<!-- source-page: 251 -->

# Defining analytical rigid surfaces when drag chain or rigid surface elements are used

An alternative method of defining analytical rigid surfaces must be used to define the surface of the seabed when three-dimensional drag chain elements (available only in Abaqus/Standard) are used. This alternative method must also be used when rigid surface elements are used; these elements are required only when CAXA or SAXA elements contact a rigid surface. For this method the rigid surface must be flat and parallel to the x–y plane.

In a model defined in terms of an assembly of part instances, the rigid surface definition must appear inside the same part definition as the drag chain or rigid surface elements.

You must indicate which type of analytical surface (planar, cylindrical, or user-defined) is being created. Cylindrical rigid surfaces are not valid for use with CAXA or SAXA elements. In addition, you must assign a name to the surface and identify the rigid body reference node that will control the motion of the surface.

Input File Usage: \*RIGID SURFACE, TYPE=surface\_type, NAME=name, REF NODE=n

Abaqus/CAE Usage: Drag chain and rigid surface elements are not supported in Abaqus/CAE.

# Two-dimensional rigid surfaces

To define a planar rigid surface, define the line segments forming the rigid surface’s cross-section in the global coordinate system. You must provide the endpoint of each line segment; the starting point is always the endpoint of the previous segment, or, in the case of the first segment, the point specified as the starting point. The centers of the circular arcs, points c and f in Figure 2.3.4–2, must be given. Abaqus can define only arcs that are less than, but not equal to, 179.74°; thus, it will use the shorter arc defined by the data provided (use two adjacent arcs to define a longer arc). For parabolic arcs you must give a third point that lies on the parabola and within the arc.

Input File Usage: \*RIGID SURFACE, TYPE=SEGMENTS, NAME=name, REF NODE=n START, starting point X- or r-coordinate, starting point Y- or z-coordinate data lines to define the endpoints of the line segments forming the surface, beginning with the word LINE (for straight line segments), CIRCL (for circular arc segments), or PARAB (for parabolic arc segments)

Abaqus/CAE Usage: Drag chain and rigid surface elements are not supported in Abaqus/CAE.

# Three-dimensional cylindrical rigid surfaces

To define a cylindrical rigid surface, specify the points a, b, and c shown in Figure 2.3.4–3 that define the local coordinate system. Give the coordinates of these points— $\cdot ( X _ { a } , Y _ { a } , Z _ { a } ) , ( X _ { b } , Y _ { b } , Z _ { b } )$ , and $( X _ { c } , Y _ { c } , Z _ { c } )$ —in the default global coordinate system. As shown in Figure 2.3.4–3, point a defines the origin of the local system; point b defines the local x-axis; and point c defines the generator vector, which is the negative local z-axis. The line segments forming the cross-section of the rigid surface are defined in the local x–y plane. The three-dimensional surface is formed by sweeping this cross-section along the generator vector. The resulting surface extends to infinity in both the positive and negative directions of the generator vector.

<!-- source-page: 252 -->

<table><tr><td>Input File Usage:</td><td>*RIGID SURFACE, TYPE=CYLINDER, NAME=name, REF NODE=n $X_{a}, Y_{a}, Z_{a}, X_{b}, Y_{b}, Z_{b}$  $X_{c}, Y_{c}, Z_{c}$ START, starting point x-coordinate, starting point y-coordinate data lines to define the endpoints of the line segments forming the surface, beginning with the word LINE (for straight line segments), CIRCL (for circular arc segments), or PARAB (for parabolic arc segments)</td></tr></table>

Abaqus/CAE Usage: Drag chain and rigid surface elements are not supported in Abaqus/CAE.

<!-- source-page: 253 -->

# 2.3.5 EULERIAN SURFACE DEFINITION

# Product: Abaqus/Explicit

# References

• “Surfaces: overview,” Section 2.3.1   
• “Eulerian analysis,” Section 14.1.1   
• “Contact interaction analysis: overview,” Section 36.1.1   
• \*EULERIAN SECTION   
• \*SURFACE

# Overview

An Eulerian surface:

• must be three-dimensional;   
• must be defined as model data;   
• can be used with the general contact algorithm in Abaqus/Explicit; and   
• is created by specifying the name of an Eulerian material instance.

# What are Eulerian surfaces and why use them?

An Eulerian surface represents the exterior surface of a particular Eulerian material instance in an Abaqus/Explicit analysis. Since Eulerian materials flow through the Eulerian mesh, their surfaces cannot be defined by a simple list of element faces. Instead, these surfaces often lie within Eulerian elements and must be computed in each time increment using element volume fraction data.

You can use Eulerian surfaces to define specific interactions with Lagrangian surfaces in Abaqus/Explicit’s general contact algorithm. Once defined, you can reference Eulerian surfaces in inclusions, exclusions, and interaction definitions. You cannot combine or crop Eulerian surfaces.

Eulerian surface definitions are not required for the use of Eulerian-Lagrangian contact. If you specify “automatic” contact for the entire model, the exterior surface of all Eulerian materials will automatically be considered for contact.

# Advantages of creating Eulerian surfaces

You can use Eulerian surfaces to:

• Assign contact properties for contact interactions involving a particular Eulerian material instance.   
• Exclude interactions between Eulerian materials and Lagrangian bodies that are unlikely to make contact, simplifying the contact problem and reducing computational cost.

