I have aquestion regarding the post processing.
The simulation I am working on right now consists of solid laminate/PCOMPS-elements.
I am trying to use the reduction command to use ply stresses and strains to implement Cuntze failure criterion.
For fiber fraction for example the formula would result into: (ABS(PSXX)+PSXX)/(2*RPT) with PSXX the ply stress in 11-direction and RPT the fiber parallel tensile strength.
It’s important, that the stresses used are in the material coordinate system. The coordinate system used as a default for ply stress seems to be the “native” coordinate system.
What I could find out about the “native” coordinate system so far is the following:
Native replaces the Local option used in previous releases of NX. The native coordinate system is the untransformed coordinate system in which results are written to the solver output file. Typically, this is the element coordinate system, but may be some other coordinate system based on the solver, analysis type, or element formulation. Native replaces the Local option used in previous releases of NX. The native coordinate system is the untransformed coordinate system in which results are written to the solver output file. Typically, this is the element coordinate system, but may be some other coordinate system based on the solver, analysis type, or element formulation. - “What’s New in NX8”
I am using the NX Multiphysics Solver with PCOMPS-elements. My question:
I noticed that the option to choose the material coordinate system with the set result -> coordinate system drop down menu wasn’t possible as it was shown grayed out. That is the case for Displacement, Rotation and for Reaction Force and Moment. Furthermore, changing the coordinate system of the ply stress is not possible at all.
Thanks in advance
Solved! Go to Solution.
The native coordinate system (ie, the system used to store the ply stresses in the Nastran results file) is the ply coordinate system, which is rotated from the material system by the angle Theta you define on the PCOMPS card.
Looking at your equation, I'm guessing that 11 is in fact the ply system, which would make sense since ply stress and strain limits are typically defined in the ply direction or normal to it.
Another, perhaps faster way of obtaining Cuntze failure metrics would be to create your own function and linking it with NX Laminate Composites. This process is explained in online help unser 'User-Defined Failure Thoery'.
The ability to transform ply stresses and strains into other coordinate systems will hopefully be supported by a future version of NX.
thanks for your quick an elaborate answer! This was very helpfull!
I found this link describing how you can define your own ply and interlaminar failure theories in NX Laminate Composites: http://mechanicalengineeringblog.tumblr.com/post/122782940509/add-a-user-defined-failure-theory-in-n...
or did you refer to a different source?
I was thinking of the NX online help:
But the link you sent contains the same information, with perhaps a bit more detail.