Within an Explicit Dynamics analysis, the body interaction feature represents contact between bodies and includes settings that allow you to control these interactions. If the geometry you use has two or more bodies in contact, a Body Interactions object folder appears by default under Connections in the tree. Included in a Body Interactions folder are one or more Body Interaction objects, with each object representing a contact pair.
You can also manually add these two objects:
To add a Body Interactions folder, highlight the Connections folder and choose Body Interactions from the toolbar. A Body Interactions folder is added and includes one Body Interaction object.
To add a Body Interaction object to an existing Body Interactions folder, highlight the Connections folder, the Body Interactions folder, or an existing Body Interaction object, and choose Body Interaction from the toolbar.
Each Body Interaction object activates an interaction for the bodies scoped in the object. With body interactions, contact detection is completely automated in the solver. At any time point during the analysis any node of the bodies scoped in the interaction may interact with any face of the bodies scoped in the interaction. The interactions are automatically detected during the solution.
The default frictionless interaction type that is scoped to all bodies activates frictionless contact between any external node and face that may come into contact in the model during the analysis.
To improve the efficiency of analyses involving large number of bodies, you are advised to suppress the default frictionless interaction that is scoped to all bodies, and instead insert additional 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 analysis.
For example, in the model shown below:
Body A is traveling towards body B and we require frictional contact to occur. A frictional body interaction type scoped only to bodies A and B will achieve this. Body A will not come close to body C during the analysis so it does not need to be included in the interaction.
Body B is bonded to body C. A bonded body Interaction type, scoped to bodies B and C will achieve this.
If the bond between bodies B and C breaks during the analysis, we want frictional contact to take place between bodies B and C. A frictional body interaction type scoped only to bodies B and C will achieve this.

A bonded body interaction type can be applied in addition to a frictional/frictionless body interaction.
A reinforcement body interaction type be can be applied in addition to a frictional/frictionless body interaction.
Object property settings are included in the Details view for both the Body Interactions folder and the individual Body Interaction objects. Refer to the following sections for descriptions of these properties.
All properties for the Body Interactions folder are included in an Advanced category and define the global properties of the contact algorithm for the analysis. These properties are applied to all Body Interaction objects and to all frictional and frictionless manual contact regions.
This section includes descriptions of the following properties for the Body Interactions folder:
The available choices are described below.
The trajectory of nodes and faces included in frictional or frictionless contact are tracked during the computation cycle. If the trajectory of a node and a face intersects during the cycle a contact event is detected.
The trajectory contact algorithm is the default and recommended option in most cases for contact in Explicit Dynamics analyses. Contacting nodes/faces can be initially separated or coincident at the start of the analysis. Trajectory based contact detection does not impose any constraint on the analysis time step and therefore often provides the most efficient solution.
Note that nodes which penetrate into another element at the start of the simulation will be ignored for the purposes of contact and thus should be avoided. To generate duplicate conforming nodes across a contact interface:
Use the multibody part option in DesignModeler and set Shared Topology to Imprint.
For meshing, use Contact Sizing, the Arbitrary match control or the Match mesh Where Possible option of the Patch Independent mesh method.

The external faces, edges and nodes of a mesh are encapsulated by a contact detection zone. If during the analysis a node enters this detection zone, it will be repelled using a penalty based force.

An additional constraint is applied to the analysis time step when this contact detection algorithm is selected. The time step is constrained such that a node cannot travel through a fraction of the contact detection zone size in one cycle. The fraction is defined by the Time Step Safety Factor described below. For analyses involving high velocities, the time step used in the analysis is often controlled by the contact algorithm.
The initial geometry/mesh must be defined such that there is a physical gap/separation of at least the contact detection zone size between nodes and faces in the model. The solver will give error messages if this criteria is not satisfied. This constraint means this option may not be practical for very complex assemblies.
Proximity Based Contact is not supported in 2D Explicit Dynamics analyses.
This property is available if Contact Detection is set to Trajectory.
The available choices are described below.
If contact is detected, a local penalty force is calculated to push the node involved in the contact event back to the face. Equal and opposite forces are calculated on the nodes of the face in order to conserve linear and angular momentum.
Trajectory based penalty force,
Proximity based penalty force,
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
Kinetic energy is not necessarily conserved. You can track conservation of energy in contact using the Solution Information object, the Solution Output, or one of the energy summary result trackers.
The applied penalty force will push the nodes back towards the true contact position during the cycle. However, it will usually take several cycles to satisfy the contact condition.
All contacts that take place at the same point in time are first detected. The response of the system to these contact events 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 cannot be used in combination with bonded contact regions. The formulation will be automatically switch to penalty if bonded regions are present in the model.
