UPGEOM, FACTOR, LSTEP, SBSTEP, Fname, Ext, --
Adds displacements from a previous analysis and updates
the geometry of the finite element model to the deformed configuration.
FACTORMultiplier for displacements being added to coordinates. The value 1.0 will add the full value of the displacements to the geometry of the finite element model. Defaults to 1.0.
LSTEPLoad step number of data to be imported. Defaults to the last load step.
SBSTEPSubstep number of data to be imported. Defaults to the last substep.
FnameFile name and directory path (248 characters maximum, including the characters needed for the directory path). An unspecified directory path defaults to the working directory; in this case, you can use all 248 characters for the file name.
The field must be input (no default).
ExtFilename extension (eight-character maximum).
The extension must be an RST extension.
--Unused field.
This command updates the geometry of the finite element model according to the displacement results of the previous analysis and creates a revised geometry at the deformed configuration. This command works on all nodes (default) or on a selected set of nodes. If this command is issued repeatedly, it creates a revised geometry of the finite element model in a cumulative fashion, i.e., it adds displacement results on the previously generated deformed geometry. The solid model geometry is not updated by this command.
When UPGEOM is issued, the current finite element model is overwritten by finite element information from the results file. For this reason, it is important that the finite element information in the results file matches the finite element model in which the nodal coordinates are being updated. No changes should be made to the model before the UPGEOM command is issued.