Integrated Output

The integrated variables that can be written to the output database in Abaqus/Explicit are defined in Integrated Variables. The integrated variables that can be written to the output database in Abaqus/Standard are defined in Section Variables.

INTEGRATED OUTPUT
list of output variables

Step module: history output request editor: Select from list below 

You can specify the surface directly for an integrated output request. Alternatively, you can associate an integrated output section that identifies the surface (see Integrated Output Section Definition) with the integrated output request.

Integrated output can be requested for a surface that includes facets, edges, or ends of various types of deformable elements. The surface can include facets of three-dimensional solid elements and continuum shell elements; edges of two-dimensional solid elements, membrane elements, conventional shell, and surface elements; and ends of beam elements, pipe elements, and truss elements.

SURFACE, NAME=surface_name, TYPE=ELEMENT
INTEGRATED OUTPUT, SURFACE=surface_name

Specifying the Surface through an Integrated Output Section Definition

If you associate an integrated output section definition with an integrated output request, the integrated output variables can be obtained in a local coordinate system that can translate and rotate with the deformation (see Figure 1). In addition, the total moment transmitted across the surface, SOM, can be computed about a moving location.

Figure 1. User-defined local coordinate system.

Input File Usage

Use both of the following options:

INTEGRATED OUTPUT SECTION, NAME=section_name, SURFACE=surface_name
INTEGRATED OUTPUT, SECTION=section_name

Abaqus/CAE Usage

Step module:

OutputIntegrated Output SectionsCreate: Name:section_name:
select regions for the surface

History output request editor: Domain: Integrated output section: 
section_name

To study the “force-flow” through various paths in a model, you must create interior surfaces that cut through one or more regions (similar to a cross-section) so that you can request integrated output of the total force transmitted across these surfaces. You can create such interior surfaces over the element facets, edges, or ends by cutting through one or more regions of the model with a plane; see Creating Interior Cross-Section Surfaces for more information.

SURFACE, NAME=surface_name, TYPE=CUTTING SURFACE
INTEGRATED OUTPUT, SURFACE=surface_name

You can request integrated output over an element set to output its total mass, the percentage change of its total mass, its average rigid body motion, or any combination of these variables. The element set must have been defined previously, and it can include any type of elements. Only dedicated integrated output quantities are supported for Eulerian or discrete particle element sets. These output quantities are defined in Integrated Variables.

INTEGRATED OUTPUT, ELSET=element set name

The frequency of integrated output is controlled as described in Controlling the Frequency of Output to the Output Database.

Preselected output variables are available only when the integrated output is requested over a surface. If integrated output is requested over an element set, you must specify the variables on the data line.

If the integrated output is requested over a surface, you can request the preselected integrated output variables SOF and SOM. In this case you can also specify additional variables as part of the output request. Alternatively, you can request all integrated variables applicable to the current procedure type. In this case any additional variables that you specify are ignored. If you do not request the preselected variables or all variables, you must specify the variables individually.

INTEGRATED OUTPUT, VARIABLE=PRESELECT 
optional additional variables

INTEGRATED OUTPUT, VARIABLE=ALL

INTEGRATED OUTPUT
individual variables

Step module: history output request editor: Preselected defaults or All

Integrated output requests over a surface are subject to the following limitations:

• Integrated output can be requested over a surface that includes facets, edges, or ends of various types of deformable elements. The surface can include facets of three-dimensional solid elements and continuum shell elements; edges of two-dimensional solid elements, membrane elements, conventional shell, and surface elements; and ends of beam elements, pipe elements, and truss elements. The surface should not contain facets of axisymmetric elements or facets of rigid elements.

• When defining the surface, elements on only one side of the surface must be used. Abaqus/Explicit computes the integrated output variables using the stresses and hourglass-mode forces in elements underlying the surface as in a free-body diagram.

• The defined surface must cut completely through the mesh, form a closed surface, or be on the exterior of the body. Figure 2 presents some typical cases of valid surfaces. If the surface cuts only partially through the mesh, a valid free-body diagram cannot be isolated (see Figure 3) and incorrect answers may be computed.

  Figure 2. Valid section definitions.
  
  

  Figure 3. Invalid section definitions.
  
  

• Elements attached to the surface can be on either side of the surface but must not cross the defined surface. Figure 3 presents a few invalid cases.

• The total force and the total moment in the section are computed based only on the stresses (internal forces) in the identified elements. Thus, inaccurate results may be obtained if distributed body loads are present in these elements since their effect on the total force in the section is not included. Common examples are the inertial loading in dynamic analyses, gravity loads, distributed body forces, and centrifugal loads. In these cases the total force in the section may depend on the choice of elements used to define the section as illustrated in Figure 4(a).

  Figure 4. Total force in the section.
  
  

  Assuming that gravity loading is the only active load, the element stresses will be different in the two elements. Hence, if the same surface is defined first using element 1 and then using element 2, different answers for the total force will be obtained. In a similar way the effects of any distributed body fluxes (heat, electrical, etc.) prescribed in the identified elements are not included.

• Depending on which side of the surface is used to define the section, different answers will be obtained in analyses similar to the case illustrated in Figure 4(b). Assuming a quasi-static analysis with the concentrated loads shown in the figure being the only active loads, a zero total force is reported if the surface is defined using element 1 and a nonzero force equal to the sum of the concentrated loads is obtained if the surface is defined using element 2.

• If the nodes that are part of the integrated output surface also participate in constraints (such as a tie constraint), the constraint force or flux is not included in the integrated output.