<!-- source-page: 51 -->

material property is completely and uniquely defined at any values of the independent variables upon which the property depends.

As an example, consider isotropic elasticity defined as a function of three field variables (but not of temperature):

\*ELASTIC, DEPENDENCIES=3 

<table><tr><td> $E_{1}$ ,</td><td> $\nu_{1}$ ,</td><td>,</td><td>1,</td><td>1,</td><td>1</td></tr><tr><td> $E_{2}$ ,</td><td> $\nu_{2}$ ,</td><td>,</td><td>2,</td><td>1,</td><td>1</td></tr><tr><td> $E_{3}$ ,</td><td> $\nu_{3}$ ,</td><td>,</td><td>1,</td><td>2,</td><td>1</td></tr><tr><td> $E_{4}$ ,</td><td> $\nu_{4}$ ,</td><td>,</td><td>2,</td><td>2,</td><td>1</td></tr><tr><td> $E_{5}$ ,</td><td> $\nu_{5}$ ,</td><td>,</td><td>1,</td><td>3,</td><td>1</td></tr><tr><td> $E_{6}$ ,</td><td> $\nu_{6}$ ,</td><td>,</td><td>2,</td><td>3,</td><td>1</td></tr><tr><td> $E_{7}$ ,</td><td> $\nu_{7}$ ,</td><td>,</td><td>1,</td><td>1,</td><td>2</td></tr><tr><td> $E_{8}$ ,</td><td> $\nu_{8}$ ,</td><td>,</td><td>2,</td><td>1,</td><td>2</td></tr><tr><td> $E_{9}$ ,</td><td> $\nu_{9}$ ,</td><td>,</td><td>1,</td><td>2,</td><td>2</td></tr><tr><td> $E_{10}$ ,</td><td> $\nu_{10}$ ,</td><td>,</td><td>2,</td><td>2,</td><td>2</td></tr><tr><td> $E_{11}$ ,</td><td> $\nu_{11}$ ,</td><td>,</td><td>1,</td><td>3,</td><td>2</td></tr><tr><td> $E_{12}$ ,</td><td> $\nu_{12}$ ,</td><td>,</td><td>2,</td><td>3,</td><td>2</td></tr><tr><td> $E_{13}$ ,</td><td> $\nu_{13}$ ,</td><td>,</td><td>1,</td><td>1,</td><td>3</td></tr><tr><td> $E_{14}$ ,</td><td> $\nu_{14}$ ,</td><td>,</td><td>2,</td><td>1,</td><td>3</td></tr><tr><td> $E_{15}$ ,</td><td> $\nu_{15}$ ,</td><td>,</td><td>1,</td><td>2,</td><td>3</td></tr><tr><td> $E_{16}$ ,</td><td> $\nu_{16}$ ,</td><td>,</td><td>2,</td><td>2,</td><td>3</td></tr><tr><td> $E_{17}$ ,</td><td> $\nu_{17}$ ,</td><td>,</td><td>1,</td><td>3,</td><td>3</td></tr><tr><td> $E_{18}$ ,</td><td> $\nu_{18}$ ,</td><td>,</td><td>2,</td><td>3,</td><td>3</td></tr></table>

<!-- source-page: 52 -->

<!-- source-page: 53 -->

# 1.2.2 CONVENTIONS

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE

# References

• Chapter 2, “Spatial Modeling”   
• Part II, “Output”   
• “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1   
• “Boundary conditions in Abaqus/CFD,” Section 34.3.2

# Overview

The conventions that are used throughout Abaqus are defined in this section. The following topics are discussed:

• Degrees of freedom   
• Coordinate systems   
• Self-consistent units   
• Time measures   
• Local directions on surfaces in space   
• Stress and strain conventions   
• Stress and strain measures in geometrically nonlinear analysis   
• Conventions for finite rotations   
• Conventions for tabular data input

# Degrees of freedom

Except for axisymmetric elements, fluid continuum elements, and electromagnetic elements, the degrees of freedom are always referred to as follows:

1 x-displacement   
2 y-displacement   
3 z-displacement   
4 Rotation about the x-axis, in radians   
5 Rotation about the y-axis, in radians   
6 Rotation about the z-axis, in radians   
7 Warping amplitude (for open-section beam elements)

<!-- source-page: 54 -->

8 Pore pressure, hydrostatic fluid pressure, or acoustic pressure   
9 Electric potential   
10 Connector material flow (units of length)   
11 Temperature (or normalized concentration in mass diffusion analysis)   
12 Second temperature (for shells or beams)   
13 Third temperature (for shells or beams)   
14 Etc.

