Writing Surface Output to the Output Database

You can write variables associated with surfaces in contact, coupled thermal-electrical-structural (Abaqus/Standard only), coupled temperature-displacement (Abaqus/Standard only), coupled thermal-electrical, and crack propagation problems to the output database. Multiple output requests can be used to customize requests among interactions, surfaces, or node sets.

This page discusses:

See Also
About Output
In Other Guides
*OUTPUT

ProductsAbaqus/StandardAbaqus/Explicit

For surface variables associated with cavity radiation, see Cavity Radiation Output in Abaqus/Standard.

Use element output requests (see Writing Element Output to the Output Database) to obtain database output for contact elements (such as gap elements; see Gap Contact Elements).

In Abaqus/Standard contact history output cannot be saved in a linear perturbation step with frequency extraction.

Displacement nodal output is generated automatically in Abaqus/Explicit when requesting surface output.

Selecting the Surface Output Variables

The surface variables that can be written to the output database are listed in Surface Variables (Abaqus/Standard) and Surface Variables (Abaqus/Explicit).

Input File Usage

CONTACT OUTPUT
list of output variables

Limiting the Extent of a Surface Output Request in Abaqus/Standard

Output requests apply to general contact and all contact pair interactions in a model by default in Abaqus/Standard. Options to limit an output request to certain interactions are discussed below.

Limiting Output to a Node Set in Abaqus/Standard

You can limit a surface output request to apply to a subset of surface nodes involved in contact pairs or general contact in Abaqus/Standard.

Input File Usage

CONTACT OUTPUT, NSET=node_set_name

Limiting Output for Contact Pairs Based on Secondary and Main Surface Names in Abaqus/Standard

You can limit output to certain contact pairs based on surface names. If you specify both the secondary and main surface names, the output request is limited to a specific contact pair. If you specify the secondary surface but not the main surface, output is written for all contact pairs that involve the specified secondary surface. If you also specify a node set, the applicability of an output request is further limited (that is, the output request will generate output only for certain nodes of a certain contact pair (or pairs). Output requests with a specific secondary and/or main surface role specified will not generate output for general contact.

Input File Usage

CONTACT OUTPUT, MAIN=main, SECONDARY=secondary, NSET=node_set_name

Limiting Output for Cracked Surfaces in Enriched Elements Based on Surface Name in Abaqus/Standard

You can limit output requests to certain cracked surfaces in enriched elements based on surface names.

Input File Usage

CONTACT OUTPUT, SURFACE=surface_name

Limiting the Extent of a Surface Field Output Request in Abaqus/Explicit

Field output requests apply to general contact and all contact pair interactions in a model by default in Abaqus/Explicit. Options to limit a surface field output request to certain interactions are discussed below.

Limiting Surface Field Output to a Contact Pair Set in Abaqus/Explicit

In Abaqus/Explicit you can select the contact pairs for which surface field output is desired. Surface output is contact pair-specific, so that contact output for a particular surface involved in a selected contact pair will include only the contributions from that contact pair if the surface is involved in multiple contact pairs. Surface output is available only for discrete (node-based or element-based) surfaces; it is not available for any analytical surfaces within a contact pair.

Input File Usage

Use the following option to request surface field output for a particular contact pair set:

CONTACT OUTPUT, CPSET=contact_pair_set_name

Limiting Surface Field Output to General Contact in Abaqus/Explicit

You can limit surface field output requests to apply only to general contact in Abaqus/Explicit, but you cannot further limit this output to a subset of the general contact domain.

Input File Usage

CONTACT OUTPUT, GENERAL CONTACT

Limiting Surface Field Output to a Single Surface in Abaqus/Explicit

You can limit surface field output requests to a single surface in the general contact domain in Abaqus/Explicit. The contact output for the specified surface will include all the contributions from other contact surfaces interacting with the surface. This type of output should not be used for surfaces involving beam, truss, or pipe elements.

Input File Usage

CONTACT OUTPUT, SURFACE=surface_name

Limiting Surface Field Output to Pairwise Surfaces in Abaqus/Explicit

You can specify a pair of surfaces in the general contact domain in Abaqus/Explicit for which the interactions on one surface due to the contact with another surface will be output. This type of output cannot be used for surfaces involving Eulerian regions and should not be used for surfaces involving beam, truss, or pipe elements.

Input File Usage

CONTACT OUTPUT, SURFACE=first_surface_name, 
SECOND SURFACE=second_surface_name

Specifying Surface History Output Regions in Abaqus/Explicit

You must specify an interaction to which a surface history output request applies with one of the methods discussed below.

Specifying Surface History Output by Contact Pair Set in Abaqus/Explicit

In Abaqus/Explicit you can select the contact pairs for which surface history output is desired. Surface output is contact pair-specific, so that contact output for a particular surface involved in a selected contact pair will include only the contributions from that contact pair if the surface is involved in multiple contact pairs. Surface output is available only for discrete (node-based or element-based) surfaces; it is not available for any analytical surfaces within a contact pair.

Input File Usage

Use the following option to request surface history output for a particular contact pair:

CONTACT OUTPUT, CPSET=contact_pair_set_name

Specifying Whole Surface History Output in Abaqus/Explicit

You can specify a surface in the general contact domain for which whole surface contact force resultants will be output. Whole surface contact force resultants for a surface in the general contact domain are available only as history output.

Input File Usage

CONTACT OUTPUT, SURFACE=surface_name

Specifying Pairwise Surface History Output in Abaqus/Explicit

You can specify a pair of surfaces in the general contact domain for which the resultant contact forces on one surface due to the contact with another surface will be output. The contact force resultants in this case consider only the contact interactions between the two specified surfaces. This type of output cannot be requested for surfaces involving Eulerian regions.

Input File Usage

CONTACT OUTPUT, SURFACE=first_surface_name, 
SECOND SURFACE=second_surface_name

Specifying Surface History Output by Fastened Node Set in Abaqus/Explicit

You can select a fastened node set for which bond history output is desired:

Input File Usage

Use the following option to request surface history output for a particular fastened node set:

CONTACT OUTPUT, NSET=node_set_name

Requesting Preselected Output

You can request the preselected, procedure-specific surface output variables described in Preselected Output Requests. In this case you can specify additional variables as part of the output request.

Alternatively, you can request all surface variables applicable to the current procedure. In this case any additional variables you specify are ignored.

Input File Usage

Use the following option to request the preselected surface output variables:

CONTACT OUTPUT, VARIABLE=PRESELECT

Use the following option to request all applicable surface output variables:

CONTACT OUTPUT, VARIABLE=ALL