Subsections

• Element-wise Results
• Element-wise Multi-Surface Results
• Node-wise Results
• Node-wise Multi-Surface Results
• Whole Model Results

Results Processed

ABAQUS outputs results in either an elementwise or nodewise manner dependant on the results type. This interface program will transfer both types of results.

Element-wise Results

Element-wise result output is requested from the ABAQUS program using the `*EL FILE' command in the ABAQUS input file. The location of the results output is specified in the ABAQUS input file using the `POSITION = ' option on the `*EL FILE' command. This interface program will transfer results at all ABAQUS positions except `REBAR'. The FEMVIEW locations to which these results are transferred is given in Table 2.1.

Abaqus Results FEMVIEW Results

Location Identifier

Integration Points GAUSSIAN

Centroid INVARIANT

Nodes ELEMENTAL

Averaged at Nodes NODAL

Appendix B contains an alphabetical list of all the ABAQUS element-wise results that can be processed by the interface program. The attribute and component names allocated to the results for use within FEMVIEW are also listed.

Notes:

• For 'CAXA' and 'SAXA' type elements, the gaussian and invariant results are not supported, the program issues a warning message if such result is present.
• In a model with more than one class of elements (structural, thermal, electrical ...) it is advisable to restrict the output of element type-dependent variables only to the elements to which they apply to. For example, the results for variable ECD (electrical current density) in a model containing both DC2D8E elements (coupled thermal-electrical elements) and DC2D8 elements (heat transfer), will be processed by postabaqus if ECD request is restricted to the coupled thermal-electrical elements DC2D8E.
• Gaussian and elemental results given in a local axis system will be defined as being local and if the data for the local axis system is present (see Section 2.4) then operations that imply transformation from the local to the global system can be done in FEMVIEW.

Element-wise Multi-Surface Results

Multiple surface results are interpreted for any results location. If the results are element-wise then any result for a shell model has its attribute name prefixed with `S-'. This allows models containing both SHELL and other elements to have their results transferred unambiguously. For example a model containing both S8R and C3D8 will have stress results output as S-STRESS and STRESS.

Surface numbers are allocated to surfaces incrementally in the order that the surfaces are found. For example, for a default ABAQUS shell model the surfaces 1 and 5 have results output. These will become surfaces 1 and 2 in a FEMVIEW model. Within FEMVIEW the results for each surface can be accessed using the command `RESULTS RANGE SURFACE surface_number'.

Appendix B contains an alphabetical list of all the ABAQUS element-wise results that can be processed by the interface. The attribute and component names allocate to the results for use within FEMVIEW is also listed.

Node-wise Results

 Node-wise result output is requested from the ABAQUS program using the `*NODE FILE' command in the ABAQUS input file. This interface program allocates the FEMVIEW attribute type NODAL to all ABAQUS node-wise results.

For a complete list of node-wise results please see Appendix C where the attribute and component names assigned to the results by this interface program for use within FEMVIEW are also shown.

In the case of 'CAXA' and 'SAXA' type elements and for vector type results, such as displacement, the components displayed are the values in the local axis system (U1, U2 and UR3 for displacement) and the values in the global axes (GU1, GU2 and GU3 for displacement). The 'all' calculation is based on the global axes values. The name of the global axes component corresponds to the name of the local axes component preceded by the letter 'G'.

Node-wise Multi-Surface Results

Surface numbers for multi-surfaces models are allocated incrementally in the order that the results are found in the ABAQUS `.fil' file. If the number of surfaces for which results are requested is greater than 12 then the record containing the information will be truncated. This limit may be increased by contacting your support centre.

Whole Model Results

ABAQUS outputs some results that are applicable to the whole model. To enable this information to be transferred the results are output as NODAL values. The values are assigned to the lowest node number found in the model. Whole model results that are transferred are listed in Appendix D. Partial model results via an element set are processed in the same way as whole model results but only one element set is accepted for a given output variable.