line

| Element | φ_constant | quadratic | φ_trial | φ_limited | | --------- | ---------- | --------- | ------- | --------- | | element 1 | high | high | high | high | | element 2 | medium | medium | medium | medium | | element 3 | low | low | low | low |

Figure 12.2.3–2 Second-order advection. 1. A quadratic interpolation is constructed from the constant values of $\phi$ at the integration points of the middle element and in its adjacent elements. 2. A trial linear distribution, $\phi _ { t r i a l } $ is found by differentiating the quadratic function to find the slope at the integration point of the middle element. 3. The trial linear distribution in the middle element is limited by reducing its slope until its minimum and maximum values are within the range of the original constant values in the adjacent elements. This process is referred to as flux-limiting and is essential to ensure that the advection is monotonic. Once the flux-limited linear distributions are determined for all elements in the old mesh, these distributions are integrated over each new element. The new value of the variable is found by dividing the value of each integral by the new element volume. (See Figure 12.2.3–3 for a first-order example of this calculation.) # Input File Usage: Use the following option to specify that the second-order advection method should be used to remap element variables: \*ADAPTIVE MESH CONTROLS, NAME=name, ADVECTION=SECOND ORDER 

line

| Layer | Value | | ----------- | ----------- | | old mesh | φ₂^new | | new mesh | φ₁^new | | old mesh | φ₁^old | | new mesh | φ₂^old | | old mesh | φ₁^new | | new mesh | φ₁^old |

Figure 12.2.3–3 First-order advection. Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, toggle on Second order # First-order advection First-order advection is simple and computationally efficient; however, it tends to diffuse sharp gradients over time, especially in transient dynamic analyses or other problems that require fairly frequent adaptive meshing. Therefore, this technique should be used only as a computationally efficient alternative for quasi-static simulations that do not require frequent adaptive meshing. Figure 12.2.3–3 illustrates the first-order method for a portion of a one-dimensional mesh. An element variable, , is remapped from the old mesh to the new mesh by first assuming a constant value of the variable for each old element. These values are then integrated over each new element. The new value of the variable is found by dividing the value of each integral by the new element volume. Input File Usage: Use the following option to specify that the first-order advection method should be used to remap element variables: \*ADAPTIVE MESH CONTROLS, NAME=name, ADVECTION=FIRST ORDER Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, toggle on First order Nodal velocities are computed on a new mesh by first advecting momentum, then using the mass distribution on the new mesh to calculate the velocity field. Advecting momentum directly ensures that momentum is conserved properly in the adaptive mesh domain during remapping. Two methods are available for advecting momentum: the default element center projection method and the half-index shift method (Benson, 1992). Both methods are applicable for all adaptive mesh applications. # Element center projection method The element center projection method is the default method used to advect momentum and requires the fewest numerical operations. The element momentum is calculated first for the old mesh based on the mass and velocity of the element nodes. The element momentum is then advected from the old mesh to the new mesh by the same first- or second-order algorithms used for advecting element variables. Finally, the element momentum on the new mesh is assembled at the nodes using a projection. The element center projection method requires the advection of only two or three extra variables in two dimensions or three dimensions, respectively.

Input File Usage:	Use the following option to request the most computationally efficient momentum advection method:
	*ADAPTIVE MESH CONTROLS, NAME=name, MOMENTUM ADVECTION=ELEMENT CENTER PROJECTION

Abaqus/CAE Usage:

Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Momentum advection: Element center projection

# Half-index shift method The half-index shift method is computationally more intensive than the element center projection method, but it may result in less wave dispersion for some problems. This method first shifts each of the nodal momentum variables from the nodes surrounding an element to the element center. The shifted momentum variables are then advected from the old mesh to the new mesh by the same firstor second-order algorithms used for advecting element variables, providing momentum variables at the center of the new elements. Finally, the momentum variables at the element centers in the new mesh are shifted back to the nodes. The half-index shift method requires the advection of 8 or 24 extra variables in two or three dimensions, respectively, which can increase the cost of each advection sweep significantly.

Input File Usage:	Use the following option to specify that the half-index shift method should be used for momentum advection:
	*ADAPTIVE MESH CONTROLS, NAME=name, MOMENTUM ADVECTION=HALF INDEX SHIFT

Abaqus/CAE Usage:

Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Momentum advection: Half-index shift

