Results Processed

In FEMVIEW results can be stored related to the nodes (refered to as nodal results), or to the elements (refered to as element results). Nodal results can be materially related or non-materially related types. Nodal related material results allow discontinuities in result data as a set of results is allowed at a node for each material present. Element results can have results at the vertices (nodes) of the element or at the centroid of the element. A summary of the elements and the types of results which can be processed is given in Table 2.

The results written to the FEMVIEW input file by the interface program depend on the result data blocks on the NASTRAN `OUTPUT2' file, the processing options specified when running the interface program and the types of elements used in the model. The rest of this section describes what results can be processed from the recognised NASTRAN data blocks.

Displacements - OUGV1

Displacements are passed to FEMVIEW as non-materially related nodal results. The translational components of displacement are retrieved. If the displacements are output in a local system these are transformed into the NASTRAN basic co-ordinate system. An option exists for the displacements in their local systems to be passed to FEMVIEW. The `OUGV1' data block contains the velocities and acelerations if calculated for transient solutions.

Eigenvectors - OPHIG

The translational components are retrieved and passed to FEMVIEW as displacements. They are differentiated from any true displacements present by starting the loadcase name with an `E' instead of an `L' (see section 3.5).

Forces and moments - OEF1 and OEF1X

Results from plate/shell elements can be passed to FEMVIEW as centroid or vertex element-wise results under the attribute name 'RSTRESS'. Results from beam elements can only be passed back as centroid results under the attribute name `BEAM'.

The `OEF1X' data block differs from `OEF1' in that it contains the corrected values for intermediate points along `BAR' or `BEAM' elements. Results from the `OEF1X' data block are differentiated from those from the `OEF1' data block by starting the loadcase name with an `X' instead of an 'L'. This allows both data blocks to be present in the `OUTPUT2' file.

Forces of single point constraint - OQG1

Grid force balance - OGPFB1

The translational components for the `TOTAL' balance at a grid point are retrieved and passed to FEMVIEW as displacements. They are differentiated from any true displacements present by starting the loadcase name with a `G' instead of an `L'.

Load Vectors - OPG1

Strains - OSTR1

These results can be passed to FEMVIEW as centroid or vertex element-wise results dependant on the user request. The principal strains are not retrieved.

Stresses - OES1

These results can be passed to FEMVIEW as centroid or vertex element-wise results dependant on the user request. The vertex principal stresses for high-order elements can only be obtained if the mid-side nodes are ignored.

An option is available to average the vertex element-wise results to nodal stresses. If this option is choosen averaging is performed within elements refering to the same `PSHELL' or `PSOLID' cards. If 'CQUAD4' or `CTRIA3' elements are present in the model the centroid value is used for the vertex value. If the model contains solid and plate/shell elements it is advised that the `PSHELL' and `PSOLID' cards have unique identifiers to avoid averaging at a node connected to a solid and a plate/shell element.

Surface and Volume Stresses - OGS1

NASTRAN allows for definition of surfaces and volumes in the Case Control deck. Stresses can then be output averaged at the nodes contained within the surfaces or volumes, for details see NASTRAN User Manual volume 1. These results can be passed to FEMVIEW by writing the `OGS1' data block to the `OUTPUT2' file.

Surface and volume stresses are passed to FEMVIEW as materially independant nodal results. Only the nodes specified in the set are passed to FEMVIEW. When contouring these results FEMVIEW will only contour on elements where every node has a value.

Each surface or volume set for each loadcase is passed to FEMVIEW as a seperate loadcase data set, the convention used in naming them is described below.

Composite Stresses - OES1C

Composite Stresses are placed in their own data block, OESC1. If the model contains both composite and non-composite elements the non-composite elements are placed in data block OES1.

Composite Stresses are returned as gaussian results with each ply as a seperate surface. To access the results for a particular ply use the Femview command RESULTS RANGE SURFACE.

Composite Failure Indices - OEFIT

Element Strain Energy - ONGRY1

Element Strain Energy results are passed to FEMVIEW as Gaussian results. with two centroid values for each element.

Element Pressures - OEP

Element Pressures results are passed to FEMVIEW as Gaussian results with a centroid value for each element.

**Table 3.2:** FEMVIEW Nodal Result Types
Element	Displace-	Eigen-	Forces	GridPoint	Load	Nodal^	Surface	Volume
Types	ments	vectors	of SPC	Balance!	Vectors	Stress	Stress	Stress
CBAR	Yes	Yes	Yes	Yes	Yes	No	No	No
CBEAM	Yes	Yes	Yes	Yes	Yes	No	No	No
CHEXA	Yes	Yes	Yes	Yes	Yes	Yes+	Yes	No
CONROD	Yes	Yes	Yes	Yes	Yes	No	No	No
CPENTA	Yes	Yes	Yes	Yes	Yes	Yes+	Yes	No
CQUAD4	Yes	Yes	Yes	Yes	Yes	Yes	Yes	No
CQUAD8	Yes	Yes	Yes	Yes	Yes	Yes+	Yes	No
CROD	Yes	Yes	Yes	Yes	Yes	No	No	No
CTRIA3	Yes	Yes	Yes	Yes	Yes	Yes	Yes	No
CTRIA6	Yes	Yes	Yes	Yes	Yes	Yes+	Yes	No

**Table 3.3:** FEMVIEW Elemental and Gaussian Result Types
Element	Elemental	Principal	Elemental	Elemental
Types	Stresses	Stresses	Strains	Forces
CBAR	No	No	No	Yes"
CBEAM	No	No	No	Yes"
CHEXA	Yes+	Yes'	Yes+	No
CONROD	No	No	No	Yes"
CPENTA	Yes+	Yes'	Yes+	No
CQUAD4	Yes*	Yes*	Yes*	Yes
CQUAD8	Yes+	Yes'	Yes+	Yes+
CROD	No	No	No	Yes"
CTRIA3	Yes*	Yes*	Yes*	Yes*
CTRIA6	Yes+	Yes'	Yes+	Yes+