Smart questions
Smart answers
Smart people
Join Eng-Tips Forums
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Member Login




Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

Join Eng-Tips
*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

chenxh (Structural) (OP)
30 Jan 03 9:37
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!
Helpful Member!  Drej (Mechanical)
30 Jan 03 17:42
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 (Structural) (OP)
5 Feb 03 18:18
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 (Structural) (OP)
6 Feb 03 12:50
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 (Mechanical)
6 Feb 03 16:45
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") - 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 (Mechanical)
7 Feb 03 4:25
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.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close