hi there,

let's say that we solve the incompressible NS equations by a marching technique. these equations are not non-dimensionalized. after we obtain the solution, it is natural for us to check with the continuity equation to see the magnitude of the mass source. then, what is the permissible value of this source, at least for normal practices, 10e-5?

thank you

You mean mass balance error, I presume.

If so, acceptable value of the error depends on the problem you are studying:

simple problems (that is simple geometries, with non deformed mesh) low error (0.01 % is a good value);

hard problems (that is deformed mesh, some unsteadyness in the solution, and so on) error must be below 1% because, usually, this is the error you get in experimental measurements. The greater the experimental error, the greater the computational error allowed.

Hope it helps,

Nicola

dear Nicola: thanks for the information. i feel it is better to state my question properly. the continuity equation: du/dx + dv/dy + dw/dz = S ----(1) for exact solution, S (mass source) should be zero. however, when we solve the NS equations together with (1), we will get solution where S is not zero but remains small in magnitude, perhaps 10e-5. the thing i did was making sure that S remained small and i am really interest to know what magnitude of S that is acceptable. in your posting, you mentioned that the error should be smaller than 1% (for hard problem), how do we calculate this (1%) since S should be zero for exact solution? thank you. i would be very grateful if you can cast some light on this. regards, yfyap

Hi yfyap,

1% error is referred to inlet and exit planes mass flux balance: that is

(MFR_inl-MFR_outl)/MFR_inl x 100

I have no idea of what value S should have, because (in my experience) it is not of practical importance. Using time marching method to solve steady problems, you have to be sure that solution has reached steady condition, that is

d/dt rho = 0, or

d/dt p =0 (Chorin formulation for incompressible flows)

and so that S is small enough.

Of course, if the problem is difficult to solve (e.g. the vortex at the tip of a marine propeller) you could have problems to get a fully converged solution because of some unsteadyness ( at the tip of the blade due to the tip vortex for the propeller problem), so you could have a high S value in several cells. But YOU are to decide if solution you have is good or not:

if you are interested in studying the local behaviour of the fluid, then you should get the lower value as possible, and so, if the solution is not fully converged, you should flush it;

if you are interested in global performance of a machine, and solution is globally converged, that is low error in mass balance, mean angles and pressures not varying with increasing iteration steps of the solver, then, in my opinion, you can use the solution you have.

I use a finite volume solver, and I can see the value of

d/dt rho x Vol

or d/dt P x Vol where (Vol is the local cell volume)

that is the MFR unbalance at the cells boundary.

Maximum values of this expression are of the order of 1. x 10^-4, but they depend on the local dimension of the cells.

Hope it helps,

Nicola

In general, if you have inlet, then you can judge as follows:

sum up of the absolute value of S for all cells:SUM(ABS(S)), and compare it with inlet mass flux, normally should be < 1.e-3.

thank you

thank you.