Did you know that there are three main ways to apply force and displacement in a structural analysis? They are:
- Displacement/Force – Most straightforward, least amount of setup work.
- Remote Displacement/Remote Force – Rigid/Deformable/Coupled behaviors available for scoped face, able to apply a rotation displacement.
- Nodal Displacement/Nodal Force – Can add to a model and still do a nonlinear restart, not necessary to scope to a geometry entity.
What are the different behaviors and how can you add a new load to an analysis you wish to restart? Read more below:
Remote Displacement Behaviors
There are three behaviors available with remote boundary conditions:
The remote boundary conditions are implemented with the Multipoint Constraint (MPC) technology. For more information, see the corresponding section in the Contact Technology Guide of the ANSYS documentation.
All of the above loads are compatible with nonlinear restarts but only tabular data after the desired restart point may be modified and only on a pre-existing load. This is because the regular and remote loads actually create surface effect elements (SURF154) to implement the load behind the scenes. While this confers several benefits, such as the ability to have overlapping loads on the same face, it is not compatible with nonlinear restarts since adding new elements would change the model too much. Direct forces and pressures are applied directly to the nodes, however, and avoid this restriction. This functionality is not available for direct displacements since a displacement of 0 is a constraint and would invalidate the restart points.
To add an entirely new load (force/pressure only) to an analysis:
- To ensure that restart points are available make sure to set Analysis Settings -> Restart Controls -> Retain Files After Full Solve to Yes
- Add a load step by setting increasing the number in Analysis Settings -> Step Controls -> Number of Steps
- Create a nodal named selection of the desired load location, either through the Named Selection Worksheet or the Mesh Selection capabilities in Mechanical
- Insert a Nodal Force or Nodal Pressure into the analysis and scope it to the above nodal named selection
- Modify only the tabular data for load steps that are not yet solved for!
- Solve the analysis (should do restart automatically, if not set it in Analysis Settings -> Restart Analysis)
Did you find this useful? Sign up for our newsletter below to receive tips like this and more every month: