Contact data

Contact data

 

Description

 

The data structures and keywords for Abaqus style input of Contact data are described. These include:

1.*CONTACT PROPERTY

2.*CONTACT SET

3.*CONTACT SURFACE

 

 

Click to expand/collapseCONTACT PROPERTY   Contact models property data

Usage

*CONTACT PROPERTY,  NAME=Property_name

Description

It is used to create a ParaGeo Contact_property data structure. It requires definition of the models to be used via *NORMAL, *TANGENTIAL and/or *ADHESION.

 

Compulsory Parameters

NAME

It defines a name for the contact property for reference. This is required to assign a contact property to a contact set for example.

 

 

Sub-Keywords
hmtoggle_plus1*ADHESION         Adhesion model and properties

Usage

*ADHESION, PENALTY=Value, TYPE=Adhesion_model

Description

Defines that an Adhesion model will be used in a contact property. It is used to incorporate the Adhesion_model keyword in the ParaGeo Contact_property data structure.

 

Compulsory Parameters

PENALTY

Defines a value for the adhesion penalty stiffness.

TYPE

Defines the adhesion model to be used. Valid values are:

- NONE

- ELASTIC

- MAXIMUM STRESS

- SIMPLE DEBONDING

 

More information on Adhesion models bellow.

 

None

Adhesion is not used in the current contact property.

 

Model 1 - Elastic (fully bonded)

This model assumes that debonding only occurs if either the normal gap is greater than the field distance or tangential slip is sufficient for the contactor node to be no longer opposite a target facet. The values expected are:

 

Location 1 - Adhesion stiffness (penalty) ( Kadh)

 

Model 2 - Maximum Stress (fully bonded)

This model assumes that debonding only occurs if either the normal gap is greater than the field distance or tangential slip is sufficient for the contactor node to be no longer opposite a target facet. The adhesion stress is however limited to a maximum value. The values expected are:

 

Location 1 - Adhesion stiffness (penalty) ( Kadh)

Location 2 - Maximum adhesion stress (+ve) ( ft)

 

Model 3 - Simple Debonding

The simple debonding model assumes that the contact points have an initial bond strength, and that if this value is exceeded the bond will be damaged resulting in a reduction in bond strength with continued opening displacement. The slope of the softening curve is defined by a specifying fracture energy ( Gf ). The values expected are:

 

Location 1 - Adhesion stiffness (penalty) ( Kadh)

Location 2 - Maximum adhesion stress (+ve) ( ft)

Location 3 - Fracture energy ( Gf)

 

Notes

•Following the definition of the ADHESION keyword and its corresponding parameters a series of comma separated values to define the adhesion properties should be provided.

•The number of adhesion properties is dependent on the adhesion model (see adhesion models above).

 
hmtoggle_plus1*DEPTH DEPENDENCE         Contact depth dependent properties

Usage

*DEPTH DEPENDENCE,  TYPE=Model_to_be_depth_dependent

Description

Defines contact properties as a function of depth. Values are provided as an space delimited table as follows:

 

Value 1

Value 2

...

Value n

Value n+1

Property 1

Property 2

...

Property n

Depth

 

Where n is the number of contact model properties (which is model dependent)

 

 

Compulsory Parameters

TYPE

Defines which contact model is linked to the current depth dependence. Valid values are:

- NORMAL

- TANGENTIAL

- ADHESION

 

 
Notes

•One *DEPTH DEPENDENCE sub-keyword for each contact model defined can be specified

•*DEPTH DEPENDENCE should not be used if *FIELD DEPENDENCE is defined in the same contact property

 
hmtoggle_plus1*FIELD DEPENDENCE         Field dependent properties

Usage

*FIELD DEPENDENCE

Description

If defined the stiffness for all active contact models (compression, adhesion and tangential) will be scaled by the amount of penetration so that the stiffness increases with increasing penetration. The stiffness factor is evaluated by linear interpolation from the lower factor at the lower reference penetration to the upper factor at the upper reference penetration. The actual stiffness factor used is also dependent on the maximum change in contact stiffness between time steps. This option will be used  to incorporate Field_dep_stiffness_model and Field_dep_stiffness_properties keywords to the current ParaGeo Contact_property data structure. When the penetration dependent model is used five space separated values should be provided:

       Location 1 - Lower factor for stiffness (default 0.1)

