I want to use inistate command to give initial stresses. The initial stresses are due to welding and cutting and i have the distribution over the area but i am not able to give it to the model can some one help with how to give these stresses to the system i am using an I Section and i am using shell elements i also tried with beam elements but it did not work. I want to get the critical buckling load of a column with geometrical and material imperfections.

# Flexural Buckling of Welded High strength steel columns with I sections

- 183 Views
- Last Post 29 May 2020

Hi,

I guess you probably have referred to this website for examples: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_adv/Hlp_G_INSTAPPL.html?q=inistate.

But can you please share an image of the error messages in Solver oupout？Are you using Mechanical or APDL?

Thanks,

Regards,

Wenlong

hi,

i am using mechanical apdl but i am using the user interface of apdl only when i want to change something i use editor my first question is i have a i section and i have residual stresses distributed throughout the section i want to use beam elements 188 for non linear analysis

my question is for beam 188 inistate can be given to cells but i do not know how many cells are there in my i section how to find out how many cells i have in my i section

hi i have successfully used inistate command to get my critical buckling load but now i want to do the non linear analysis i have written a code for it can some one see why it is not converging and how to converge my non linear solution

Hi,

Please provide more information about the simulation as simply knowing "it is not converging" can't help us give you related suggestions.

Regards,

Wenlong

hi I am not able to send you my text file how can I do that

please have a look what is my mistake why it is not converging

Prasanna

hi i am using arc length method but it is not converging can you please check my code and tell me what mistake i am doing

/SOL !! arc-length olmadan nonlinear cozum

ANTYPE,0

PSTRES,ON

NLGEOM,1

NSUBST,1000,10000,1

AUTOTS,0 !!! 0: Auto time step kapali 1: Autotimestep acik

CUTCONTROL,CRPLIMITexp,0.2,0

CUTCONTROL,CRPLIMITimp,0.2,1

CUTCONTROL,PLSLIMIT,0.5

LNSRCH,1

NEQIT,25

PSTRES,1

STABILIZE,CONSTANT,ENERGY,0.0015,NO

SOLVE

Hi Prasanna,

Sorry about my late reply. Your code above looks fine to me. Could you please attach all your code as you did above? That way I can run it and see where goes wrong.

Regards,

Wenlong

! S690 Major and Minor Axis

FINISH ! Exits normally from a processor

/CLEAR,START ! Clears the database

/TITLE,Buckling

/FILNAME,file,0

/PREP7 ! create and set up the model

BCSOPTION,,DEFAULT ! Sets memory option for the sparse solver

bw = 16 ! (mm)

bf = 26 ! (mm)

B1 = 150 ! (mm)

B2 = 150 ! (mm)

D = 150 ! (mm)

t = 16 ! (mm)

L = 4000 ! (mm)

E = 210000 ! (N/mm2)

v = 0.3 !

fy= 690 ! (N/mm2)

N1 = 2 ! NO FOR OFFSET CONTROL

Umax = 60 ! (mm) DISPLACEMENT, STOP CRITERIO IN ARCTRM

imp = L/1000 ! INITIAL IMPERFECTION

TM = 21

! ********************************************************** !

! DEFINE BEAM 188 ELEMENTS

! ********************************************************** !

ET,1,BEAM188 ! Define the element of the beam to be buckled Defines a local element type from the element library

! ********************************************************** !

! MATERIAL

! ********************************************************** !

MP,EX,1,E ! Defines a linear material property as a constant

MP,PRXY,1,v ! Defines a linear material property as a constant

! ********************************************************** !

! SECTION

! ********************************************************** !

SECTYPE ,1,BEAM, I,,2 ! Associates section type information with a section ID number

SECOFFSET , CENT ! Defines the section offset for cross sections

SECDATA,B1,B2,D,bf,bf,bw,0,0,0,0,0,0

! ********************************************************** !

! SET 'KEYPOINTS' COORDINATES

! ********************************************************** !

K,1,0,0 ! Define the geometry of beam

K,2,0,L

K,3,0,L/2

K,4,0,L/4

K,5,0,3*L/4

! ********************************************************** !

! DEFINE LINES

! ********************************************************** !

!Defines a straight line irrespective of the active coordinate system

!L,1,2 ! Draw the line

LSTR, 1, 4

LSTR, 4, 3

LSTR, 3, 5

LSTR, 5, 2 ! Defines a straight line irrespective of the active coordinate system

! ********************************************************** !

! PROFILE MESH

! ********************************************************** !

ESIZE,L/40 ! Set element size to 83 mm

LMESH,ALL,ALL ! Mesh the line

! ********************************************************** !

! COMPLETE PRE -PROCESSING

! START PROCESSING

! ********************************************************** !

FINISH ! Exits normally from a processor

/SOLU ! Enters the solution processor

ANTYPE,STATIC ! Specifies the analysis type and restart status

PSTRES,ON ! Prestress can be accounted for - required during buckling analysis

! ********************************************************** !

! SUPPORT

! ********************************************************** !

