Creating an assembly and a step definition

Create a dependent instance of the part. In this simulation you can accept the default r–z (1–2) axisymmetric coordinate system.

Then, define a single static, general step named Compress mount. When hyperelastic materials are used in a model, Abaqus assumes that the model may undergo large deformations; but large deformations and other nonlinear geometric effects are not included by default in Abaqus/Standard. Therefore, you must include them in this simulation by toggling on Nlgeom; otherwise, Abaqus/Standard will terminate the analysis with an input error. Set the time period to 1.0 and the initial time increment to 0.01 (i.e., 1% of the total step time).

For the purpose of restricting output, create a geometry set named Out at the vertex located at the lower-left corner of the steel plate region.

Write the preselected variables and nominal strains as field output to the output database file every increment. In addition, write the displacements at a single point on the bottom of the steel plate to the output database file as history data so that the stiffness of the mount can be calculated. Use the geometry set Out for this purpose.