hi,

i currently 've a working 2D FVM solver. It can simulate flow past a stationary airfoil with a c-grid. i need to modify it to simulate (for a start) flow past a heaving (up/down motion) airfoil.

i've read thru some papers & messages in the forums. i believe formulating the NS eqns in the ALE form is the best way to go, and since no deformation is necessary, it is not required to apply the GCL. So these are the modifications:

1. replace original NS eqns to the ALE form with convective velocity replaced by the relative velocity (u-u(b)) where u(b)=mesh velocity 2. besides the standard BC for boundary cells, such as u=1,v=0 at the LHS of the grid for the inlet velocity, there is also a need to include the presribed velocity of the motion e.g. v=0.5 (airfoil moving up at a velocity of v=0.5) to all the boundary cells.

Is that all there is to it?

Thanks alot

Close. I agree on the best way to go

However, there are some details you need to be careful about.

Firstly, you will need to move the vertices of the grid rather than mess about with the "grid velocity" because the second approach has got conservation problems.

Secondly, you need to us old and new cell volumes (before and after the motion) in the ddt (rate of change) term.

Thirdly, doing (u-u(b)) is a problem - you will need to operate on fluxes instead. For this purpose, the u(b) actually converts to a "mesh motion flux", which shold be calculated as the area swept by the face in motion during the current time-step.

The last trap is the formulation of the pressure equation (depending which algorithm you're using. If the flow is incompressible and you're using a SIMPLE-like algorithm, you need to be careful with relative and absolute velocities, ut more on that in due course.

Enjoj,

Hrv

Dear Dr.Jasak,

If the grid vertices are moved, there is in fact a grid velocity coming into picture. In deforming grids, the conservation of volumes is an issue and the Geometric Conservation Law is enforced. there have been contoversies over the same. My personal experience and some literature suggest that the GCL is important only when there is structure-fluid interaction and involves energy exchange, so there is little difference it could bring in purely unsteady aerodynamic problems, but is a serious cause for concern in aeroelastic problems. It would be nice if you could clarify on the first point of conservation.

It is true that incompressible flow would pose a problem, but I believe that pseudo-compressibility or otherwise a preconditioned compressible solver could do a good job.

Regards,

Ganesh

thank you both Dr. Hrvoje & Ganesh!

just to clarify some pts:

1. there is no grid deformation so I believe GCL is not required, right?

2. I'm using a colocated grid arrangment so my velocity variables are at the cell's center. that is why my grid velocity will also be at the cell center. Is there a problem? may I know why and is there any solution?

3. may i know why there is a problem with incompressible? i'm using the fractional step scheme and hence there is a need to solve the poisson equation at each time step. what is the modification i need to make?

Hope you can answer these questions or refer me to some references.

thanks again!

Dear Quarkz,

If there is no grid deformation, then GCL is not required. But since you talk about grid velocity, in which case the volumes are time dependent and non-constant, GCL would be advisable, but even without GCL reports of correct solutions exist.

I am not well versed with incompressible unsteady flows, but I think you could look at the following reference

Kallinderis et.al. Unsteady Flow Structure Interaction for Incompressible Flows Using Defomable Hybrid Grids," Journal of Computational Physics,Vol.143,1998,pp569-597

Hope it helps

Regards,

Ganesh