DK,1,UX

DK,1,UY

DK,1,UZ

DK,1,ROTY ! Constrain the bottom of beam

DK,2, UX

DK,2, UZ

DK,2, ROTY ! Constrain the top of beam

!Defines DOF constraints at keypoints

! ********************************************************** !

! FORMULAES

!********************************************************** !

FK,2,FY,-1 ! Load the top vertically with a unit load.

! This is done so the eigenvalue calculated

! will be the actual buckling load, since

! all loads are scaled during the analysis.

! ********************************************************** !

! CONFIGURE ELASTIC LINEAR ANALYSIS

! ********************************************************** !

ANTYPE,STATIC ! Specifies the analysis type and restart status

PSTRES,ON ! Specifies whether prestress effects are calculated or included.

SOLVE ! Starts a solution

FINISH ! Exits normally from a processor

! ********************************************************** !

! CONFIGURE ELASTIC STABILITY ANALYSIS

! ********************************************************** !

/SOLU ! Enters the solution processor

ANTYPE,BUCKLE ! Specifies the analysis type and restart status

BUCOPT,LANB,2 ! Specifies buckling analysis options

SOLVE ! Starts a solution

FINISH ! Exits normally from a processor

/SOLU ! Enters the solution processor

EXPASS,ON ! Specifies an expansion pass of an analysis, ON - An expansion pass will be performed.

MXPAND,2,0,0,1,0.001, ! Specifies the number of modes to expand and write for a modal or buckling analysis

SOLVE ! Starts a solution

FINISH ! Exits normally from a processor

/POST1 ! Enters the database results postprocessor

SET,LIST ! Defines the data set to be read from the results file

SET,LAST ! Defines the data set to be read from the results file

PLDISP ! Displays the displaced structure

FINISH ! Exits normally from a processor

/POST1 ! Enters the database results postprocessor

PLNSOL,U,SUM ! Displays results as continuous contours

! ********************************************************** !

! INITIAL IMPERFECTION (BUCKLING MODE)/FILNAME,Plate,0

! ********************************************************** !

!!!! Prepare for nonlinear analysis

/PREP7 ! create and set up the model

*SET,NONSUBST,2 ! HERE BE CAREFULL WHICH MODE YU CHOOSE AS INITIAL DEFL.

UPGEOM,imp,1,NONSUBST,file1,rst ! update geometry for initial deflections ! Adds displacements from a previous analysis and updates the geometry of the finite element model to the deformed configuration

CDWRITE,db,file,cdb ! Writes geometry and load database items to a file

FINISH ! Exits normally from a processor

/POST1 ! Enters the database results postprocessor

PLDISP,0 ! Displays the displaced structure

!NonLinear Buckling

! These two commands clear current data

/TITLE, Nonlinear Buckling Analysis

/PREP7 ! Enter the preprocessor

!The procedure for inistate command must be like this:

! First set initial state datatype, you will implement stress

inistate,set,dtype,stre ! here we tell the program we will implement stress data

! Then implement the initial stress to the cells of associated element.

*SET,nel,40

*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

inistate,define,i,,33,,-0,15*fy

inistate,define,i,,34,,-0,15*fy

inistate,define,i,,35,,-0,15*fy

inistate,define,i,,36,,-0,15*fy

inistate,define,i,,37,,-0,15*fy

inistate,define,i,,38,,-0,15*fy

inistate,define,i,,39,,-0,15*fy

inistate,define,i,,40,,-0,15*fy

inistate,define,i,,40,,-0,15*fy

inistate,define,i,,42,,-0,15*fy

inistate,define,i,,43,,+0,9*fy

inistate,define,i,,44,,+0,9*fy

inistate,define,i,,45,,+0,9*fy

inistate,define,i,,46,,+0,08*fy

inistate,define,i,,47,,-0,408*fy

inistate,define,i,,48,,-0,408*fy

inistate,define,i,,49,,+0,9*fy

inistate,define,i,,50,,+0,9*fy

inistate,define,i,,51,,+0,9*fy

inistate,define,i,,52,,-0,408*fy

inistate,define,i,,53,,-0,408*fy

inistate,define,i,,54,,+0,08*fy

inistate,define,i,,55,,+0,08*fy

inistate,define,i,,56,,-0,408*fy

inistate,define,i,,57,,-0,408*fy

inistate,define,i,,58,,+0,9*fy

inistate,define,i,,59,,+0,9*fy

inistate,define,i,,60,,+0,9*fy

inistate,define,i,,61,,-0,408*fy

inistate,define,i,,62,,-0,408*fy

inistate,define,i,,63,,+0,08*fy

inistate,define,i,,64,,+0,08*fy

inistate,define,i,,65,,-0,408*fy

inistate,define,i,,66,,-0,408*fy

inistate,define,i,,67,,+0,9*fy

inistate,define,i,,68,,+0,9*fy

inistate,define,i,,69,,+0,9*fy

inistate,define,i,,70,,-0,408*fy

inistate,define,i,,71,,-0,408*fy

inistate,define,i,,72,,+0,08*fy

*enddo

! ********************************************************** !

