Mechanical APDL Basic Analysis Guide - Ansys

7.4.4. Mapping Results onto a Different Mesh or to a Cut Boundary
Just as the PDEF command (Main Menu> General Postproc> Path Operations> Map onto Path) maps
results onto an arbitrary path in the model, POST1 also has the ability to map results on to an entirely new
mesh or to a portion of a new mesh. This functionality is mainly used in submodeling, where you initially
analyze a coarse mesh, build a finely meshed submodel of a region of interest, and map results data from
the coarse model to the fine submodel.
POST1 offers two options for mapping results to a different mesh:
Command(s):
CBDOF
GUI:
Main Menu> General Postproc> Submodeling> Interpolate DOF
Command(s):
BFINT
GUI:
Main Menu> General Postproc> Submodeling> Interp Body Forc
The CBDOF command maps degree-of-freedom results from the coarse model to the cut boundaries of the
submodel. BFINT maps body force loads (mainly temperatures for a structural analysis) from the coarse
model to the submodel. Both commands require a file of nodes to which results are to be mapped, and
both commands write a file of appropriate load commands. Details about the submodeling technique are
presented in the Advanced Analysis Techniques Guide.
7.4.5. Creating or Modifying Results Data in the Database
You can do postprocessing without ever producing an ANSYS results file. All you need to do is create an
ANSYS database containing nodes, elements, and property data, and then put your own results into the
database using the following commands:
Command(s): DESOL
GUI: Main Menu> General Postproc> Define/Modify> Elem Results
Command(s): DETAB
GUI: Main Menu> General Postproc> Define/Modify> ElemTabl Data
Command(s): DNSOL
GUI: Main Menu> General Postproc> Define/Modify> Nodal Results
Once the data are defined, you can use almost any postprocessing function: graphics displays, tabular listings,
path operations, etc.
Note
7.4.5. Creating or Modifying Results Data in the Database
Issuing the DNSOL command requires that you have placed the data type (stress/strain) in the
element nodal records. To get around this requirement, use the DESOL command to add a
"dummy" element stress/strain record.
ANSYS performs all load case combinations in the solution coordinate system, and the data resulting from
load case combinations are stored in the solution coordinate system. The resultant data are then transformed
to the active results coordinate system when listed or displayed. Therefore, unless RSYS,SOLU is set (no
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
181