The External Gap contact algorithm is implemented for all Lagrange, ALE, shell, beam and unstructured solvers.
A gap is required for the interaction logic. The size of this gap must be in the range 1/10 to 1/2 the dimension of the smallest element face of Parts involved in interactions.
There are two contact algorithms available in 3D, External Gap and Trajectory
For most models you should set the gap size close to the smallest allowed value (1/10 the dimension of the smallest element face).
Enter a value for the Gap size in this field or click Calculate to have Autodyn set it for you.
Click this button to have Autodyn automatically calculate the Gap size for you. The Gap size will be set to 1/10 the dimension of the smallest element face of Parts involved in interactions.
All interacting Parts in your model must be separated by at least the Gap size. Click this button to automatically insert the required gap between Parts.
You may want to insert gaps manually using the Translate and / or Scale options in the zoning Panel Zoning panel.
Click this button to check that the Gap size is valid and that all Parts involved in interactions are separated by the Gap size.
Check this box if you want the interaction calculation to include testing for edge on edge impacts (significantly more computing is required if you check this box).
Select the size of work unit to be used for interactions:
The work unit size is based on the average cell dimension.
The work unit size is based on the smallest element dimension.
The work unit size is based on the largest element dimension.
Check this box if you want to retain the inertial of eroded nodes (otherwise eroded nodes are removed from the model).
Check this box if you want the interaction calculation to be used to stop elements from becoming degenerate. This option only works for Lagrange volume elements.
Warning: Activating this option can lead to unphysical results, particularly if a large Gap size is used.
Check this box if you want elements with over penetrated faces to be eroded.
You should only check this box if you know this option is required to successfully complete your calculation.
Sets interactions between Parts.
Sets all Parts to interact with each other.
Removes interactions between Parts.
Removes all interactions between Parts.
Sets interactions using a Part matrix.
Sets the index range of each Part that will be checked for interactions.
Sets static friction coefficients between different Parts.
Enables a review of all of your interaction settings.
Check this box if you want Parts to interact with themselves (i.e. test for self-impact).
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 the 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 available to faces of unstructured Parts and doesn't include friction.
Autodyn automatically calculates an Interaction Timestep based on the Gap size and the maximum velocity of the Parts involved in interactions.
The safety factor you want to use to calculate the Interaction Timestep.
You cannot enter a value greater than the default value (0.2).
The maximum velocity you want to use for calculating the Interaction Timestep.
This option is useful if you have large velocities controlling the timestep that are not involved in interactions.
The default limiting velocity is larger than any velocity your model should encounter.