Thread Content
【Software Operation】Q&A Series on AWB: Introduction to Modules and Selection Techniques. Ansys Workbench, the analysis software promoted by ASE Asia Pacific, has now been updated to version 19.0; when I first started learning to use it, it was still version 14.5. The company acquired version 18.2 this year. It must be said that AWB is truly a premium software – the cost of purchasing one license is 940,000. As the saying goes, a good horse requires a good saddle, but having just a good saddle isn’t enough; it also depends on the skill and ability of the person who rides it. With the powerful features of the latest version of AWB, I feel that there is always more to learn. Before I even had time to fully understand version 14.5, I already had to start learning the new version. For beginners, it is not only necessary to have a solid foundation in theoretical knowledge but also to be thoroughly familiar with the software. I encountered many problems while learning*, and I could only find answers by searching online; however, there is very little information available online regarding AWB, so often one has to figure things out on their own. Here, I would like to share some of the minor problems I faced as a beginner, in the hope of providing some help to others and allowing them to avoid unnecessary detours. This article mainly focuses on various issues related to units in AWB. 1. What is the default unit type for AWB? Element type: The default is the 20-node solid186 element; by removing the middle nodes, it becomes the 8-node solid185 element ； Shell element: The default is the 8-node shell281 element; removing the middle nodes results in the 4-node shell181 element ； Beam element: The default is the 3-node beam189 element; removing the middle node results in the 2-node beam188 element. 2. How to remove the interior nodes of a element to convert a higher-order element into a lower-order one? In Mechanical, click on “Mesh”. In the Details of Mesh information panel, there is a function called ElementMidside Nodes (as shown in the figure below). Selecting Program Controlled sets it as the default element type; Keeping retains the intermediate nodes, while Dropping removes them, transforming higher-order elements with intermediate nodes into lower-order elements without such nodes (for example, the Solid186 element becomes the Solid185 element). 3. How to view the unit type? Method 1: Under “Setup” in A, create a “FiniteElement Modeler” via “Transfer Data To New”. Double-click on “Model” in B, and a “Import Summary” data table will appear; “TABLE 3” is shown in the figure below, from which it can be seen that the Solid186 element is selected by default by the system. Method 2: During the post-processing stage, click on “Solution Information”; the Worksheet displayed on the right side of the window shows the solution information and process for the entire model, including detailed information about the elements assigned to each body. 4. What are first-order, second-order, fully integrated, and reduced integral elements? (1) Linear element: Also known as a first-order element, it features nodes located only at the corners of the element, with linear interpolation used in all directions. (2) Quadratic element: Also known as a second-order element, it has nodes not only at the corners but also intermediate nodes along each edge, with quadratic interpolation used in all directions. (3) Complete integration: This refers to the situation where, when the element has a regular shape, the number of Gaussian integration points used is sufficient to accurately integrate the polynomials in the element stiffness matrix. For hexahedral and quadrilateral elements, a \"regular shape\" refers to the situation where the edges of the element intersect at right angles, and any node is located at the midpoint of an edge. (4) Reduced integration: A reduced integration element refers to one fewer integration point in each direction compared to a full integration. 5. Degrees of freedom of the unit? In the element library provided by Ansys, all stress/displacement solid elements and truss elements have only translational degrees of freedom along the x, y, and z axes, with no rotational degrees of freedom ； Beam elements, shell elements, and rigid body elements possess both translational degrees of freedom along the x-y-z directions and rotational degrees of freedom about the x-y-z directions. 6. How to select a unit? For finite element numerical simulations using ANSYS, element types with intermediate nodes should be preferred. For stress analysis, fatigue analysis, etc., the 3D solid Solid186 high-order elements are preferred (with the corresponding temperature elements being Solid90); when the number of computational elements is large, the Solid185 low-order elements can also be used (with the corresponding temperature elements being Solid70) ； For buckling analysis, ultimate load analysis, modal analysis, etc., the Shell181 shell element is preferred ； For two-dimensional planar structures, the Plane82 element is preferred ； For beam structures, the Beam189 beam element is preferred ； When performing contact analysis, the Conta173 contact element and the Targe170 target element should be preferred ； Inter195 gasket units should be preferred for gaskets ； For quality units, Mass21 is preferred ； The selection of the remaining units can be found in the ANSYS help file. Depending on the structural characteristics, different units can also be selected for combination. For other finite element simulation software, the element types should be selected in accordance with the principles mentioned above. 