ANSYS-Listing the element stresses at centroid and Integration Points 1

[HStruct]

Dear FEA gurus,

1. I solve a model for "load step -1"
2. I can get the stresses from this solved model in POST1.
3. I want to apply these stresses as initial stresses in NEXT Load Step which is "Load Step -2" after I make some modifications in the model.

I want to use the command "isfile", which, needs a input file containing stresses at either at ELEMENT Integration points

or at Element centroid (or I dont understand what this means "Element specific locations").

Could you please let me know how I can get a list of stresses at Element centroids and at the integration points of

elements in POST PROCESSOR POST1?

Sincerely,
-HMT

 

[Stringmaker]

HMT,
To my knowledge there is no way to generate an initial stress file from /POST1. I believe that for linear analyses the stress when using ISWRITE is calculated at the element centroid. Whereas, when performing a nonlinear analysis the stresses are calculated at the integration points. I believe the ISFILE command is only valid in load step one. If this is true it won't work on load step two like you're attempting to do. If I were doing this I would create my geometry and then read in a macro:

/INPUT,filename,mac

That macro would look something like this:

/INPUT,filename,db !Read in geometry
/SOLU
!Apply loading and constraints here
ALLSEL
ANTYPE,STATIC !Static Analysis
ISWRITE,ON !Writes Initial Stress File
SOLVE !Solve
FINISH

You should at this point end up with a *.IST file in your working directory. Once you have this issue /CLEAR write another macro to read as input:

/INPUT,filename,db !Same db as above
/SOLU
ISFILE,READ,,,1 !Read in initial stress file with stress results read at integration points
SOLVE
FINISH !Finish load step one

Good luck,
-Brian

 

[HStruct]

Hi Brian,

Thanks alot for addressing my query.

Yeah, I also thought that I could NEVER get the POST1 write the elemental data at centriod or integration point but I thought might be was underestimating the power of ANSYS. Thanks for confirming that.

Yeah thats true that I can't use the ISFILE in 2nd load step but I was also planning to do what u have suggested here, like running another maroc for evry next load-step.

However, the BUGGEST problem is "ISWRITE,ON" writes initial stress data only and only if u have applied any initial stresses on the model. Thus while running the macro 1st time "ISWRITE,ON" wont write any data in the file (thus will creat an empty file bcoz there were no initial stresses applied).

And thats why I would need POST1 to write the data in the way ISFILE recognizes.

Please help me out here if u can think of somthing ...
Sincerely,
-HMT

 

[Stringmaker]

HMT,
Are you certain that you're executing the SOLVE command during load step one? If you aren't this will certainly generate a blank file.

-Brian

 

[Stringmaker]

Correction: Are you certain that you're issuing the SOLVE command after issuing the ISWRITE,ON command? Otherwise Ansys doesn't know to solve the model...hence no initial stress output.

 

[HStruct]

Thanks both, Brian and StringMaker,

Yes, I am certain that I'm givingt "ISWRITE,ON" command after the "SOLVE", however all it creates is like this

!
! ******* INITIAL STRESS FILE file.ist
!

I think that "Iswrite" writes stresses to ".IST" file only if the initial stresses have been applied on the model.

If you guys have worked on this kinds stuff (iswrite, isfile) please tell me if that is correct.

Sincerely,
HMT

here is my code
/prep7
/title, Example of Initial stress import into ANSYS
et,1,PLANE42 ! Plane stress PLANE42 element
mp,ex,1,1.0e9
mp,nuxy,1,0.3

! Define the nodes
n,1
n,2,2.0
n,3,4.0
n,4,6.0
n,5,8.0
n,6,10.0
n,7,,1.0
n,8,2.0,1.0
n,9,4.0,1.0
n,10,6.0,1.0
n,11,8.0,1.0
n,12,10.0,1.0

! Define the 5 elements
e,1,2,8,7
e,2,3,9,8
e,3,4,10,9
e,4,5,11,10
e,5,6,12,11

! Constrain all dofs on all nodes at x=0 to be zero
nsel,s,loc,x,
d,all,all
nall
finish

/solu
!isfile,read,1_Initial_Stresses,txt,,2

outres,all,all

FLST,2,1,1,ORDE,1
FITEM,2,12
F,P51X,FY,1E5

solve
SAVE
iswrite,on
finish

/post1
set,last
prnsol,u
AVPRIN,0, ,
PLNSOL,U,Y,0,1
finish

 

[Stringmaker]

HMT,
Brian and Stringmaker are the same person...me. But your problem is that you need to issue ISWRITE BEFORE issuing the SOLVE command.

/SOLU
!All other solution information here
ISWRITE,ON !Tells Ansys to write out initial stresses
SOLVE !Solve after issuing ISWRITE
FINISH

The ISFILE command is used to read the .ist file into Ansys during load step one. Follow the format of my first posting and you should be successful.

 

[HStruct]

Sorry for the confusion about your name and ID.

Yeah I guess I was making this mistake of either
1. Using iswrite without solve command or
2. Using iswrite after solve.

Thanks for pointing out the mistake n helping me out here, its writing the .ist file now.

Thanks again...
Sincerely,
-Hemant

 

[Stringmaker]

Sure thing Hermant. Also, there is a forum on there dedicated strictly to Ansys. Next time you may want to post Ansys specific questions on there

-Brian