The following steps describe how to perform a 2-D to 3-D analysis:
It is typical in a 2-D to 3-D analysis to use the results at the end of the 2-D analysis as the starting point for the 3-D extrusion. You can, however, select any substep to initiate the 2-D to 3-D analysis process (if the restart files for that substep exist), especially if convergence issues exist for the 2-D analysis.
When you have determined a suitable substep, proceed to Step 2: Initiate the 2-D to 3-D Analysis.
2-D to 3-D analysis is based on a new model with a higher dimension (3-D), extruded from a specific substep of a lower dimensional (2-D) model solution. The analysis process therefore requires a clean database.
To initiate a 2-D to 3-D analysis:
Clear the database (/CLEAR,NOSTART).
Reenter the solution processor (/SOLU).
Initiate 2-D to 3-D analysis, specifying
the load step and substep at which 2-D to 3-D analysis should
occur
(MAP2DTO3D,START,VALUE1,VALUE2).
Result: The program updates the geometry to the deformed configuration.
Proceed to Step 3: Extrude the 2-D Mesh to a New 3-D Mesh .
Issue the EEXTRUDE command to extrude the 2-D mesh to the 3-D mesh.
The following figures illustrate how extrusion generates 3-D meshes from an axisymmetric and a plane strain 2-D mesh, respectively:
Extrusion preserves the 2-D mesh topology on the generating plane and replicates it through the depth of the extruded body.
Extruded elements and nodes have the properties or equivalent properties of the elements and nodes from which they were created. If a given element or a node belongs to specific components, the extruded elements and nodes belong to the same components. If a given node is rotated on the 2-D modeling plane (global XOY), the extruded nodes are rotated in the radial plane (axisymmetric or tire option), or rotated in the planes parallel to XOY (plane strain).
For axisymmetric cases (EEXTRUDE,AXIS) and
for the tire option (EEXTRUDE,TIRE), you can control the nodal
orientation in the third direction (BCKEY on the
EEXTRUDE command).
The extrusion process generates 3-D contact and target elements with the solid elements. 2-D rigid target elements are deleted, and corresponding 3-D rigid target elements are generated. EEXTRUDE can control how the contact elements and target elements are generated in the third direction and the corresponding mesh density.
After extrusion, proceed to Step 4: Map Boundary Conditions and Loads to the New 3-D Mesh.
To add contact pairs manually, do so immediately after issuing the EEXTRUDE command.
Newly added contact pairs must be in a pre-contact state or just touching; otherwise, they affect the equilibrium of (and thereby change the solution of) the extruded 3-D model.
Rigid-to-flexible contact-pair limitations:
If adding a rigid-to-flexible contact pair to the 3-D model, you cannot add a pilot node if the contact pair in the 2-D model does not have one.
For existing rigid-to-flexible contact pairs in the 3-D model, you cannot modify or replace rigid target surfaces, even if they are in a pre-contact state.
Issue the MAP2DTO3D,FINISH command to transfer boundary conditions, pressure loads, applied nodal forces, applied nodal displacements, and applied nodal temperatures from the 2-D mesh to the corresponding entities in the extruded 3-D model.
Applied nodal displacements in the 2-D model X and Y directions transfer to the
3-D model in the radial and axial directions. If applying rotation ROTY via the
axisymmetric option with torsion, the program applies a displacement constraint in
the hoop direction (Uz = 0) on the 3-D model. If rotating only the nodes with loads
or displacements to a local Cartesioan coordinate system
(BCKEY = 1 on the EEXTRUDE
command), the program resets displacement values so that displacements re-accumulate
from zero.
Temperatures and pressures transfer to the nodes and elemental facets of the 3-D model.
In the same way that pressure is applied, the program redistributes applied forces at nodes in the 2-D model to all extruded nodes in the hoop direction of the 3-D model. For the axisymmetric option with torsion, the program converts applied torsion MY in the 2-D model into a concentrated force (by dividing it by the current radius [x coordinate]), then redistributes the force to all nodes in the hoop direction as an applied force.
Constraints and loads applied at nodes not associated with any 2-D elements (such as pilot nodes) remain unchanged during boundary-condition mapping.
After mapping the boundary conditions and loads to the 3-D mesh, proceed to Step 5: Map Solution Results to the New 3-D Mesh and Rebalance.
Issue the MAP2DTO3D,SOLVE command to map the nodal and element solutions to the 3-D model and to initiate rebalancing.
