you are here:   / News & Insights / Engineering Advantage Blog / CFD Meshing in Tight Spots

CFD Meshing in Tight Spots

February 20, 2015 By: Hsin-Hua Tsuei

Generating a computational mesh is an integral part of any analysis, FEA and CFD alike.   A good mesh is essential to obtaining the highest level of accuracy and best results.  Meshing for CFD is almost always a challenge unless you are fortunate enough to be analyzing flow over an airfoil, or flow in a pipe.  One of the most intriguing features of fluids is their ability to seep into many tight spots in a system. For example, gaps between two solid parts, clearances, seals, etc. all present micro-scale flow passages in a CFD analysis. Unlike FEA meshing, these tight spots are often included in a CFD analysis, and therefore require additional meshing consideration in order to generate an appropriate mesh for resolving the flow physics in these regions.

Let’s look at an example of a typical flow in the gap between two surfaces, shown in Figure 1. This type of flow domain often represents flow gaps in an electric motor. The inner surface is usually rotating at a certain speed. There is an attached cavity representing an object like a stator pole face. If the cavity does not exist, the flow domain is simply the annulus region between two concentric cylinders.  It will be straightforward to generate a sweep mesh for the flow gap. However, the addition of the cavity on top makes the flow volume more interesting.  A symmetric annulus gap morphs into a non-sweepable 3D flow domain with a tight gap. Now, how do we mesh this for CFD analysis?

Figure 1

CFD mesh 1.png

The easiest approach is to use tetrahedron elements for the non-sweepable flow volume, simply because we know a tetrahedron mesh can handle a wide variety of complex geometry. In addition, the inner surface is rotating, which creates a shear flow in the gap, so we need to include prism layers on all surfaces to resolve the strong shear gradient. With appropriate mesh size specifications, about 10 elements are placed across the gap, and we arrive at the mesh shown in Figure 2. The combined tet and prism mesh has a total of about 1.26 million elements. Figure 3 shows a close-up view of the mesh in the gap and cavity regions. The quantity of elements is sufficient to resolve flow physics associated with this configuration.  However, upon close examination of the mesh in Figure 2, it’s clear that there are excessive elements in the axial direction, simply because of the nature of tetrahedron elements. Well-shaped tets are isotropic, not easily stretched in one or more directions to reduce element count. This raises the question: is there another meshing method available for this type of situation?

Figure 2 - Tet & Prism Mesh

CFD mesh 2.png

Figure 3: Close-up View of Mesh in Gap and Cavity

CFD mesh 3.png

Let’s explore another way to mesh this part.  Take a look at the flow domain for this CFD analysis again. We know it is not sweepable. However, if we can simply divide the domain into three flow volumes, as shown in Figure 4, then each volume becomes sweepable. This gives the flexibility to use a sweep mesh for each flow volume, which makes it much easier to assign the appropriate mesh element size in the gap as well as in the axial direction.  Better yet, with the sweep mesh, we can use hexahedron elements for all three flow volumes. The resultant mesh is shown in Figures 5 and 6. We can clearly see the gap and cavity regions are nicely meshed with an all hex mesh. This approach should provide a better suited mesh to resolve the strong shear flow in the gaps.  By the way, did I mention the total element count? Get ready for this. The total element count for the all hex mesh in both the gap and cavity is only 145 K elements, only a small fraction - 11% of the total number of elements of the first tet  and prism mesh. Yes, 11%,  an almost 90% reduction of element count! It’s rather remarkable, isn’t it? - by simply dividing the flow volume into three parts and taking advantage of the sweep meshing.

So, before settling into the conventional tet and prism mesh for tight spots in a flow domain, it may be best take a step back from your CFD analysis, take a sip of whatever delicious beverage you have at hand, and look at the flow domain again to see if you can divide it up in any way to take advantage of the sweep mesh method.  The result may surprise you.

Figure 4: Flow Domain Decomposition

CFD mesh 4.png

Figure 5 - All Hex CFD Mesh

CFD mesh 5.png

Figure 6: All Hex Mesh in Gap and Cavity