Crushing of a Pipe: pipeCrush
Prepared by Philip Cardiff and Ivan Batistić
Tutorial Aims
- Demonstrate a large-strain elastoplastic analysis with frictionless solid contact.
- Compare the predicted crushing force and deformation pattern with FE results.
Case Overview
This case considers a thick-walled pipe compressed between two parallel rigid frictionless platens, as shown in Figure 1. The pipe is represented as a plane-strain 2-D problem. The inner radius \(r_i\) is \(48.28\) mm, and the outer radius \(r_o\) is \(57.15\) mm.
The full pipe is crushed by \(70\) mm, reducing the pipe diameter in the loading direction from \(114.3\) mm to \(44.3\) mm. Because of symmetry, only one quarter of the pipe cross-section is modelled, and the rigid platen in this quarter model is displaced by \(35\) mm. The loading is applied over 100 quasi-static increments. Transient and gravitational effects are neglected.
Frictionless penalty contact is applied between the rigid platen and the outer pipe boundary using the solidContact boundary condition. The updated Lagrangian solid model is selected in constant/solidProperties using nonLinearGeometryUpdatedLagrangian.
Figure 1 - Pipe-crushing geometry [1]
Figure 2 - Initial mesh
The pipe is modelled using the neoHookeanElasticMisesPlastic mechanical law. The mechanical properties are given in Table 1, and the tabulated hardening curve is given in Table 2.
Table 1 - Mechanical properties
| Parameter | Symbol | Value |
|---|---|---|
| Young's modulus | \(E\) | \(186\) GPa |
| Poisson's ratio | \(\nu\) | \(0.3\) |
| Initial yield stress | \(\sigma_Y\) | \(241.32\) MPa |
| Initial density | \(\rho\) | \(7800\) kg/m\(^3\) |
Table 2 - Hardening behaviour
| Plastic strain | Yield stress (in MPa) |
|---|---|
| \(0.000\) | \(241.32\) |
| \(0.0035\) | \(275.79\) |
| \(0.0083\) | \(301.65\) |
| \(0.0133\) | \(318.88\) |
| \(0.0182\) | \(344.74\) |
| \(0.0281\) | \(361.98\) |
| \(0.0380\) | \(379.21\) |
| \(1.000\) | \(1482.37\) |
Expected Results
Figure 3 shows the predicted force-displacement response for different mesh densities reported by Cardiff et al. [1], including a comparison with an Abaqus finite-element solution on a 4096-cell mesh. The solids4foam predictions approach the Abaqus fine-mesh result as the mesh is refined. Oscillations in the force trace are reduced on finer meshes and are attributed to the contact force calculation on faces in partial contact.
Figure 3 - Force-displacement response for different mesh densities [1]
Figure 4 shows the deformed pipe geometry at four stages of compression. The hydrostatic pressure distribution is also compared with the Abaqus prediction. More information is available in Cardiff et al. [1].
Figure 4 - Deformed geometry and hydrostatic pressure distribution [1]
The solidForcesDisplacements function object is added in system/controlDict. It records the contact force and displacement for the pipeContact patch, which can be used to plot the force-displacement response shown in Figure 3.
Video 1 - Pipe crushing animation
Running the Case
The tutorial case is located at solids4foam/tutorials/solids/elastoplasticity/pipeCrush. The case can be run using the included Allrun script, i.e. > ./Allrun.
The Allrun script first adjusts the gradient scheme for the selected OpenFOAM variant when required. It then creates the mesh using blockMesh and runs the solids4Foam solver.