Essential experience for learning Fluent – every question is a classic example; you can take a look at the questions related to Fluent first (collect and share them)

6. Residual – it is the sum of the fluxes through each Face of the cell; once convergence is achieved, theoretically, when there are no source phases within the cell, the sum of the fluxes entering each face, which represents the total transport of the physical quantity, should be 0. The maximum residual, or RSM residual, reflects the difference between the flow field and the flow field that is intended to be simulated (i.e., the flow field that should be obtained after convergence; of course, there is still a certain discrepancy between the flow field obtained after convergence and the actual flow field). The smaller the residual, the better. Due to numerical precision issues, it is not possible to achieve a residual of 0. For single-precision calculations, it is generally desirable for the residual to be below 1e-03 of the initial residual, though this depends on the specific situation. Generally, in Fluent, it is possible to add monitoring for inlet and outlet flow rates (by printing or plotting them). After the residuals converge to a certain level, it is necessary to check whether the inlet and outlet flow rates have reached a stable equilibrium in order to determine whether convergence has occurred. The residuals fluctuate at higher levels; it is necessary to check whether the boundary conditions are reasonable. Next, it is important to verify whether the initial conditions are appropriate – in flow fields with shock waves, inappropriate initial conditions can lead to fluctuations in the flow field. Sometimes the flow field may experience separation or backflow, which is itself a unsteady phenomenon; during computation the residuals will fluctuate to some extent. In such cases, if the inlet and outlet flow rates reach a stable equilibrium, it can also be considered that the flow field has converged (provided that other unreasonable factors are eliminated). Additionally, Fluent uses a multigrid approach for defects; by setting the multigrid to zero at the later stages of computation, it is possible to prevent residuals of certain wavelengths from oscillating on the fine grids. 7. The model is quite complex; it was created in Pro/E and then imported into Gambit using IGES. However, this results in many fragmented lines and surfaces, as well as sharp corners at the junctions of some surfaces. I have successfully merged them all into a single virtual surface, with a parameter that allows for sharp corners; I can also divide the mesh up, but when the resulting MSH file is imported into Fluent, an error occurs. Is this due to the virtual geometry or to the sharp corners? Also, what is the difference between virtual geometry and ordinary real geometric objects? It seems that the biggest difference is that virtual geometry does not support boolean operations. What exactly are boolean operations? What issues should be considered when using virtual geometry? Virtual geometry is a very troublesome issue. You merge them all into a single virtual surface; logically, since everything is virtual, it can be considered as such. It might be due to the sharp corners that the biggest difference between virtual and real geometry exists: virtual geometry cannot be used for Boolean operations, which are necessary for generating meshes with complex shapes. In such cases, virtual geometry, virtual faces, and virtual edges are inevitably required. 1) When creating a mesh, it’s not a good idea to combine all the faces into one virtual face, especially when dealing with meshes of complex shapes. It’s better to divide the model into more faces in areas where there are significant changes in shape; this allows for more effective control over the mesh, enabling it to form structured or unstructured grids in areas with high curvature on the model surface. 2) Regarding the issue of many fragments being generated when you enter gambit, you can appropriately reduce the model precision and tolerances in ProE, as the modeling tools in gambit themselves do not have high precision. 3) Boolean operations refer to operations such as combining faces with faces, volumes with volumes, and performing subtractions. This is a common problem in all CAD modeling processes. 4) For the computational grids used in generating virtual bodies, there is no difference in computation compared to those used for generating solid bodies; what matters is the quality of grid generation, which has nothing to do with whether the body is solid or virtual. When performing calculations on complex models, I mostly use virtual solids; especially for complex models imported from other modeling software, it’s basically not possible to create solid models. As for the quality of the calculations, it depends on your settings in Fluent and the quality of the mesh; it has nothing to do with the model itself. You can use Gambit’s check function to examine the quality of your mesh and see how good it is. There is a difference between solid and hollow elements. In modeling, solid… and hollow… elements are often encountered, and it seems that the calculation domain of hollow elements can also be used to obtain the desired results. As for the fundamental differences between them and their functional differences, there is no impact on solving problems, as long as you can create the necessary mesh on either solid or hollow elements. When it comes to mesh generation and calculations, solid and hollow elements have no effect on the results. The main differences between solid and hollow elements are as follows: 1) Solid elements can undergo Boolean operations, while hollow elements cannot. Although they cannot be used for Boolean operations, hollow elements do have functions such as merge and split. 