The decomposition response algorithm is more impulsive (in a given cycle) than the penalty method. This can give rise to large hourglass energies and energy errors.
This option is available if Contact Detection is set to Trajectory.
When a contact event is detected part way through a cycle and the contact node has a tangential velocity relative to the face it has made contact with, the node needs to slide along the face for the remainder of the cycle. If the node should slide to the edge of the face before the end of the cycle, it is necessary to determine whether the node needs to begin to slide along an adjacent face. Two options described below are available for determining which (if any) face the node needs to slide to.
When a node slides to the edge of a face, the next face the node needs to slide on is determined using the contact detection algorithm. This option is the default and will provide the most time efficient solution. However, penetrations of nodes may be seen in situations where the faces that the nodes are sliding on are experiencing large deformations or rotations. When such penetrations occur, it is recommended the user switches to the Connected Surface option.
When a node slides to the edge of a face, the next face the node needs to slide on is determined using the mesh connectivity.
These properties are available if the geometry includes one or more surface bodies and if Contact Detection is set to Trajectory.
The Shell Thickness Factor allows you to control the effective thickness of surface bodies used in the contact. You can specify a value between 0.0 and 1.0.
A value of 0.0 means that contact will ignore the physical thickness of the surface body and the contact surface will be coincident with the mid-plane of the shell.
A value of 1.0 means that the contact shell thickness will be equal to the physical shell thickness. The contact surface will be offset from the mid-plane of the shell by half the shell thickness (on both sides of the shell).
Nodal Shell Thickness is only active when the Shell Thickness Factor value is not zero (0). It allows you to obtain the most accurate shell to shell contact by improving on the Shell Thickness Factor approach.
When set to Yes, contact between shells is improved by eliminating the inherent small overlap that may occur even when the Shell Thickness Factor is set to 1.0. Essentially this setting (along with a thickness factor of 1.0) will provide the most accurate shell thickness contact behaviour.
When set to No, the contact shell thickness will be determined by the value of the Shell Thickness Factor and the nodal shell thickness will not have any effect.
When set to Program Controlled, the behavior of nodal shell thickness is determined by the Analysis Settings Preference Type.
When set to Yes, the contact detection algorithm will check for external nodes of a body contacting with faces of the same body in addition to other bodies. This is the most robust option since all possible external contacts should be detected.
When set to No, the contact detection algorithm will only check for external nodes of a body contacting with external faces of other bodies. This setting reduces the number of possible contact events and can therefore improve efficiency of the analysis. This option should not be used if a body is likely to fold onto itself during the analysis, as it would during plastic buckling for example.
When set to Program Controlled, the behavior of self contact is determined by the Analysis Settings Preference Type.
Presented below is an example of a model that includes self impact.

When set to Yes, automatic erosion (removal of elements) is enabled when an element deforms such that one of its nodes comes within a specified distance of one of its faces. In this situation, elements are removed before they become degenerated. Element self contact is very useful for impact penetration examples where removal of elements is essential to allow generation of a hole in a structure. Element removal through Element Self Contact is only activated when one of the erosion options under Erosion Controls is also set to Yes.

When set to Program Controlled, the behavior of self contact is determined by the Analysis Settings Preference Type.
This property is available if Contact Detection is set to Trajectory and Element Self Contact is set to Yes.
Tolerance defines the size of the detection zone for element self contact when the trajectory contact option is used (see Element Self Contact). The value input is a factor in the range 0.1 to 0.5. This factor is multiplied by the smallest characteristic dimension of the elements in the mesh to give a physical dimension. A setting of 0.5 effectively equates to 50% of the smallest element dimension in the model.
Note: The smaller the fraction the more accurate the solution.
This property is available if Contact Detection is set to Proximity Based.
The pinball factor defines the size of the detection zone for proximity based contact. The value input is a factor in the range 0.1 to 0.5. This factor is multiplied by the smallest characteristic dimension of the elements in the mesh to give a physical dimension. A setting of 0.5 effectively equates to 50% of the smallest element dimension in the model.
Note: The smaller the fraction the more accurate the solution. The time step in the analysis could be reduced significantly if small values are used (see Time Step Safety Factor).
This property is available if Contact Detection is set to Proximity Based.
For proximity based contact, the time step used in the analysis is additionally constrained by contact such that in one cycle, a node in the model cannot travel more than the detection zone size, multiplied by a safety factor. The safety factor is defined with this property and the recommended default is 0.2. Increasing the factor may increase the time step and hence reduce runtimes, but may also lead to missed contacts. The maximum value you can specify is 0.5.
This property is available if Contact Detection is set to Proximity Based.
For proximity based contact, this setting limits the maximum velocity that will be used to compute the proximity based contact time step calculation.
