My task for today was very simple. Make geometry and mesh for air flow in 240x245 mm channel. It's pretty simple I guess. Just as usual I've created new ANSYS Workbench project. I've added new mesh component, made geometry and... meshing.
Nightmare starts...
Like in good (or bad) horror movie it starts very innocently. The nightmare I mean... So I don't know like you guys, but I usually start with simple math. Firstly, I want pretty fine mesh. So lets say it will be discretized with square elements with 2,5 mm side. It gives 96 elements per width and 98 elements per height. In one layer (I use sweep method) there are 96x98=9408. I've also decided that there are 20 layers (numer of divisions in sweep method), so total number of elements, should be 188160.
These two pics indicate my plan works perfectly, and domain was discretized as I predicted. Every CFD practitioner knows knows that we cant go with that mesh. It lacks Inflated boundary, which is region of thinner elements in the wall vicinity. Elements grow by specified factor in the way that thinnest element is touching the wall. Velocity equals zero at wall - layer of stagnant fluid particles affects strongly velocities of traveling neighbor particles, which cause steep velocity gradient near wall (talking about viscous fluids). This needs to be taken into account with thinner elements in that place.
It's going to be ugly...
This is the moment when ugly monster face appears in a movie for the first time. I must add finer elements near wall with Inflated boundary option. I like to use Total thickness option because I can control total thickness of inflated layer. I have made it 2.5 mm. thick. It's the same as element size. In effect Inflated boundary should "steal" first layer of elements adjacent to walls. Best practice is to right click (RC) Sweep Method and choose option Inflate this Method (see picture below on the left).
After selecting four sides of rectangle which is a source face (in Sweep method) of the domain and setting 10 layers of Inflated Boundary, mesh can be updated. It will look like on the right side of the picture above. Why is it bad in my case? Why do I call it bad, look closely at below screens.
First lets look at top picture, this is a corner when Inflated Boundary can be seen. Because at edge elements are 2.5 mm wide and there is 96 elements, the same number of elements has to be at inner edge of inflated boundary. This edge is not 240 mm long but 240 mm - 2*2.5 mm (inflated boundaries thickness) = 235 mm. So element width at inner edge of Inflated Boundary is 235 mm/96=2.45 mm (approximately). This will create mesh which is the most distorted in the middle, which can be seen at bottom picture above. Maybe the geometrical constraints, like the same number of elements aren't clear for you, so see illustration below.
In the above picture square is first divided into 25 square cells. Next, inflated boundary is introduced (one element thick). Inflation edges (pink) and inner mesh edges (yellow) are divided into eqal number of sections. It seems the reason why ANSYS meshing produces warped and smaller elements in the center is my sizing strategy. I have used face sizing with element size 2.5 mm. So if ANSYS meshing is forced to preserve number of divisions it has to deal with "inside" elements that are smaller than element size (2.45 mm < 2.5 mm). So it creates some number of 2.5 mm side elements that messes up mesh structure. ANSYS meshing won't make uniform mesh like in the picture, because element size constraint. Let me introduce some possible remedy for that...
Run through dark forest.
Running through dark forest to hide from the monster. While running, we can think about solution (usually killing it). Sizing strategy seems to be the problem, so we have to change it. If my theory is correct, edge sizing will make mesh regular. I'll specify how many divisions of edges there are and ANSYS won't care about size of element. To introduce edge sizing, you just have to select edges instead of faces.
Select also Type: Number of Divisions and fill the number that is characteristic to 2.5 mm element (96 horizontal, 98 vertical for this geometry). Hit Update button, and... nothing is changed! Mesh is messed up the same way. I even won't bother to post a picture. Someone could think Mapped Face Meshing is a solution but it is not compatible with Inflation. Conclusion is we can't do it without dividing domain into at least two regions.
There is no happy end...
It seems to be impossible to get Inflation with regular, structural mesh if domain is not divided. Do you agree? Or is there a way?
Brak komentarzy:
Prześlij komentarz