4.4. Performing a 2-D to 3-D Analysis

The following steps describe how to perform a 2-D to 3-D analysis:

4.4.1. Step 1: Determine the Substep to Initiate

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.

4.4.2. 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:

  1. Clear the database (/CLEAR,NOSTART).

  2. Reenter the solution processor (/SOLU).

  3. 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 .

4.4.3. 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:

Figure 4.2:  Axisymmetric to 3-D Solid Extrusion

Axisymmetric to 3-D Solid Extrusion

Figure 4.3:  2-D Plane Strain to 3-D Solid Extrusion

2-D Plane Strain to 3-D Solid Extrusion

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.

4.4.3.1. Adding Contact Pairs

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.

4.4.4. Step 4: Map Boundary Conditions and Loads to the New 3-D Mesh

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.

4.4.5. 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.

After mapping the solution results, proceed to Step 6: Continue Your Analysis on the 3-D Model.

4.4.5.1. Example: Solution Variable Mapping and Rebalancing

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).

4.4.5.2. Mapped Solution Results in Axisymmetric Cases

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.

4.4.5.3. Mapped Solution Results in Plane Strain Cases

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.

4.4.5.4. Rebalancing Considerations

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).

4.4.5.4.1. Axisymmetric Rebalancing Cases with Reinforcing Elements

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.

4.4.5.4.2. Large Penetration and Rebalancing

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.

4.4.5.5. Adding Contact Pairs

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.

4.4.5.6. Reviewing Results After Exiting Mechanical APDL

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.


Note:  For /GRAPHICS,FULL, reinforcing element results are not included.


4.4.6. Step 6: Continue Your Analysis on the 3-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).


Release 18.2 - © ANSYS, Inc. All rights reserved.