Here the $x \cdot , y \cdot ,$ and z-directions coincide with the global X-, Y-, and Z-directions, respectively; however, if a local transformation is defined at a node (see “Transformed coordinate systems,” Section 2.1.5), they coincide with the local directions defined by the transformation.

A maximum of 20 temperature values (degrees of freedom 11 through 30) can be defined for shell or beam elements in Abaqus/Standard.

# Axisymmetric elements

The displacement and rotation degrees of freedom in axisymmetric elements are referred to as follows:

1 r-displacement   
2 z-displacement   
5 Rotation about the z-axis (for axisymmetric elements with twist), in radians   
6 Rotation in the r–z plane (for axisymmetric shells), in radians

Here the r- and z-directions coincide with the global X- and Y-directions, respectively; however, if a local transformation is defined at a node (see “Transformed coordinate systems,” Section 2.1.5), they coincide with the local directions defined by the transformation.

# Fluid continuum elements

Fluid continuum elements in Abaqus/CFD are used to define the element shape and to discretize the continuum. Degrees of freedom in a fluid flow analysis are not determined by the element type but by the analysis procedure and options specified (e.g., turbulence models and auxiliary transport equations).

# Electromagnetic elements

Electromagnetic elements in Abaqus/Standard are used to define the element shape and to discretize the continuum. The eddy current and magnetostatic analyses formulations use magnetic vector potential as a degree of freedom (see “Boundary conditions” in “Eddy current analysis,” Section 6.7.5, and “Boundary conditions” in “Magnetostatic analysis,” Section 6.7.6).

<!-- source-page: 55 -->

# Activation of degrees of freedom

Abaqus/Standard and Abaqus/Explicit activate only those degrees of freedom needed at a node. Thus, some of the degrees of freedom listed above may not be used at all nodes in a model, because each element type uses only those degrees of freedom that are relevant. For example, two-dimensional solid (continuum) stress/displacement elements use only degrees of freedom 1 and 2. The degrees of freedom actually used at any node are the envelope of those needed in each element that shares the node.

In Abaqus/CFD the active degrees of freedom in a fluid flow analysis are determined by the analysis procedure and the options specified. For example, using the energy equation in conjunction with the incompressible flow procedure activates the velocity, pressure, and temperature degrees of freedom. For more information, see “Active degrees of freedom” in “Boundary conditions in Abaqus/CFD,” Section 34.3.2.

# Internal variables in Abaqus/Standard

In addition to the degrees of freedom listed above, Abaqus/Standard uses internal variables (such as Lagrange multipliers to impose constraints) for some elements. Normally you need not be concerned with these variables, but they may appear in error and warning messages and are checked for satisfaction of nonlinear constraints during iteration. Internal variables are always associated with internal nodes, which have negative numbers to distinguish them from user-defined nodes.

# Coordinate systems

The basic coordinate system in Abaqus is a right-handed, rectangular Cartesian system. You can choose other systems locally for input (see “Node definition,” Section 2.1.1), for output of nodal variables (displacements, velocities, etc.) and point load or boundary condition specification (see “Transformed coordinate systems,” Section 2.1.5), and for material or kinematic joint specification (see “Orientations,” Section 2.2.5). All coordinate systems must be right-handed.

# Units

Abaqus has no units built into it except for rotation and angle measures. Therefore, the units chosen must be self-consistent, which means that derived units of the chosen system can be expressed in terms of the fundamental units without conversion factors.

# Rotation and angle measures

In Abaqus rotational degrees of freedom are expressed in radians, and all other angle measures are expressed in degrees (for example, phase angles).

