김경종
8.0 KiB
Requesting sampling as elements pass the exit plane for a Lagrangian analysis
You can request that all steady-state norms be calculated as each plane of elements crosses the exit plane.
Input File Usage: *STEADY STATE DETECTION, ELSET=elset, SAMPLING=PLANE BY PLANE
Requesting sampling at uniform intervals for an Eulerian analysis
Alternatively, you can request that all steady-state norms be calculated at an interval based on the time required for material to progress the length of an average element.
Input File Usage: *STEADY STATE DETECTION, ELSET=elset, SAMPLING=UNIFORM
Steady-state criteria
Any number of steady-state criteria definitions can be specified. Only when all of the criteria specified under any one steady-state criteria definition have been satisfied will the analysis be considered to have reached steady state.
To define the criteria, you specify the norm type identifier, the norm tolerance, and the global coordinates of a point on the exit plane. For force and torque norms, you also specify the rigid body reference node of the forming tool at the exit plane and the direction cosines of the force or torque. Exit planes can be defined separately for each norm definition.
Input File Usage: Use the following options to define the criteria needed to achieve steady state:
*STEADY STATE DETECTION, ELSET=elset, SAMPLING=PLANE BY PLANE or UNIFORM
*STEADY STATE CRITERIA
*STEADY STATE CRITERIA
...
For example, assume that two sets of criteria are of interest and that the analysis can be terminated as soon as either is satisfied. The input might be as follows:
*STEADY STATE DETECTION, ELSET=sheet,
SAMPLING=PLANE BY PLANE
1.0, 0.0, 0.0, 6.0, 0.0, 0.0
*STEADY STATE CRITERIA
SSPEEQ,.002, 5.0, 0.0, 0.0
SSSPRD,.002, 5.0, 0.0, 0.0
SSFORC,.005, 5.0, 0.0, 0.0, 1000, 1.0, 0.0, 0.0
SSFORC,.005, 5.0, 0.0, 0.0, 1000, 0.0, 1.0, 0.0
SSTORQ,.005, 5.0, 0.0, 0.0, 1000, 0.0, 0.0, 1.0
*STEADY STATE CRITERIA
SSPEEQ,.001, 5.0, 0.0, 0.0
SSSPRD,.001, 5.0, 0.0, 0.0
SSFORC,.010, 5.0, 0.0, 0.0, 1000, 0.0, 1.0, 0.0
Materials
Steady-state detection is intended to be used with plasticity-based materials since the equivalent plastic strain norm would be zero for nonplasticity-based material models.
Procedures
One steady-state detection definition is allowed per analysis. The definition can be entered in any step and is continued through subsequent steps in an analysis. A steady-state detection definition cannot be entered in an annealing step or continued through an annealing step.
Elements
The current steady-state detection capabilities support the use of C3D8R and C3D8RT elements only.
Output
The output variables SSPEEQn, SSSPRDn, SSFORCn, and SSTORQn are used to output the equivalent plastic strain, spread, force, and torque norms, respectively. Abaqus/CAE can be used to obtain history plots of each of the steady-state detection norm variables. Individual norms can be output by requesting the norm number n, which is based on the order in which the norms are specified. Referring to the example above, if the force norm of the second steady-state criteria definition were to be requested, the output identifier would be SSFORC3. If a steady-state detection norm is requested that does not include a norm number, SSFORC for example, all norms of that type are output.
Once steady state has been detected, an element set is created automatically by Abaqus/Explicit and written to the output database consisting of the plane of elements that first satisfied the steady-state criteria. The element set created is named SteadyStatePlane-StepN, where N is the step number; and it can be viewed with Abaqus/CAE. If no output requests are made to the output database, the element set SteadyStatePlane-StepN is not created.
Input file template
*HEADING
...
*ELSET, ELSET=WORKPIECE
**************************
*STEP
*DYNAMIC, EXPLICIT
Data line to specify the time period of the step
...
*STEADY STATE DETECTION, ELSET=WORKPIECE, SAMPLING=PLANE BY PLANE
Data line specifying rolling direction and cutting plane position
*STEADY STATE CRITERIA
Data lines specifying steady-state detection norm criteria
...
*OUTPUT, HISTORY, TIME INTERVAL=1.E-6
*INCREMENTATION OUTPUT
SSPEEQ, SSSPRD, SSFORC, SSTORQ
...
*END STEP
12. Adaptivity Techniques
Adaptivity techniques: overview 12.1
ALE adaptive meshing 12.2
Adaptive remeshing 12.3
Analysis continuation after mesh replacement 12.4
12.1 Adaptivity techniques: overview
• “Adaptivity techniques,” Section 12.1.1
12.1.1 ADAPTIVITY TECHNIQUES
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “ALE adaptive meshing: overview,” Section 12.2.1
• “Adaptive remeshing: overview,” Section 12.3.1
• “Mesh-to-mesh solution mapping,” Section 12.4.1
• *ADAPTIVE MESH
• “Understanding adaptive remeshing,” Section 17.13 of the Abaqus/CAE User’s Guide
Overview
The finite element discretization that results from suboptimal meshing of models can limit your ability to obtain adequate analysis results at a reasonable CPU cost. This section provides an overview of the adaptivity techniques available in Abaqus that help you optimize a mesh and, therefore, obtain quality solutions while controlling the cost of your analysis. The term “adaptivity” reflects the adaptive, or solution-dependent, processes that Abaqus uses to adapt your mesh to meet your analysis goals.
Selecting an adaptivity technique
Three adaptivity techniques are available in Abaqus: Arbitrary Lagrangian-Eulerian (ALE) adaptive meshing; varying topology adaptive remeshing; and mesh-to-mesh solution mapping, to enable rezoning analysis. Table 12.1.1–1 shows that the adaptivity techniques can be classified according to
• their applicability to achieving particular goals, either accuracy or control of mesh distortion;
• their impact on mesh definitions, either through smoothing a single mesh or through generating multiple dissimilar meshes; and
• when adaptivity occurs with respect to analysis steps.
Table 12.1.1–1 The characteristics of the adaptivity techniques.
| Accuracy | Distortion control | Single mesh | Multiple meshes | Adaptivity occurs | |
| ALE adaptive meshing | √ | √ | Throughout a step | ||
| Adaptive remeshing | √ | √ | Separately from analysis steps | ||
| Mesh-to-mesh solution mapping | √ | √ | Between analysis steps |
ALE adaptive meshing
Arbitrary Lagrangian-Eulerian (ALE) adaptive meshing provides control of mesh distortion. ALE adaptive meshing uses a single mesh definition that is gradually smoothed within analysis steps. ALE adaptive meshing is available for limited applications in Abaqus/Standard and is more generally applicable in Abaqus/Explicit. The term ALE implies a broad range of analysis approaches, from purely Lagrangian analysis, in which the node motion corresponds to material motion, to purely Eulerian analysis, in which the nodes remain fixed in space and material “flows” through the elements. Typically ALE analyses use an approach between these two extremes. The ALE feature is distinct from the Eulerian analysis capability in Abaqus/Explicit, which is described in “Eulerian analysis,” Section 14.1.1.
You can use adaptive meshing to control element distortion in cases where large deformation or loss of material occurs. Figure 12.1.1–1 illustrates a case where adaptive meshing limits mesh distortion in a bulk forming simulation.
Figure 12.1.1–1 Use of ALE adaptive meshing to control element distortion.