ANSYS 10 Questions and Answers Series: Meshing Techniques

Thread Content

This post was last edited by Freestyle-sky on 2018-4-1 at 18:09. Meshing is an important step in the pre-processing phase of ANSYS analysis and design; it serves, firstly, as a test of the analyst’s ability to work with models； Secondly, the quality of the grid directly determines the computation time and accuracy of the model, as well as whether the problem can be solved. Therefore, for analysis and design engineers, mastering the skills of mesh generation and improving their ability to handle models is crucial for enhancing both computational efficiency and accuracy. AWB currently integrates various professional mesh generation tools such as ICEM CFD, Tgrid, and GAMBIT, giving it strong capabilities in this area; however, the effectiveness of these functions ultimately depends on the operator’s understanding of the models and their ability to make flexible use of the tools available in the software. This article mainly introduces some useful grid division tips for using AWB in analysis and design within this industry, in the hope of providing a little help to everyone. 1. What is the meaning of the grid division tool in AWB? 【Automatic】: The program divides the grid automatically; the grids generated in this way are usually tetrahedral in structure. It does not refine the grid in the areas that are important for the analysis and design, and it represents a simple, straightforward method of grid division. It is not recommended to use this approach ； 【Tetrahedrons】: It employs a tetrahedral meshing approach; however, tetrahedral meshes are generally not used in the analysis and design of pressure vessels, and this method is also not suitable for such applications ； 【Hex Domiant】: It primarily uses a hexahedral mesh, but for shapes that are complex or at areas where there are structural transitions, pyramid-shaped and tetrahedral meshes, which are easier to use for meshing, are employed. Since pressure vessel analysis and design require pure hexahedral meshes, this method is generally not recommended. However, it can be used for models where it is difficult to create hexahedral meshes or for areas that are not critical from a stress perspective; as long as the calculation accuracy at the stress-critical points can be ensured, it is not impossible to use this method ； 【Sweep】: This is the sweeping-based meshing method, which is the most commonly used approach. For solids that can be swept, a full hexahedral mesh can be generated by sweeping from the source surface along a specified path to the target surface. However, this is possible only if all solids are sweepable. After meshing the model, you can right-click on “Show Sweepable Bodies” to check whether all solids are indeed sweepable. As shown in the figure below, the green areas represent solids that are sweepable, while the gray areas represent those that are not ； The 【Sweep】 method is the best approach for flexibly dividing a full hexahedral mesh through manual control; mastering this method is sufficient to create very nice and regular hexahedral meshes. 【Multizone】: This is a multi-region mesh division method that does not require us to divide the entities manually, as the division is carried out automatically internally. It can determine which elements can be swept to form hexahedral meshes, while for elements that do not meet the requirements, better division methods such as tetrahedra are used. Therefore, this method can also be employed to generate full hexahedral meshes for relatively simple models that are easy to convert into sweepable forms. However, for complex models, non-hexahedral meshes are produced, resulting in a lack of flexibility and manual control. 2. How can complex models be divided entirely into sweepable bodies? (1) First and foremost, designers need to clearly understand what kind of geometry constitutes a sweepable body. Based on this understanding, it is possible to analyze and break down a complex model, so as to determine which components require being divided into separate entities – this is the foundation and prerequisite ； (2) Make flexible use of the “Slice” function. For some 3D models with complex geometric shapes, it is necessary to first gain a clear understanding of the model and analyze it to determine where to divide the solid so that it can be broken down into solids that can be swept. Subsequently, methods such as “Slice by surface” and “Slice by plane” can be used to divide the solids appropriately. The process of dividing solids for sweeping still relies on the analyst’s understanding of swept solids and their ability to analyze the model ； For example, in the lock hopper model shown in the figure below, the ear seat area is the most difficult part to divide. In particular, the junctions between the bottom plate and the backing plate, between the backing plate and the housing, and between the rib plates and the backing plate present challenges. Therefore, it is necessary to make use of the “Slice” function to divide these areas appropriately, turning the solid into sweepable entities so that a full hexahedral mesh can be created. The lock hopper model in the figure below was divided into 863 such sweepable entities using the “Slice” function. 3. In what situations is it necessary to use splitting tools such as “Slice” when dividing a grid? (1) For some three-dimensional models with complex geometric shapes, the key to the segmentation process is to perform segmentation at all locations where the cross-section changes ； (2) For areas with complex stress gradients where finer grids are required, the slice function can be used to divide a small area, and the grid size can be set within this area ； (3) If different areas of a component have distinct material properties, it is necessary to divide the component at those points where the materials change, and assign different material attributes to each area ； (4) If different parts of an edge or a face have distinct loads or boundary conditions, it is necessary to perform a segmentation at the points where the loads or boundary conditions change, and then define different loads and boundary conditions for each part ； 4. Is it necessary to perform the “Form new part” operation after dividing the entities? For beginners, it’s easy to overlook this node-sharing operation when there is no one