<!-- source-page: 281 -->

# 2.5.1 INTEGRATED OUTPUT SECTION DEFINITION

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Output to the output database,” Section 4.1.3   
• \*INTEGRATED OUTPUT SECTION   
• \*INTEGRATED OUTPUT   
• \*SURFACE   
• “Defining integrated output sections,” Section 14.13.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

An integrated output section:

• can be two-dimensional or three-dimensional;   
• can be used to track the average motion of a surface;   
• can be used in association with integrated output requests to study the “force-flow” in the model; and   
• does not impose any constraint on the motion of the surface.

# Introduction

An integrated output section is a way to associate a surface with a coordinate system and/or a reference node for one or both of the following purposes:

• tracking the average motion of the surface; and/or   
• expressing the force and the moment transmitted through the surface in a local coordinate system, with the moment taken about a point that moves with the surface.

The average motion of a surface can be obtained as the displacement and/or rotation history at the reference node on an integrated output section definition. You must define a reference node that is not connected to any other part of the finite element model and select whether the reference node follows only the average translation of the surface or both the translation and the rotation. Since the reference node is not connected to the rest of the model, an integrated output section definition used to track the average surface motion does not form a constraint on the motion of any nodes in the model.

The “force-flow” in a complicated model can be studied using integrated output sections defined over a number of interior cross-section-like surfaces cutting through various parts of the model. It can be equally useful to sum forces over an exterior surface in contact or to sum forces transmitted through a tie constraint between surfaces, which is done by associating an integrated output section definition with an integrated output request. The vector output quantities can be expressed in a coordinate system

<!-- source-page: 282 -->

of choice by specifying an orientation on an integrated output section definition. This coordinate system can rotate by an amount given by the rotational degrees of freedom at the reference node. In addition, the output of the integrated moment across the surface can be taken about a location that can translate by an amount given by the translational degrees of freedom at the reference node. Integrated output over a given surface can be requested with different coordinate systems and reference nodes by employing multiple integrated output section definitions over the same surface.

# Creating an integrated output section

You must assign a name to each integrated output section. This name is used to associate the section with an integrated output request. In addition, you must identify the surface over which the section is being defined (see “Element-based surface definition,” Section 2.3.2).

Input File Usage: \*INTEGRATED OUTPUT SECTION, NAME=section\_name, $\mathrm { S U R F A C E } { = } s u r f a c e \_ n a m e$

Abaqus/CAE Usage: Step module: Output→Integrated Output Sections→Create: Name: section\_name: select surface region

# Creating interior cross-section surfaces

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 and moment transmitted across these surfaces. You can create such interior surfaces over the element facets, edges, or ends by simply cutting through one or more regions of the model with a plane; see “Creating interior cross-section surfaces” in “Element-based surface definition,” Section 2.3.2, for more information.

# The integrated output section reference node

A reference node can be associated with an integrated output section for one or both of the following purposes:

• tracking the average motion of the surface; and/or   
• computing the variables from an integrated output request in a coordinate system that moves with the motion of the reference node.

If the average surface motion must be tracked, you must define a reference node that is not connected to any other part of the finite element model and select whether the reference node follows only the average translation of the surface or both the translation and the rotation. The rotational degrees of freedom will be activated in addition to the translational degrees of freedom at the reference node if it is selected to follow the average rotation of the surface. Further, the initial position of the reference node may be adjusted to lie at the center of the surface automatically.

When an integrated output section with a reference node is associated with an integrated output request, the total moment transmitted through the section is computed with respect to the current location of the reference node. If the reference node has active rotational degrees of freedom, the coordinate system used to express the integrated output variables rotates with the rotation of the reference node.

<!-- source-page: 283 -->

Positioning the reference node at the center of the surface

The reference node can be repositioned automatically at the center of the surface in the initial configuration when the reference node is not connected to the rest of the model.

The default is to leave the reference node in its specified position.

