Use the Contact Browser to create, review and modify contact
interfaces and surfaces in a model.
From the menu bar, click View > Browsers > HyperMesh > Contact.
Contact interfaces and surfaces can be imported, created manually, or generated
automatically using the AutoContact option. Upon importing a solver deck or HyperMesh model, existing contacts are created and populated in the
Contact Browser. Contact interfaces and surfaces are
organized into their respective folders in the browser.
Browser Interface
The Contact Browser consists of three panes; the first pane
displays the entities needed for contact definition, the second pane displays the
contact information, and the third pane displays the Entity Editor. Figure 1.
Create Contacts
Create Contacts Manually
In the Contact Browser you can manually create
contacts.
In the first pane of the Contact Browser, right-click and
select Create from the context menu to create all of the entities needed for contact definition, such as contact
surfaces.
In the second pane of the Contact Browser, right-click and
select Create from the context menu to create contacts.
The Entity Editor opens and displays the new
contact.
Note: The entities available in the context menu will vary depending on the user profile
loaded.
Assign Main and Secondary entities when creating contact pairs and contact
ties.
Define additional entity parameters and properties accordingly.
Figure 2. . Contact Browser and Entity Editor in the OptiStruct user profile.
Generate Contacts Automatically
Auto contact generation works independent of whether the model is FE or geometric.
When you elect to generate contacts automatically, contact bodies are detected and contact
pairs and contact sets are created.
In the Contact Browser, right-click and select
AutoContact from the context menu.
The Create AutoContact dialog opens.
Tip: To select all of the components in the model, right-click on the
Components folder.
In the Pick application region field, select components to create contact
interfaces and contact surfaces between.
Note: You must select a minimum of two components.
Define contact parameters and properties accordingly.
Select a Contact tolerance type.
If Vicinity tolerance is selected, you must enter a vicinity tolerance
value.
Enable Consolidate contact pair to group
multiple isolated surfaces into one surface.
Create and assign, or pick an existing property to attach to the
contact pair.
Specify a Thickness Type (either Add
On or Multiplier).
Click Create.
Based on a vicinity tolerance, the AutoContact tool searches throughout
all of the selected components and automatically creates new Contact interfaces
and contact surfaces between them. All the objects created are populated in the
Contact Browser into their respective folders. Figure 3.
AutoContact Logic
The following logic applies in the selection of surfaces for AutoContact in the order
it is written.
The surface of the component or element set defined as rigid body, and the
surface defined as rigid surface, will always be a main surface.
The surface of a component, or an element set with coarser mesh, will be a main
surface.
The surface of a component, or an element with less stiffness in comparison with
the mating surface, will be a secondary surface.
The larger surface will be identified as a main surface.
Modify Contact Interfaces and Surfaces
The Contact Browser lists every contact interface and surface
within a HyperMesh session and organizes them into their respective
folders. You can modify these contact interfaces and surfaces using the Entity Editor.
In the Contact Browser, click a contact interface or
surface.
The Entity Editor opens and displays the
entities corresponding data.
Note: If you select multiple entities in the
browser, the Entity Editor displays the selected entities common corresponding data. The rows that
contain ### indicate that these fields do not contain common data but can
still be modified. When you modify the data, both common and ambiguous,
HyperMesh applies the changes to all of the selected
entities. To select multiple entities, left-click entities while pressing
Control.
Figure 4.
In the Entity Editor, modify the contact parameters and
properties accordingly.
Modifications are automatically applied throughout the model.
Solver Specific Details
Abaqus
The Contact Browser supports the following contact and
constraint definitions for Standard and Explicit profiles of Abaqus:
AutoContact
Contact pair
General contact
Contact Tie
Shell to Solid coupling
The AutoContact option creates contact pairs and tie constraints depending
on whether you set Contact Type to Contact or Tie.
While using AutoContact, you can specify to have the secondary surface be
created as a node-based surface.
All contact pair definitions in Abaqus will
require a surface interaction definition.
AutoContact creates a surface interaction property with default
solver behavior.
You can choose an existing surface interaction to be used for
contact pairs recognized by AutoContact.
AutoContact can create contact pair/tie with review status before
confirming.
In the contact information pane (middle pane in the browser), you can
interactively add friction, adjust, and specify other optional
parameters.
Use Advanced delete to delete contact pair/tie. The corresponding main and
secondary surfaces and surface property are used for the contact pair unless
the surface property is otherwise specified to be used in other contact pair
definitions.
ANSYS
Creating and managing contact surfaces and pairs is handled by the Contact Browser.
Both manual contacts and AutoContact options are available. The AutoContact
option can be used to create Surface to Surface contacts.
Before creating contact pairs in HyperMesh, it is
recommend that you know which ANSYS contacts are
supported in HyperMesh.
ANSYS contact regions are modeled like ordinary
FE elements over the regions of FE models that represent the geometry. In
ANSYS terms, both CONTACT and TARGET
surfaces are sets of elements at contact regions. Prior to HyperMesh 14.0.130, the ANSYS
interface supported the same principle as ANSYS,
therefore both CONTACT and TARGET regions were elements over model geometry
in HyperMesh.
Starting in HyperMesh 14.0.130, both contact and target
regions are identified as CONTACT SURFACES. A pair of contact and target
surfaces which interact with each other in analysis are GROUPS. You need to
create contact surfaces for both CONTACT and TARGET regions. They will then
be paired together under groups to successfully define the contacts.