       Location 2 - Upper factor for stiffness (default 2.0)

       Location 3 - Lower reference field penetration factor (default 0.0)

       Location 4 - Upper reference field penetration factor (default 0.2)

       Location 5 - Maximum change factor (default 1.002)

 

Notes

•*FIELD DEPENDENCE should not be used if *DEPTH DEPENDENCE is defined in the same contact property

 
hmtoggle_plus1*NORMAL         Normal contact model and properties

Usage

*NORMAL,  PENALTY=Value,  TYPE=Normal_penetration_model

Description

Defines that a Normal penetration contact model will be used in a contact property. It is used to incorporate the Compression_model keyword in the ParaGeo Contact_property data structure.

 

Compulsory Parameters

PENALTY

Defines a value for the normal penalty stiffness.

TYPE

Defines the normal penalty model to be used. Valid values are:

- CONSTANT (Default)

 
hmtoggle_plus1*TANGENTIAL         Tangential model and properties

Usage

*TANGENTIAL,  PENALTY=Value,  TYPE=Tangential_model

Description

Defines that a Tangential contact model will be used in a contact property. It is used to incorporate the Tangential_model keyword in the ParaGeo Contact_property data structure.

 

Compulsory Parameters

PENALTY

Defines a value for the tangential penalty stiffness.

TYPE

Defines the tangential contact model to be used. Valid values are:

- ELASTIC

- COULOMB

- MAXIMUM STRESS

- MOHR COULOMB

 

More information on contact tangential models bellow.

 

Model 1 - Elastic (no slip)

This model assumes that all contact points are fully bonded ("tied") and the expected parameters are:

 

Location 1 - Tangential Stiffness (Penalty) ( Kt )

 

 

Model 2 - Coulomb friction model

The Coulomb friction model allows frictional slip if:

|σt|>μ |σn|

where σt the tangential stress, σn is the normal stress and μ is the friction coefficient.

The expected values are:

 

Location 1 - Tangential Stiffness (Penalty) ( Kt )

Location 2 - Friction coefficient ( μ )

 

 

Model 3 - Maximum stress model

The maximum stress model allows frictional slip if:

|σt|>σt(max)

where σt the tangential stress and σt(max) is the maximum allowable tangential stress.

The expected values are:

 

Location 1 - Tangential Stiffness (Penalty) ( Kt )

Location 2 - Maximum stress (σt(max))

 

 

Model 4 - Mohr Coulomb friction model

The Mohr Coulomb friction model allows frictional slip if:

|σt|>c+μ |σn|

where σt the tangential stress, σn is the normal stress, c is the cohesion and μ is the friction coefficient.

The expected values are:

 

Location 1 - Tangential Stiffness (Penalty) ( Kt )

Location 2 - cohesion ( c )

Location 3 - Friction coefficient ( μ )

 

 

Notes  

•Following the definition of the TANGENTIAL keyword and its corresponding parameters a series of comma separated values to define the tangential contact properties should be provided.

•The number of tangential properties is dependent on the tangential model (see tangential contact models above).

 

 

 

Examples

 

*CONTACT PROPERTY,NAME=Contact_fault

*NORMAL, PENALTY=500, TYPE=CONSTANT

*TANGENTIAL, PENALTY=500, TYPE=COULOMB

 0.2

*ADHESION, PENALTY=1000, TYPE=ELASTIC

*FIELD DEPENDENCE

 0.1, 4.0, 0.0, 0.2, 1.002

 

1The contact property is named "Contact_fault"

2The contact property will consider Normal, Tangential and Adhesion contact models.

3The reference normal penalty stiffness is 500 MPa

4The tangential model is Coulomb with a penalty stiffness of 500 MPa and a coefficient of friction of 0.2

5Adhesion model is elastic with a normal penalty of 1000 MPa

6All Normal, Tangential and Adhesion model are field dependent so the stiffness will be scaled accordingly

 

 

*CONTACT PROPERTY,NAME=Contact_fault2

*NORMAL, PENALTY=500, TYPE=CONSTANT

*TANGENTIAL, PENALTY=500, TYPE=COULOMB

 0.2

*ADHESION, PENALTY=1000, TYPE=ELASTIC

*DEPTH DEPENDENCE, TYPE=NORMAL

 50,   0

 500,  500

 750,  1000

 1000, 2000

*DEPTH DEPENDENCE, TYPE=TANGENTIAL

 50,   0.2, 0

 500,  0.2, 500

 750,  0.2, 1000

 1000, 0.2, 2000

*DEPTH DEPENDENCE, TYPE=ADHESION

 50,   0

 1000, 500

 2000, 1000

 2000, 2000

 

 

1The contact property is named "Contact_fault2"

2The contact property will consider Normal, Tangential and Adhesion contact models.

