To improve performance, distributed-memory parallel (DMP) processing is enabled by default in Solve Options, and the application automatically performs contact splitting for static structural and transient structural analyses. Since contact splitting does not support the 2-D to 3-D analysis capability, it is necessary to set the Contact Split (DMP) property to "Off" (under Advanced in the details view of Analysis Settings) for this example problem.
The analysis solution involves the following steps:
A nonlinear static structural analysis is performed with five load-steps. Large Deflection is set On to include large-deflection effects. The analysis involves two complete loading/unloading cycles of the pressure and end-cap loads. In the fifth load step, the final values of the pressure and end-cap loads are applied.
The 3-D model is extruded from the 2-D model. Since this feature is not supported in workbench Mechanical, it is implemented with a command snippet. The main analysis steps are described below.
| Step 2 | Description | Command | Comments |
|---|---|---|---|
| 2.1 | Initiate the 2-D to 3-D analysis. | MAP2DTO3D,START,5,4 | Begins the analysis by rebuilding the 2-D analysis database at the last converged substep (the fourth in this case) of the fifth load step. |
| 2.2 | Extrude the 3-D mesh from the 2-D deformed mesh. | EEXTRUDE,AXIS,40,,,,,,1 |
Revolves the 2-D deformed geometry about the global Y-axis with 40 elements in the hoop direction. Important: Ensure an adequate number of elements in the hoop direction to reproduce correct contact results during mapping. After extrusion, you can modify some contact settings if necessary to resolve convergence issues during rebalancing. Limited preprocessing is possible. You can create a new contact pair, modify material properties for later use in the 3-D analysis, and change KEYOPT settings. (Use caution when changing KEYOPTs, however, as an inappropriate modification can lead to different 3-D model results after rebalancing.) |
| 2.3 | Map boundary conditions and loads. | MAP2DTO3D,FINISH | Transfers 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. |
| 2.4 | Map solution variables. | MAP2DTO3D,SOLVE | Transfers nodal and element solutions from the 2-D model to the 3-D model and initiates rebalancing. |
Extrude from 2D to 3D is done using below commands.
finish /clear,nostart /solu MAP2DTO3D,START,5, allsel,all 00shpp,off EEXT,axis,40,,,,,, allsel,all csys,5 nsel,s,loc,y,0,180 esln,,1 cm,te,element cmsel,r,Thread_Section cm,thread_section,element allsel,all cmsel,s,te cmsel,r,Full_Model cm,Full_Model,element allsel,all cmsel,s,te cmsel,r,Thread_Part cm,Thread_Part,element allsel,all csys,0 !keyopt,45,5,2 !keyopt,45,9,0 map2dto3d,finish rmod,21,6,-0.1 map2dto3d,solve finish
The analysis continues on the 3-D model (via a multiframe restart) with the applied bending load. This is done using a command snippet, as 2D to 3D extrude is not supported in Mechanical.
| Step 3 | Description | Command | Comments |
|---|---|---|---|
| 3.1 | Restart the analysis. | ANTYPE,,RESTART,5,5 | Performs a multiframe restart at the last converged substep after MAP2DTO3D,SOLVE. (In this case, it is the fifth substep of the fifth load step.) |
| 3.2 | Apply the bending load. |
D,Pilotnode,ROTZ,-0.00698 | Applies the bending load on the pilot node of the rigid-to-flexible contact pair on the top face of the 3-D model. A bending load of 0.4 degrees is applied on the pilot node. |
| 3.3 | Solve and review results. | SOLVE | Solves the 3-D analysis and enables results viewing via standard output commands (PLNSOL and *GET) in POST1. |