresses on a part and expect nothing to happen, the software is too "real" for that. Imagine you can apply a completely random and/or non-equilibrium stress state (with subroutines for example or from a non-converged solution or defining fields, etc.) and you would then want to keep solving from that state and expect the program to work? Whatever you apply initially needs to be equilibrated before anything else can be solved, and that is what causes deformations.
So to achieve a stressed but seemingly undeformed state what you really want to do is to apply the stress on some shape that after the deformations will look like your initial desired shape. You can try to do it by applying -1x the deformation you see after applying the stresses to the mesh, before the analysis starts. In case of small deformations you should end up very close to the desired shape. I have to admit I only had limited success with this approach (I used it to prevent bearing carriers ovalizing due to assembly loads).
Option B is to deactivate the elements on the sides of the "sandwich", deform the core the way you want, then reactivate those elements (*model change if I remember correctly). This way there is no need to map anything, you just continue the analysis in the next step.
David Sziroczak Thank you a lot for explaining why what I have asked is not possible and providing me other options. I have one more query:
I am turning off the NLGEOM as I am working with a crack (XFEM) to get the SIFs and J-integrals, in this case how the results of the first analysis are taken into the assembly for the rest of the analysis? Whether the INITCOND or the model change works best?
If some part of the assembly have crack and first step have these parts only. Then the result taken into full assembly with stress details to the rest of the assembly. Here XFEM method used for finding out SIF. In this case how the results of the first step of the analysis taken into assembly for rest of the analysis?
- Badges
- Science topic
- Similar topics
- Biological Science
- Physiology
- Physiological Processes
- Stress