[probl3m]

Hi all,

I was running a simulation of a high pressure inside an object venting out to atmosphere.

I originally had the boundary condition set as a static pressure of 1 bar at the opening, but as it was creating a vortex and I realised this wasn't a very accurate representation of reality so I've put the object into a large 'chamber' and set the boundary condition on the surface of this.

This is still giving the 'vortex crosses the pressure opening warning'. My question is does this matter if all I'm interested in is the mass flow out of the object and not what the flow does after it has exited the object? (bearing in mind I think the 'chamber' is probably large enough to accurately represent the flow in the region of the opening.)

Thanks.

[Boris_M]

Hi,

Is your application a pressurized canister that for example has 50 bar and you want to see the mass flow rate over the emptying of the canister?

Do you need to see anything else than numerical values of the flow rate. Meaning do you need to see flow trajectories or cut plot of the velocity?

Boris

[probl3m]

Sort of it's at 20 bar pressure, then a convoluted path to the opening to atmosphere. I'm not interested in changing the 20 bar, just what the mass flow rate is at that input pressure.

The flow trajectories and cut plots are of secondary importance, as they'd just be for showing others a rough visualisation of the results.

[Boris_M]

So you probably model the pipe end ending into an external environment. I would use the inlet some length into the pipe to avoid any vortex to form directly at the surface and then apply the 20 bar on that. You should consider using the high mach number option as velocities might reach that range and you need to resolve the mesh very fine at the exit of the pipe.
If you get errors, as there is a rapid expansion from 20 bar inlet to 1bar environment, you can run an internal calculation with a plenum and a pressure applied to that to 1 atm and use a higher initial pressure of maybe 10 bar, something in between.
If that still gives errors you can also slowly reduce the 1 atm and always continue the calculation after you changed the value but deactivate the goal convergence as it checks for converged goals right after start and will stop if it has converged before.

In general the vortex crossing pressure opening in a large plenum is normal as flow is not only leaving through the large surface of the boundary condition but also entering and therefore it is considered as a vortex.
If it is far away from the nozzle then the influence is very small.

You can also try to use the calculator under "Flow Simulation" menu, then "Tools" and then "Calculator".
Right click on a row and say new formula and select the tank evacuation under numeric calculation. Here you have to enter the first row values for the reference and how many time steps/iterations for the frequency. So 1000 will give 1000 steps from full to empty tank. The very first value at time 0s would show you your initial mass flow rate and how that is reducing than from time step to time step.

I hope this helps,
Boris

[probl3m]

Ok, thanks for your help.

I'd been running it as a internal analysis, so may try it as an external for comparison. But from what you've said I think it's ok, as it is a large plenum, so there's flow entering near the bottom and leaving a the top.