to guide them. The author also missed this point when first learning*; without the “Form new part” option, it seemed quite simple to divide the mesh, and the resulting meshes were beautiful and regular. It seemed so easy, but that was a huge mistake. Without performing the “Form new part” operation, each entity existed as an individual unit, and the meshing was done for those individual entities alone, with no node sharing between adjacent entities. Once “Form new part” is performed, it means that the junctions between adjacent entities need to have identical mesh nodes. Achieving node sharing between two entities of different shapes and sizes is not easy. Therefore, after meshing the entities, be sure to perform the “Form new part” operation on all of them to enable node sharing. Only through node sharing can calculation values such as displacement and force be transmitted and resolved. As mentioned above, the lockbox model consists of 493 entities in total, and these 493 entities need to undergo the “Form new part” operation to enable node sharing. 5. Grid settings and division order? (1) \"Start with the larger ones first\": The grid division sequence is to first apply grid settings and division to larger entities, and then to the smaller entities that share nodes with them. After the larger model has been divided into a neat and regular hexahedral grid, it becomes easier to divide the smaller model that is meant to match it into a grid ； (2) “Start with the difficult ones first, then move on to the easier ones”; grid division order: First, create reasonable grids for models that are difficult to divide, while it is easier to form grids for simpler models, thereby enabling node sharing ； (3) “Complex first, then rules”: The grid division sequence is to first divide complex models into grids with reasonable structures; it is easier to divide the grids of simpler models, thereby enabling node sharing ； 6. Use “Sweep+Sizing” flexibly to divide grids? Once a complex 3D model is divided into all the entities that can be swept, the “Sweep” method can be used to generate hexahedral meshes. The “Sizing” function is also utilized to control the mesh size for bodies, faces, and edges, thereby allowing for proper regulation of the mesh density and quality. This results in well-structured and high-quality meshes, and it’s also possible to refine the mesh in specific areas. However, the most common practice is to apply “Sizing” to edges – settings such as “Element Size” and “Number of Divisions” can be used to set a fixed size for the edges or to divide them into equal segments. As shown in the figure below, the edges of the tube sheets and heat exchange tubes were divided into equal segments, which facilitates the creation of refined and high-quality meshes ； There is also a very useful feature called “Bias Type”, which enables the gradient division of the grid. As shown in the diagram of the tube sheet cylinder section, the grid spacing is smaller near the chamfered area of the tube sheet, and it increases thereafter. This feature allows for different grid densities and quality requirements to be applied in various areas: the grids in areas where stress is a concern are made finer, while those in areas where stress is not a concern are made sparser. This helps to reduce the number of grids, thereby improving computational efficiency while maintaining accuracy. 7. What are the metrics for measuring grid quality? The quality of a mesh can generally be evaluated using parameters such as element mass and mesh distortion (ranging from 0 to 1). When the average element mass is above 0.6, the mesh quality is considered satisfactory; as for distortion, the higher the distortion factor, the worse the mesh quality. The quality of the grid can be fully determined based on these two indicators, with other indicators serving as supplementary references. 8. What are the methods to assess grid quality and convergence? (1) The most common approach is to perform the solution verification by refining the grid. If the calculation results after refining the grid are similar to those obtained without refinement, it can be assumed that the results are reliable at the current grid density and quality. If there is a significant difference between the results after refinement and those before refinement, it indicates that the results are inaccurate at the current grid density; in such cases, the grid density needs to be further refined to obtain more accurate solutions ； (2) The AWB includes a convergence function that compares the results obtained by progressively refining the grid by defining its tolerance and the number of iteration cycles, in order to determine whether convergence has been achieved and to obtain the final calculated value. However, the convergence function relies on the refine function to refine the grid, resulting in a tetrahedral grid; thus, all calculation results are based on a tetrahedral grid structure. This method is not suitable for models that require a fully hexahedral grid. 9. How to reasonably control grid density to improve computational accuracy and reduce computation time? Principle: Refine the grid division in certain areas of particular interest (such as stress concentration zones, regions with changing stress gradients, areas with high plastic strain, or contact surfaces) to improve computational accuracy, while using coarser grids in areas that do not require much attention or are less important, thereby reducing the model size and shortening computation time. In practical engineering applications, it is often possible to predict which areas have higher stress levels; thus, during modeling, the grid can be refined selectively in these key areas ； If it is not possible to determine in advance where the maximum stress will occur, a coarser mesh can be used for the entire model to carry out preliminary calculations and obtain an approximate distribution of stresses. Once the areas with high stress levels are identified, the mesh can be refined in those areas, after which the entire model can be analyzed again, or sub-modeling techniques can be employed to analyze only the regions of interest. For more interesting content, please search for and follow the WeChat official account \"ANSYS Analysis and Design Professionals\" – a platform dedicated to sharing insights on analysis and design with everyone.