SIMPLE method small time step
 

Hi, I have created a CFD code following the SIMPLE method. It is a co-located grid and uses Rhie-Chow interpolation. The problem is, I need to take rediculously small time steps for it to be stable.

Has anyone ever had this issue? Fixes?

Any response will be much appreciated!

what discretization are you using in time? first order explicit? How about the Re_h?

First order implicit. I've tried with multiple Re, but it seems the time step is always limited by a CFL of 1.0. Which seems very low for an implicit solver.

Your program has a bug and it could be anywhere. Instablity in cfd solver could creep in from anything from small to big.

It is not possible to point out bug from your information.

But is it safe to say that there is definitely a bug? That I should be able to run with much higher time steps?

With his kind of behavior, the first place to look for the error is your implementation of the temporal discretization.

Could it be related to the rhie chow or pressure correction methods which both use the coefficient value from momentum (which depends on the time step)? Or any other suggestions? My temporal discretization method comes straight from the Versteeg textbook.

What is the nature of the instability? flow variables going to infinity? If so, which one starts it? Or do linear systems fail to converge? If so, which field? Or does the nonlinear iteration fail to converge?

The pressure correction equation goes unstable first. If I just do heat conduction, I can use a large time step. The instability seems to occur during velocity-pressure coupling.

just check after one time step if your pressure solution appears regular and if the gradients added to the partial velocity field satisfy the continyuity equation.

If my time step is too big (not really even that big), my pressure correction equation diverges (first time step, first loop).

that demonstrates you have some bugs in the code..check the BC.s for the pressure

Ok thanks. What should I expect for time step (based on cell size, velocity, etc.)?

After a single time step do you satisfy the continuity equation?

If you are using the SIMPLE method, then the algorithm is completely implicit and (in principle) there is no timestep limit. In fact, taking the limit of dt->inf should lead you to the normal steady SIMPLE formulation. This, of course, assumes that the SIMPLE algorithm (outer iterations) converge at each timestep.

I am aware of no theory...or even heuristic...that gives time-step guidance with regard to the convergence of SIMPLE. There are requirements on pressure and velocity underrelaxation factors for the steady state case under assumptions of simple models...no reactions, no buoyancy, etc.

I agree with the others advice. Verify that the face fluxes after pressure correction application results in conservation of mass. If that is not true both globally and in every cell, then your first problem to solve is there. There may be other bugs, but you will not be able to check because the fluxes driving the convection of other properties will be garbage.

And remember that because this is colocated, the cell values of velocity are (almost) irrelevant. The face fluxes are the primary metric with regard to pressure correction and mass conservation.