The Loads and Boundary Conditions form will appear when the Loads/BCs toggle, located on the Patran application selections, is chosen. When creating loads and boundary conditions there are several option menus. The selections made on the Loads and Boundary Conditions menu will determine which loads and boundary conditions form appears, and ultimately, which PAMCRASH loads and boundary conditions will be created.

The following pages give an introduction to the Loads and Boundary Conditions form, and details of all the loads and boundary conditions supported by the Patran PAMCRASH Analysis Preference.

This form appears when Loads/BCs is selected on the main form. The Loads and Boundary Conditions form is used to provide options to create the various PAMCRASH loads and boundary conditions. For a definition of full functionality, see Loads and Boundary Conditions Form (p. 21) in the Patran Reference Manual.

The following table outlines the options when Create is the selected action.

This subordinate form appears when the Input Data button is selected on the Loads and Boundary Conditions form when the Current Load Case Type is Static. The Current Load Case Type is set on the Load Case form, for more information see Loads and Boundary Conditions Form (p. 21) in the Patran Reference Manual. The information on the Input Data form will vary depending on the selected Object. Defined below is the standard information found on this form. Note that this form is not used with the Pamcrash Preference.

This subordinate form appears when the Input Data button is selected on the Loads and Boundary Condition form when the Current Load Case Type is Time Dependent. The Current Load Case Type is set on the Load Case form, for more information see Loads and Boundary Conditions Form (p. 21) in the Patran Reference Manual and Load Cases. The information on the Input Data form will vary, depending on the selected Object. However, it should be noted that not all LBC Objects support time dependence. Defined below is the standard information found on this form.

This section describes the user interface provided by Patran to access the contact features of explicit dynamics finite element codes. This interface is used during definition of the contact LBC types: Self Contact, Subsurface, Master-Slave Surface, and Master-Slave Node.

Tools have been provided to enable the user to quickly and easily define contact conditions. Specification of contact is conceptually simple, involving either one or two contact surfaces, and a set of contact parameters which control the interaction of the surfaces.

A contact condition in which a single logical surface may come into contact only with itself is described as self-contact, and requires the specification of a single Application Region. A contact condition in which two logical surfaces may contact each other is described as Master-Slave contact, and requires specification of two Application Regions. Master-Slave contact is further subdivided by the definition of Master-Slave Surface and Master-Slave Node. Master-Slave Surface describes the condition in which both the master and slave surfaces are defined using element faces, whereas Master-Slave Node describes the condition where the Slave surface is described only using nodes.

Tools are provided to enable the construction of contact surfaces, using the standard Patran select tool mechanisms (2D elements, 3D element faces), or groups. Contact subsurfaces can also be constructed using these tools, and later used to define a complete logical contact surface. This functionality allows the user to use the select tool to specify application regions on Patran geometry or the associated FEM entities or to define a more complex contact surface that is assembled from a mixture of 2D and 3D element faces, and to simply combine groups of 2D elements taking into account the direction of the contact outward normal. (For 2D elements, the outward normal can be reversed for contact purposes without modifying the underlying element topology.) Use of the group select mechanism is restricted to FEM entities only. Visualization of the specified contact condition is provided by graphically previewing but is not currently supported for geometry entities.

“Simple” contact surfaces include surfaces which may be described entirely by the faces of 3D elements, or by 2D elements whose outward normals are aligned with the desired contact normal direction. These contact surfaces may be constructed entirely using a single select mechanism (either Select Tool or Group method). Simple contact surfaces may not include a mixture of 3D element faces and 2D elements, or 2D elements whose outward normals are not all aligned with the desired contact normal direction.

“Complex” contact surfaces are defined as those surfaces which consist of a mixture of 2D elements and 3D element faces, or all 2D elements but with some of the outward normals incorrectly aligned. Contact conditions which include complex contact surfaces must be constructed using “Subsurfaces,” where each subsurface is a “Simple” contact surface. Definition of contact surfaces is limited to one method, i.e. it is not permissible to mix “Select Tool,” “Group,” or “Subsurface” within the definition of a contact surface.

The select tool is used to graphically select the desired entities from the model. When this method is selected, the user must specify which dimensionality the intended object has, i.e. 3D, 2D or Nodal. If the selected dimensionality is 2D, then the user can further specify whether the top, bottom or both surfaces option is required. Selection of top will result in a contact surface whose outward normal is coincident with the element outward normal, whereas selection of bottom will result in a contact surface whose outward normal is in the opposite direction to the element outward normal. The user can toggle
between Top, Bottom or Both at any time during selection; however, all of the selected entities will be assigned the same logical direction. Selection of 3D allows the user to select either all or all free faces
of 3D elements. No user specification of the contact normal direction is required for 3D elements since the program automatically specifies this direction. No contact direction is applicable to Nodal
contact surfaces.

It is not permissible to mix 3D, 2D and Nodal entities within a single Application Region. (This functionality is provided through the use of contact subsurfaces.) The select tool can be used to select on the basis of either FEM or Geometry entities.