2) Solid operations are available in many CAD software, but virtual solids are a major feature of Gambit; with virtual solids, Gambit gains much greater flexibility in modeling and mesh generation. 3) During the mesh generation process, if there are several faces with relatively high curvature, you can merge them into one. This helps to reduce the number of steps required for mesh generation. For faces with high curvature, the quality of the generated mesh may be poor; in such cases, you can split those faces into smaller ones to improve the mesh quality. 8. Question 1: When creating a mesh for a model, the message “Initialization failed: perturb boundary nodes and try again” appears, but the process of mesh creation continues anyway. I think there must be a problem. But I don’t know where the problem lies? I earnestly ask the experts for their guidance! Question 2: Since spacing has already been defined in the image grid, will defining it again when creating the 3D model grid cause any conflicts? Also, what is a reasonable definition? First question: When creating grids, all the error messages indicate that some of the grids either fail to be generated or are of poor quality; it’s necessary to recheck the geometry and grid type. Second question: If grids can be generated, redefining them isn’t a problem, but there might be conflicts arising from inconsistencies in the spacing between the faces of the grid and the spacing within the volume grid. In such cases, Gambit will handle it automatically, but the quality of the resulting grid may still not be good. 9. When using Gambit to generate volume grids, an error occurred: “Initialization failed to mesh 23 nodes. ERROR: TG_mesh_domain failed with error code 1. ERROR: Tegrahedral meshing has failed for volume v_volume.1. This is usually caused by problems in the face meshes. Check the skewnesses of your face meshes and ensure that the face mesh size isn’t too large in areas with small gaps.” I understand this is due to too many narrow faces in the model, but even after modifying many of these narrow faces, the problem persists. I created a grid for each face to see what the quality would be like; it seemed there shouldn’t be any issues. Yet, when trying to generate the volume grid, the same problem arose. I’m not sure what to do. Solutions: 1) Reduce the size of the volume grid. When there are multiple volumes, the transition from a smaller grid size to a larger one should be gradual, without large differences. 2) Merge small faces (combine small faces together or merge them into larger faces), turning them into virtual volumes. I think merging small faces is an effective method, as it can improve the quality of the grid. The key issue is when the angle between two small faces is very large; after merging, a corner-like surface is created, which worsens the quality of the grid. What the person mentioned about merging into virtual faces likely refers to situations where the angle between the two faces isn’t too large. I also tried reducing the grid size, but doing so resulted in too many grids, and the computer couldn’t handle the computation. In such cases, it might be better to separate those two faces with a large angle into a single volume, give that volume a very small size, and try again. If that doesn’t work, just ignore that volume. The quality of grids generated by Gambit is often a problem; with ICEM, negative volumes hardly ever occur. This is probably related to Gambit’s algorithm. For areas with high curvature, the only option is to increase the grid density in those areas. 10. Initialization 1) In FLUENT’s initialization panel, there is an option for specifying where the calculation should start (compute from). Is it significant to choose to start the calculation from different boundaries? How should one decide where to start the calculation based on the specific problem at hand? For example, if there are two velocity inlets, A and B, as well as a pressure outlet, should one choose the velocity inlets or the pressure outlet? If velocity inlets are chosen, and there are two of them, which one should be selected? Are there any principles or guidelines to follow? Generally, ALL ZONE is selected, which means an average treatment of all areas; alternatively, a representative inlet can also be chosen for initialization (when there are multiple inlets). For general flow problems, the choice of initial values is not important, as the calculations converge easily. However, when the geometric conditions are complex and the flow velocity is high with rapid changes (such as sonic flow), the initial conditions must be carefully selected. If convergence does not occur, different initial conditions should also be tried, and even the boundary conditions may need to be changed step by step until the desired conditions are achieved. 2) To determine whether one’s simulated results are correct, it seems that the convergence of the solution is more important than the initial and boundary conditions – is that correct? In other words, for a specific problem, the values of the initial conditions and boundary conditions are not unique; in order to make the solution converge, it is necessary to keep adjusting these conditions until the solution does converge, right? If the solution converges, can we basically be sure that the result of the simulation is correct? For a specific problem, the setting of boundary conditions is certainly unique; however, different initial conditions can be chosen at the time of initialization (by specifying a constant flow). To ensure better convergence of the solution, I generally adjust the boundary conditions gradually toward their nominal values. By “nominal values” I mean the inlet or outlet conditions specified in the problem – for example, when calculating flow within a pipe, if the required inlet pressure and temperature are 10 