Model.detectandcreateface2facecontacts

Model.detectandcreateface2facecontacts(collection, tolerance, reverse_angle, use_shell_thickness, consolidate_surfaces, run_intersection_check, contact_type, main_entity_type, secondary_entity_type, property_option, contact_property_id, static_friction_value, contact_material_id, contact_main_sensor_id, contact_secondary_sensor_id, skip_preview, consider_self, thickness_type, thickness_value, friction_direction, set_name_prefix, csurf_name_prefix, include_whole_components, copy_tolerance_to_contact, numExtraMainLayers, featureAngleForLayers)

Detects if the specified components are within the contact distance specified and creates contact entities relevant to the solver interface.

The current solver template is used as an implicit input.

The output contact entities are created specific to a supported solver. For example, in it will create contact surfaces and groups whereas in it will create groups with card images.

This is supported for ANSYS, OptiStruct, Nastran (MSC), and ADVC.

Parameters:

• collection (Collection) – The collection containing the entities to search for contact within the specified distance. Valid entities are components and elements.

• tolerance (double) – A non-zero search distance specified as the vicinity within which the contact is to be detected by executing the penetration collision logic. Components spaced greater than the vicinity tolerance are not considered to be in contact.

• reverse_angle (double) – The angle value used to compute the extent of the contact surface. This parameter is used in detecting the span of a convex contact surface on non-planar surfaces.

• use_shell_thickness (unsigned int) – A flag to use element thickness values specified on shell elements as the search distance. When this flag is specified as 1, then tolerance is ignored or can be 0.

• consolidate_surfaces (unsigned int) – After the contact is detected, contact surfaces are created. Those contact surfaces can be on different topological locations (discontinuous) on the base component that is in contact with that particular target component. When set as 0, a contact surface for each discontinuous patch is created and updated in the contact group. If set as 1, then only 1 contact surface is created for all the discontinuous patches.

• run_intersection_check (unsigned int) –

  Before a contact is detected and established using the penetration algorithm, the user has the option to execute the intersection check between any two components for the same input parameters of tolerance and reverse_angle by setting this as 1. Intersection is detected even if one element on the source component physically intersects an element on the target component. In such cases the contact surface normal is not uniquely defined for those intersecting elements.

  When this is 0, the intersection check is not executed. However, the contact will be detected and contact surfaces will be created, but the resulting contact surface normal may not be desirable.

• contact_type (unsigned int) –

  The type of contact to create. The following values are supported:

  Solver	Value	Type
  OptiStruct	0	contact
  	1	Tie
  Nastran (NX)	0	BCTSET
  	1	BGSET
  ADVC	0	Not specified
  	1	Tying
  	2	ShearTying
  	3	SmallSliding
  	4	FiniteSliding
  	5	NotSliding

• main_entity_type (unsigned int) –

  The main entity type. The following values are supported:

  Solver	Value	Type
  OptiStruct	0 (default)	SET_ELEM
  	1	SURF

• secondary_entity_type (unsigned int) –

  The secondary entity type. The following values are supported:

  Solver	contact_type	Value	Type
  OptiStruct	all	0	SET_GRID
  		1	SET_ELEM
  		2	SURF

• property_option (unsigned int) –

  The property option. The following values are supported:

  Solver	contact_type	Value	Type
  ANSYS	N/A	0	Existing property ID is used
  		1	Infer sensors and auto-generate properties
  OptiStruct	0 (Contact)	0	SLIDE
  		1	STICK
  		2	FREEZE
  Nastran (MSC)	N/A	<prop_id>	Geometric contact property ID (BCGPIC)

• contact_property_id (unsigned int) –

  On creation of contact pairs, some of the interfaces have attributes to select property ID as the input. When this argument is specified with an ID, and if it exists, it is attached to the contact pair. For non-relevant interfaces this will be ignored.

  Note that this argument supersedes property_option and static_friction_value, except for ANSYS. In ANSYS, if property_option is specified, then contact_property_id is ignored.

  In this is the physical contact property (BCPPID).

  This is relevant for ANSYS, Nastran, Nastran (NX), and OptiStruct.

  For the ADVC interface, a contact pair can be assigned with friction ID. When this argument is specified with friction ID (as an integer), and if it exists, it is attached to the generated contact pair.

• static_friction_value (double) –

  The value for the static friction coefficient. This is superseded by contact_property_id and property_option arguments. If contact_property_id, property_option arguments and static_friction_value are all specified, contact_property_id takes precedence. If property_option and static_friction_value are both specified, property_option takes precedence. In both cases, the friction value is adjusted internally to a negative number to establish precedence and thus will be ignored.

  This is only relevant for OptiStruct.

• contact_material_id (unsigned int) –

  On creation of contact pairs, some of the interfaces have attributes to select material ID as the input. When this argument is specified with such an ID, and if it exists, it is attached to the contact pair. For non-relevant interfaces this will be ignored.

  This is only relevant for ANSYS.

• contact_main_sensor_id (unsigned int) –

  On creation of contact pairs, some of the interfaces have attributes to select main sensor ID as the input. When this argument is specified with such an ID, and if it exists, it is attached to the contact pair. For non-relevant interfaces this will be ignored. In ANSYS, property_option is ignored when specified along with this option.

  This is only relevant for ANSYS.

• contact_secondary_sensor_id (unsigned int) –

  On creation of contact pairs, some of the interfaces have attributes to select secondary sensor ID as the input. When this argument is specified with such an ID, and if it exists, it is attached to the contact pair. For non-relevant interfaces this will be ignored. In ANSYS, property_option is ignored when specified along with this option.