7. What is the Solid185 enhanced strain element? Those who have studied Ansys’ classic versions know that in many cases the Solid185 reinforced strain element can be used; especially for large models with a large number of grid nodes, employing the Solid185 reinforced strain element allows for calculation results with the same accuracy as those obtained using the Solid186 element, while simultaneously reducing the required computing memory and improving computational efficiency. In my understanding, the enhanced strain element is used to overcome the shear locking problem of first-order fully integrated elements, which prevents the elements’ edges from bending and deforming. Enhanced strain involves introducing additional degrees of freedom for the deformation gradient of the reinforcement elements into the first-order elements, so that the deformation of these elements occurs in a linearly graded manner. Therefore, using first-order elements with enhanced strain can yield results comparable to those of second-order elements, while significantly reducing the computation time. However, it is highly sensitive to grid distortion; in the case of complex models with severe grid distortion, the results obtained using first-order elements that enhance strain are not accurate. 8. How is the Solid185 enhanced strain element defined in AWB? Currently, it is not possible to directly select enhanced strain elements in AWB; the Solid185 enhanced strain elements can only be defined by inserting command streams. Right-click on the entity “Solid” and select “Insert Commands (APDL)” to insert the following command sequence: *DO,I,1,12 ET,I,Solid185 ! Defined the Solid185 element *ENDDO *DO,J,1,12 KEYOPT,J,2,2 ! How are fully integrated and reduced integration elements selected in the enhanced strain element *ENDDO 9.AWB? In AWB, just like in the classic version, it is possible to choose between full integration and reduced integration elements: click on “Geometry”, and under “Details of Geometry” there is a section titled “Element Control”. By default, WB uses “Program Control”; changing this to “Manual” will do. Then, click on the solid entity under “Part”. In the “Definition” section of “Details of Solid”, an additional field named “Brick Integration Scheme” will appear, allowing you to select either “Full or Reduced” (i.e., full integration elements or reduced integration elements). 10. What is the impact of unit selection on analysis results? The essence of finite element analysis is to transform problems with infinite degrees of freedom into those with finite degrees of freedom, and to convert continuum models into discrete models composed of a finite number of elements. When selecting unit types during the analysis process, one often faces many choices. There are significant differences in the number of nodes, cell shape, order of interpolation functions, and cell construction methods for various cell types; each type of cell has its specific area of application, and it is necessary to choose the appropriate one based on the type of analysis and the specific problem at hand. If the unit type is selected incorrectly or inappropriately, even if calculation results can be obtained in the end, these results may have large errors or even be incorrect. For a detailed introduction to first-order or second-order fully integrated elements and reduced integration elements, please refer to the article titled “Discussion on the Concepts, Differences, and Application Scenarios of First-Order, Second-Order Fully Integrated, and Reduced Integration Elements in Ansys” on the WeChat official account “Ansys Analysis and Design Professionals” No further explanation is needed here. The above introduction to elements and the selection of element types helps people understand and apply them by combining element selection with software operations. By understanding the different concepts and types of elements, as well as how to define element types and integration methods, analysts gain greater flexibility. This enables them to choose appropriate element types and integration methods based on specific models and analysis types, thereby improving calculation efficiency while maintaining accuracy, and avoiding the need to rely passively on the default element types and integration methods provided by AWB. The above are some of the author’s personal opinions; there may be inaccuracies, so everyone is welcome to discuss them!