This property is available if Contact Detection is set to Proximity Based.
By default, contact events in Explicit Dynamics are detected by nodes impacting faces. Use this option to extend the contact detection to include discrete edges impacting other edges in the model.
Note: This option is numerically intensive and can significantly increase runtimes. It is recommended that you compare results with and without edge contact to make sure this feature is required.
A model with edge on edge contact cannot be run in parallel.
This section includes descriptions of the interaction types for the Body Interaction object:
Setting Type to Frictionless activates frictionless sliding contact between any exterior node and any exterior face of the scoped bodies. Individual contact events are detected and tracked during the analysis. The contact is symmetric between bodies (that is, each node will belong to a master face impacted by adjacent slave nodes; each node will also act as a slave impacting a master face).
Explicit Dynamics
| Connection Geometry | Volume | Shell | Line |
|---|---|---|---|
| Volume | Yes | Yes | Yes |
| Shell | Yes | Yes | Yes |
| Line | Yes | Yes | *Yes |
*Only for Contact Detection = Proximity Based and Edge on Edge Contact = Yes (This option switches on contact between ALL lines / bodies / edges; that is, there is no dependence on the scoping selection of body interactions.)
Workbench LS-DYNA
| Connection Geometry | Volume | Shell | Line |
|---|---|---|---|
| Volume | Yes | Yes | No |
| Shell | Yes | Yes | No |
| Line | No | No | No |
Setting Type to Frictional activates frictional sliding contact between any exterior node and any exterior face of the scoped bodies. Individual contact events are detected and tracked during the simulation. The contact is symmetric between bodies (that is, each node will belong to a master face impacted by adjacent slave nodes, each node will also act as a slave impacting a master face).
Friction Coefficient: A non-zero value will activate Coulomb type friction between bodies (F = μR).
The relative velocity (ν) of sliding interfaces can influence frictional forces. A dynamic frictional formulation for the coefficient of friction can be used.
(2–3) |
where
= friction coefficient
= dynamic coefficient of friction
β = exponential decay coefficient
ν = relative sliding velocity at point of contact
Non-zero values of the Dynamic Coefficient and Decay Constant should be used to apply dynamic friction.
Explicit Dynamics
| Connection Geometry | Volume | Shell | Line |
|---|---|---|---|
| Volume | Yes | Yes | Yes |
| Shell | Yes | Yes | Yes |
| Line | Yes | Yes | *Yes |
*Only for Contact Detection = Proximity Based and Edge on Edge Contact = Yes (This option switches on contact between ALL lines / bodies / edges; that is, there is no dependence on the scoping selection of body interactions.)
Workbench LS-DYNA
| Connection Geometry | Volume | Shell | Line |
|---|---|---|---|
| Volume | Yes | Yes | No |
| Shell | Yes | Yes | No |
| Line | No | No | No |
Descriptions of the following properties are also addressed in this section:
Maximum Offset
Breakable
Stress Criteria
Normal Stress Limit
Normal Stress Exponent
Shear Stress Limit
Shear Stress Exponent
External nodes of bodies included in bonded interactions will be tied to faces of bodies included in the interaction if the distance between the external node and the face is less than the value defined by the user in Maximum Offset. The solver automatically detects the bonded nodes/faces during the initialization phase of the analysis.
Note that it is important to select an appropriate value for the Maximum Offset. The automatic search will bond everything together which is found within this value.
During the analysis the nodes are kept at the same relative position on the face to which they are bonded. This is done by means of penalty forces which are either dependent on the mass of the nodes/faces or the stiffness of the material. The stiffness is weighted based on materials on either side of the bond. In models with mass scaling the penalty method is chosen based on the mass scaling setting:
Mass scaling off: Penalty method based on harmonic mass in the bonded pair.
Mass scaling on: Penalty method based on harmonic stiffness in the bonded pair.
| Origin of Model | Mass Scaling Off | Mass Scaling On |
|---|---|---|
| Any Workbench project opened in R18.0 or later | Harmonic Mass | Harmonic Stiffness |
Note: The stiffness weighted penalty method is typically superior to a mass weighted penalty and increases the robustness of (offset) bonds. By switching on mass scaling and still using a small target timestep (eg 1e-20) no mass will be added, but the penalty method will be switched to harmonic stiffness.
When large material stiffness occurs between two materials that are bonded, it is recommended that you use an asymmetric definition where the contact scope (nodes to be bonded) refers to the soft material and the target scope (faces to bond to) refers to the stiffer material.
Use the custom variable BOND_STATUS to check bonded connections in Explicit Dynamics. The variable records the number of nodes bonded to the faces on an element during the analysis. This can be used not only to verify that initial bonds are generated appropriately, but also to identify bonds that break during the simulation.
