Flexural Buckling of Welded High strength steel columns with I sections
-
-
-
-
-
-
-
-
-
-
-
-
-
-
Hi Prasanna,
One issue I can see is in your nonlinear buckling analysis input, you are trying to read in the initial geometrical imperfections from file1.rst, but that file1 does not exist.
To solve this, I think it will be easier if you can:
1. Read the linear buckling input (the first input you shared) into APDL, then click on "preprocessing" on the manual panel --> Archive model --> Write, and save a cdb file.
2. In Workbench, insert an External model component, and import that cdb file you just generated.(make sure the unit system of the external model is correct)
3. Link that external model to a static structural analysis, then link the solution of that static structural analysis to an eigenvalue buckling analysis.
4. Run that eigenvalue buckling analysis, you will generate a file.rst file. You can find it by opening the eigenvalue analysis in Mechanical, right-click on Solution --> open the result folder.
For reference, you can check this website: https://www.simutechgroup.com/tips-and-tricks/fea-articles/221-fea-tips-tricks-post-processing-apdl-ansys-workbench
Moreover, you can also use Workbench to add geometry imperfection (and hopefully that will make your life easier). Please refer to this post for more info: /forum/forums/topic/thin-walled-3/ (you will need to scroll down a lot to see a relevant discussion)
If this file1.rst is not your issue, please feel free to follow up.
Regards,
Wenlong
-
-
Hi,
Yes, the Arc-length method can be used with initial stress. And I just run a small simulation to verify that.
!
1. In your nonlinear buckling input, there is something I don't understand: you are applying your initial stress to 72 cells of the beam section, how do you know there are 72 cells?
2. In your nonlinear buckling input, you have /Prep7 defined after /SOLU. /Prep7 is used to create a model, material, section, and so on and it should be defined before you solve the model.
3. In your nonlinear buckling input, you don't have many parameters defined, such as fy and the vertices. And when I run it, it will show errors like "Vertices not defined".
This is what I did in my test model. I was using Workbench Mechanical.
In the last static structural analysis, I inserted a command snippet and pasted part of your inputs like shown below:
/PREP7 ! Enter the preprocessor
inistate,set,dtype,stre ! here we tell the program we will implement stress data
fy=600 !MPa
! Then implement the initial stress to the cells of associated element.
*SET,nel,40
inistate,set,dtype,stre ! here we tell the program we will implement stress data
*do,i,1,nel ! loop over the elements (nel: number of elements).
inistate,define,i,,,,+0.1*fy ! here you will input cell number and stress value with direction (sxx, syy etc.).
*ENDDO
FINISH
/SOLU
ARCLEN,ON,, ! Activates the arc-length method
DELTIM,0.01,0.0001,0.1 ! Specifies the time step sizes to be used for the current load step
And the stress plot looks like below, you can see the initial stress effect taking place.
To get your input up to running, I suggest you start simple (instead of applying that many INISTATE to every cell, you can apply all the cell the same initial stress, just as a test), start with a small load, and only include necessary solution control commands (like ARCLEN, NLGEOM and DELTIM). Once you get your code running, you can start adding complex behaviors.
Hope this is helpful.
Regards,
Wenlong
-
-
-
-
Hi,
can you have a look at this image by this i know where are the cells and i give them different stress as in my I section the residual stress is variable and it is both in compression and Tension
Please reply to this query
-
HI;
HAVE A LOOK at this
-
-
-
-
Hi Prasanna,
I found the issue in your code, in your INISTATE, you accidently put 0.15*fy as 0,15*fy. After correcting it, the INISTATE works fine now. I attached a small test where I applied INISTATE, hold both ends of the beam and run, now you can see the beam deform under the initial stress, and the stress distribution at different cells.
!ANSYS Command Listing
!Test the INISTATE
FINISH ! These two commands clear current data
/CLEAR
/TITLE,buckling
/PREP7 ! Enter the preprocessor
ET,1,BEAM188 ! Define the element of the beam to be buckled
MPTEMP,,,,,,, MPTEMP,1,0
MP,EX,1,210000 ! Young's modulus (in MPa)
MP,PRXY,1,0.3 ! Poisson's ratio
TB,BISO,1,1,2 TBTEMP,0
TBDATA,,460,21,,,
SECTYPE, 1, BEAM, I, mysec, 1
SECOFFSET, CENT
SECDATA,150,150,150,10,10,10,0,0,0,0,0,0
K,1,0,0 ! Define the geometry of beam (3000 mm high)
K,2,0,3000
L,1,2 ! Draw the line
CM,_Y,LINE
LSEL, , , , 1
CM,_Y1,LINE
CMSEL,S,_Y
ESIZE,300 ! Set element size to 300 mm
LMESH,ALL,ALL ! Mesh the line
fy = 600
*SET,nel,10
*do,i,1,nel ! loop over the elements (nel: number of elements).
inistate,define,i,,1,,+0.08*fy ! here you will input cell number and stress value with direction (sxx, syy etc.).
inistate,define,i,,2,,-0.408*fy
inistate,define,i,,3,,-0.408*fy
inistate,define,i,,4,,+0.9*fy
inistate,define,i,,5,,+0.9*fy
inistate,define,i,,6,,+0.9*fy
inistate,define,i,,7,,-0.408*fy
inistate,define,i,,8,,-0.408*fy
inistate,define,i,,9,,+0.08*fy
inistate,define,i,,10,,+0.08*fy
inistate,define,i,,11,,-0.408*fy
inistate,define,i,,12,,-0.408*fy
inistate,define,i,,13,,+0.9*fy
inistate,define,i,,14,,+0.9*fy
inistate,define,i,,15,,+0.9*fy
inistate,define,i,,16,,-0.408*fy
inistate,define,i,,17,,-0.408*fy
inistate,define,i,,18,,+0.08*fy
inistate,define,i,,19,,+0.08*fy
inistate,define,i,,20,,-0.408*fy
inistate,define,i,,21,,-0.408*fy
inistate,define,i,,22,,+0.9*fy
inistate,define,i,,23,,+0.9*fy
inistate,define,i,,24,,+0.9*fy
inistate,define,i,,25,,-0.408*fy
inistate,define,i,,26,,-0.408*fy
inistate,define,i,,27,,+0.08*fy
inistate,define,i,,28,,+0.9*fy
inistate,define,i,,29,,+0.9*fy
inistate,define,i,,30,,+0.9*fy
inistate,define,i,,31,,-0.15*fy
inistate,define,i,,32,,-0.15*fy
*enddo
/SOLU ! Enter the solution mode
ANTYPE,STATIC ! Before you can do a buckling analysis, ANSYS
! needs the info from a static analysis
PSTRES,ON ! Prestress can be accounted for - required
! during buckling analysis
DK,1,UX
DK,1,UY
DK,1,UZ
DK,1,ROTX
DK,1,ROTY ! Constrain the bottom of beam
DK,1,ROTZ ! Constrain the bottom of beam
DK,2,all
SOLVE
FINISH
/SOLU ! Enter the solution mode again to solve buckling
ANTYPE,STATIC ! Buckling analysis
SOLVE
!*
/ESHAPE,1.0
/POST1 ! Enter post-processor
SET,LIST ! List eigenvalue solution - Time/Freq listing is the
SET,FIRST ! Read in data for the desired mode
PLDISP ! Plots the deflected shape
PLNSOL, S,X
Regards,
Wenlong
-
-
-
- The topic ‘Flexural Buckling of Welded High strength steel columns with I sections’ is closed to new replies.
You are navigating away from the AIS Discovery experience