Hi I dont know why I am getting this 'negative densities' error everytime I try running my model. Densities in all materials are set as ideal gases, den=p/(rt(sum(mm/Mm))). I have not got a big pressure drops or big temperature changes along my model. I got inlets and outlets at atmospheric pressures. I dont understand, becuase when I do the calculations by myself this should not be happening. Has there anyone who have come across something like this? any suggestions will be appreciated. CM

I get this error in the following setup inlet fixed velocity outlet = outlet rho = f(T,p) high pressure drop

I can cure this problem with the following procedure 1. rho=const, run until convergence 2. rho=f(T,p) 3. diminish relaxation factors for p and rho.

I get this error in the following setup inlet fixed velocity outlet = outlet rho = f(T,p) high pressure drop

I can cure this problem with the following procedure 1. rho=const, run until convergence 2. rho=f(T,p) 3. diminish relaxation factors for p and rho. In my case down to 0.005 for p and 0.001 for rho -> very slow convergence

If there is a better approach I'd be very interested.

Thank you, that is quite useful. Indeed decreasing density's and pressure relaxation factor makes it easier to converge. But I got a question, first I have to admit that i have very little idea about the control volume method. Is'nt this decrease in the relaxation factor very high?, I mean does this still valid, as an approximation? in other words is it unrealistic to use this values. I might as well be very wrong. We have noted that convergence is easily obtained by using the AMG method to resolve the pressure equation, you can activate it by 'solu,scalar,AMG' and we have been working all this time with 0.05 pressure r.f. and 0.5 for density, but we might give it a try with lower values and see if it works. Many thanks CM

Hello! Without changing your physical BCs, you could try pseudo-transient or single-transient with very small time steps. I found out that this is a way to resolve my neg. density issue for compressible flow case. A big jump in grid sizes (e.g. from small grid size to very big grid size at coupled interphase) might also cause the error.