The automatic search algorithm for bonded regions will search for the minimum distance to any of the faces. If this minimum distance falls within the maximum offset value, the bond pair will be established. In order to compute the proper distance to a face the algorithm will determine if the perpendicular projection to the face falls within the face. If that is not the case, the perpendicular projection to the face edges is considered. If that is not the case, the distance to one of the face nodes is considered. This algorithm guarantees that a minimum distance is always found and can be properly compared against the value input for Maximum Offset.
Verification of the initialized bonds can be done by inspection of the prt file. A summary is given which lists the number of candidate nodes for bonding and the actual number of nodes that were bonded. If the percentage of nodes to be bonded is 0% it means none of the nodes are actually bonded. You should consider increasing the Maximum Offset in this case.

Maximum Offset defines the tolerance used at initialization to determine whether a node is bonded to a face.
Breakable = No implies that the bond will remain throughout the analysis.
Breakable = Stress Criteria implies that the bond may break (or be released) during the analysis. The criteria for breaking a bond is defined as:
(2–4) |
where
= Normal Stress Limit
n = Normal Stress Exponent
= Shear Stress Limit
m = Shear Stress Exponent
The Behavior option can be used as described in Behavior.
Auto Asymmetric behavior is dependent on the type of scoping:
Bonded connections with only faces scoped will behave symmetrically.
All other bonded connections (if the Contact or Target is scoped to a vertex or edge) will behave asymmetrically.
Note that there are two distinguishing factors during initialization based on behavior:
For symmetric bond behavior the perpendicular projection of a node to a face has to fall within the face bounds otherwise the bond pair is disregarded a candidate.
For asymmetric bond behavior the perpendicular projection of a node to a face does not have to fall within the face bounds in order to be considered as a candidate.
For both types of behavior the Maximum offset is always taken into account.
If needed, a symmetric bond definition can also be changed to search out-of-plane by taking the following steps:
Set the definition to Asymmetric in order to search out-of-plane
Duplicate the definition of the bond object (right-click operation)
Subsequently "flip" Contact and Target (right-click operation)
Effectively, you have created a symmetric definition (Contact->Target, Target->Contact) and bonds will be searched out of plane.
Symmetric bonds are disregarded for definitions that scope to a single part.
Asymmetric bonds are considered for definitions that scope to a single part.
The Trim Contact option is ignored by the Explicit solver.
Explicit Dynamics
See Supported Contact Types for more information.
Note: Bonded body interactions and contact are not supported for 2D Explicit Dynamics analyses.
Workbench LS-DYNA*
| Connection Geometry | Volume | Shell | Line |
|---|---|---|---|
| Volume | Yes | Yes | No |
| Shell | Yes | Yes | No |
| Line | Yes | Yes | No |
*The above matrix is valid only for Contact Regions. Bonded body interactions are not supported at all.
This body interaction type is used to apply discrete reinforcement to solid bodies. All line bodies scoped to the object will be flagged as potential discrete reinforcing bodies in the solver. On initialization of the solver, all elements of the line bodies scoped to the object which are contained within any solid body in the model will be converted to discrete reinforcement. Elements which lie outside all volume bodies will remain as standard line body elements.
The reinforcing beam nodes will be constrained to stay at the same initial parametric location within the volume element they reside during element deformation. Typical applications involve reinforced concrete or reinforced rubber structures likes tires and hoses.
If the volume element to which a reinforcing node is tied is eroded, the beam node bonding constraint is removed and becomes a free beam node.
On erosion of a reinforcing beam element node, if inertia is retained, the node will remain tied to the parametric location of the volume element. If inertia is not retained, the node will also be eroded.
Note: Volume elements that are intersected by reinforcement beams, but do not contain a beam node, will not be experiencing any reinforced beam forces. Good modeling practice is therefore to have the element size of the beams similar or less than that of the volume elements.
Note that the target solid bodies do not need to be scoped to this object – these will be identified automatically by the solver on initialization.
Explicit Dynamics
| Connection Geometry | Volume | Shell | Line |
|---|---|---|---|
| Volume | No | No | *Yes |
| Shell | No | No | No |
| Line | *Yes | No | No |
*Only the line body needs to be included in the scope. The Explicit Dynamics solver automatically detects which volume bodies that the line body passes through.
Note: Reinforcement body interactions are not supported for 2D Explicit Dynamics analyses.
Workbench LS-DYNA
| Connection Geometry | Volume | Shell | Line |
|---|---|---|---|
| Volume | No | No | No |
| Shell | No | No | No |
| Line | No | No | No |
See the description for Body Interactions for Selected Bodies in the section Correlating Tree Outline Objects with Model Characteristics in the ANSYS Mechanical User's Guide.