ANSYS solver files
(*.cdb files) with contacts are imported into
HyperMesh, and identify the contact regions from the
contact elements to show the regions as contact surfaces. Contact pairs can
be seen in groups.
During export, HyperMesh creates contact elements from the
contact regions and exports them as elements. In ANSYS, they are explained above elements with contact
element type.
The Contact Browser currently supports the creation of
edge to edge, surface to surface, and point o surface contacts with pilot
node and symmetry contact options. Figure 5. HyperMesh 14.0.120 and
Earlier Figure 6. HyperMesh 14.0.130
Nastran (MSC)
The AutoContact option will create new contact cards using their default
values.
When reading legacy models (.bdf, .dat and .hm), old contacts will be mapped
to new contact cards.
Contact parameters in the BCTABLE card are mapped to equivalent contact
properties (BCONPRP and BCONPRG) in new contact cards.
Properties associated with BCPROP should be assigned to either elements or
respective components in the contact card.
You can export old contact cards by enabling the Export old Contact Card
checkbox, which can be accessed in the in the Export-Solver Deck Browser
when you click Select Options.
The Contact group entity is mapped to the BCTABL1 solver card.
The BCTABL1 solver card contains a list of contact pair (BCONECT)
cards.
The AutoContact option will create a BCONECT card for each pair, and group
all pairs in the BCTABL1 card.
BSURF and BCBODY1 solver cards are remapped from group entities to set
entities.
BSURF and BCBODY1 are combined into one entity. Input for BCBODY1 can be
defined in the BSURF card with the Entity Editor.
Nastran (NX)
The Contact group entity is mapped to the BCTADD/BGADD solver cards.
The BCTADD and BGADD solver card contains a list BCTSET and BGSET cards
respectively.
The AutoContact option will create BCTSET/BGSET card for each pair, and
group all pairs in the BCTADD/BGADD solver card.
BSURF and BCRPARA solver cards are combined into one entity and migrated
from group entity to set entity. BSURF defines the contact region using
shell elements.
BSURFS and BCRPARA are combined into one entity and migrated from group
entity to set segment entity. BSURFS defines the contact region using solid
elements.
Input for BCRPARA can be defined in the BSURF/BSURFS card with the Entity Editor.
BGPARM, BCTPARM, BCTPARA are migrated to property entity. BGPARM is valid
only for glue contact BGSET and BCTPARM/BCTPARA are valid only for friction
contact BCTSET.
Subcase dependent contacts can be defined through the case control card
under subcase options in the loadstep entity.
OptiStruct
The Contact type, Contact, creates a contact pair, and the Contact type,
Tie, creates a Tie contact.
Master ID and Slave ID types will be as per solver default Set of elements
for master ID and Set of nodes for slave ID.
Auto contact will honor the entity type in Master and Slave entity
type.
Master entity types have the following mutually exclusive options: Set of
elements or SURF. Similarly Slave entity type will have Set of nodes, Set of
elements, and SURF. You can only select one of the entities.
The Contact property option is only available when the Contact type is
Contact.
You can assign Contact contacts a Property type (SLIDE,
STICK, FREEZE), a Static Friction
Coefficient, or an existing property (PCONT).
Permas
The Contact Browser supports the following definitions for the
Permas interface:
CONTACT_SURFACE_SURFACE
CONTACT_SURFACE_SURFNODE
CONTACT_SURFACE_NODE
CONTACT_NODE_NODE
Using AutoContact:
The AutoContact option creates a contact type based on the secondary and
main, which are set in the AutoContact Window.
While using AutoContact, you can specify having the secondary surface be
created as a node-based surface.
All contact pair definitions in Permas require a
friction to be defined. This is set to NO by default, but can be
changed.
AutoContact can create contact pairs with review status before
confirming.
In the contact information pane (middle pane in the browser), you can
interactively add friction, adjust, and specify other optional
parameters.
Use Advanced Delete to delete contact pairs with corresponding main and
secondary surfaces.
Samcef
Automatically detect the contacts between selected parts.
Create different type of contacts (.MCT/.STI).
Modify the contacts already created: add/remove elements/nodes into the
main/secondary groups, change the type of the contacts (MCT to STI or STI to
MCT).
Review the contacts in the model.
Context Menu
The following options are available in the Contact Browsercontext menu:
Review
Highlights the secondary and main surfaces in two different colors,
while the rest of the model is transparent and gray. Figure 7.
Show
Displays the contact's main and secondary surfaces in their assigned
colors. The rest of the model display is left unchanged.
Hide
Turns off the display the contact's surfaces. The rest of the model
display is left unchanged.
Isolate Only
Fits the selected contact to the graphics area, and displays the
secondary and main bodies in two different colors. The rest of the model
is turned off.
Swap Master-Slave
Switches the contact surfaces identified as master and slave. Upon
selecting Swap Master-Slave, the surfaces switch from places in the
master to slave positions in the browser.
To select multiple entities, left-click entities while pressing Control.
Swap Cp-Tie
Changes the type of interface created. A surface interaction is required
for Contact Pairs but not for a Tie, therefore any surface interaction
identified earlier will be lost upon swapping from CP to TIE. If you
switch back from TIE to CP, the surface interaction will not be
retained.
Reverse Normals
Flips all the normals of selected elements or surfaces.
Display Normals
Displays the normals of selected elements or surfaces as vectors or in
color mode.
Display Base Element Normals
Displays the normals for parent elements of the surface.