MPa and 3000 K, then at the start of the iterations I choose an inlet pressure and temperature of 1 MPa and 500 K (this is just an assumption; it depends on the specifics of your problem). Once the flow field calculation has progressed to a certain extent and convergence has improved, I then gradually increase the pressure and temperature. After several such adjustments, the values finally reach the nominal levels of 10 MPa and 3000 K. This approach leads to better convergence compared to setting those values from the beginning. In this way, each iteration can converge more easily; after each adjustment, there is no need for re-initialization, as the previous solution is automatically used as the initial condition for the next iteration, allowing the process to continue. Even if the solution converges, this does not mean that the results of the simulation can be considered correct with certainty; it is still necessary to compare them with experimental results and theoretical analyses.

11. Where does shadow come from? How should its boundary layer be set? You define two computational domains with different properties (for example, regions A and B), and the two regions share a common interface. The faces of domain A retain their previous names, while the faces of domain B take the name of that shadow. By defining this surface as interior in the boundary conditions, these two regions can be combined into a connected computational domain. Is the shadow generated automatically or does it need to be defined manually? The automatically generated ******shadow surface appears in two situations: 1. When both sides of a wall are fluid domains, one side of the wall is defined as wall.1, while the other side is automatically defined by the software as wall.1_shadow. Its properties are the same as those of the regular wall, and there is no difference in how it should be handled compared to a regular wall surface; 2. Another situation occurs when you remove the periodicity from a periodic surface in Fluent software – in this case, a shadow surface is also created. This situation is easy to understand, as the shadow surface and the original surface together form two periodic surfaces. A shadow surface also appears when one side of a wall is fluid and the other side is solid. At this point, fluid-solid coupling calculations can be performed. 12. Static temperature and total temperature: Total temperature refers to the stagnation temperature, the temperature when the velocity is completely zero. Static temperature is the local thermodynamic temperature. There are formulas for calculating these two values; they are similar to total pressure and static pressure, but there are also differences... For example, total temperature can be regarded as a measure of the fluid’s energy, whereas total pressure cannot... In an adiabatic flow, the total temperature remains constant along the flow path, while total pressure decreases (in a non-isentropic process)... Velocity represents the macroscopic motion of the fluid. According to the law of conservation of energy, the sum of mechanical energy and thermal energy remains constant. When all mechanical energy is converted into thermal energy – more precisely, when all kinetic energy is converted – the temperature at that point is the stagnation temperature, which is also the total temperature. Such a point may exist in an actual flow field, such as at a stagnation point, or it may not; it is simply a parameter used to describe the total energy of the fluid. Static temperature is the temperature in the ordinary sense – it’s the temperature that can be measured at a particular point. For example, in the case of a fire, the actual temperature, say 1000 degrees, is the static temperature.:) Static temperature is used to distinguish it from total temperature. 13. How to determine whether the calculation results have converged! 1) Check that the values at the relevant point no longer change as more calculation steps are taken ； 2) The residuals of each parameter decrease as the number of calculation steps increases, eventually leveling off ； 3) Mass conservation must be satisfied (energy is not involved in the calculations), or both mass and energy conservation must be satisfied (energy is involved in the calculations). It should be particularly noted that even if the first two criteria are satisfied, it does not mean that a reasonably convergent solution has been obtained; this is because if the relaxation factor is set too tightly, the changes in various parameters in each calculation step will not be significant, and thus the first two criteria can still be met. At this point, we need to look at the third criterion again. It should also be noted that generally we hope that, in the case of convergence, the residuals are as small as possible. However, the residual curve is the result of averaging over the entire domain, and its magnitude does not necessarily indicate the quality of the calculation results. Sometimes, even if the calculated residuals are large, the results might still be good; what matters is whether the calculation results are consistent with physical facts. In other words, the magnitude of the residuals is related to the complexity of the physical phenomena being simulated, and it is necessary to evaluate the calculation results based on the actual physical conditions. For example, in a full-machine model that was recently analyzed, the solution experiences severe oscillations at high angles of attack, and the magnitude of the residuals doesn’t decrease over time. Yet the result remains correct; why? Because this is indeed how the actual flow behaves at high angles of attack – there is continuous periodic shedding of vortices, and the flow field itself is unsteady, so the solution is also fluctuating. Taking an average value when processing such data suffices.