  This is only relevant for ANSYS.

• skip_preview (unsigned int) – After creation of contact entities, when specified as 0, all the newly created contact entities are considered to be “under review” and their export flag is turned off. If you choose to confirm all the auto-contact created entities and have their export flag turned on, this should be 1 or 2. When specified as 1, a confirmation dialog box with the entities list is also skipped.

• consider_self (unsigned int) – Consider elements in the same component for creation of contacts. By default (0), elements within the same components are not considered for the creation of contacts. If a single component is selected as input, this should be set to 1.

• thickness_type (unsigned int) –

  The parameter defining the interpretation of thickness_value.

  0 - thickness_value will be added to the thicknesses of shell elements. (default)

  1 - thickness_value specifies a multiplication factor for shell elements.

• thickness_value (double) – Based on the thickness_type value, this is either an add-on value or a multiplication factor for shell thicknesses during proximity detection.

• friction_direction (hwString) –

  The value of parameter friction on the created $CONTACT cards.

  This is only relevant for Permas.

• set_name_prefix (hwString) –

  The optional prefix string for created Set entities.

  This is only relevant for OptiStruct, Radioss, LS-DYNA, Nastran, Permas, and ADVC.

• csurf_name_prefix (hwString) –

  The optional prefix string for the created contact surface entities.

  This is only relevant for OptiStruct, Radioss, Abaqus, and LS-DYNA.

• include_whole_components (unsigned int) –

  0 - Only the elements detected during the proximity check are included in the created contact surfaces (default).

  1 - The contact surfaces will include entire components even if only a few elements of the component are detected during the proximity check.

  This is only relevant for Abaqus.

• copy_tolerance_to_contact (unsigned int) –

  Copies the tolerance value specified by the user to a relevant search distance parameter on the created group entity. By default (0), no value is copied to the createdgroup entity. When specified as 1, the specified tolerance value is copied to the following parameter on the created group entity:

  Solver	Group Parameter
  OptiStruct	SRCHDIS

• numExtraMainLayers (unsigned int) –

  Applicable only to Abaqus. Defines the number of extra face or element layers to add to the main surfaces. This ensures that the main surfaces are larger than their corresponding secondary surfaces.

  If set to 0 (default), no extra face or element layers are added to the main surfaces.

  The extra face or element layers are terminated at feature edges defined by featureAngleForLayers.

• featureAngleForLayers (double) –

  Applicable only to Abaqus. Specifies the angle in degrees that defines feature edges when adding extra face or element layers to the main surfaces, that is, when numExtraMainLayers > 0.

  If less than 0, extra layers of faces or elements are not terminated at any feature edges and numExtraMainLayers of faces or elements are simply added to the main surfaces.

Examples

Detect contacts between all components in the model by use tolerance of 1.o and reverse angl of 15.0 degrees

import hm
import hm.entities as ent

model = hm.Model()

# Creating a collection that contains the elements to be detached
components_collection = hm.Collection(model, ent.Component)

model.detectandcreateface2facecontacts(
    collection=components_collection, tolerance=1.0, reverse_angle=15.0
)

Create contacts between components by use shell thickness and consolidate surfaces

import hm
import hm.entities as ent

model = hm.Model()

# Creating a collection that contains the elements to be detached
components_collection = hm.Collection(model, ent.Component)

model.detectandcreateface2facecontacts(
    collection=components_collection,
    tolerance=0,
    reverse_angle=15.0,
    use_shell_thickness=1,
)

Create contacts in ANSYS with property with ID 1 , material with ID 2 , main and secondary sensor with IDs ( 3,4 respectively ) specified

import hm
import hm.entities as ent

model = hm.Model()

# Creating a collection that contains the elements to be detached
components_collection = hm.Collection(model, ent.Component)

model.detectandcreateface2facecontacts(
    collection=components_collection,
    tolerance=1.0,
    reverse_angle=15.0,
    thickness_type=0,
    use_shell_thickness=0,
    consolidate_surfaces=1,
    run_intersection_check=0,
    contact_type=0,
    main_entity_type=0,
    secondary_entity_type=0,
    property_option=1,
    contact_property_id=0,
    contact_material_id=2,
    contact_main_sensor_id=3,
    contact_secondary_sensor_id=4,
)

Run an intersection check and create contact entities in OptiStruct with main entity type as SURF(1 ) and secondary entity type as SURF(2 ) with static friction coefficient as 0.18

import hm
import hm.entities as ent

model = hm.Model()

# Creating a collection that contains the elements to be detached
components_collection = hm.Collection(model, ent.Component)

model.detectandcreateface2facecontacts(
    collection=components_collection,
    tolerance=5.0,
    reverse_angle=15.0,
    use_shell_thickness=0,
    consolidate_surfaces=1,
    run_intersection_check=1,
    contact_type=0,
    main_entity_type=1,
    secondary_entity_type=2,
    property_option=0,
    contact_property_id=0,
    static_friction_value=0.18,
)

Run intersection check and create contact entities in OptiStruct with main entity type as SET OF ELEMENTS(0 ) and secondary entity type as SET OF NODES(1 ) with property option as STICK(1 )

import hm
import hm.entities as ent

model = hm.Model()

# Creating a collection that contains the elements to be detached
components_collection = hm.Collection(model, ent.Component)

model.detectandcreateface2facecontacts(
    collection=components_collection,
    tolerance=5.0,
    reverse_angle=15.0,
    use_shell_thickness=0,
    consolidate_surfaces=1,
    run_intersection_check=1,
    contact_type=0,
    main_entity_type=0,
    secondary_entity_type=1,
    property_option=1,
)