For more information about the solution-mapping phase of the 2-D to 3-D analysis, see:
After mapping the solution results, proceed to Step 6: Continue Your Analysis on the 3-D Model.
After issuing the MAP2DTO3D,SOLVE command, the program displays a message similar to the following, then performs rebalancing iterations for the mapped solution results:
S O L U T I O N O P T I O N S
PROBLEM DIMENSIONALITY. . . . . . . . . . . . .3-D
DEGREES OF FREEDOM. . . . . . UX UY UZ ROTY
ANALYSIS TYPE . . . . . . . . . . . . . . . . .STATIC (STEADY-STATE)
MAP2DTO3D,SOLVE FOR 2D TO 3D MAPPING. . . . .YES
NONLINEAR GEOMETRIC EFFECTS . . . . . . . . . .ON
STRESS-STIFFENING . . . . . . . . . . . . . . .ON
EQUATION SOLVER OPTION. . . . . . . . . . . . .SPARSE
NEWTON-RAPHSON OPTION . . . . . . . . . . . . .PROGRAM CHOSEN
GLOBALLY ASSEMBLED MATRIX . . . . . . . . . . .SYMMETRIC
L O A D S T E P O P T I O N S
LOAD STEP NUMBER. . . . . . . . . . . . . . . . 1
TIME AT END OF THE LOAD STEP. . . . . . . . . . 1.0000
AUTOMATIC TIME STEPPING . . . . . . . . . . . . ON
INITIAL NUMBER OF SUBSTEPS . . . . . . . . . 10
MAXIMUM NUMBER OF SUBSTEPS . . . . . . . . . 10
MINIMUM NUMBER OF SUBSTEPS . . . . . . . . . 10
MAX. NUMBER OF SUBSTEPS FOR MAP2DTO3D. . .500
MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS. . . . 15
STEP CHANGE BOUNDARY CONDITIONS . . . . . . . . NO
STRESS-STIFFENING . . . . . . . . . . . . . . . ON
TERMINATE ANALYSIS IF NOT CONVERGED . . . . . .YES (EXIT)
CONVERGENCE CONTROLS. . . . . . . . . . . . . .USE DEFAULTS
COPY INTEGRATION POINT VALUES TO NODE . . . . . YES
PRINT OUTPUT CONTROLS . . . . . . . . . . . . .NO PRINTOUT
DATABASE OUTPUT CONTROLS
ITEM FREQUENCY COMPONENT
ALL ALL
When rebalancing is complete, the program displays a message similar to the following:
*** LOAD STEP 1 SUBSTEP 11 COMPLETED. CUM ITER = 23
*** TIME = 1.00000 REBALANCE FACTOR = 1.00000
MAP2DTO3D,SOLV IS DONE SUCCESSFULLY IN 1 SUBSTEPS FOR 2D TO 3D MAPPING.
Results of the analysis on the 3-D model after rebalancing are output to the results file regardless of any prior results file setting. If you have set the postprocessing option to list a summary of each load step (SET,LIST), the program generates following output:
*** LOAD STEP 1 SUBSTEP 11 COMPLETED. CUM ITER = 23
*** TIME = 1.00000 REBALANCE FACTOR = 1.00000
MAP2DTO3D,SOLV IS DONE SUCCESSFULLY IN 1 SUBSTEPS FOR 2D TO 3D MAPPING.
FINISH SOLUTION PROCESSING WITH 1 SUCCESSFUL REMESHING(S)
***** INDEX OF DATA SETS ON RESULTS FILE *****
SET TIME/FREQ LOAD STEP SUBSTEP CUMULATIVE
1 0.10000 1 1 2
2 0.20000 1 2 4
3 0.30000 1 3 6
4 0.40000 1 4 8
5 0.50000 1 5 10
6 0.60000 1 6 12
7 0.70000 1 7 14
8 0.80000 1 8 16
9 0.90000 1 9 18
10 1.0000 1 10 20
11 1.0000 1 11 23 mesh changed
In this example, the 2-D to 3-D analysis occurred at TIME = 1.
Two result data sets are generated, one for the 2-D model, the other for the
3-D model (indicated by mesh changed).
In axisymmetric cases (EEXTRUDE,AXIS), the element coordinate system for the new 3-D elements is the co-rotated 2-D material system on the radial plane. The third direction is in the hoop direction (similar to a cylindrical coordinate system). This behavior differs from that of the coordinate systems of elements created directly from 3-D geometry.
