Learning Forum

[mpirkle]

When graphing stress-strain results in POST26 for a composite laminate, are the results (see graph below) for the laminate, or for a particular lamina?

 

 

Is there a way to plot stress-strain results for a specific node within a particular lamina (0, +/-45, 90, etc.)?

 

Here is the /POST26 code:

/POST26

SHELL,MID                                                               

ANSOL,3,14944,S,X,SXNODE14944                      

ANSOL,2,14944,EPEL,X,EPSXNODE14944           

/AXLAB,Y,STRESS [MPa]                                        

/AXLAB,X,STRAIN                                                  

PLVAR,3                                                                   

XVAR,2                                                                   

 

Also, I receive the following warning:

 

 

Is this warning cause for concern? If so, how can I avoid it? Should I be using NSOL instead?

 

Any help is greatly appreciated!

 

Thank you!

 

 

[Chandra Sekaran]

To get results for a particular layer, you will need to use "Layerp26" command in Post26. Then you can use ESOL (and ANSOL) to get results for a particular layer. 

https://ansysproducthelpqa.win.ansys.com/account/secured?returnurl=/Views/Secured/corp/v232/en/ans_cmd/Hlp_C_LAYERP26.html

Yes, the warning is important. Post26 does not do coordinate transformations. The ANSOL documentaiton gives the below note:  Shell elements: The default shell element coordinate system is based on node ordering. For shell elements the adjacent elements could have a different RSYS,SOLU, making the resultant averaged data inconsistent. A message to this effect is issued when ANSOL is used in models containing shell elements. Ensure that consistent coordinate systems are active for all associated elements used by the ANSOL command.

 

[mpirkle]

Chandra,

Great! So If I want the results from the middle layer of the shell281 element for node 14944 in the first lamina (0 degree fiber orientation for this lamina), my code should look like this:

 

/POST26

LAYERP26,1

SHELL,MID                                                               

ANSOL,3,14944,S,X,SXNODE14944                      

ANSOL,2,14944,EPEL,X,EPSXNODE14944           

/AXLAB,Y,STRESS [MPa]                                        

/AXLAB,X,STRAIN                                                  

PLVAR,3                                                                   

XVAR,2               

 

 

Do I need to activate the coordinate system using RSYS,11 in POST1, or does it automatically use the coordinate system for the fiber orientation (0 degrees in this case) based upon the LAYERP26 choice?

 

Also, do you know if the ANSOL averaged nodal results are typically preferred for a tensile test stress study?

 

Thank you!                                          

[Chandra Sekaran]

The solver writes element results such as stress/strain in element coordinate system for each element, and nodal results such as displacements in nodal coordinate system. By default the results will be in layer coordinate system.  Layer results are written in layer coordinate system. So Post26 will display results in layer coordinate system. RSYS is not valid in Post26. 

ESOL is the more accurate number to use because there is no averaging. ANSOL is a convenience tool to get average values at a node.You may want to compare ANSOL results against individual element ESOL and see if it makes sense.