Solved! Go to Solution.
1. Define a table with the desired behaviour and allocate to the appropriate k value on the cbush
2. Can’t do that with nx nastran. Might be able with a sensitivity tool/module. You need to do it by hand by changing the appropriate k values and and record the omega value
Your image shows the PBUSH dialog with the Nominal Values tab active.
Switch to the Dependent Properties tab. Expand the Nonlinear (bottom) group and define the appropriate table(s).
Dear @JimB, I add the force-displacement relation in the appropriate table, but I get the following errors:
FATAL ERROR There is no stiffness or damping defined for "CBUSH" elements in mesh "Cbush Collector(1)::1d_mesh(1)". Job is not ready to submit to the solver. ACTION: Edit the physical property specified in the mesh collector to apply a spring stiffness and/or damping value. WARNING There is no orientation specified for mesh "Cbush Collector(1)::1d_mesh(1)". ACTION: Define an orientation for the mesh in the "Edit Mesh Associated Data" dialog.
I add the files in order to help me for the debugging phase (it is a very easy model hence it take few minutes).
Thanks a lot!
In this model, you had specified only the PBUSHT force/displacement table. You need to specify the nominal stiffness for PBUSH as well. This will eliminate the first error.
The warning can be ignored since there are only axial frces/displacements. To eliminate the warning, edit the mesh associated data and specify an orientation. For this model, you can simply check the Uniaxial box.
Finally, node 2 is only connected to node 1 with stiffness in the X direction. The other 5 dof are unconnected. You need to define a SPC for DOF 2-6 at node 2.
The attached updated model contains all 3 of these changes and solves without error.
Thank you very much @JimB for your very clear explanation!
Last questions are:
Thank you very much for your availability!