14. What are structured grids and unstructured grids? 14.1 Structured grids: Strictly speaking, a structured grid refers to a grid domain in which all interior points have identical neighboring elements. It can easily perform boundary fitting for regions, and is suitable for calculations related to fluid and surface stress concentrations. Its main advantage is: fast grid generation speed. The quality of grid generation is good. The data structure is simple. The fitting of surfaces or spaces is mostly achieved using parametric or spline interpolation methods, resulting in smooth regions that are more closely aligned with the actual model. Its most typical drawback is its limited scope of application, as it is only suitable for figures with regular shapes. Especially with the rapid development of computers and numerical methods in recent years, there are increasing demands for handling the complexity of the geometric shape of the solution domain, and under such circumstances, structured mesh generation techniques prove to be insufficient. 14.2 Unstructured grids: As opposed to structured grids, unstructured grids refer to grid regions in which the internal points do not have identical neighboring elements. That is, the number of grids connected to different interior points within the meshed region varies. By definition, structured grids and unstructured grids have overlapping parts; that is, an unstructured grid may contain portions of a structured grid. 15. If a geometric shape contains both structured grids and unstructured grids, and it has been divided into sections, the grids generated for each section can be directly imported into Fluent for calculation. 16. In Fluent, for the same geometric shape, it is possible to generate both structured and unstructured grids; of course, generating a structured grid is much more complex than generating an unstructured one. Which type of grid should be chosen? Are the calculation results of the two types identical, or does one yield better results? Generally, the computational results of structured grids converge more easily and are more accurate than those of unstructured grids. But the latter is easy to do. The accuracy is primarily affected by the quality of the grid; it doesn’t really matter much what type of grid is used. If the quality of the grid is poor, the results will also be unreliable. Relatively speaking, structured grids are more conducive to computer storage of data and to faster computation speeds. Structured grids are said to be faster for computations, but grid generation requires skill and patience. Unstructured grids are easy to generate, but they are relatively slower. 17. In Gambit, only map and submap generate structured grids; all others are unstructured grids. 18. We often encounter situations where the calculation domain is symmetric, such as natural convection within concentric rings or flow around cylinders. To save computational resources, we often divide the calculation domain in half. However, in some cases, the actual flow field and distribution of physical quantities across the two halves are not symmetric. How can we determine whether to use such a divided domain? Symmetric problems are generally applied to steady-state flow fields; for this to hold, three conditions must be met: 1. The geometric shape must be symmetric; 2. The boundary conditions must be symmetric, that is, the physical conditions must also be symmetric; 3. The structural grid must be symmetric. Therefore, the flux and property gradients along the axis of symmetry must be zero. 19. After studying various examples for some time, it’s possible to determine whether the analysis for simple problems is correct or not. But for those problems for which one doesn’t have a clear conceptual understanding, even after creating many graphs and vector diagrams, it can be difficult to conduct a thorough and comprehensive analysis of their validity. Answer: Generally speaking, calculations should be supported by high-precision experiments as proof. When experiments are not possible or difficult to carry out, it’s common to use calculations of classic examples or those already solved by others for comparison. Since many graphs have already been created, one can try to analyze them to see if they are consistent with classical theories. The diagram has been created, but if we really want to convey the message, there is likely still a long way to go. 20. The Courant number actually refers to the relative relationship between the time step and the spatial step; the system automatically reduces the Courant number. This situation usually occurs in computational domains with sharp shapes, and errors arise when the local flow velocity or pressure