# International System of units (SI)

The International System of units (SI) is an example of a self-consistent set of units. The fundamental units in the SI system are length in meters (m), mass in kilograms (kg), time in seconds (s), temperature in degrees kelvin (K), and electric current in amperes (A). The units of secondary or derived quantities

<!-- source-page: 56 -->

are based on these fundamental units. An example of a derived unit is the unit of force. A unit of force in the SI system is called a newton (N):

$$
1 \mathrm{newton} = 1 \mathrm{kg} \mathrm{m} / \mathrm{s} ^ {2}.
$$

Similarly, a unit of electrical charge in the SI system is called a coulomb (C):

$$
1 \text {   coulomb   } = 1 \text {   A   s.   }
$$

Another example is the unit of energy, called a joule (J):

$$
1 \text {   joule   } = 1 \text {   N   m   } = 1 \text {   A   volt   s   } = 1 \text {   kg   m } ^ {2} / \text { s } ^ {2}.
$$

The unit of electrical potential in the SI system is the volt, which is chosen such that

$$
1 \text {   joule   } = 1 \text {   volt   } C = 1 \text {   volt   A   s.   }
$$

Sometimes the standard units are not convenient to work with. For example, Young’s modulus is frequently specified in terms of megapascals (MPa) (or, equivalently, N/mm2 ), where 1 pascal = 1 N/m2 . In this case the fundamental units could be tonnes (1 tonne = 1000 kilograms), millimeters, and seconds.

# American or English units

American or English units can cause confusion since the naming conventions are not as clear as in the SI system. For example, 1 pound force (lbf) will give 1 pound mass (lbm) an acceleration of g ft/sec2 , where g is the value of acceleration due to gravity. If pounds force, feet (ft), and seconds are taken as fundamental units, the derived unit of mass is lbf sec2 /ft. Since density is commonly given in handbooks as lbm/in3 , it must be converted to lbf sec2 /ft4 by

$$
1 \mathrm{lbm} / \mathrm{in} ^ {3} = \frac {1 2 ^ {3}}{g} \mathrm{lbf} \sec^ {2} / \mathrm{ft} ^ {4}.
$$

Frequently it is not made clear in handbooks whether lb stands for lbm or lbf. You need to check that the values used make up a consistent set of units.

Two other units that cause difficulty are the slug, defined as the mass that will be accelerated at 1 ft/sec2 by 1 lbf, and the poundal, defined as the force required to accelerate 1 lbm at 1 ft/sec2 . Useful conversions are

$$
1 \mathrm{slug} = g \mathrm{lbm}
$$

and

$$
1 \mathrm{lbf} = g \text {   poundals },
$$

where g is the magnitude of the acceleration due to gravity in ft/sec2 .

<!-- source-page: 57 -->

# Symbols used in Abaqus for units

Units are indicated for the value to be given on load and flux types as follows:

<table><tr><td>Dimension</td><td>Indicator</td><td>Example (S.I. units)</td></tr><tr><td>length</td><td>L</td><td>meter</td></tr><tr><td>mass</td><td>M</td><td>kilogram</td></tr><tr><td>time</td><td>T</td><td>second</td></tr><tr><td>temperature</td><td>θ</td><td>degree Celsius</td></tr><tr><td>electric current</td><td>A</td><td>ampere</td></tr><tr><td>force</td><td>F</td><td>newton</td></tr><tr><td>energy</td><td>J</td><td>joule</td></tr><tr><td>electric charge</td><td>C</td><td>coulomb</td></tr><tr><td>electric potential</td><td>φ</td><td>volt</td></tr><tr><td>mass concentration</td><td>P</td><td>Parts per million</td></tr></table>

# Time

Abaqus has two measures of time—step time and total time. Except for certain linear perturbation procedures, step time is measured from the beginning of each step. Total time starts at zero and is the total accumulated time over all general analysis steps (including restart steps; see “Restarting an analysis,” Section 9.1.1). Total time does not accumulate during linear perturbation steps.

# Local tangent directions on surfaces in space

Local tangent directions are needed on surfaces in space; for example, to provide a convention for describing components of slip on an element-based contact surface or components of stress and strain in a shell. The convention used in Abaqus for such directions is as follows.

