Chapter 7 Explicit Dynamics: Body Interactions ANSYS Explicit Dynamics

Body Interactions The Body Interactions folder, under Connections, is used to define global connection options for Explicit Dynamics Contact Detection Trajectory (default) Formulation Shell Thickness Factor Tolerence Proximity Based Pinball Factor Timestep Safety Factor Limiting Timestep Velocity Edge On Edge Contact Body Self Contact Element Self Contact

Trajectory Contact Recommended option for impact and sliding contact between Solids, Shells and Beams. The trajectory of nodes and faces are tracked during the computation cycle. If the trajectory of a node and a face intersects during the cycle a contact event is detected (see figure). Trajectory based contact does not constrain the time step Often provides the most efficient solution. Nodes which penetrate into another element at the start of the simulation will be ignored for contact and should be avoided. To generate duplicate conforming nodes across a contact interface Use the multi-body part option in DesignModeler and set the Shared Topology Method to either Imprint or None In Meshing use Arbitrary Match Control (Sweep) or Match mesh where possible (Patch Independent Tetrahedrons).

Trajectory Contact Shell Thickness Factor The Shell Thickness Factor (STF) defines the shell (surface body) thickness used for contact A factor of 1.0 takes the true physical shell thickness into account, which means that the contact surface is positioned at half the true shell thickness on both sides of the shell mid plane. A factor of 0.0 means that the shell has no contact thickness and the contact surface is positioned at the shell mid plane. Value must be between 0.0 and 5.0 For shell node on shell face impacts, the node is always located at the mid-surface of the shell.

Trajectory Contact Formulations Penalty Formulation (default, recommended) A penalty force is calculated to push a penetrating node back to the face. Penalty forces are calculated to conserve linear and angular momentum. where D is the depth of penetration M is the effective mass of the node (N) and face (F) Δt is the simulation time step Nodes will be pushed back towards the contact position, but it will usually take several cycles to satisfy the contact condition. Decomposition Response All contacts that take place at the same point in time are first detected. The response of the system is then calculated to conserve momentum and energy. During this process, forces are calculated to ensure that the resulting position of nodes and faces does not result in further penetration at that time point The decomposition response algorithm is more impulsive (in a given cycle) than the penalty method. This can in some situations give rise to large hourglass energies and energy errors.

Proximity Based Contact Alternative option for impact and sliding contact between Solids, Shells and Beams The external faces, edges and nodes of a mesh are encapsulated by a contact detection zone. If a node enters this zone, it is repelled using a penalty based force that conserves linear and angular momentum Pinball Factor defines the size of the contact detection zone (Gap). Smallest element size is multiplied by this factor to give the physical size of the contact detection zone. Value must be between 0.1 to 0.5. The smaller the fraction the more accurate the solution. Initial geometry / mesh must be defined such that there is a physical gap / separation of at least the contact detection zone size between interacting nodes and faces in the model. Solver will give error messages if this criteria is not satisfied. May not be practical for very complex assemblies. F R Gap

Proximity Based Contact Time step is constrained so that contact nodes can travel no more than (contact detection zone size) x (Timestep Safety Factor) in one cycle. Default Timestep Safety Factor is 0.2 (strongly recommended) Increasing to 0.5 (maximum value) may increase time step and reduce runtimes, but contacts may be missed. Time step is computed using the maximum velocity of all contact nodes, but limited by the Limiting Timestep Velocity (default very large). Use with care or contacts may be misses

Proximity Based Contact Edge on Edge Contact Edge on Edge contact can be used to extend contact detection to include edge to edge contacts (standard detection is node to face). All edges of Solid, Shell and Beam elements will be included in the contact detection. This option is numerically intensive and can significantly increase runtimes. Compare results with and without edge contact to make sure this option is required.

Trajectory and Proximity Based Contact Body Self Contact By default, the contact detection algorithm will check for external nodes of a body contacting with faces of the same body in addition to other bodies. Most robust option since all possible external contacts should be detected. If self impact of a body is unlikely, set Body Self Contact = No Reduces the number of possible contact events Improve efficiency of the simulation. Do not use if a body is likely to fold onto itself during the simulation e.g. during plastic buckling.