<!-- source-page: 254 -->

# Creating an Eulerian surface

To create an Eulerian surface, you must specify the name of a material instance that is present in the model. The material instance names are defined as part of the Eulerian section (see “Eulerian elements,” Section 32.14.1). Abaqus/Explicit calculates the exterior boundary of the specified material instance and defines a surface corresponding to that boundary. The surface is recalculated in each time increment as the material deforms.

Input File Usage: \*SURFACE, TYPE=EULERIAN MATERIAL, NAME=name material instance name,

<!-- source-page: 255 -->

# 2.3.6 OPERATING ON SURFACES

Products: Abaqus/Standard Abaqus/Explicit

# References

• “Surfaces: overview,” Section 2.3.1   
• “Coupling constraints,” Section 35.3.2   
• “Mesh-independent fasteners,” Section 35.3.4   
• “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1   
• \*SURFACE

# Overview

# Combined surfaces:

• are created by performing a Boolean operation (union, intersection, or difference) on existing surfaces;   
• can be formed from element-based or node-based surfaces;   
• cannot be formed from Eulerian surfaces;   
• can be used in the same way as other element-based or mode-based surfaces in Abaqus/Standard; and   
• cannot be used with contact pairs in Abaqus/Explicit (but can be used with general contact in Abaqus/Explicit).

# Cropped surfaces:

• are created by cropping an existing surface and keeping only that part of the surface that is enclosed in a specified rectangular box;   
• can be formed from element-based or node-based surfaces;   
• cannot be formed from Eulerian surfaces;   
• can be used in the same way as other element-based or mode-based surfaces in Abaqus/Standard; and   
• cannot be used with contact pairs in Abaqus/Explicit (but can be used with general contact in Abaqus/Explicit).

# Creating a combined surface

You must assign a name to the combined surface; this name can be used with other features that refer to surfaces.

<!-- source-page: 256 -->

In models that are defined in terms of an assembly of part instances, all surfaces must belong to a part, part instance, or the assembly. Surfaces can be created at the part level and combined at the assembly level. Additional rules are given in “Defining an assembly,” Section 2.10.1.

The surfaces being combined must be the same type; i.e., an element-based surface can be combined with another element-based surface but not with a node-based surface. Combined surfaces can be used to create another combined surface.

# Union of existing surfaces

Any number of existing surfaces can be combined to create a new surface. If the surfaces being combined are element-based surfaces, the new surface will also be an element-based surface and any overlap among the surfaces will be merged. Similarly, if the surfaces being combined are node-based surfaces, the new surface will be a node-based surface and any overlap among the surfaces will be merged.

Input File Usage:

\*SURFACE, NAME=name, COMBINE=UNION

list of surface names

# Intersection or difference of existing surfaces

The intersection or difference of two existing surfaces can be used to create a new surface. The difference operation subtracts the second surface from the first surface. When the intersection or difference operations are performed on element-based surfaces, they act only on the facets. A warning message is issued if the intersection operation results in an empty surface.

Input File Usage:

Use the following option to create a new surface based on the intersection of two existing surfaces:

\*SURFACE, NAME=name, COMBINE=INTERSECTION

first surface name, second surface name

Use the following option to create a new surface based on the difference of two existing surfaces:

\*SURFACE, NAME=name, COMBINE=DIFFERENCE

first surface name, second surface name

# Creating a cropped surface

You can create a new surface that will contain only those faces of an existing surface that have nodes inside a specified cropping box. For a node-based surface the new surface will contain only those nodes that are enclosed inside the cropping box. If the face has at least one node inside the box, the entire face is accepted as valid. You must assign a name to the new surface and specify the name of the existing surface from which the new surface is to be generated. Only one surface can be specified.

To define the location of the box, specify the coordinates of the lower corner of the box $( X _ { m i n }$ , $Y _ { m i n } , Z _ { m i n } )$ and the coordinates of the opposite (upper) corner of the box $( X _ { m a x } , Y _ { m a x } , Z _ { m a x } )$ . The cutting box can be rotated about the lower corner $( X _ { m i n } , Y _ { m i n } , Z _ { m i n } )$ if an optional rotation is defined. The coordinates of the two points, a and $b ,$ that define the rotation are given in the unrotated system.

<!-- source-page: 257 -->

These points should be defined such that point a lies on the rotated X-axis and point b lies on the X–Y plane and close to the Y-axis.

# Input File Usage:

*SURFACE, NAME=name, CROP
old_surface_name $X_{min}, Y_{min}, Z_{min}, X_{max}, Y_{max}, Z_{max}$ $X_{a}, Y_{a}, Z_{a}, X_{b}, Y_{b}, Z_{b}$

For example, to crop the surface that contains all exposed faces in the model, use the following input:

* SURFACE, TYPE=ELEMENT, NAME=entire_surface
,
* SURFACE, NAME=name, CROP
entire_surface $X_{min}, Y_{min}, Z_{min}, X_{max}, Y_{max}, Z_{max}$ $X_{a}, Y_{a}, Z_{a}, X_{b}, Y_{b}, Z_{b}$

<!-- source-page: 258 -->

<!-- source-page: 259 -->

# 2.4 Rigid body definition

• “Rigid body definition,” Section 2.4.1

<!-- source-page: 260 -->
