Showing results for 
Search instead for 
Do you mean 
Reply

How to select in FEMAP Stress/Strain output at GAUSS points with solid elements?

Hello!,
Field 6 of the PSOLID entry provides you with some control over the stress output location for solid elements. By default, the stress output for the solid elements is at the center and at each of the corner points. If no midside nodes are used, you may request the stress output at the Gauss points instead of the corner points by setting Field 6 of the PSOLID entry to “GAUSS” or 1.
For linear SOL101: Stress and strain output may be requested at the Gauss points (STRESS = “GAUSS” or 1) on the CHEXA and CPENTA elements with no midside grids, on the CTETRA and CPYRAM elements with or without midside grids, and on the CTRAX3, CTRAX6, CQUADX4, CQUADX8 elements.
For nonlinear SOL106/129: Stress and strain output may be requested at the Gauss points on the CHEXA, CPENTA, CPYRAM and CTETRA elements with or without midside grids. The Gauss point locations for the solid elements are documented in “Elements for Nonlinear Analysis” in the NX Nastran Basic Nonlinear Analysis User’s Guide.



In FEMAP still not possible to define the location of stress/strain output at solid elements using the GUI, hopefully available soon in future releases!!. Instead, the user may need to edit the Nastran input deck and modify the PSOLID card by hand.

 

 

The following picture shows the stress results computed in solid elements using the default output location at the center and at each of the corner points:

 

The following picture shows the stress results computed at GAUSS points:

 

 

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/