In plane strain cases (EEXTRUDE,PLANE), extra boundary conditions UZ = 0 are applied at nodes where UX and UY = 0 are applied in the 2-D model. The boundary conditions restrain the rigid-body motions in the global Z direction.
Always verify that sufficient boundary conditions exist to constrain the rigid-body motion. If needed, you can apply additional constraints after issuing the MAP2DTO3D,FINISH command but before issuing the MAP2DTO3D,SOLVE command.
Successful 2-D to 3-D solution rebalancing is typically achieved using the default maximum allowed number of substeps.
If rebalancing is unsuccessful, you can increase the number of allowed
substeps (via VALUE1 on the
MAP2DTO3D,SOLVE command). Before doing so, however, check
the extruded 3-D model to ensure that all contact pairs are reconstructed
completely, and that all boundary conditions and loads have transferred
correctly.
Rebalancing difficulties can occur if the extruded 3-D model is not:
a full circle in the hoop direction (axisymmetric case), or
of sufficient length in the global Z direction (plane strain case).
To aid convergence, you can constrain the motion in the normal direction of the two ending planes. If needed, you can constrain more planes parallel to the ending planes (the radial plane in axisymmetric cases, and the plane parallel to the global XOY direction in plane strain cases).
For axisymmetric cases, rebalancing may fail if reinforcing elements exist and:
the reinforcing elements are oriented in a direction other than in the hoop and radial directions, and
the torsion degree of freedom is not enabled.
Failure occurs if the orientation of the reinforcing elements causes torsion but the torsion option was not set in the 2-D model. Not setting the torsion option is equivalent to introducing extra constraints in the hoop direction; however, after torsion transfers to the 3-D model, the equivalent constraints are not constructed. To resolve the issue, allow torsion in 2-D analysis, or constrain the motion in the hoop direction for all the nodes of the 3-D model.
During rebalancing, the porgram may issue a warning message similar to the following:
*WARNING*: Initial penetration 4.28926118 may be too large for contact element 12685 (with target element 14190). Check whether the pinball region is big enough to capture initial interference.
If you encounter such a message during rebalancing, consider these remedies:
Increase the number of elements (thereby increasing the
corresponding number of contact and target elements) in the hoop
direction during the 2-D to 3-D extrusion process
(EEXTRUDE,,NELEM).
Ensure that target surfaces are at least equal to or larger than the contact surfaces.
During the mapping process (after EEXTRUDE and before MAP2DTO3D,FINISH), try reducing the pinball region (via the real constant PINB) for the problem contact pair.
Contact pairs added manually after extrusion should be in a pre-contact state or just touching. If contact occurs, the new contact pairs can affect the equilibrium of (and thereby change the solution of) the extruded 3-D model or cause convergence difficulties.
If you exit the Mechanical APDL program after the solution of a 2-D to 3-D analysis
and want to review the results of the analysis later, issue the
/FILNAME,Jobname command the
after starting the program.
To compare the 2-D to 3-D analysis results to those of either the original 2-D model or the new 3-D model, consider issuing the ERESX,NO command to prevent the program from introducing integration-point extrapolation results in the 2-D and 3-D model results.
Because the default PowerGraphics display mode (/GRAPHICS,POWER) displays the results on the model's exterior facets only, you may prefer to compare all geometry and results (/GRAPHICS,FULL) of the 2-D to 3-D analysis to the PowerGraphics-only results of the 2-D model.
Using the rebalanced solution results for the new 3-D model, you can continue your analysis via a multiframe restart (or by starting a new 3-D analysis using the 2-D solution as the initial state, as described in Overview of the 2-D to 3-D Analysis Process).
If the MAP2DTO3D command used the results at the end of a load step, you can apply new loads directly on the 3-D model and proceed with the 3-D analysis. If the command used the results at a substep in the middle of a load step, end the current load step (ANTYPE,RESTART) before continuing as a new load step with new loads..
If you rotated only the nodes with loads or displacements to a local Cartesian
coordinate system during extrusion (BCKEY = 1 on the
EEXTRUDE command), the program resets displacement values and
initiates re-accumulation from zero. Newly applied displacements are therefore the
new values accumulated during the 3-D analysis phase only, rather than from the
beginning of the 2-D analysis. Regardless of the BCKEY
value specified on the EEXTRUDE command, however, displacements
shown in the results file after mapping indicate the displacements at the 3-D phase
only (and not from the initial stress-free state).