Trajectory and Proximity Based Contact Element Self Contact This option automatically removes (erodes) an element if it deforms such that one of it’s nodes comes within a tolerance of one of it’s faces, i.e. before it becomes degenerate or inverted. For Trajectory Contact a Tolerance factor is specified Smallest element size is multiplied by this factor to give the physical tolerance. Value must be between 0.1 to 0.5. For Proximity Based Contact, the Pinball Factor is used for the tolerance factor

Body Interaction Objects Each Body Interaction object activates a body interaction for the bodies scoped in the object Four Types of Body Interaction Bonded Frictionless (contact) Frictional (contact) Reinforcement Contact detection is completely automated. Every node of the scoped bodies interacts with every face of the scoped bodies. A default Frictionless interaction is scoped to all bodies To improve the efficiency of simulations involving large number of bodies: Suppress the default Frictionless interaction Insert new Body Interaction objects which limit interactions to specific bodies. The union of all Frictional / Frictionless body interactions defines the matrix of possible body interactions during the simulation.

Body Interaction Objects Example Body A is travelling towards body B and we require Frictional contact to take place. A body Interaction of type frictional scoped only to Bodies A and B will achieve this. Body A will not come close to body C during the simulation so does not need to be included in the interaction. Body B is bonded to Body C. A body Interaction of type bonded, scoped to Bodies B and C will achieve this If the bond between bodies B and C breaks during the simulation. We want frictional contact to take place between bodies B and C. A body interaction of type frictional scoped to bodies B and C will achieve this A bonded body interaction of can be applied in addition to a frictional / frictionless body interaction

Body Interaction Objects Types of Body Interactions Frictionless (default) Sliding contact is frictionless. Frictional Friction Coefficient A non-zero value will activate Coulomb type friction between bodies: F = μsR Dynamic Coefficient, Decay Constant Non-zero values will activate dynamic friction where the relative velocity (v) of sliding interfaces can influence frictional forces: μs = Friction Coefficient μd = Dynamic coefficient β = Decay Constant ν = relative sliding velocity at point of contact

Body Interaction Objects Types of Body Interactions Bonded External nodes of bodies included in Bonded interactions are tied to faces of bodies included in the interaction if the nodes are within the defined Maximum Offset distance of a face Solver automatically detects bonded nodes / faces during initialization. Bonds can break during a simulation based on a specified Stress Criteria. Effective normal and shear stresses are calculated at each node involved in a bonded connection. If the following criteria is exceeded, the node will be released from bonded contact. All released nodes will subsequently be added to the sliding contact detection algorithm.

Body Interaction Objects Types of Body Interactions Bonded (continued) It is important to select an appropriate value for the Maximum Offset. The automatic search will bond a node which is to be tied to a face within the offset distance, the selected face will be the closest one which is most parallel to a face to which the tied node belongs. The breakable bond criteria works best when equivalent, or similar, meshes are used on the faces at either side of the bond. Bonded connections must be used with Trajectory Contact Bonded connections are only available for Solid and Surface bodies Flexible to Rigid body bonded connections can only be made using Body Interaction objects

Body Interaction Objects Types of Body Interactions Reinforcement Used to apply discrete reinforcement to solid bodies Line body elements scoped to the object, contained within any solid body in the model, are converted to discrete reinforcement elements / nodes Elements which lie outside solid bodies remain standard beam elements Reinforcing beam nodes are constrained to stay at the same parametric location within the solid element they reside during element deformation For good modeling, the size of the beam elements should be similar or less than that of the volume elements If volume elements erode, reinforcing nodes tied to them become free beam nodes If reinforcing beam elements erode, and inertia is retained, the eroded nodes will remain tied to the parametric location of their solid elements Typical applications involve reinforced concrete or reinforced rubber structures likes tires and hoses

Contact Regions Used to define specific face to face contact interactions Contact and target faces are scoped to each manual contact region For shell bodies, target shell face option is not respected for Explicit Dynamics. The nearest shell face is always selected Types Bonded Bonds can be breakable No Separation not supported for Explicit Dynamics Frictionless Rough Frictional Static and dynamic friction options Settings defined under Body Interactions are used for Body Interaction Object and Contact Region Object May reduce Solve times

Spot Welds Rigidly connect two discrete points to model welds, rivets, bolts e.t.c. Points usually belong to two different surfaces Defined on the geometry (DesignModeler) Respected by Meshing Points are connected by a rigid beam element Can fail (break) using Breakable Stress Criteria or Force Criteria. Where fn and fs are normal and shear interface forces (normal force is only non-zero for tension), Sn and Ss are the Normal and Shear Force Limit, and n and s are the Normal and Shear Stress Exponent (For stress criteria an Effective Diameter is used to convert the stress limits to equivalent force limits) Spot welds of zero length are permitted Failure criteria is modified since local normal and shear directions cannot be defined where Δf are component force differences across the spot weld

Spot welds Connecting shell points have both translational and rotational degrees of freedom linked Points on solid bodies, have additional rigid beam elements automatically generated to enable transfer of rotations at the spot weld location Beam elements are automatically deleted if weld fails