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
RE: Geometric Imperfections in Ansys
RE: Geometric Imperfections in Ansys
regards,
Ahmed
RE: Geometric Imperfections in Ansys
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
regards,
Ahmed
RE: Geometric Imperfections in Ansys
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
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 solvehope this helps
petb
RE: Geometric Imperfections in Ansys
Thank u again for this helpful example.
regards,
Ahmed