difference is too high. Try increasing the grid resolution in those areas. In Fluent, the Courant number is used to regulate the stability and convergence of calculations. Generally, as the Courant number increases from small to large, the convergence rate gradually speeds up, but the stability gradually decreases. So, for specific problems, during the calculation process, it is best to start with a low value for the Courant number, and observe how the iterative residuals converge. If the convergence rate is slow but stable, the Courant number can be increased appropriately. By considering the specifics of one’s problem, a suitable value for the Courant number can be found that allows for a fast enough convergence rate while still maintaining stability. 21. Explanation of the relaxation factor in FLUENT: Since fluid mechanics involves solving nonlinear equations, it is necessary to adjust the control variables during the solution process, and this is achieved through the relaxation factor. It controls the amount by which the variables change in each iteration. In other words, the new value of a variable is the original value plus the change amount multiplied by the relaxation factor. For example: A1 = A0 + B * DELTA, where A1 is the new value, A0 is the original value, B is the relaxation factor, and DELTA is the change amount. The relaxation factor can control the speed of convergence and improve its quality! A value of 1 means no use of a relaxation factor; values greater than 1 represent an over-relaxation factor, which speeds up convergence, while values less than 1 represent an under-relaxation factor, which improves the conditions for convergence. Generally, a smaller under-relaxation factor is used when convergence is not satisfactory. In Fluent, under-relaxation is used, primarily to prevent divergence caused by large differences between values from two iterations. The value of the relaxation factor ranges from 0 to 1; the smaller it is, the smaller the change between two iterations, which means greater stability, but also slower convergence.

22. Experience in using Fluent to generate MPG files: The first step is to define an animation sequence under Solve\Animate; then, during the calculation, Fluent will keep track of the corresponding frames. After calculation, use Playback to review or generate an mpg file. Experience shows that when using that Playback to generate an mpg file at this time, success is achieved about once in ten attempts! The solution is to shut down Fluent, restart it, then use Playback to read that sequence and generate an MPG file; this approach has a higher success rate. When dividing the volume mesh into smaller parts in order to obtain a high-quality mesh, should one use tmerge to combine those parts back into a single volume mesh when importing it into Fluent? You can see this example in fluent 6.1.22 Using Sliding Meshes. Answer: No. When meshing different volumes in the same GAMBIT file, the final output mesh file contains all the meshes. Note: When using split to divide the domain, select the “connected” option; otherwise, FLUENT will default the interface to a wall. Mesh partitioning is similar as well. 24. When dividing the grid into blocks and defining boundaries, is it still necessary to define the junction surfaces? If not defined, are they assumed to be walls by default? To make them internal interfaces, should they be defined as interfaces? Answer: For the region created by splitting, if you do not define boundaries, Gambit will assume an interior boundary by default. 25. Sub-relaxation factor: 1) Under Relaxation: Under relaxation refers to appropriately reducing the difference between the results of the current level and those of the previous level, in order to prevent divergence in the nonlinear iterative process caused by excessive differences. When expressed using generic variables, they are known as Relaxation Factors. “Numerical Heat Transfer - 214” 2) Sub-relaxation in FLUENT: Due to the non-linearity of the equations solved by FLUENT, it is necessary to control the variation of . Control is generally achieved using the sub-relaxation method, which reduces the amount of change in each iteration. The simplest form of relaxation is: the variable within a unit equals its original value plus the product of the relaxation factor a and the change. The decomposition solver uses relaxation to control the updating of the computational variables in each iteration. This means that the equations solved using a separate solver, including the decoupled equations (turbulence and other scalars) solved by the coupled solver, will all have a corresponding sub-relaxation factor. In FLUENT, the default sub-relaxation factor for all variables