I am using Abaqus CAE to model a I- 3

[chenxh]

I am using Abaqus CAE to model a I-Section steel Brige Girder. I want to include the residual stress (due to the welding between flange and web) into my model. I've got the distribution pattern of the residual stress and I know how much stress I should put into each element. since there is only one integration point in each element (I am using Shell element S4R and reduced integration), I am thinking I can assign the stress value to the integration point. Does anybody here have some idea how to perform it in Abaqus CAE? I just can't find the command, or, I can't do it at all? Any relpy are welcome, Thanks!

 

[Drej]

I did the exact same thing for my PhD, but using ABAQUS/Standard v5.8, but it won't matter which version of AB you use. If you wish to include residual stresses at the weld, you will have to apply this using a user subroutine (see *USER SUBROUTINES) known as SIGINI. This is a small fortran script used to assign stress values to section points of the shells or any arbitrary element you choose. In it, you will have to state the magnitude of the stress and the location i.e.

if(noel.eq.5.and.kspt.eq.9) then
Sigma(1)=225E6
...
...
...
endif

which will apply residual stress of 225E6 units to the shell (in the '1' direction) at Section Point 9 (KSPT9) at element 5 (check the exact syntax/stress card in the manual, as it's been a while!!). Once you write this, it may be beneficial if you solve the residual stress load in a single step (to obtain equilibrium) - just constrain applicable nodes and let the model gain equilibrium. You can then apply other loads in subsequent steps.

Hope this helps
-- drej --

 

[chenxh]

Hi, Drej,
Thank you for the reply. Right now I'am trying to use
( *initial conditions, type=stress )
to describe the residual stress. Also, I tried to add a static step to obtain equlibrium. But after I run the job, clearly there is no stress at all after that step. Also, the part about Initial Conditions was erased after running. (It was gone from the .inp file.) I can't figure out what was incorrect there. Is there some constrain I need to add in that step? Following is some data line in the input file, do you have some clue? Thanks again!
**
*initial conditions, type=stress
_G5, 40.
**_G5: elset for residual stress 40.0
**
** STEP: Equilibrium
**
*Step, name=Equilibrium
Initial Equilibrium
*Static
1., 1., 1e-05, 1.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=1
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, variable=PRESELECT
*El Print, freq=999999
*Node Print, freq=999999
*End Step
**

 

[chenxh]

Error messgae:
-----------------------------------------------------
***WARNING: in keyword *INITIALCONDITIONS, file "Beam_Test.inp", line 426: Unknown instance id 1
***ERROR: in keyword *INITIALCONDITIONS, file "Beam_Test.inp", line 426: Unknown assembly id
-----------------------------------------------------
But *INITIAL CONDITIONS doesnot require parameters or data about instance or assembly. any idea?

 

[Drej]

Chenxh,

(1) As far as I can tell, if you use the *Initial Conditions keycard, AB will ignore as soon as some other "load" is applied (zero displacement being a "load&quot - hence, you have no residual stress in the model after running. (As these are only initial conditions, it makes sense.) From the information above, it also appears you have no constraints on the model (*BOUNDARY) - you will need these to be zero to obtain equilibrium i.e.

*BOUNDARY
nodes, 1, 6

(zero displacemtn on node set "nodes" in dof 1 to 6)

(2) I would recommend you use the SIGINI method instead as it is the best method for applying a residual stress state in AB.
(3) Also, try and avoid using any named sets using the underscore as the initial character (e.g. use A_G5 not _G5), as AB uses this first character underscore convention for internal files and fortran subroutines.
(4) You are trying to solve in a single step - is the model linear? If not, it would be wise to reduce the initial time step.

Good luck!
-- drej --

 

[corus]

The error regarding missing instance is because Abaqus needs to know the assembly name and instance when you are outside of the assembly defintion. The underscore is used as the initial letter by default in Abaqus for naming sets but you need to name the assembly and instance too. Try using Assembly."Instance name"._G5,40. or Assembly._G5,40. in your set definition, I forget which.