Hi

I have an compressible flow. I have specified all my boundary conditions and thermophysical properties and there is no problem, But after 20 iterations the program stops and it tells me i have negative densities.

Can anyone tell me what is happening? How can i solve it?

Thanks

Please use the search function of this forum.

Reduce your underrelaxation factors, especially the pressure, run 50-100 iterations and increase them etc

Thsi situation often happens when you have some starting value for the pressure field (typically 0.) which is very different from the solution of the compressible Navier-Stokes equations. A good trick is to underrelax the continuity equation a lot (e.g in the range of 0.01~0.025 or less) or to run the simulation using the pseudo-transient approach (which corresponds to using very low underrelaxation factors but which will be different in each cell). With this method, I was able to capture chocked flow with local Mach numbers exceeding 2.5...

Hope this helps...

There is some more to tell about negativ density in compressible flows. Please read the report on www.adapo-online.com -> Feature Articles -> Compressible Flows. Depended on the case and boundary please note this:

- First, in case of pressure outlets it can be helpfull to switch on the "Mean" button in combination with the option "piezo". Then the pressure is set at this boundary as constant.

- Second, switch on the the Envir(-onmental) pressure (pstat + pdyn). In case of inflow the pressure type is switch from piezo to total. This (helps to) avoids inflow. In case of inflow, the Navier Stokes and Conti. are satisfied too (!!!), but the numeric has some problems with it. The pressure value at this boundary is still the piezo pressure, not the total.

- The LUD differencing scheme is good for the start of the calculation.

- Please not the allowed combinations of the boundary types.

- I am using the following URFs: p (0.001 near mach=1, and 0.01 in normal case), u v w (0.4, in extrem cases 0.2), t (0.7), ke,ed(0.4), dens (0.7), vis (0.9)

- The residual tolerance should be reduced to 0.01 instead of 0.1 (exeption p 0.005)

- differencing sheme for turbulance allways Upwind

- diff. sch. dens. allways CDS with 0.01 (that means to 99% Upwind)

- In case of convergency make a restart with the MARS scheme with blending factor increasing from 0.5 to 0.9.

- place the reference pressure in areas of known pressure (e.g. near a pressure boundary). The value of the ref. pres. should be the wanted pressure at the boundary.

- be sure that there are no tet cells at the pressure boundary. Take care of good cells, especially at the pres. bound.

- Take care of a proper flow at the boundary regions. Extrude the mesh a little bit.

- In case of enthalpy residuals don't converge switch from static enthalpy to total enthalpy, as a last chance to get convergency.

- As a last remdy make a pseudo transient calculation.

- there are other points (y+, ....)

In case of big strong swirls Fluent has some better stability.

All this points should help you to avoid NEGATIV DENSITY. Please let me know if this helps.

By the way, what also helps a lot is to make use of the total enthalpy (hey, that is the quantity that should be conserved in a compressible flow, so we have to solve for it) instead of the standard energy equation formulation (roughly speaking you use H=Cp*T + 1/2*p*V^2 instead of H=Cp*T)

Hope this helps...