# Additional references • Benson, D. J., “Momentum Advection on a Staggered Mesh,” Journal of Computational Physics, vol. 100, pp. 143–162, 1992. • Van Leer, B., “Towards the Ultimate Conservative Difference Scheme III. Upstream-centered Finite-Difference Schemes for Ideal Compressible Flow,” Journal of Computational Physics, vol. 23, pp. 263–275, 1977. • Van Leer, B., “Towards the Ultimate Conservative Difference Scheme IV. A New Approach to Numerical Convection,” Journal of Computational Physics, vol. 23, pp. 276–299, 1977. # 12.2.4 MODELING TECHNIQUES FOR EULERIAN ADAPTIVE MESH DOMAINS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE # References • “ALE adaptive meshing: overview,” Section 12.2.1 • “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2 • \*ADAPTIVE MESH CONSTRAINT • “Understanding ALE adaptive meshing,” Section 14.6 of the Abaqus/CAE User’s Guide # Overview An Eulerian adaptive mesh domain: • is used to model material flowing through the mesh; and • typically has two Eulerian boundary regions, one inflow and one outflow, connected by Lagrangian and/or sliding boundary regions. The correct combination of mesh constraints and material boundary conditions applied to an Eulerian boundary region depends on whether the region acts as an inflow or an outflow boundary. The region types and mesh constraints assigned to the boundary regions that are connected to the Eulerian boundary regions must be chosen to simulate the correct physical behavior as well. The adaptive meshing technique in Abaqus/Explicit is robust if the mesh is underconstrained: the modeling techniques presented in this section are intended to provide guidance in properly defining Eulerian models. # ALE adaptive mesh constraints on Eulerian boundaries ALE adaptive mesh constraints should be applied normal to an Eulerian boundary region; otherwise, the motion of the mesh on the boundary is ambiguous. If no mesh constraints are applied normal to the boundary, Abaqus/Explicit will treat the region as if it were sliding, and the mesh will follow the material normal to the boundary. Although there are no restrictions on specifying adaptive mesh constraints at nodes on an Eulerian boundary region, the following guidelines should be followed in most cases: • Mesh constraints should be applied to every node on the Eulerian boundary region, including the corners and edges. • Mesh constraints should be applied either only normal to the Eulerian boundary region or in every direction. Mesh constraints should not be specified in only the direction tangential to an Eulerian boundary region; such constraints are ambiguous and may result in undesirable motion of the mesh at the boundary. Loads and boundary conditions on Eulerian boundaries act on the material that instantaneously coincides with the mesh at the surface. When used in combination with spatial adaptive mesh constraints, physically meaningful Eulerian flow conditions can be defined. # Defining inflow Eulerian boundaries The material flowing into an adaptive mesh domain through an Eulerian boundary will have the same stress and material state as the material in the elements immediately adjacent to the boundary. Therefore, it is important to maintain the stress and material state in those elements at the desired values (which in many cases will be zero, to simulate stress-free material entering the Eulerian domain). To accomplish this goal: • position the inflow boundary far enough upstream from high solution gradients to ensure that the response at the inflow boundary is smooth, and • apply sufficient mesh and material constraints at the boundary (as described later in this section). To be physically meaningful, the size and shape of the inflow boundary region must be maintained. For example, applying sufficient constraints is crucial for steady-state process simulations where the cross-section of the workpiece entering the adaptive mesh domain is known and affects the response downstream. The types of constraints appropriate for an inflow boundary depend on whether the precise location of the inflow boundary region is known or whether it is part of the solution. # Known inflow boundary location In many problems the area, shape, and position of the inflow boundary are known a priori. For example, in the steady-state analysis of a forward extrusion process, an inflow Eulerian boundary can be used to model the flow of material into the adaptive mesh domain. The size of the inflow boundary is based on the known billet cross-section, and the location of the inflow boundary is fixed because of the confined conditions on the material. When the area, shape, and location of the inflow boundary are known, both material and mesh constraints should be applied. Figure 12.2.4–1 shows a typical model setup for a two-dimensional forward extrusion problem where either a prescribed mass flow rate or a prescribed uniform pressure is applied to a known inflow boundary. Apply boundary conditions at all nodes on the inflow boundary region to prescribe material constraints in the directions tangential to the boundary surface. Preventing motion of the material tangential to the inflow boundary helps to maintain the stress and material state of the elements adjacent to the Eulerian boundary. Apply adaptive mesh constraints in the normal direction at all nodes on the inflow boundary. In addition, apply mesh constraints in all tangential directions at the edges and corners surrounding the Eulerian boundary region. These constraints fix the location and size of the cross-sectional area at the inflow boundary. If a nonuniform boundary condition or load is applied to the material at the inflow boundary or if the initial material state in the elements adjacent to the boundary is nonuniform in the tangential direction, apply tangential mesh constraints to the nodes strictly in the interior of the Eulerian boundary region. 

