How to Setup a Plane Strain Analysis in OptiStruct
Altair Employee
Use case
The plane strain formulation assumes that the strains in the plane perpendicular to the axis (or simply out-of-plane) are zero or irrelevant.
When running a CAE analysis, using the plane strain assumption can lead to considerable savings in computational time and file storage. The simplification to a 2D mesh also allows the user to use a finer mesh resulting in a more accurate analysis than a coarsely 3D meshed full model. A typical example of plane strain application is for the analysis of pressure vessels. In this article we will see how to use this technique correctly in OptiStruct and the necessary updates in the boundary conditions.
Plane Strain Analysis in OptiStruct
Element Support: Plane strain element is a two-dimensional element with 3 or 6 nodes (CTPSTN) & 4 or 8 nodes (CQPSTN) with PPLANE property.
Analysis Support: New plane strain elements are supported in OS for linear analysis, modal analysis, and small and large displacement nonlinear static analysis.
Material Support: MAT1, MATS1, MAT3 and MATHE (for 1st order elements)
Loading support: Forces, PLOADE1 and PLOADSF with follower effects
Contact Support: OptiStruct v2020.0 supports Large Sliding (N2S CONSLI contacts)
Note: The node ordering for CQPSTN/CTPSTN is critical. Thus, make sure that the elements’ normal of all components are pointed in the same direction.
Model Setup
The following example examines the expansion of a pressure vessel due to internal pressure. Plane Strain elements are used to model the quarter symmetric slice of the pressure vessel with a radius of 100 mm and thickness of 20 mm. The internal pressure of 10 MPa is applied on the nodes of the inner surface of the pressure vessel and a Linear Static analysis is performed. We will compare OptiStruct results for principal stresses and compare them with the theoretical values.
To setup a plane strain analysis in OptiStruct the user needs to pay attention to four main steps:
- The model must be in the XY or XZ plane, which means, for XY plane all nodes must have Z coordinates equal to zero and for XZ plane all Y coordinates are zero.
- Make sure that all element normals are pointed to the positive Z or Y direction.
Otherwise, OptiStruct will show the following warning and the results can be wrong:
- Update the element type, trias to CTPSTN and quads to CQPSTN.
- Create PPLANE property.
The 10MPa load will be applied using PLOADE1 type and selecting the internal edge of the model:
Validation
For thick-walled cylinders, stresses can be expressed as:
Circumferential Direction - Hoop Stress
Radial Direction
Where,
σc = stress in circumferential direction (MPa, psi)
σr = stress in radial direction (MPa, psi)
pi = internal pressure in the tube or cylinder (MPa, psi)
po = external pressure in the tube or cylinder (MPa, psi)
ri = internal radius of tube or cylinder (mm, in)
ro = external radius of tube or cylinder (mm, in)
r = cylinder wall radius where stress is calculated (mm, in) (ri < r < ro)
Considering external pressure zero and r = ri, we have for our validation model:
|
| Hoop Stress | Radial Stress |
| Theoretical | 55.45 MPa | -10.00 MPa |
| OptiStruct | 54.68 MPa | -9.21 MPa |
| Error | 1.4% | 7.9% |
The model can be found attached to this article.