3The reference normal penalty stiffness is 500 MPa

4The tangential model is Coulomb with a penalty stiffness is 500 MPa and a coefficient of friction of 0.2

5Adhesion model is elastic with a normal penalty of 1000 MPa

6A depth dependence function is provided for all contact models active in property "Contact_fault2"

 

 

Click to expand/collapseCONTACT SET     Contact set data

Usage

*CONTACT SET,  NAME=Contact_set_name, PROPERTY=Property_name, FREQUENCY=Value, OUTPUT=Value, BUFFER=Value, FIELD=Value, SELF CONTACT=Value

Description

It is used to create a ParaGeo Contact_set data structure. It is used to define properties and options common to a list of contact surfaces (geometry sets). The list of geometry sets included in the present contact set should be provided after *CONTACT SET keyword and its corresponding parameters in a comma separated format.

 

Compulsory Parameters

NAME

Defines a name for the contact set for reference.

PROPERTY

Assigns a contact property (by name) to the contact set.

FREQUENCY

Defines the frequency (steps) of global searches to update the contact list.

OUTPUT

Defines the output level for contact search information

 

Optional Parameters

OUTPUT

Defines the output level for contact search information (Default 1)

BUFFER

Defines the global contact search buffer (Default 5.0)

FIELD

Defines the contact search field (Default 0.2)

SELF CONTACT

Defines whether self contact should be considered

- YES - consider self contact

- NO - no not consider self contact (Default)

 

 

Examples

 

*CONTACT SET,NAME=Contact_set1, PROPERTY=Friction1, FREQUENCY=1000, OUTPUT=2

 Fault1_hgw, Fault1_ftw, Detachment_hgw, Detachment_ftw

 

1A contact set named "Contact_set1"  is defined for the listed geometry sets "

2The default contact property assigned to the geometry sets included in the contact set is "Friction1". Note that this can be overwritten by defining specific *CONTACT SURFACE for any of the geometry sets included in the contact set with assignment of a different contact property.

3A global search will be performed every 1000 steps.

 

 

 

Click to expand/collapseCONTACT SURFACE     Contact surface data

Usage

*CONTACT SURFACE,  NAME=Geometry_set_name, PROPERTY=Property_name, SELF CONTACT=Yes_or_No, PRIORITY=Value

Description

It is used to create a ParaGeo Contact_surface data structure in order to define the contact surface interaction.  A contact surface corresponds to a single geometry set (NSET or ELSET).  These interact with other contact surfaces within the same contact set.    Defining the contact surface allows for:

1Specific contact properties to be assigned to the contact surface.

2Definition of the surfaces which can interact (establish contact) with the current surface (useful to exclude interaction with some other contact surfaces included in the same contact set).  

 

Compulsory Parameters

NAME

Assigns a geometry set (by name) so that it is treated as a contact surface.

PROPERTY

Assigns a contact property (by name) to the contact surface.

SELF CONTACT

Defines whether self contact should be considered

- YES - consider self contact

- NO - no not consider self contact (Default)

PRIORITY

Defines a priority number for the contact property assigned to the contact surface so that if two contact surfaces with different properties establish contact interaction the property assigned to the contact surface with highest priority number will be used (Default not used).

 

Following the keywords and parameters for *CONTACT SURFACE the list of contact surfaces (geometry sets) which can establish contact with the current contact surface should be provided separated by commas.

 

 

Examples

 

*CONTACT SURFACE,NAME=Fault1_hgw, PROPERTY=Contact_fault1, PRIORITY=5

 Fault1_ftw, Detachment_ftw

 

1A contact surface is defined for geometry set "Fault1_hgw"

2The contact property named "Contact_fault1" is assigned to the contact surface and is given a priority number of 5

3Fault1_hgw can establish a contact relationship with Fault1_ftw and Detachment1_ftw