Nastran laminate results

Output Request	Output Format	Output Result
Force	PCOMP/PCOMPG/PCOMPG1/PSHELL	Shell stress resultants
PCOMPS (Simcenter Nastran only)	Solid element forces
Stress/Strain	PCOMP/PCOMPGNOTE/PCOMPG1	Ply stresses and strainsPly and bond failure indicesPly and bond strength ratiosNOTE
PCOMP/PCOMPGNOTE/PCOMPG1PSHELL	Element stressesElement strains
PCOMPS (Simcenter Nastran only)	Ply stresses and strainsFailure indicesStrength ratiosNOTE

Results coordinate systems

For different objects, the native coordinate system indicates that the results are extracted from the solver results file without transformation. By default, the software displays:

• Shell stress resultant, solid element force, element stress, and element strain results in the native element coordinate system.

• Ply stress and ply strain results in native ply coordinate system.

• Interlaminar ply stress and strain results in the native material coordinate system for 2D elements and native ply coordinate system for 3D elements.

Results locations

Ply results are located at:

• The middle of the ply for 2D elements.

• The middle of the ply, the top and bottom of the ply, or the top, middle, and bottom of the ply for 3D elements. You request the location from the Composite Solid Ply Output list in Structural Output Requests dialog box.

Interlaminar results are located at:

• The top of the ply for 2D elements.

• The top and bottom of the ply for 3D elements.

Elemental, nodal output

For heritage solutions, 2D element ply results are at the element centroid only. They have the string Elemental in the results node name in the Post Processing Navigator.

For heritage solutions, 3D element ply results are at the element centroid and at the element nodes depending on the option you select from the Location list in the Structural Output Requests dialog box.

• When you select CENTER from the Location list, 3D element ply results are displayed at the element centroid, which are identified with the Elemental string in the results node name, in the Post Processing Navigator.

• When you select CORNER or SGAGE from the Location list, 3D element ply results are at both the element centroid and element nodes.The results at the element centroid are identified with the Elemental string in the results node name, in the Post Processing Navigator.The results at the element nodes are identified with the Elemental-Nodal string in the results node name, in the Post Processing Navigator.

For SOL 401 Multi-Step Nonlinear and SOL 402 Multi-Step Nonlinear Kinematics solutions, 2D and 3D element ply results are only at the element nodes, which are identified with the Elemental-Nodal string, in the results node name, in the Post Processing Navigator.

If the Simcenter Nastran ply results are elemental and the post report Element Nodal Results option is set to Element-Nodal, the post report computes stresses at nodes.

Nastran solutions that support ply results

• SOL 101 Linear Statics — Global Constraints

• SOL 101 Linear Statics — Subcase Constraints

• SOL 103 Real Eigenvalues

• SOL 105 Linear Buckling

• SOL 106 Nonlinear Statics — Global Constraints

• SOL 106 Nonlinear Statics — Subcase Constraints

• SOL 108 Direct Frequency Response

• SOL 109 Direct Transient Response

• SOL 111 Modal Frequency Response

• SOL 112 Modal Transient Response

• SOL 114 Cyclic Statics

• SOL 129 Nonlinear Transient ResponseNOTE

• SOL 200 Design Optimization

• SOL 401 Multi-Step Structural SolutionNOTE

• SOL 402 Multi-Step Structural Solution Large Rotations

• SOL 601 Advanced Nonlinear Statics

How do I

View laminate physical properties for a selected element in post processing

Look up more details

Nastran shell stress resultant convention

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Nastran laminate results, Simcenter 3D 2021.1 Series

© 2020 Siemens

PARAM,NOCOMPS = 0 or 1 (default = 1)

PARAM,SRCOMPS = YES (default = NO)

PARAM,NOCOMPS = 0 or -1

PARAM,SRCOMPS = YES (default = NO)

Not available for large displacement analysis.

Used by Simcenter 3D Multiphysics structural and coupled analyses.

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });