# Specifying pressure loads Distributed pressure loads can be specified on any two-dimensional, three-dimensional, or axisymmetric elements. Hydrostatic pressure loads can be specified in Abaqus/Standard on two-dimensional, threedimensional, and axisymmetric elements. Viscous and stagnation pressure loads can be specified in Abaqus/Explicit on any elements. # Distributed pressure loads Distributed pressure loads can be specified on any elements. For beam elements, a positive applied pressure results in a force vector acting along the particular local direction of the section or a global direction, whichever is specified. For conventional shell elements, the force vector points along the element SPOS normal. For continuum solid or a continuum shell elements with the distributed load on an explicitly identified facet, the force vector acts against the outward normal of that facet. Distributed pressure loads are not supported for pipe and elbow elements. Distributed pressure loads can be specified on a surface formed over elements; a positive applied pressure results in a force vector acting against the local surface normal. Input File Usage: Use one of the following options to define a pressure load: \*DLOAD element number or element set, load type label, magnitude where load type label is Pn, P, PnNU, or PNU. \*DSLOAD surface name, P or PNU, magnitude Abaqus/CAE Usage: Use the following input to define an element-based pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: select an analytical field or a discrete field Use the following input to define a surface-based pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Uniform or User-defined Nonuniform element-based pressure loads are not supported in Abaqus/CAE. Hydrostatic pressure loads on two-dimensional, three-dimensional, and axisymmetric elements in Abaqus/Standard To define hydrostatic pressure in Abaqus/Standard, give the Z-coordinates of the zero pressure level (point a in Figure 34.4.3–5) and the level at which the hydrostatic pressure is defined (point b in Figure 34.4.3–5) in an element-based or surface-based distributed load definition. For levels above the zero pressure level, the hydrostatic pressure is zero. 

text_image

z a b

Figure 34.4.3–5 Hydrostatic pressure distribution. In planar elements the hydrostatic head is in the Y-direction; for axisymmetric elements the Z-direction is the second coordinate. Input File Usage: Use one of the following options to define a hydrostatic pressure load: \*DLOAD element number or element set, HPn or HP, magnitude, Z-coordinate of point a, Z-coordinate of point b \*DSLOAD surface name, HP, magnitude, Z-coordinate of point a, Z-coordinate of point b Abaqus/CAE Usage: Use the following input to define a surface-based hydrostatic pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Hydrostatic Element-based hydrostatic pressure loads are not supported in Abaqus/CAE. Mechanical pore pressure loads on two-dimensional, three-dimensional, and axisymmetric coupled pore pressure elements in Abaqus/Standard In a coupled pore fluid diffusion and stress analysis (see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1) the pore pressure degrees of freedom, $P _ { p o r e } ,$ can be applied automatically as mechanical surface pressures for two-dimensional, three-dimensional, and axisymmetric coupled pore pressure elements. Abaqus/Standard applies a mechanical pressure, $P _ { m e c h } = P _ { p o r e }$ , onto the surfaces you prescribe. Since the mechanical pressure loads are determined by the solution pore pressures, Abaqus/Standard ignores any amplitude definition on the distributed load definition. You can include a nonzero scaling factor, , which will be applied to the pore pressures to give $P _ { m e c h } = \alpha P _ { p o r e }$ . By default, the scaling factor is set to unity. This loading is supported only for continuum elements that have pore pressure degrees of freedom during a geostatic (“Geostatic stress state,” Section 6.8.2) or coupled pore fluid diffusion and stress analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). Input File Usage: Use one of the following options to define a mechanical pore pressure load: \*DLOAD element number or element set, PORMECHn, scaling factor \*DSLOAD surface name, PORMECH, scaling factor Abaqus/CAE Usage: Mechanical pore pressure loads are not supported in Abaqus/CAE. Viscous pressure loads in Abaqus/Explicit Viscous pressure loads are defined by $$ p = - c _ {v} \left(\mathbf {v} - \mathbf {v} _ {r e f}\right) \cdot \mathbf {n}, $$ where p is the pressure applied to the body; $c _ { v }$ is the viscosity, given as the magnitude of the load; is the velocity of the point on the surface where the pressure is being applied; $\mathbf { v } _ { r e f }$ is the velocity of the reference node; and is the unit outward normal to the element at the same point. Viscous pressure loading is most commonly applied in structural problems when you want to damp out dynamic effects and, thus, reach static equilibrium in a minimal number of increments. A common example is the determination of springback in a sheet metal product after forming, in which case a viscous pressure would be applied to the faces of shell elements defining the sheet metal. An appropriate choice for the value of $c _ { v }$ is important for using this technique effectively. To compute $c _ { v } ,$ , consider the infinite continuum elements described in “Infinite elements,” Section 28.3.1. In explicit dynamics those elements achieve an infinite boundary condition by applying a viscous normal pressure where the coefficient $c _ { v }$ is given by $\rho c _ { d } ; \rho$ is the density of the material at the surface, and $c _ { d }$ is the value of the dilatational wave speed in the material (the infinite continuum elements also apply a viscous shear traction). For an isotropic, linear elastic material $$ c _ {d} = \sqrt {\frac {\lambda + 2 \mu}{\rho}} = \sqrt {\frac {E (1 - \nu)}{\rho (1 + \nu) (1 - 2 \nu)}}, $$ where and $\mu$ are Lamé’s constants, E is Young’s modulus, and is Poisson’s ratio. This choice of the viscous pressure coefficient represents a level of damping in which pressure waves crossing the free surface are absorbed with no reflection of energy back into the interior of the finite element mesh. For typical structural problems it is not desirable to absorb all of the energy (as is the case in the infinite elements). Typically $c _ { v }$ is set equal to a small percentage (perhaps 1 or 2 percent) of $\rho c _ { d }$ as an effective way of minimizing ongoing dynamic effects. The $c _ { v }$ coefficient should have a positive value. Input File Usage: Use one of the following options to define a viscous pressure load: $\scriptstyle * \mathrm { D L O A D } , \mathrm { R E F ~ N O D E } = r e f e r e n c e \_ n o d e$ element number or element set, VPn or VP, magnitude \*DSLOAD, REF NODE=reference\_node surface name, VP, magnitude Abaqus/CAE Usage: Use the following input to define a surface-based viscous pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Viscous, toggle on or off Determine velocity from reference point Element-based viscous pressure loads are not supported in Abaqus/CAE. Stagnation pressure loads in Abaqus/Explicit Stagnation pressure loads are defined by $$ p _ {s} = - c _ {s} \left(\mathbf {v} \cdot \mathbf {n} - \mathbf {v} _ {r e f} \cdot \mathbf {n}\right) ^ {2}, $$ where $p _ { s }$ is the stagnation pressure applied to the body; $c _ { s }$ is the factor, given as the magnitude of the load; is the velocity of the point on the surface where the pressure is being applied; is the unit outward normal to the element at the same point; and $\mathbf { v } _ { r e f }$ is the velocity of the reference node. The coefficient $c _ { s }$ should be very small to avoid excessive damping and a dramatic drop in the stable time increment. Input File Usage: Use one of the following options to define a stagnation pressure load: \*DLOAD, REF NODE=reference\_node element number or element set, SPn or SP, magnitude \*DSLOAD, REF NODE=reference\_node element number or element set, SP, magnitude Abaqus/CAE Usage: Use the following input to define a surface-based stagnation pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Stagnation, toggle on or off Determine velocity from reference point Element-based stagnation pressure loads are not supported in Abaqus/CAE. Pressure on pipe and elbow elements You can specify external pressure, internal pressure, external hydrostatic pressure, or internal hydrostatic pressure on pipe or elbow elements. When pressure loads are applied, the effective outer or inner diameter must be specified in the element-based distributed load definition. The loads resulting from the pressure on the ends of the element are included: Abaqus assumes a closed-end condition. Closed-end conditions correctly model the loading at pipe intersections, tight bends, corners, and cross-section changes; in straight sections and smooth bends the end loads of adjacent elements cancel each other precisely. If an open-end condition is to be modeled, a compensating point load should be added at the open end. A case where such an end load must be applied occurs if a pressurized pipe is modeled with a mixture of pipe and beam elements. In that case closed-end conditions generate a physically non-existing force at the transition between pipe and beam elements. Such mixed modeling of a pipe is not recommended. For pipe elements subjected to pressure loading, the effective axial force due to the pressure loads can be obtained by requesting output variable ESF1 (see “Beam element library,” Section 29.3.8). Input File Usage: Use the following option to define an external pressure load on pipe or elbow elements: \*DLOAD element number or element set, PE or PENU, magnitude, effective outer diameter Use the following option to define an internal pressure load on pipe or elbow elements: \*DLOAD element number or element set, PI or PINU, magnitude, effective inner diameter Use the following option to define an external hydrostatic pressure load on pipe or elbow elements: \*DLOAD element number or element set, HPE, magnitude, effective outer diameter Use the following option to define an internal hydrostatic pressure load on pipe or elbow elements: \*DLOAD element number or element set, HPI, magnitude, effective inner diameter Abaqus/CAE Usage: Use the following input to define an external or internal pressure load on pipe or elbow elements: Load module: Create Load: choose Mechanical for the Category and Pipe pressure for the Types for Selected Step: Side: External or Internal, Distribution: Uniform, User-defined, or select an analytical field Use the following input to define an external or internal hydrostatic pressure load on pipe or elbow elements: Load module: Create Load: choose Mechanical for the Category and Pipe pressure for the Types for Selected Step: Side: External or Internal, Distribution: Hydrostatic # Defining distributed surface loads on plane stress elements Plane stress theory assumes that the volume of a plane stress element remains constant in a large-strain analysis. When a distributed surface load is applied to an edge of plane stress elements, the current length and orientation of the edge are considered in the load distribution, but the current thickness is not; the original thickness is used. This limitation can be circumvented only by using three-dimensional elements at the edge so that a change in thickness upon loading is recognized; suitable equation constraints (“Linear constraint equations,” Section 35.2.1) would be required to make the in-plane displacements on the two faces of these elements equal. Three-dimensional elements along an edge can be connected to interior shell elements by using a shell-to-solid coupling constraint (see “Shell-to-solid coupling,” Section 35.3.3, for details). # Edge tractions and moments on shell elements and line loads on beam elements Distributed edge tractions (general, shear, normal, or transverse) and edge moments can be applied to shell elements in Abaqus as element-based or surface-based distributed loads. The units of an edge traction are force per unit length. The units of an edge moment are torque per unit length. References to local coordinate systems are ignored for all edge tractions and moments except general edge tractions. Distributed line loads can be applied to beam elements in Abaqus as element-based distributed loads. The units of a line load are force per unit length. The distributed edge and line load types that are available in Abaqus, along with the corresponding load type labels, are listed in Table 34.4.3–7 and Table 34.4.3–8. Part VI, “Elements,” lists the distributed edge and line load types that are available for particular elements and the Abaqus/CAE load support for each load type. For element-based loads applied to shell elements, you must identify the edge of the element upon which the load is prescribed in the load type label (for example, EDLDn or EDLDnNU). # Follower edge and line loads By definition, the line of action of a follower edge or line load rotates with the edge or line in a geometrically nonlinear analysis. This is in contrast to a non-follower load, which always acts in a fixed global direction. With the exception of general edge tractions on shell elements and the forces per unit length in the global directions on beam elements, all the edge and line loads listed in Table 34.4.3–7 and Table 34.4.3–8 are modeled as follower loads. The normal, shear, and transverse edge loads listed in Table 34.4.3–7 and Table 34.4.3–8 act in the normal, shear, and transverse directions, respectively, in the current configuration (see Figure 34.4.3–6). The edge moment always acts about the shell edge in the current configuration. The forces per unit length in the local beam directions rotate with the beam elements. Table 34.4.3–7 Distributed edge load types.

Load description	Load type label for element-based loads	Load type label for surface-based loads
General edge traction	EDLDn	EDLD
Normal edge traction	EDNORn	EDNOR
Shear edge traction	EDSHRn	EDSHR
Transverse edge traction	EDTRAn	EDTRA
Edge moment	EDMOMn	EDMOM

Load description	Load type label for element-based loads	Load type label for surface-based loads
Nonuniform general edge traction	EDLDnNU	EDLDNU
Nonuniform normal edge traction	EDNORnNU	EDNORNU
Nonuniform shear edge traction	EDSHRnNU	EDSHRNU
Nonuniform transverse edge traction	EDTRAnNU	EDTRANU
Nonuniform edge moment	EDMOMnNU	EDMOMNU
Force per unit length in global X-, Y-, and Z-directions (only for beam elements)	PX, PY, PZ	N/A
Nonuniform force per unit length in global X-, Y-, and Z-directions (only for beam elements)	PXNU, PYNU, PZNU	N/A
Force per unit length in beam local 1- and 2-directions (only for beam elements)	P1, P2	N/A
Nonuniform force per unit length in beam local 1- and 2-directions (only for beam elements)	P1NU, P2NU	N/A

Table 34.4.3–8 Distributed edge load types in Abaqus/CAE.

Load description	Abaqus/CAE load type
General edge traction	Shell edge load
Normal edge traction
Shear edge traction
Transverse edge traction
Edge moment
Nonuniform general edge traction	Shell edge load (surface-based loads only)
Nonuniform normal edge traction
Nonuniform shear edge traction
Nonuniform transverse edge traction
Nonuniform edge moment

Load description	Abaqus/CAE load type
Force per unit length in global X-, Y-, and Z-directions (only for beam elements)	Line load
Nonuniform force per unit length in global X-, Y-, and Z-directions (only for beam elements)
Force per unit length in beam local 1- and 2-directions (only for beam elements)
Nonuniform force per unit length in beam local 1- and 2-directions (only for beam elements)

The forces per unit length in the global directions on beam elements are always non-follower loads. General edge tractions can be specified to be follower or non-follower loads. There is no difference between a follower and a non-follower load in a geometrically linear analysis since the configuration of the body remains fixed. Input File Usage: Use one of the following options to define general edge tractions as follower loads (the default): \*DLOAD, FOLLOWER=YES \*DSLOAD, FOLLOWER=YES Use one of the following options to define general edge tractions as non-follower loads: \*DLOAD, FOLLOWER=NO \*DSLOAD, FOLLOWER=NO Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: General, toggle on or off Follow rotation # Specifying general edge tractions General edge tractions allow you to specify an edge load, , acting on a shell edge, L. The resultant load, , is computed by integrating over L: $$ \mathbf {f} = \int_ {L} \mathbf {t} d L. $$ To define a general edge traction, you must provide both a magnitude, , and direction, $\mathbf { t } _ { u s e r }$ , for the load. The specified load directions are normalized by Abaqus; thus, they do not contribute to the magnitude of the load. 

flowchart

```mermaid graph TD 1 -->|EDTRA| 4 1 -->|EDNOR| 4 1 -->|EDSHR| 4 2 -->|EDTRA| 3 2 -->|EDNOR| 3 2 -->|EDSHR| 3 3 -->|EDTRA| 4 3 -->|EDNOR| 4 4 -->|EDTRA| 3 4 -->|EDSHR| 3 ```


flowchart

```mermaid graph TD 1["1"] -->|EDNOR| 2["2"] 1 -->|EDSHR| 3["3"] 2 -->|EDNOR| 3 2 -->|EDSHR| 3 3 -->|EDNOR| 2 3 -->|EDSHR| 3 3 -->|EDTRA| 1 3 -->|EDTRA| 2 3 -->|EDTRA| 3 ```

Figure 34.4.3–6 Positive edge loads. If a nonuniform general edge traction is specified, the magnitude, , and direction, $\mathbf { t } _ { u s e r }$ , must be specified in user subroutine UTRACLOAD. ```txt Input File Usage: Use one of the following options to define a general edge traction: *DLOAD element number or element set, EDLDn or EDLDnNU, magnitude, direction components *DSLOAD surface name, EDLD or EDLDNU, magnitude, direction components ``` Abaqus/CAE Usage: Use the following input to define an element-based general edge traction: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: General, Distribution: select an analytical field Use the following input to define a surface-based general edge traction: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: General, Distribution: Uniform or User-defined Nonuniform element-based general edge traction is not supported in Abaqus/CAE. Rotation of the load vector In a geometrically linear analysis the edge load, , acts in the fixed direction defined by $$ \mathbf {t} = \alpha \frac {\mathbf {t} _ {u s e r}}{\| \mathbf {t} _ {u s e r} \|}. $$ If a non-follower load is specified in a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state), the edge load, , acts in the fixed direction defined by $$ \mathbf {t} = \alpha \frac {\mathbf {t} _ {u s e r}}{\| \mathbf {t} _ {u s e r} \|}. $$ If a follower load is specified in a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state), the components must be defined with respect to the reference configuration. The reference edge traction is defined as $$ \mathbf {t} ^ {o} = \alpha \frac {\mathbf {t} _ {u s e r}}{\| \mathbf {t} _ {u s e r} \|}. $$ The applied edge traction, , is computed by rigidly rotating onto the current edge. Defining the direction vector with respect to a local coordinate system By default, the components of the edge traction vector are specified with respect to the global directions. You can also refer to a local coordinate system (see “Orientations,” Section 2.2.5) for the direction components of these tractions. Input File Usage: Use one of the following options to specify a local coordinate system: $$ \begin{array}{l} * D L O A D, O R I E N T A T I O N = n a m e \\ * \text { DSLOAD, ORIENTATION } = \text { name } \\ \end{array} $$ Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: select CSYS: Picked and click Edit to pick a local coordinate system, or select CSYS: User-defined to enter the name of a user subroutine that defines a local coordinate system