Ansys results extraction in probaility analysis 1

[StrucEng23]

Hi,

I am currently running a nonlinear analysis on a steel frame and then doing a probability design (monte carlo analysis). But I am having trouble with the information i am extracting, as it is incorrect. I have set up in the attached script a section that is meant to pick out the maximum displacement at a particular node, but when i view the results for each analysis, the displacements are too small, could any one please help me understand what am i doing wrong in the script.

Also, I would like to extract the load factor at which the frame fails for each of the frame analysis, but I am not sure how to do this, as this value comes up as time in the analysis, so if anyone could please help me to extract this information it would be much appreciated.

Kind regards

 

[Drej]

It appears that you're doing a non-linear analysis over 500 substeps, but when you retrieve the displacement at a node you are only doing this from the first results set (SET,FIRST), hence why it is likely your displacements will be small.

You will need to run your script in /post26 and use, for example, NSOL to retrieve nodal displacements in an array and then search the array for the max/min value.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[StrucEng23]

Dear Drej,

Thank you for your helpful advice, but I still remain unclear with how I can get the time (load Step) to be extracted like a random output variable (like DMAX), how is this done? The reason I would like to do this is so that i can assess the general load factor at which a particular frame fails with repect to the varying elastic moduli, yield stress and other factors

Thank you

 

[Drej]

In /post26 you'll have to obtain the time history of a displacement at a node using the NSOL command:

NSOL, NVAR, NODE, Item, Comp, Name

Then dump this data to an array. First dimension the array to store the data:

*DIM,

and then VGET this data and put it into the array:

VGET, Par, IR, TSTRT, KCPLX

The array will store the data from the NSOL command. Then, use *VSCFUN (see manual) to obtain the max/min in the array and store these in variables names of your choice.

Hope this helps.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com