**Interaction Trajectory (Trajectory options)**The Trajectory contact algorithm is implemented for all unstructured Lagrangian solvers and SPH.

**Method**Method in which a contacting node is pushed back to the true contact position during the computational cycle.

There are three methods available:

**None**No contact defined.

**Penalty**If a contact event is detected, a local penalty force is calculated to push the node back to the face. Equal and opposite forces are calculated on the nodes of the face in order to conserve linear and angular momentum. The applied penalty force will push the node back towards the true contact position during the cycle. However, it will take several cycles to satisfy the contact condition. Kinetic energy is not necessarily conserved. The conservation of energy can be tracked using the energy time history.

**Decomposition Response (DCR)**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 the nodes and faces does not result in further penetration at that point in time. The decomposition response algorithm is more impulsive (in a given computational cycle) than the penalty method. This can give rise to large hourglass energies and energy errors.

**Shell thickness factor**The value of the factor has to be taken between 0.0 and 1.0 and determines the amount of the shell thickness that is taken into account as the interaction distance. A factor of 1.0 takes the full shell thickness into account, which means that the contact surface is positioned at half the 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.

Note that for shell node on shell face impacts, the node is always located at the mid-surface of the shell. Therefore, two shell parts with thickness δ

_{1}and δ_{2}will not contact at a distance of (δ_{1}/2 + δ_{2}/2), but at a distance which is half of the largest shell thickness as is depicted below.Note that for shell node on solid face impacts, the node will be able to get to within zero distance of the solid face; the thickness for the shell nodes will not be taken into account. The solid nodes will, however, find the shell faces at contact distance.

**Initial Penetrations****Check**On clicking this button, Autodyn will search the model for initial penetrations of nodes into surfaces. If any penetrating nodes/surfaces are found, a new Group will be created so that they can be identified/displayed using the Groups panel. Nodes that initially penetrate surfaces will be "missed" by the contact algorithm.

**Fix**When this option is selected the initially penetrated nodes are set back to the closest contact surface and no initial penetrations are present at the start of the analysis.

This option is meant for situations where small initial penetrations occur (for example because of round-off) and should be used with care because the analysis model geometry is changed.

Note that it may not be possible to remove all initial penetrations with this algorithm. Features are available in the DesignModeler and Meshing application to prevent initial penetrations occurring.

**Undo**This option will restore the geometry of the analysis model before the initial penetrations were fixed.

It is recommended that the fixed initial penetrations are checked before the model is modified further otherwise it may not be possible to undo the last fix operation.

**Erosion****Retain inertia of eroded nodes**Check this box if you want to retain the inertial of eroded nodes (otherwise eroded nodes are removed from the model).

**Interaction by Part****Add**Sets interactions between Parts.

**Add All**Sets all Parts to interact with each other.

**Remove**Removes interactions between Parts.

**Remove All**Removes all interactions between Parts.

**Matrix**Sets interactions using a Part matrix.

**Range**Sets the index range of each Part that will be checked for interactions.

**Friction**Sets static friction coefficients between different Parts.

**Review**Enables a review of all of your interaction settings.

**User defined friction**Aside from the friction definition through the interaction by Part method described above there is also a user defined friction option available through the use of a user-subroutine called EXFRICTION.

**Self Interaction**If the self-interaction option is switched on the contact detection algorithm will also check for external nodes of a part contacting with faces of the same part in addition to other parts. This is the most robust contact setting since all possible external contacts should be detected.

**Self-interaction Tol.**The self-interaction option enables automatic erosion when an element deforms such that one of its nodes comes within a specified distance of one of its faces. This option will prevent volume elements becoming degenerate.

The specified distance is calculated using the Self-interaction Tol. value which 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.

**Interaction by Group**In many calculations, the contact region may be relatively small in comparison to the entire model, and as the interactions calculation is numerically intensive, it would be beneficial if the scope of its work were limited to this smaller area. The Group Contact option enables you to select a set of face groups to describe the extent of the interactions in unstructured models.

Select the "Specify Group Contacts by Group" toggle and click Select, to open the "Select Groups to include in Contact" dialog, and use the Add/Remove button to specify which face groups are to be included in the contact calculations.

During execution, any faces eroded will be removed from the group, and any new faces uncovered will be added to a group named "Uncovered faces". Unstructured Beams and SPH can also be included as a node group to participate in contact.

Note that Group Contact is additive to Part contact. Selecting a Part for contact results in all external faces in that Part being checked for contact. Group contact should be used to add additional external faces from Parts that have been excluded from contact in the Part interaction matrix.

Group contact is only applicable to faces of unstructured Parts and does not include friction.