Input File Usage: Use the following option to position the reference node at the center of the surface:

\*INTEGRATED OUTPUT SECTION, REF NODE=n, POSITION=CENTER

Abaqus/CAE Usage: Step module: integrated output section editor: Anchor at reference point:

Edit: select reference point: Move point to center of surface

Setting the reference node to track the average motion of the surface

It is often meaningful to obtain integrated output over a surface using a coordinate system and a point that moves with the average surface motion. When the reference node is not connected to the rest of the model, it can be specified to translate with the average translation of the surface without any rotation or to both translate and rotate with the average motion of the surface. The average motion is based on the mass weighted motion of the individual nodes that are on the surface and are not part of any rigid body.

By default, the reference node does not track the average motion of the surface.

Input File Usage: Use the following option if the reference node must translate with the average translation of the surface:

\*INTEGRATED OUTPUT SECTION, REF NODE=n, REF NODE MOTION=AVERAGE TRANSLATION

Use the following option if the reference node must both translate and rotate with the average translation of the surface:

\*INTEGRATED OUTPUT SECTION, REF NODE=n, REF NODE MOTION=AVERAGE

Abaqus/CAE Usage: Step module: integrated output section editor: Anchor at reference point: Edit: select reference point: Point motion: Average translation and rotation or Average translation

# The integrated output section local coordinate system

You can define a local coordinate system on an integrated output section and associate the section with an integrated output request to express the integrated output variables in the local coordinate system. You can specify an orientation as the local coordinate system and, possibly, further project it onto the surface. Alternatively, you can form a local coordinate system by projecting the global coordinate system onto the surface following the Abaqus conventions (see “Conventions,” Section 1.2.2). If a local system is not defined explicitly, the local system is initialized to the global coordinate system.

The initial coordinate system, whether explicitly defined or initialized to the global coordinate system, will rotate with the deformation if a reference node is specified and that reference node has active rotational degrees of freedom. If the reference node is not connected to the rest of the model

<!-- source-page: 284 -->

and its motion is based on both the average translation and rotation of the surface, the rotational and translational degrees of freedom are activated at the reference node.

Input File Usage: Use the following option to define the initial coordinate system for the section:

\*INTEGRATED OUTPUT SECTION, ORIENTATION=orientation\_name

Abaqus/CAE Usage: Step module: integrated output section editor: CSYS: Edit: select orientation

Projecting the coordinate system onto the section surface

Either the coordinate system defined by the specified orientation or the global coordinate system can be projected onto the section surface to obtain a local coordinate system. Projection onto the surface is based on the average normal of the surface; the local 1-direction is formed perpendicular to the surface (see Figure 2.5.1–1).

Input File Usage: Use the following option to project the coordinate system onto the section surface:

\*INTEGRATED OUTPUT SECTION, PROJECT ORIENTATION=YES

Abaqus/CAE Usage: Step module: integrated output section editor: Project orientation onto surface

![](images/page-284_c02c7bc4fda8c34261d98b15b6a8c8f1f718484117a2ef51e10c61ac90e51e85.jpg)

<details>
<summary>text_image</summary>

defined section
anchor point
2
a
1
Y
X
elements used to
define the section
anchor point
1
3
b
2
a
Z
Y
X
defined section
2D and axisymmetric
3D
</details>

Figure 2.5.1–1 User-defined local coordinate system.

<!-- source-page: 285 -->

# Associating an integrated output section with an integrated output request

An integrated output request is used to obtain history output of variables such as total force transmitted across a surface (see “Integrated output” in “Output to the output database,” Section 4.1.3). Such a request may refer to an integrated output section definition to identify the surface where output is needed and to provide a local coordinate system and/or a reference node as a point about which the total moment across the surface is computed.

Input File Usage: Use both of the following options to associate an integrated output section with an integrated output request:

```txt
*INTEGRATED OUTPUT SECTION, NAME=section_name
*INTEGRATED OUTPUT, SECTION=section_name 
```

Abaqus/CAE Usage: Step module:

```txt
Output→Integrated Output Sections→Create: Name: section_name 
```

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

# Limitations

Integrated output sections are subject to the following limitations:

• The surface associated with an integrated output section cannot be an analytical rigid surface.   
• The surface associated with an integrated output section can contain facets over rigid or axisymmetric elements. However, such an integrated output section cannot be associated with an integrated output request (see “Output to the output database,” Section 4.1.3).

