|INSIGHT: Tips for Preparing a Quality Mesh for Conjugate Heat Transfer Analysis
Preparing a mesh for conjugate heat transfer (CHT) analysis on complex geometries such as film cooled turbine vanes can be a daunting task. In this month's issue of The Flow, we sit down with ADS CFD Engineer Will Humber to discuss how best to grid up an unstructured mesh of high quality for conjugate analysis.
FLOW: Will, having spent the past two years working on meshing for CHT, what have been the toughest aspects of the process?
WILL: I think designers will consistently need to tackle four challenges:
- Manufacturing vs. CFD-ready CAD definition
- Determination of proper boundary conditions
- Method for distributing mesh elements
- Generating a point-to-point interface between fluid and solid
FLOW: Let's take each of these in sequence. Why can't manufacturing-ready CAD definitions be used directly for CHT analysis?
WILL: There are three primary problems encountered when tyring to use a manufacturing-ready CAD definition for CFD: hot vs. cold definitions, periodic boundaries and unrealistic features. A manufacturing definition will typically be defined at room temperature, which gives a smaller part than would be seen when running at operating conditions, especially for a part such as turbine inlet guide vane or first blade; this can lead to discrepancies such as changes in overall mass flow rate and tip clearance. Periodic boundaries are often not respected due to the use of shims to reduce vibration or other attachments between airfoils. Finally, CAD defintions sometimes contain idealized features that are unrealistic. For example, a fan-shaped cooling hole may be defined by planar surfaces that meet with a zero radius junction. These impossible to manufacture features both misrepresent the true manufactured geometry and can often times be difficult to mesh, especially when trying to create smooth prism layers around a sharp turn for capturing boundary layer effects. Furthermore, some manufacturing features such as casting holes, bolt holes and slots for shims should be filled in within the CAD before being brought in for meshing.
FLOW: Let's talk about boundary conditions?
WILL: Boundary conditions need to be simplified to some degree when creating the geometry and associated boundaries. If infinite computer resources were available, the entire aircraft engine or even aircraft might be simulated, but in reality the domain must be reduced to the point where the boundary conditions reasonably represent the real boundary conditions while minimizing computational cost. The primary challenge on the fluid side is how to best feed the cooling flow. On the solid side, the decision is between isothermal, adiabatic, specified heat flux, and specified heat transfer coefficient on the boundaries. The different boundary conditions can have quite a strong effect on the final solution. Ultimately, we don't think there's a right answer here, we think it will depend heavily on your application and operating conditions.
FLOW: And how do you tackle the issue of mesh element distribution?
WILL: There are three different approaches to generating the mesh that we can take depending on how much user interaction will be involved. The first is to control the mesh by using the local curvature from the incoming CAD geometry to control the element sizing. This, however, can lead to problems on features like shaped film holes where the features are small but the local curvature is very low. This ties back into the problem of unrealistic, zero-radius features. The second method is to manually specify the element size for each section of the geometry; this method generally runs into problems where the section will be assigned an average size that will be too coarse in some areas and too fine in others unless the user spends very large amounts of time breaking the boundaries into small pieces. We've found it most effective to employ a hybrid of the two, where a method based on curvature is used in a global sense while local limits are placed where the local curvature does not accurately represent the need for mesh density.
FLOW: Got it. What are your thoughts on generating a point-to-point interface between fluid and solid?
WILL: There are two different ways to generate a point-to-point interface. The first is to generate a surface mesh on the interface using a Delaunay or advancing-front method. Once the surface mesh is generated, the volume mesh is then grown from the surface mesh and since both the fluid and solid volume meshes are grown from the same surface mesh, the point-to-point match is guaranteed. This method can produce a very high quality mesh but is patch dependent, meaning that it is highly sensitive to small sliver-like faces in the incoming CAD. The result of this is that it is not very robust when dealing with large geometries with thousands of small features.
The second method is to start with the volume mesh using an octree approach. The octree meshing approach works by beginning with a background mesh and then subdividing that mesh until local sizing requirements are met. Once refinements finish, elements may be projected onto nearby geometry features if close enough in order to allow the mesh to follow the geometry. The fluid and solid elements are then separated using aflood fill technique. The advantages of this method are that it is the most robust and able to ignore small sliver-like faces in the CAD definition. However, because octree meshes always grow by factors of two, the resulting volume mesh does not transition well between element sizes so the resulting volume mesh is not as well suited to CFD.
Having worked on a number of complex geometries over the past two years, we've found again that a hybrid approach has worked best. We use the octree method first to generate a surface mesh and then use that surface mesh with a Delaunay or advancing-front method to generate a higher quality volume mesh.
FLOW: So what are your takeaways for CHT meshing?
WILL: The most important lesson is that the quality of the mesh and CFD simulation are extremely dependent on the quality of the CAD definition--both in terms of how well constructed the CAD comes in to the mesher (translation errors can often turn a good definition into a bad CAD definition) and how well suited the geometry is for a CFD simulation. Additionally, we've found that when robustness of mesh generation is the primary goal, the octree method of tetrahedral mesh generation is by far the most reliable and least sensitive to problems in the geometry.
FLOW: Thanks, Will.
WILL: You're welcome.
CASE STUDY: Three-Dimensional Film-Cooled Vane CFD Simulations and Preliminary Comparison to Experiments The High Impact Technologies (HIT) Research Turbine Vane at the U.S. Air Force Research Laboratory is a three-dimensional, fully film-cooled modern turbine inlet vane. In this paper, Captain Jamie Johnson and Paul King from the Air Force Institute of Technology conduct 3D simulations using local source terms to model the cooling holes and make preliminary comparisons to experimental data. Copyright 2011 American Institute of Aeronautics and Astronautics. Posted with permission. <more>
TECHTIPS: Leading and Trailing Edge Enhancement in Code Wand
Code Wand provides capabilities to help improve mesh quality around leading and trailing edges. These capabilities can be used to create or enhancement leading and trailing edges for axial or radial blades. <more>
Welcome to The Flow
Welcome to The Flow, a newsletter for monthly insights on turbomachinery CFD published by AeroDynamic Solutions, Inc.
Each month we'll spotlight a topic of interest, discuss a case study and/or provide useful pointers about how to get the most out of the ADS CFD system.
You are receiving this email because you or someone else you know thought you would be interested. To unsubscribe please click here. We value your privacy.