flowchart

```mermaid graph TD A["node set TOP"] --> B["node set INFLOW element set INFLOW"] B --> C["node set BOTTOM"] C --> D["Prescribed inflow velocity: or"] style A fill:#f9f,stroke:#333 style B fill:#ccf,stroke:#333 style C fill:#cfc,stroke:#333 style D fill:#fcc,stroke:#333 note right of A node_set_TOP node_setINFLOW node_setINFLOW node_setTOP node_setINFLOW node_setINFLOW node_setTOP node_setINFLOW node_setINFLOW node_setTOP node_setINFLOW node_setINFLOW node_setTOP node_setINFLOW node_setINFLOW node_setTOP node_setINFLOW node_setINFLOW node_setTOP node_setINFLOW node_setINFLOW flow symmetry end note right of A Eulerian boundary region defined by a velocity-type boundary condition applied to node_set INFLOW in direction 1 ```


text_image

zero-displacement adaptive mesh constraints applied to node set INFLOW in direction 1 and to node sets TOP and BOTTOM in direction 2 Eulerian boundary region defined by a zero-displacement boundary condition applied to node set INFLOW in direction 2 Prescribed inflow pressure: Eulerian boundary region defined by a pressure load applied to element set INFLOW in direction 1

Figure 12.2.4–1 Known inflow boundary. Although the application of mesh and material constraints tangential to and along the edges and corners of an inflow Eulerian boundary may appear to be redundant, they are actually independent. For example, consider a long billet with a variable cross-section, as shown in Figure 12.2.4–2. 

flowchart

```mermaid graph TD A["Inflow boundary; node set INFLOW"] --> B["Symmetry"] B --> C["Outflow boundary; node set OUTFLOW; element set OUTFLOW"] D["N"] --> E["v₀"] style A fill:#f9f,stroke:#333 style B fill:#ccf,stroke:#333 style C fill:#cfc,stroke:#333 ```


text_image

Eulerian boundary region created by a surface defined on the S3 faces of element set OUTFLOW ← zero-displacement adaptive mesh constraints applied to node sets INFLOW and OUTFLOW in direction 1 ↑ velocity-type adaptive mesh constraint with amplitude INCOMING applied to node N in direction 2 ↓ Eulerian boundary region defined by a zero-displacement boundary condition applied to node set INFLOW in direction 2 → Eulerian boundary region defined by a velocity-type boundary condition with a variable amplitude applied to node set INFLOW in direction 1

Figure 12.2.4–2 Modeling a billet with a variable cross-section. The adaptive mesh domain, with its inflow and outflow Eulerian boundary regions, is assumed to represent a portion of the billet along its length. The entire billet moves with a rigid body velocity along its length (x-direction) so that material flows into one Eulerian boundary and out the other. Boundary conditions are applied to the material at the inflow boundary to maintain this velocity. Mesh constraints are applied normal to the inflow and outflow boundary regions. The mesh constraint applied in the y-direction at node N is used to prescribe the known variable incoming cross-section of the material. The motion of this node does not affect the velocity field of the material entering the domain. # Unknown inflow boundary location Sometimes, the location of the inflow boundary region is known only approximately; its precise location will be determined from the solution. For these problems, apply adaptive mesh constraints only in the direction normal to the Eulerian boundary region. In the absence of tangential mesh constraints at the edges and corners of the Eulerian boundary region, Abaqus/Explicit will move these edges and corners with the material in the tangential direction but with the mesh constraints in the normal direction. Therefore, material constraints should be applied using multi-point constraints (see “General multi-point constraints,” Section 35.2.2) or linear constraint equations (see “Linear constraint equations,” Section 35.2.1) to preserve the cross-sectional area of the inflow boundary. For example, consider a steady-state rolling simulation with multiple rollers in an asymmetric configuration, as shown in Figure 12.2.4–3. 