<!-- source-page: 286 -->

<!-- source-page: 287 -->

# 2.6 Mass adjustment

• “Adjust and/or redistribute mass of an element set,” Section 2.6.1

<!-- source-page: 288 -->

<!-- source-page: 289 -->

# 2.6.1 ADJUST AND/OR REDISTRIBUTE MASS OF AN ELEMENT SET

# Product: Abaqus/Explicit

# References

• “Density,” Section 21.2.1   
• “Point masses,” Section 30.1.1   
• “Nonstructural mass definition,” Section 2.7.1   
• “Mass scaling,” Section 11.6.1   
• \*MASS ADJUST

# Overview

# Mass adjustment:

• is useful to set the net mass of one or more components in the model to a known value;   
• is useful to scale the net mass of one or more components in the model (without the need to know the mass of the component);   
• is useful to account for any errors in mass due to modeling approximations;   
• is useful to account for mass from nonstructural features otherwise omitted from the model, such as paint;   
• can be applied over all element types that have mass;   
• adjusts the mass of the individual elements in an element set in proportion to their pre-adjusted mass including any nonstructural mass, so as to meet the specified target value for the set;   
• can be used to redistribute mass among elements in the set to raise the minimum stable time increment to a target value;   
• can be used to redistribute mass to maximize the stable time increment of the elements in the element set;   
• can be specified only once in an Abaqus/Explicit analysis during the model definition; and   
• can be applied in a hierarchical fashion to adjust the mass for individual parts first and then for an assembly of these parts.

# Defining mass adjustment

To adjust or scale the total mass of one or more components in the model, you first identify the corresponding element sets. If you specify multiple elements sets, the mass is adjusted or scaled in the order in which the element sets are specified. For element sets that share elements, you must determine the order in which to specify the element sets to obtain the desired results.

Input File Usage: \*MASS ADJUST

<!-- source-page: 290 -->

The mass of a component in a numerical model may differ from its actual value for a number of reasons including modeling approximations and omission of minor features from the model. You can specify mass adjustment in the numerical model for such components by identifying the element sets defining these components and their respective total mass values. For a given element set, the mass is adjusted at the start of the analysis such that the adjustment in each element in that set is in proportion to the preadjusted mass of that element, thus preserving the center of mass and the principal directions of the rotary inertia. The pre-adjusted mass of an element includes the mass due to any associated material density; any mass directly specified on the section definition as in the case of beam, pipe, shell, membrane, rigid, and surface elements; and any nonstructural mass applied directly to that element. “Knee bolster impact with general contact,” Section 2.1.9 of the Abaqus Example Problems Guide, is an example of setting the total mass of an element set using mass adjustment.

When mass is adjusted for an element with active rotational degrees of freedom, the rotary inertia contribution from that element is also modified proportionally to correspond with the scaling in the element mass from mass adjustment, thus preserving the principal directions of the rotary inertia. The adjusted mass value is considered when calculating the stable time increment of an element. Loads such as mass proportional damping (see “Material damping,” Section 26.1.1) and gravity take the adjusted mass into account.

Mass adjustment can be applied in a hierarchical fashion to adjust the mass for individual parts first and then for an assembly of these parts. In this scenario, the mass adjustment defined over the assembly may further modify the adjusted mass of the individual parts. You must associate all of the mass-adjusted element sets in the desired order with a single mass adjustment definition.

Abaqus/Explicit automatically calculates the mass, center of mass, and rotary inertia of each element set and prints the results to the data (.dat) file if model definition data are requested (see “Controlling the amount of analysis input file processor information written to the data file” in “Output,” Section 4.1.1). The contributions from mass adjustment are also listed in these tables. Element output variable MASSADJUST can be requested as output to the output database (.odb) file, and it will indicate how the mass of the set is adjusted or redistributed to each element included in the set (see “Abaqus/Explicit output variable identifiers,” Section 4.2.2). This output variable is available as field output (contour plots) in the first output frame of the first analysis step.

Mass adjustment contributions applied to an element set are always included when transferring model data between Abaqus/Explicit analyses (see “Transferring results from one Abaqus/Explicit analysis to another,” Section 9.2.4). There is no need to redefine these contributions in the import analysis unless different mass adjustment is required for the element set.

# Input File Usage:

Use the following option to define total mass for an element set without altering its center of mass:

\*MASS ADJUST

elem\_set\_name, elem\_set\_mass
