×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • 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!
  • Students Click Here

*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.

Students Click Here

Jobs

Geometric Imperfections in Ansys

Geometric Imperfections in Ansys

Geometric Imperfections in Ansys

(OP)
I need a help to apply geometric imperfection in a steel girder by Ansys ...I use Ansys Classic ver 9.00 and want to apply initial out of plan deformations by an an equation equation(sinusoidal function)as an example to the nodes before run the analysis....could i have some helps?.

RE: Geometric Imperfections in Ansys

apply a load to the structure and use the deformed shape as the "initial state"

RE: Geometric Imperfections in Ansys

(OP)
thank you for your help, do you mean applying load out of buckling plan?.

RE: Geometric Imperfections in Ansys

(OP)
I will be grateful if you provide me with an example including the procedures.
regards,
Ahmed

RE: Geometric Imperfections in Ansys

Hi,

Use tabular boundary conditions to deform your geometry/mesh to the desired shape (i.e. use displacement BC:S). A good primer on how to use tabular BC:s using the function builder is available here:
Link

After solving the first displacement load case, return to the pre-processor, then use upgeom to update your geometry to your desired imperfection. Example here:
Link

Hope this helps

petb

RE: Geometric Imperfections in Ansys

(OP)
petb (Marine/Ocean); thank you very much that's what i was searching for

regards,

Ahmed

RE: Geometric Imperfections in Ansys

(OP)
Dear Petb,
I used the example to create the function.
I understood that i can change initial displacements from the the first step (by loading the function).IS this right ?
or can this done with initial conditions (DOF) (It is a fixed value of DOF).
Is Update Geom can be done after the first load step ?
Regard,

RE: Geometric Imperfections in Ansys

Ahmed,

Below is a skeleton for a apdl-input file that you can use as a base, it covers the steps you need to do, and to some extent how you do it. The rest you can find in the manual.

! 	USE the function editor to define a function like this:
!	0.0025*sin(2*{Y}) or whatever you want to do
! 	save as "sinfun" in your working directory
! 	Read function into a table

! /INPUT,sinfun.func,,,1
/prep7
! Apply functional BC:SET
nsel,all !or the nodal set you wish to apply the displacements to
D,all, , %SINS% , , , ,ALL, , , , ,

/solu
solve

! enter the post processing environment
/POST1  ! Check the displacements...
/EFACET,1   
PLNSOL, U,SUM, 0,1.0

! return to prep7 and update geometry, set up the new analysis type
/prep7
UPGEOM,1,LAST,LAST,'file','rst',' ' 

!* New analysis (Eigenbuckling)
ANTYPE,1
!*  
BUCOPT,LANB,1,0,0,CENTER
ddele,all,all,all ! remove all constraints from previous loadstep

! apply boundary conditions and loads for your buckling analysis
/Solu 
solve 

hope this helps

petb

RE: Geometric Imperfections in Ansys

(OP)
petb,

Thank u again for this helpful example.

regards,
Ahmed

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

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!


Resources