flowchart

```mermaid graph TD A["billet is free to move"] --> B["node set INFLOW"] B --> C["free surface"] C --> D["flow of material"] D --> E["node 1"] E --> F["free surface"] F --> G["node 1"] style A fill:#f9f,stroke:#333 style B fill:#ccf,stroke:#333 style C fill:#cfc,stroke:#333 style D fill:#fcc,stroke:#333 style E fill:#cff,stroke:#333 style F fill:#ffc,stroke:#333 style G fill:#fcf,stroke:#333 note1["zero-displacement adaptive mesh constraints applied to node 1 and node set INFLOW in direction 1"] --> note2["PIN-type multi-point constraints applied to node set INFLOW and node 1"] ```

Figure 12.2.4–3 Unknown inflow boundary location. It may be impractical to extend the analysis domain as far as the guides on the upstream side, but spatially fixing the inflow boundary at an arbitrary position in the y- and z-directions may cause unrealistic stress on the workpiece as it finds an equilibrium position between the rollers. Mesh constraints are applied normal to the Eulerian boundary region to fix the position of the inflow boundary relative to the rollers in the x-direction. Material constraints (applied with a PIN MPC) are used to ensure that material enters the domain at a uniform velocity and that the cross-section does not rotate. The material constraints will maintain the cross-sectional shape of the section while allowing it to move laterally to the correct equilibrium position. Since tangential mesh constraints are not used, the mesh will follow the material in the directions tangential to the Eulerian boundary region. # Defining outflow Eulerian boundaries Typically, adaptive mesh constraints should be applied only in the direction normal to the surface on an Eulerian boundary region that acts as an outflow boundary. No tangential mesh constraints should be applied to the edges or corners of an outflow boundary adjacent to a Lagrangian (or sliding) boundary region acting as a free surface. In contrast to inflow boundaries, the cross-section of an outflow boundary adjacent to a free surface is determined by the solution in the domain. At the edge or corner where an Eulerian boundary region meets a Lagrangian or sliding boundary region, Abaqus/Explicit will satisfy the applied mesh constraint normal to the Eulerian boundary region and the inherent mesh constraint normal to the Lagrangian or sliding boundary region simultaneously, thus correctly handling the evolution of the free surface adjacent to the outflow boundary. Figure 12.2.4–4 shows the evolution of an outflow boundary from $t _ { 0 }$ to $t _ { 1 }$ , where material continues to flow through the outflow boundary. 

text_image

free surface N v₀ symmetry Eulerian boundary region created by a surface defined on the S2 faces of element set OUTFLOW zero-displacement adaptive mesh constraint applied to node set OUTFLOW in direction 1 motion of node N to satisfy constraint position of free surface at time t₀ position of free surface at time t₁

Figure 12.2.4–4 Abaqus/Explicit will respect the free surface at an Eulerian outflow boundary. The mesh constraint normal to the Eulerian outflow boundary is applied by moving node N along the free surface of the material, so that the outflow boundary “expands” with the material arriving from upstream. Although not shown in the figure, mesh smoothing causes all other nodes on the outflow boundary, with the exception of the node on the symmetry plane, to move up toward node N as the boundary expands. No special material boundary conditions are required at outflow Eulerian boundaries. Boundary conditions tangential to the outflow boundary are recommended only if they are the same as those defined upstream (e.g., a symmetry plane running along the length of an Eulerian domain). However, to improve convergence to the steady-state solution in steady-state process simulations, it is often useful to constrain the material velocity to be uniform normal to the outflow boundary using multi-point constraints or linear constraint equations. # Defining Eulerian boundary regions that act as both inflow and outflow boundaries Although it is rarely appropriate, an Eulerian boundary region can act as both an inflow and an outflow boundary at different times during the same analysis step. Adaptive mesh constraints and material boundary conditions at such a boundary should be chosen to be physically meaningful for both inflow and outflow situations. For each node on the edges and corners of an Eulerian boundary region that does not have mesh constraints tangential to the boundary surface, Abaqus/Explicit will determine in each adaptive mesh increment whether the boundary at the node is acting as an inflow or an outflow boundary. If an inflow condition is detected, the node will move with the material in the tangential direction but with the mesh constraints in the normal direction. If an outflow condition is detected, the movement of the node will both follow the adjacent Lagrangian boundary region and satisfy the mesh constraint normal to the Eulerian boundary region. # Lagrangian versus sliding boundary regions on Eulerian domains Many applications using Eulerian adaptive mesh domains, including the simulation of steady-state processes, have a primary direction of material flow and use a control volume approach to model the process zone. These problems usually include two Eulerian boundary regions, representing an inflow boundary and outflow boundary. The remaining surfaces between the Eulerian boundaries can be either Lagrangian or sliding boundary regions. Determining which type of boundary region to use between the two Eulerian boundary regions depends on the type of load or boundary condition that is required: • Use a sliding boundary region to define boundary conditions or loads that act at a spatial location on a portion of the surface along the length of the control volume. Apply adaptive mesh constraints to fix the mesh spatially in the flow direction (and possibly in the direction transverse to the flow). For example, a distributed pressure can be applied around the circumference of the control volume, as shown in Figure 12.2.4–5. The distributed pressure load is defined using a sliding boundary region. Mesh constraints are applied to fix the boundary region spatially in the flow direction. Similarly, a concentrated load could be applied to a specific spatial location to model the effect of a very sharp body pressing into the workpiece at a known location with a known force. • Use a sliding boundary region to define boundary conditions or loads that act along the entire length of the Eulerian control volume between the inflow and outflow boundaries and act in a spatial manner transversely to the flow. If the load acts on only a portion of the surface in the transverse direction, it may be necessary to apply mesh constraints in the direction transverse to the flow. For example, a boundary condition that acts as a knife edge along the length of the domain is shown in Figure 12.2.4–6. Mesh constraints are applied in the transverse direction (and, if the line of application is curved, along the line) to keep the boundary condition fixed spatially. • Use a Lagrangian boundary region (default) to define boundary conditions or loads that act along the entire length of the surface of the Eulerian control volume between the inflow and