is the optimal value for most problems. This value is suitable for many problems, but for some special nonlinear problems (such as certain turbulence or natural convection problems with high Rayleigh numbers), care should be taken when reducing the sub-relaxation factor at the start of the computation. It is a good practice to start the calculations using the default sub-relaxation factor. If the residuals continue to increase after 4 to 5 iterations, you need to reduce the sub-relaxation factor. Sometimes, if you notice that the residuals start to increase, you can change the sub-relaxation factor and recalculate. This usually occurs when the sub-relaxation factor is too high. The safest approach is to save the data file before making any changes to the sub-relaxation factor, and to run a few iterations of the solution algorithm in order to adjust to the new parameters. In the most typical case, an increase in the sub-relaxation factor leads to a slight increase in the residuals, but this increase in residuals disappears as the solution process progresses. If the residual variation spans several orders of magnitude, you need to consider stopping the calculations and returning to the last saved, better-quality data file. Note: The sub-relaxation of viscosity and density occurs between each iteration. Furthermore, if the enthalpy equation is solved directly rather than the temperature equation (that is, for PDF calculation), the temperature update based on enthalpy requires sub-relaxation. To view the value of the default sub-relaxation factor, you can click the Default button in the solution control panel. For most flows, there is no need to modify the default sub-relaxation factor. However, if instability or divergence occurs, you need to reduce the default sub-relaxation factors; the default values for the sub-relaxation factors of pressure, momentum, k, and e are 0.2, 0.5, 0.5, and 0.5 respectively. For the SIMPLEC format, a sub-relaxation factor to reduce pressure is generally not required. In problems where density and temperature are strongly coupled, such as natural or mixed convection flows with relatively high Rayleigh numbers, sub-relaxation of temperature and/or density should be applied (using a sub-relaxation factor less than 1.0). Conversely, when the temperature and momentum equations are uncoupled or have weak coupling, the flow density is constant, and the sub-relaxation factor for temperature can be set to 1.0. For other scalar equations, such as vortices, components, and PDF variables, the default sub-relaxation for certain problems may be too large, especially for initial calculations. You can set the relaxation factor to 0.8 to make convergence easier. 26. Comparison between SIMPLE and SIMPLEC: In FLUENT, the standard SIMPLE algorithm and the SIMPLEC (SIMPLE-Consistent) algorithm can be used. The default algorithm is SIMPLE, but for many problems, SIMPLEC may yield better results, especially when additional sub-relaxation iterations are employed. The details are described as follows. For relatively simple problems (such as laminar flow without model-activated terms), convergence is already limited by the pressure-velocity coupling, and you can usually obtain a convergent solution quickly using the SIMPLEC algorithm. In SIMPLEC, the pressure correction sub-relaxation factor is usually set to 1.0, which helps with convergence. However, in some cases, increasing the pressure correction relaxation factor to 1.0 may lead to instability. For all calculations of transitional flow, the PISO algorithm with neighbor correction is highly recommended. It allows you to use large time steps, and a sub-relaxation factor of 1.0 can be used for both momentum and pressure. For steady-state problems, PISO with neighboring correction is not better than SIMPLE or SIMPLEC with a better under-relaxation factor. PISO tilt correction is recommended for steady-state and transition calculations on grids with significant distortion. When using PISO neighbor correction, it is recommended to use a sub-relaxation factor of 1.0 or close to 1.0 for all equations. If you use PISO tilt correction only for highly distorted grids, set the sum of the momentum and pressure sub-relaxation factors to 1.0; for example, a pressure sub-relaxation factor of 0.3 and a momentum sub-relaxation factor of 0.7). If you use both correction methods of PISO simultaneously, it is recommended to refer to the method used in PISO’s neighboring correction

What a rare and wonderful thing indeed!:victory:

The original poster is thoughtful! Saved!

Some learning materials on Fluent can be downloaded from the Baisi Forum; it seems that there are relatively few such materials available on Haichuan. www.baisi.net