Learning Forum

[Marek11x]

Hey there,
I do a transient structural mechanics in ANSYS Workbench and want to export the results of a defined path for each time step. Can anyone help me with this command?
Thank you so much

[Sandeep Medikonda]

What are you already using?
You can try using something like this:

set,last
set,list
*get,total_sets,active,0,set,nset

[Marek11x]

Hey, thank you for tip,

currently I try it this way, but it doesn't work:

/POST1
set, first
node2=node(100,0,0)
node1=node(100,50,0)
PATH,TPATH,2,30,100
PPATH,1,node1
PPATH,2,node2

PDEF,PfadSigX,S,X,AVG
PAGET,PathData,TABLE
*GET,nline,PARM,PathData,DIM,1 !retrieve the number of values of the paget table
*GET,nsets,ACTIVE,0,SET,NSET
*DIM,PATHSig,array,nline,nsets+1

*do,i,1,nline
PATHsig(i,1)=PathData(i,4)
*enddo
*do,i,1,nsets ! do it for every time
PDEF,CLEAR
PDEF,PfadSigX,S,X,AVG
PAGET,PathData,TABLE
*do,j,1,nline
PATHsig(j,i+1)=PathData(j,5)
*enddo
set,next
*enddo
*MWRITE,PATHsig(1,1),RESULTS_PathSig,txt,,JIK,,, 1 !write it on a file
(98(F15.10))
*CFCLOS

[Sandeep Medikonda]

echo what you have for in 'nline' and 'nsets' and double-check? You are not using the set commands as specified earlier. Refer to the *GET help on what each argument means.

Let's say I want to export 2 columns of data (substep, max equivalent stress) into an external file. 

I would use something as follows (not for the path):

!Beginning of script

set,last

*get,total_sets,active,0,set,nset

*dim,seqv_max,array,total_sets,1

*dim,substep,array,total_sets,1



*do,i,1,total_sets

set,,,,,,,i

*vget,all_seqv,node,,s,eqv

*vscfun,mymax,max,all_seqv

*get,substep(i,1),active,0,set,sbst

seqv_max(i,1) = mymax

*enddo



*cfopen,seqv_data,txt

*vwrite,substep(1),seqv_max(1)

(f3.0,tl1,F10.6)

*cfclose

!End of script

 

[fredjahnert]

I did this and it worked. I had 1503 sets. 

 

SET, first

PATH,TTTPATH,2,30,100

PPATH,1,,5.6896E-22,-2.0355E-21,0

PPATH,2,,5.6896E-22,-2.0355E-21,0.5

PDEF,StrainZ,EPTO,Z,AVG

PAGET,PathData,TABLE

*GET,ndat,PARM,PathData,DIM,1 

*GET,total_sets,active,0,set,nset  

*DIM,PATHStrain,array,ndat,total_sets+1

 

*do,i,1,ndat

PATHStrain(i,1)=PathData(i,4)

*enddo

 

*do,i,1,total_sets ! do it for every time

set,,,,,,,i

PDEF,CLEAR

*del,PathData,,nopr

PDEF,StrainZ,EPTO,Z,AVG

PAGET,PathData,TABLE

*do,j,1,ndat

PATHStrain(j,i+1)=PathData(j,5)

*enddo

*enddo

 

*MWRITE,PATHStrain(1,1),RESULTS_,txt,,,,,  !write it on a file

(1505E)

*CFCLOSE

[bojandimeski1]

I would like to ask you something about the code, that you wrote before. When I use it and compare the results I see that the results, which have been output with APDL differ from those in Ansys Workbench. The equivalent stress in my txt file is always lower that the one in the solution in Workbench. For the last substep in solution I have a value 4798.8 MPa and in txt file is around 2500Mpa... How do I know that the node with the maximum value has been chosen? n