The default local 1-direction is the projection of the global x-axis onto the surface. If the global x-axis is within $0 . 1 ^ { \circ }$ of being normal to the surface, the local 1-direction is the projection of the global z-axis onto the surface. The local 2-direction is then at right angles to the local 1-direction, so that the local 1-direction, local 2-direction, and the positive normal to the surface form a right-handed set (see Figure 1.2.2–1). The positive normal direction is defined in an element by the right-hand rotation rule going around the nodes of the element. The local surface directions can be redefined; see “Orientations,” Section 2.2.5.

The local 1- and 2-directions become local 2- and 3-directions, respectively, when considering gasket elements or the local systems associated with integrated output sections (“Integrated output section definition,” Section 2.5.1) or user-defined sections (“Section output from Abaqus/Standard” in “Output to the data and results files,” Section 4.1.2).

<!-- source-page: 58 -->

![](images/page-058_fa5326aa168468ebf769522dcd1b67d4740925e8dd561605d4e44e83cb2eb9a9.jpg)

<details>
<summary>text_image</summary>

surface normal
projection of x-axis onto surface
surface normal
z
y
x
1
2
3
4
1
2
3
4
</details>

Figure 1.2.2–1 Default local surface directions.

For “line”-type surfaces defined on beam, pipe, or truss elements in space, the default local 1-direction and 2-direction are tangential and transverse to the elements. In this case the local surface directions can also be redefined as described in “Orientations,” Section 2.2.5.

# Rotation of the local directions

For geometrically linear analysis, stress and strain components are given by default in the material directions in the reference (initial) configuration.

For geometrically nonlinear analysis, small-strain shell elements in Abaqus/Standard (S4R5, S8R, S8R5, S8RT, S9R5, STRI3, and STRI65) use a total Lagrangian strain, and the stress and strain components are given relative to material directions in the reference configuration. Gasket elements are small-strain small-displacement elements, and the components are output by default in the behavior directions in the reference configuration.

For finite-membrane-strain elements (all membrane elements, S3/S3R, S4, S4R, SAX, and SAXA elements) and for small-strain shell elements in Abaqus/Explicit, the material directions rotate with the average rigid body motion of the surface to form the material directions in the current configuration. Stress and strain components in these elements are given relative to these material directions in the current configuration.

For a more thorough discussion of the definition of the rotated coordinate directions in membrane elements; S3/S3R, S4, and S4R elements; S3RS, S4RS, and S4RSW elements; and SAXA elements, see:

<!-- source-page: 59 -->

• “Membrane elements,” Section 3.4.1 of the Abaqus Theory Guide,   
• “Finite-strain shell element formulation,” Section 3.6.5 of the Abaqus Theory Guide,   
• “Small-strain shell elements in Abaqus/Explicit,” Section 3.6.6 of the Abaqus Theory Guide, and   
• “Axisymmetric shell element allowing asymmetric loading,” Section 3.6.7 of the Abaqus Theory Guide.

You can determine whether the local system associated with a user-defined section is fixed or rotates with the average rigid body motion; see “Section output from Abaqus/Standard” in “Output to the data and results files,” Section 4.1.2, for details.

You can determine whether the local system associated with an integrated output section is fixed, translates with average rigid body motion, or translates and rotates with the average rigid body motion; see “Integrated output section definition,” Section 2.5.1, for details.

See “Contact formulations in Abaqus/Standard,” Section 38.1.1, for information on how the local tangent directions evolve during an Abaqus/Standard contact analysis.

# Convention used for stress and strain components

When defining material properties, the convention used for stress and strain components in Abaqus is that they are ordered:

<table><tr><td> $\sigma_{11}$ </td><td>Direct stress in the 1-direction</td></tr><tr><td> $\sigma_{22}$ </td><td>Direct stress in the 2-direction</td></tr><tr><td> $\sigma_{33}$ </td><td>Direct stress in the 3-direction</td></tr><tr><td> $\tau_{12}$ </td><td>Shear stress in the 1–2 plane</td></tr><tr><td> $\tau_{13}$ </td><td>Shear stress in the 1–3 plane</td></tr><tr><td> $\tau_{23}$ </td><td>Shear stress in the 2–3 plane</td></tr></table>

