Geometric Imperfections in Ansys

[Ahmedarhman]

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?.

 

[inline6]

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

 

[Ahmedarhman]

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

 

[Ahmedarhman]

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

 

[petb]

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

 

[Ahmedarhman]

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

regards,

Ahmed

 

[Ahmedarhman]

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,

 

[petb]

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.

[pre]! 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[/pre]

hope this helps

petb

 

[Ahmedarhman]

petb,

Thank u again for this helpful example.

regards,
Ahmed