! CONFIGURE NON LINEAR ANALYSIS

! ********************************************************** !

/PREP7 ! create and set up the model

TB,BISO,1,1,2 ! Activates a data table for material properties or special element input

TBTEMP,0 !

TBDATA,,fy,TM,,,, ! Defines data for the material data table.

/SOLU ! Enters the solution processor

N1 = NODE(0,0,L/2) !

DK,3,UX

DK,4,UX

DK,5,UX

DK,2,ROTX

DK,1,ROTX

ANTYPE,STATIC ! Specifies the analysis type and restart status

NLGEOM,ON ! Includes large-deflection effects in a static or full transient analysis

OUTRES,ERASE ! Controls the solution data written to the database

OUTRES,ALL,ALL ! Controls the solution data written to the database

ARCLEN,ON,1,0.0001 ! Activates the arc-length method

! Controls termination of the solution when the arc-length method is used.

ARCTRM,U,Umax,N1,UY

AUTOTS,OFF

DELTIM,100000,50000,200000 ! Specifies the time step sizes to be used for the current load step

CUTCONTROL,CRPLIMITexp,0.2,0

CUTCONTROL,CRPLIMITimp,0.2,1

CUTCONTROL,PLSLIMIT,0.5

TIME,9000000 ! Sets the time for a load step

NEQIT,20 ! Specifies the maximum number of equilibrium iterations for nonlinear analyses.

NCNV,2,60,0,0,0 ! Sets the key to terminate an analysis

CNVTOL,U,60,0.05,0,0.0 ! Sets convergence values for nonlinear analyses

/PREP7 ! create and set up the model

FK,2,FX,18000

FK,2,FY,-9000000

FINISH ! Exits normally from a processor

/SOL ! Enters the solution processor

SOLVE ! Starts a solution

SAVE

/POST26 ! Time history post processor

RFORCE,2,1,F,Y ! Reads force data in variable 2

NSOL,3,2,U,Y ! Reads y-deflection data into var 3

XVAR,3 ! Make variable 3 the x-axis

PLVAR,2 ! Plots variable 2 on y-axis

/AXLAB,Y,LOAD ! Changes y label

/AXLAB,X,DEFLECTION ! Changes X label

/REPLOT

!*IF,ARG1,EQ,0,THEN

!NSEL,S,D,U,-1E20,+1E20

!WhatNodes='CONSTRAINED'

!*ELSEIF,ARG1,EQ,1,THEN

!WhatNodes='SELECTED'

!*ENDIF

!*GET,NumNodes,NODE,0,COUNT

!/POST1

!i=0

!MaxRForce=-1E20

!MaxNode=0

!*DO,n,1,NumNodes

!i=NDNEXT(i)15:56 16/05/2020

!*GET,RForceY,NODE,i,RF,FY

!*GET,RForceX,NODE,i,RF,FX

!*GET,RForceZ,NODE,i,RF,FZ

!RForce=SQRT(RForceX**2+RForceY**2+RForceZ**2)

!*IF,RForce,GT,MaxRForce,THEN

!MaxRForce=RForce

!MaxNode=i

!*ENDIF

!*ENDDO

please help me this is a code for major axis buckling with residual stress and geometrical imperfections

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: https://studentcommunity.ansys.com/thread/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

i checked it but can you please check that as i am using arc length method my initial stresses will be neglected ?

Can you check that if residual stresses are correctly applied ?

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

thanks i am very thankful to you just a small question when i apply initial stresses to the system when i change the pattern but if they are in equilibrium why my ultimate column strength is not changing i mean residual stress distribution should have a effect on the ultimate critical buckling load can you explain why ?

Hi,

Can you make sure your initial stress is applied properly? You can do a small test without any loading, just give enough constraint, then after running the simulation, request a stress plot, does the column have stress at the beginning? I agree that applying initial stress should affect the buckling load.

Regards,

Wenlong

i did that but my displacements are in 10-6 and also

can you send me a snippet to check for residual stresses

Prasanna

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

Ok, so you have a total of 32 cells. In your input, can you make the INISTATE stop at "inistate,define,i,,32,,-0,15*fy".

Also just making sure, did you correct your input to move /prep7 before /solu ?

Regards,

Wenlong

hi

no 32 cells was just an example as you asked me why i am doing it to 72 cells and how do i know where are these cells can you please do a small model run with two different residual stresses to get the buckling loads and check if they are the same or not as for me they are coming same

prasanna

Hi Prasanna,

Sure, I am running a small test and will send the input back to you soon.

Regards,

Wenlong

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

thanks now my results are better

hi can you please tell me if i can have 2 material properties in a beam element

1 for flange and 1 for web but the E modulus of elasticity is different and yield strength also

##### Search

##### Change Language

##### Categories

##### This Weeks High Earners

- peteroznewman 111
- rwoolhou 61
- abenhadj 48
- kkanade 47
- Kremella 35
- tsiriaks 33
- rahkumar 26
- sdeogeka 11
- Wenlong 10
- Emmanuel001 9