For example, a fully anisotropic, linear elasticity matrix is

$$
\left( \begin{array}{c} \sigma_ {1 1} \\ \sigma_ {2 2} \\ \sigma_ {3 3} \\ \tau_ {1 2} \\ \tau_ {1 3} \\ \tau_ {2 3} \end{array} \right) = \left[ \begin{array}{c c c c c c} D _ {1 1 1 1} & D _ {1 1 2 2} & D _ {1 1 3 3} & D _ {1 1 1 2} & D _ {1 1 1 3} & D _ {1 1 2 3} \\ & D _ {2 2 2 2} & D _ {2 2 3 3} & D _ {2 2 1 2} & D _ {2 2 1 3} & D _ {2 2 2 3} \\ & & D _ {3 3 3 3} & D _ {3 3 1 2} & D _ {3 3 1 3} & D _ {3 3 2 3} \\ & \text {symm.} & & D _ {1 2 1 2} & D _ {1 2 1 3} & D _ {1 2 2 3} \\ & & & & D _ {1 3 1 3} & D _ {1 3 2 3} \\ & & & & & D _ {2 3 2 3} \end{array} \right] \left( \begin{array}{c} \varepsilon_ {1 1} \\ \varepsilon_ {2 2} \\ \varepsilon_ {3 3} \\ \gamma_ {1 2} \\ \gamma_ {1 3} \\ \gamma_ {2 3} \end{array} \right).
$$

The 1-, 2-, and 3-directions depend on the element type chosen. For solid elements the defaults for these directions are the global spatial directions. For shell and membrane elements the defaults for the 1- and 2-directions are local directions in the surface of the shell or membrane, as defined in Part VI, “Elements.” In both cases the 1-, 2-, and 3-directions can be changed as described in “Orientations,” Section 2.2.5.

<!-- source-page: 60 -->

For geometrically nonlinear analysis with solid elements, the default (global) directions do not rotate with the material. However, user-defined orientations do rotate with the material.

Abaqus/Explicit stores the stress and strain components internally in a different order: , , , , , . For geometrically nonlinear analysis, the internally stored components rotate with the material, regardless of whether or not a user-defined orientation is used. This distinction is important when a user subroutine (such as VUMAT) is used.

# Nonisotropic material behavior

When nonisotropic material behavior is defined in continuum elements, a user-defined orientation is necessary for the anisotropic behavior to be associated with material directions. See “State storage,” Section 1.5.4 of the Abaqus Theory Guide, for a description of how material directions rotate.

# Zero-valued stress components

Stress components that are always zero are omitted from storage. For example, in plane stress Abaqus stores only the two direct components and one shear component of stress and strain in the plane where the stress values are nonzero.

# Shear strains

Abaqus always reports shear strain as engineering shear strain, :

$$
\gamma_ {i j} = \varepsilon_ {i j} + \varepsilon_ {j i}.
$$

# Stress and strain measures

The stress measure used in Abaqus is Cauchy or “true” stress, which corresponds to the force per current area. See “Stress measures,” Section 1.5.2 of the Abaqus Theory Guide, and “Stress rates,” Section 1.5.3 of the Abaqus Theory Guide, for more details on stress measures.

For geometrically nonlinear analysis, a large number of different strain measures exist. Unlike “true” stress, there is no clearly preferred “true” strain. For the same physical deformation different strain measures will report different values in large-strain analysis. The optimal choice of strain measure depends on analysis type, material behavior, and (to some degree) personal preference. See “Strain measures,” Section 1.4.2 of the Abaqus Theory Guide, for more details on strain measures.

By default, the strain output in Abaqus/Standard is the “integrated” total strain (output variable E). For large-strain shells, membranes, and solid elements in Abaqus/Standard two other measures of total strain can be requested: logarithmic strain (output variable LE) and nominal strain (output variable NE).

Logarithmic strain (output variable LE) is the default strain output in Abaqus/Explicit; nominal strain (output variable NE) can be requested as well. The “integrated” total strain is not available in Abaqus/Explicit.
