I am trying to construct the existing residual stress in a structure into Abaqus V.6.7 so that I can calculate and consider some structural behaviour on influence of residual stress , say fracture process. Does anyone know how to do this ?!!. I have some knowledge of eigenstrain concept but I do not know the way to implement it into commercial code Abaqus.
Submitted by Joe Kelleher on Fri, 2007-07-27 10:34.
I don't think Abaqus will let you specify eigenstrain directly, or at least it didn't when I last looked at this problem. You can achieve the same effect using thermal expansions, however. At each point that you know eigenstrain, specify the direction-dependent thermal expansion coefficients to be the relevant components of eigenstrain, then raise the temperature of your model by one degree. The stress due to thermal strain misfit should then behave the same as 'real' residual stress with regard to stress redistribution on cutting or cracking etc.
I don't know if and how the fracture mechanics parameters take this misfit stress into account. Also I've not experimented with the 'Initial Conditions' type of residual stress either, and I'm not sure what physical aspects of a residual stress field this simulates. I'd be interested to know about both.
I have already used the keyword: *initial condition, type=stress and type=outputfile for creating residual stress fields. It works well.
I also tested by using alternative thermal stress with isotropic and anisotropic thermal expansion factors but the obtained result were out of control (the values and distribution of thermal stress are different than it should be...) even I spent a lot of time. So I do believe that I should go on by FORMAL way in which the problem of eigenstrain must be formulated in consistent with Abaqus. I am wondering if someone already has experience on this !!?.
Concerning the aspects of residual stress, in my opinion, is is very worldwide and interesting, we can find this in every branches of Mechanics...As far as I know the residual stress makes big influence on Britle Fracture but less on Ductile Fracture, also Residual stress can create the influence on triaxility in Fracture problems.
Submitted by Mingji Wang on Sat, 2007-07-28 02:19.
The residual stress should have a physical cause. It should be better to used ABAQUS to generate it through STEP simulation rather than specifying. The residual stree prescribed by initial condition can be nonequilibrium. If this is the case, ABAQUS will find a 'dstorted' equilibrium state in the following step analysis.
As you said Abaqus will seek for an equilibrium during the step. But, how can we simulate the distortion with free boundary conditions?
We should introduce some boundary conditions in the model in order to avoid numerical singularities. But this will result in a non-physical distorded shape.
Submitted by Mingji Wang on Tue, 2007-09-04 00:36.
If it is free boundary, no residual/plastic deformation or statically determined structure, then I assume there must be som inhomogeneity in either tempature or solvent absorption. Otherwise, as you pointed, there will be no residual stress.
i am new to abaqus software. i just want to ask how can i generate the residual stresses using thermal expansion coefficients using Abaqus software ( a little about procedure) and secondly i just want to use thses calculated residual stress state as an intial condition for my tensile test how can i used that analysis as an intial step for tensile test.
Residual Stress
Dear all,
I am trying to construct the existing residual stress in a structure into Abaqus V.6.7 so that I can calculate and consider some structural behaviour on influence of residual stress , say fracture process. Does anyone know how to do this ?!!. I have some knowledge of eigenstrain concept but I do not know the way to implement it into commercial code Abaqus.
All help or even hints are appreciated very much
regards
Hamanh
Is it prestress?
Is it a prestress like in the steel concrete? It can be easily used in the ANSYS like "pstres,on".
Lee
For residual stress in
For residual stress in abaqus, before defining the load steps, you can use the following keyword:
*Initial conditions, type=stress
<element set name>, residual Sxx value, residual Syy value
Mike
Eigenstrain in Abaqus
I don't think Abaqus will let you specify eigenstrain directly, or at least it didn't when I last looked at this problem. You can achieve the same effect using thermal expansions, however. At each point that you know eigenstrain, specify the direction-dependent thermal expansion coefficients to be the relevant components of eigenstrain, then raise the temperature of your model by one degree. The stress due to thermal strain misfit should then behave the same as 'real' residual stress with regard to stress redistribution on cutting or cracking etc.
I don't know if and how the fracture mechanics parameters take this misfit stress into account. Also I've not experimented with the 'Initial Conditions' type of residual stress either, and I'm not sure what physical aspects of a residual stress field this simulates. I'd be interested to know about both.
Thank you for your
Thank you for your replies,
I have already used the keyword: *initial condition, type=stress and type=outputfile for creating residual stress fields. It works well.
I also tested by using alternative thermal stress with isotropic and anisotropic thermal expansion factors but the obtained result were out of control (the values and distribution of thermal stress are different than it should be...) even I spent a lot of time. So I do believe that I should go on by FORMAL way in which the problem of eigenstrain must be formulated in consistent with Abaqus. I am wondering if someone already has experience on this !!?.
Concerning the aspects of residual stress, in my opinion, is is very worldwide and interesting, we can find this in every branches of Mechanics...As far as I know the residual stress makes big influence on Britle Fracture but less on Ductile Fracture, also Residual stress can create the influence on triaxility in Fracture problems.
Residual stress
The residual stress should have a physical cause. It should be better to used ABAQUS to generate it through STEP simulation rather than specifying. The residual stree prescribed by initial condition can be nonequilibrium. If this is the case, ABAQUS will find a 'dstorted' equilibrium state in the following step analysis.
Equilibrium under residual
As you said Abaqus will seek for an equilibrium during the step. But, how can we simulate the distortion with free boundary conditions?
We should introduce some boundary conditions in the model in order to avoid numerical singularities. But this will result in a non-physical distorded shape.
Residual stress
If it is free boundary, no residual/plastic deformation or statically determined structure, then I assume there must be som inhomogeneity in either tempature or solvent absorption. Otherwise, as you pointed, there will be no residual stress.
Thanks
Hi,
I used this keywords, "*Initial conditions, type=stress" to define residual stress on a region on my model.
can i define node set instead of element set? and how can i exert a parabolic distribution of residual stress in the region?
Thanks
Residual stress generation
Hi,
i am new to abaqus software. i just want to ask how can i generate the residual stresses using thermal expansion coefficients using Abaqus software ( a little about procedure) and secondly i just want to use thses calculated residual stress state as an intial condition for my tensile test how can i used that analysis as an intial step for tensile test.
thanks in advance