The Group tool is used to define simple contact surfaces on the basis of Patran group names. When this method is selected, the user must specify which dimensionality the intended object has, i.e. either 3D, 2D or Nodal. The entities which will be selected for use in the contact surface in this case are either all 3D free surfaces in the group, all 2D elements or all nodes contained in the selected group. In the case of 2D elements, the user may specify whether the contact normal direction is coincident with the element top, bottom or both faces. Multiple groups may be selected. However, it should be noted that both the selected element dimensionality and contact normal direction apply across all selected groups.

Contact Subsurfaces may be defined using either of the above methods. Subsurfaces may then be used in the specification of Master, Slave or Self contact surfaces. When this option is used, the user may not specify element dimensionality or contact normal direction since this information has already been defined during subsurface definition. As many sub-surfaces as required may be selected to form the desired complex contact subsurface.

This form is used to define contact surfaces. The form will vary depending upon which options are selected; however, two basic configurations are used depending on whether the contact condition requires specification of a single contact surface or two contact surfaces.

The following form is used to define a single surface contact or a subsurface.

The following form is used to define either of the master slave contact types.

The Input Data form is used to specify parameters which control the behavior of the contact condition. The contents of the form will vary depending upon which option is selected. No Input Data is required for the Subsurface option since subsurfaces do not constitute a contact condition on their own.

There are areas on the static and transient input data forms where the load data values are defined. The data fields which appear depend on the selected load Object and Type. In some cases, the data fields also depend on the selected Target Element Type. The following Object Tables outline and define the various input data that pertains to a specific selected object:

This LBC type is used to define a BOUNC_/_ entry. The optional rigid body information on this entry is not supported. The optional local coordinate definition is generated if a local coordinate system is selected (FRAME_/_ entry). Time history information is ignored. The scale factor has no effect.

This LBC type is used to define a CONLO_/_ entry for concentrated loads on nodes. An auxiliary FUNCT_/_entry is defined from the time dependent field selected. The scale factor is used to scale the function, with default 1.0.Note that moments are not applicable

This LBC type is used to define a CONLO_/_ entry for follower forces on a plane defined by three nodes. An auxiliary FUNCT_/_ entry is defined from the time dependent field selected. The scale factor is used to scale the function, with default 1.0. Note that moments are not applicable. Note that Follower Forces are not supported for this Patran Pamcrash Preference version.

This LBC type is used to define a INVEL_/_ entry. The coordinate type will be cartesian unless a cylindrical axis is selected. Note that an initial velocity is required for every node in the model. Time history information is ignored.

Is this LBC type is used to define one or more VELBC_/_ entries. Displacement or Rotation Type 4 or 8 are used if a local coordinate is selected (but no FRAME_/_ entry is required). An auxiliary FUNCT_/_ entry is defined from the time dependent field selected (these apply to all translational and all rotational degrees of freedom). The scale factor is used to scale the function, with default 1.0. Note that PAMCRASH only allows for a center of rotation at the global origin. However, local coordinate systems can be used to define the components of velocity.

Four types of contact exist. Three of these are complete definitions and have associated input data. The fourth is the subsurface type which is used to define part of a contacting surface. This LBC type defines SLINT_/_ and SLINT2/_ entries. The following table outlines the options:

The contact input parameters are defined in the following table:

Note that there is a preview facility on the application Tool Form.

This LBC type is used to define a RIGWA_/_ entry and an auxiliary FUNCT_/_entry if a motion time history is defined. The following table outlines the options:

The input data for geometric rigid walls are as follows:

Note that you must select a local coordinate system that is used when generating the geometry of the wall (although the default global coordinate system can also be used). This coordinate system is centroidal-based not face-based as used by PAMCRASH. The Z-axis of this coordinate system defines the rigid wall outward normal. But note that the direction of motion is defined by the velocity vector not the outward normal vector. Note also that a facility for preview of the Rigid Wall and the slave nodes is provided on the input forms.

This LBC type is used to define a RIGWA_/_ entry for an infinite rigid wall and an auxiliary FUNCT_/_ entry if a motion time history is defined. The following table outlines the options:

The input data for planar rigid walls are as follows:

Note that you must select a local coordinate system that is used when generating the geometry of the wall (although the default global coordinate system can also be used). This coordinate system is centroidal-based not face-based as used by PAMCRASH. The Z-axis of this coordinate system defines the rigid wall outward normal. Note that the direction of motion is defined by the velocity vector, not the outward normal vector.

This LBC type is used to define a RIGBO_/_ entry for a rigid body defined by an assembly of nodes. No input data is required for the Computed option. The following table outlines the input data for the Defined Locally option:

Note that spotwelds and rivets are not supported.

This LBC type is used to define one or more NODCO_/_ entries for a group of nodes. The only input data required for nodal constraints is Translations and Coordinate Frame. Note that rivets are not supported. Time history information is ignored. The scale factor has no effect.

This LBC type is used to define a DAMP__/_ entry for a group of nodes. Time history information is ignored. The scale factor has no effect.