Abaqus Equivalents

The conversion of entities is handled behind the scenes during the model preparation portion of the simulation. The following list maps various DesignSight features and parameters to their Abaqus finite element counterparts. Understanding these mappings does not expose hidden behavior or functionality, but it may prove interesting to those with previous experience in Abaqus interfaces or finite element analysis.

Ball joints	A reference node is created corresponding to the center of rotation for the ball joint; a boundary condition on this reference node fixes all three translational degrees of freedom. A kinematic coupling between the reference node and the selected ball joint surface constrains the nodes on the surface to follow the rotation of the reference node as a rigid body.
Bonds	A tied contact pair is defined between the two selected surfaces. The underlying nodes on one of the surfaces must lie within a small tolerance distance of the opposing surface; nodes that fall outside of this tolerance do not participate in the tied contact pair. The tolerance distance is calculated based on the representative dimensions of the model.
Clamps	A clamp is applied to the nodes underlying the selected surface as a boundary condition that fixes all three translational degrees of freedom.
Forces	A reference node is created corresponding to the location of the robot in the force definition. A continuum distributing coupling with uniform weighting is defined between the reference node and the selected force transmission surface. A concentrated load (defined by the magnitude and direction of the force) is applied to the reference node and distributed to the nodes on the transmission surface via the coupling.
Frequency Simulation	A natural frequency extraction using the Lanczos eigensolver.
Heat Fluxes	A heat flux is applied to the element faces underlying the selected surface as a distributed surface flux load.
Material	The properties specified in the Simulation domain for your material are used to create an Abaqus material definition. This material definition is referenced by the section properties for the elements in the finite element model. DesignSight finite element models are meshed using general-purpose quadratic tetrahedrons with midside nodes—C3D10I elements in Abaqus terms.
Torques	A reference node is created corresponding to the location of the robot in the moment definition. A continuum distributing coupling with uniform weighting is defined between the reference node and the selected moment transmission surface. A concentrated moment load (defined by the magnitude and orientation of the torque) is applied to the reference node and distributed to the nodes on the transmission surface via the coupling.
Pressure	A pressure is applied to the element faces underlying the selected surface as a distributed surface pressure load.
Stress Simulation	A static stress analysis using the nonlinear large-displacement formulation.
Temperatures	A temperature is applied to the nodes underlying the selected surface as a boundary condition on the temperature degree of freedom.
Thermal Simulation	A steady-state heat transfer analysis.