Hi

can someone tell me how to increase the triangular grid density in some region of the domain, which is not close to the boundary?

For example, suppose i have to generate unstructured grid for flow over a 2D wedge. I know approximately where the shock would appear. I tried to increase the density along that region by increasing nodal density near the beginning of the wedge and also on the outflow boundary.. but density of grid increases only near the boundaries.

Thanks in advance for any advice.

prapanj

The way to do this is create a stand alone connector (i.e. grid line) in the interior of the domain with an appropriate grid spacing. When you create the domain, using your wedge as an example, you will need to select the outer boundary as the first loop, the wedge boundary as the next loop and the free connector as the third loop.

The trick with the free connector when selecting it as the third loop is to select it twice (one direction and then the other). Its like a two connector domain with zero area. Its kind of an undocumented trick.

BTW, make sure the orientation of both inner loops is opposite of the outer loop.

The way to do this is in 3D is with baffle faces. There is a built in tutorial about baffle faces.

excuse the weird text in my first post - Safari was doing strange things with form.

but then i will be drawing a connector approximately at the position of the shock. since i dont know the angle of shock before i run the code, how would i draw an appropriate connector?

And how would this trick work for the case of simulating a bow shock in flow over a circular infinite cylinder?

To answer your first question, we never really know a priori the nature of the flow - we can only make educated guesses and cluster the grid appropriately.

Using your wedge example again, based on the inflow Mach number, angle of attack and included angle of the wedge you can make a inviscid estimate of the angle of the shocks and expansion fans using a velocity triangle and the normal shock tables. This would give you a pretty decent guess as to the location of the shock and then I would use grid adaptation to improve the shock resolution (that is if your CFD solver has this capability).

The bow shock case would obviously be a little trickier but again cluster the mesh where you think the shock will be, perhaps by finding some prior work with the same flow conditions, and then using grid adaptation.

If your solver does not have grid adaptation then you will have to resort to the traditional method - cluster the mesh based on a guessed location of the flow gradients, run the calculation, check the solution and repeat if necessary.

You run into to same meshing problems as everyone else - how to choose the mesh clustering when you're not sure where the flow gradients are located?

Good Luck!

Thank you.

Your answer indeed edified me of impossibilities too. In this case the flow solver is one I myself wrote. Which does not have grid adaptation. Though that is in my mind.. will be incorporated soon.

And as u said i am using additional connectors now.. Then i run solver, set attributes->geometric variables-> boundary influence, i vary this value close to 1. so the grid is more dense near these edges and the density prevails for quite a wider region.

Anyways thank you.. And this is my first solver. 2D euler solver with 2 types of boundary conditions. Roe scheme is used.

prapanj