I have the same problem about 'negative density'.

I would like to know about the relationship between boundary condtion and negative density. I am eager to know about this unhappy message. Please post your wonderful advices.

Thank you

(1). I am curious about this negative density message. (2). Could you describe your problem and the situation when you got this message. (3). Even though I don't use this code, I normally don't have such problem unless I am running a density-based code at low Mach number. (4). If you are not using the density-based code, then it is likely that the trouble lies somewhere else. So, what is the problem you are trying to solve?

The problem that I want to solve is the flow mixing in IC engine cylinder. Before that, I am doing some kind of test about simple geometry and boundary conditions.

The boundary is 'inlet' and 'outlet'. The flow model is 'k-e'. The property is 'ideal gas'. Temperature option is 'on'.

If the inlet velocity is low, it converge but if the inlet velocity is high, negative density message is showed up. 'Negative densities found over 100 hundred cells.'

I want to know the general idea about this error message.

(1). You will have to be more specific about this "low" and "high" inlet velocity. (2). You will have to use numbers, so we can understand it. Can you do it in numbers? I mean the inlet and wall conditions. And the size and the shape of your test case.(in numbers if possible).

Generally, the (-ve) density message appear when something goes wrong in the calculation of the equation of state. For example for diverging solution, it start with very small or very high temperatures or enthalpy then the solution of the equation of state produce (-ve) pressure. This (-ve) pressure causes this (-ve) density.

Is it possible to avoid this kind of situation and let calculations go on?

Roughly, low velocity is 10m/s and high means 50m/s.

The geometry is 10cm height and 10cm diameter.

I turned on temperature option.

I agree this kind of error message is related to temperature calculaton(Energy equ).

The enthlpy residual is really big in many cases. (for ex 2x10E+15)

Thank you for your interest. I am really appreciate your response.

As I have said below, look at the file (case.info) to find out what exactly caused this message and when it started, then discuss your findings with us here.

Since there is no much details about the cases here, the general guidance is : 1. for steady flow calculation, lower pressure and temperature under-relaxation factors, you may also use under-relaxation factir for density; 2. for unsteday calculation, reduce under-relaxation factor for PISO from 1.0 (default) to 0.5 (say). There could also be possibility of code bug in certain case, so if you can not sort it out, passing the case to your support engineer is always good option.

I had the same problem. To a great extend these problems were solved when I used the latest version of STAR (3.100B)

The unfortunate fact is that this message results from a variety of errors. It is more a last desperate message from the code that something is wrong. In most cases, this happens because the solution is diverging (or diverged) and the first thing that the code notices is definitely wrong is that the physical property density is negative. So in general, as Hassaneen pointed out, you need to look at your .info file to see where the problem started.

In your case, though, I think the situation is not so bleak. From your description, I would guess that your pressure reference location is at or near the inlet. When you start the flow off with a large inlet velocity, the "pressure drop" in your channel during the first few (unconverged) iterations is probably larger than the inlet pressure. This would result in a negative absolute pressure near the exit, causing the negative density in Ideal Gas cases.

If this is a startup problem, you can get over it by either ramping up the velocity (for example, use your low velocity solution as an initial guess for the higher velocity solution) or reducing the underrelaxation factors. If this persists, it is possible that this is an inconsistent set of boundary conditions. That is, with this inlet pressure, there is no way this much mass would flow in this channel. Another way of avoiding this problem is to place the reference pressure location at the outlet. Then the pressure drop would simply raise the upstream absolute pressure, and there would be no absolute negative pressures anywhere. It depends on where you have measured values of pressure to impose on the simulation.

If all this doesn't help, it could still be a problem with divergance - perhaps a bad mesh etc., I encourage you to contact user support.

in the file case.info I got these kind of messages:

"warning #65 out of bounds value for scalar variable enth"

"out of bound values found at more than 100 cells"

"negative press found at cell no. ..."

For you Roberto and Sangwon, if you don't have any moving mesh, so most propably you should use finer mesh to avoid that message assuming that your boundary condition is fine. Another thing is try the MARS differencing scheme instead of UD.

Actually mine is a transient state run (moving piston in a cylinder during intake stroke); I also have used MARS diff. sch. for U V W. Should I still use a finer mesh?

Thanks for your interest

Roberto

No, I belive it's not a mesh problem. In your case if it happens at the end of compression or the start of expansion (the first event in the expansion) so it is related to the event module and I can give you some suggestion if this is the case. If it happens after the first time step, so reducing the length of time step by 1 order of magnitude may help. Could you tell us when that happen??

It happened at the beginning of the compression stroke 3 degrees before intake valve closing (LIVC = 70 deg.). I wanted to see what happened during compression but the error stopped the run.

Thanks, Roberto

P.S.: Here are a few parameters that may help you:

start crank angle= 590 deg.

stop crank angle= 630 deg.

intake valve closing= 610 deg.

engine speed= 2000 rpm

time step size= 0.5 deg.= 4.16667e-05

transient post frequency= 2

number of time steps= 80

Look at the file (protemp.info) and find out how many events are processed before the message and at which time step. Also, is it related to the last event of the inlet valve??

Actually I cannot find the file (protemp.info)...I might have deleted it; is there another way to get those informations? If not let me know, so that I'll run again the same case.

Bye, Roberto

I'm not sure if it is PROTEMP.INFO or PROTEMP.something else. Try to look at all the PROTEMP.*, one of the file has info for one event and the other has info for all events up to the moment.

Dear Sangwon Kim

I agreed with Mr. Sreenadh Jonnavithula. I have also encountered this problem of negative density on various cases, sometimes even in solving the sample problem. If there is no hardware specific problem the certainly it is due to diversion of the solution. I would suggest to have a finer mesh and reduced the time step value. We were succesful in solving the problem by this way.

Pavan