Pressure boundary condition ANSYS Fluent
 

Dear all,

I want to simulate a high pressure vessel. Carbondioxide enters at 40 psi to the vessel and exits with some pressure loss which is not known. What I want to understand is the flow field inside the vessel and the pressure loss through the vessel so that I can estimate the exit pressure. However, when I want to use the pressure inlet-outlet boundary conditions, I am required to submit the exit pressure along with the inlet pressure. How would you handle this?

By the way, in Fluent material database there are two different CO2 as follows:
1- carbon dioxide (co2)
2= carbon dioxide- (co2-)

what does that - refer to?

THANKS.

First of, CO2- is probably the carbonate ion, hence the properties do not include a density and Thermal cond. CO2 is the gaseous carbon dioxide.
Regards to your BC, if you do not know your outlet pressure you cannot specify a pressure outlet. You could do the following,
1. Extend your outlet to a region where the pressure is know and then specify the pressure outlet
2. Use the outflow BC, BUT this BC cannot be used along with a pressure inlet, you would have to specify a mass flow or velocity at the inlet.

Hope this helps
Regards
Luke

1- I can not extend the region where the pressure outlet is known. It is not possible. The exit of the vessel will be the inlet of a compressor. The exit pressure is the main thing I want to see.
2- I know about the outflow condition, but as you said it can not be used along with pressure inlet condition.

For carbon dioxide, what you said makes sense. Given the flow conditions, the carbon dioxide will be compressible and will possibly not an ideal gas. So, what would you offer in order to take compressiblity effect into account? which kind of density method should be used?

THANKS.

If you want to know the pressure loss in the vessel, you can set BC like this:
velocity inlet /mass flow, pressure outlet.

Hope this helps.

Reds.
Guava

This won't work well for a compressible flow.

The best thing to do is use a pressure inlet. It is the most physically meaningful, and it is what you are interested in.

You can use a pressure outlet, and activate the target mass flow rate option. It will iterate the pressure at the outlet to achieve the mass flow rate that you specified. This is exactly what you are trying to solve for is this outlet pressure. But you need to know the mass flow rate. I believe you should already know the mass flow rate, as you do not have a fully defined problem without it (you just probably just forgot to mention it).

You do not need to and should not extend your domain, that suggestion does not make any sense, so do not do that.

Properties should not be a problem. It is doable at some point. However, I would worry about this last. You can use real gas models (which do account for compressibility effects). If that is not sufficient, you can specify polynomial relations for each property. If that is not enough, you can use a UDF to specify arbitrary properties. Don't forget the additional computational cost with having to calculate the properties, they may become significant depending on your problem.

Hope that helps,

Hi LuckyTran

[QUOTE=LuckyTran;355915]This won't work well for a compressible flow.

As described, the flow in calculation region is imcompressible, but not a compressible flow.

The unconsidering region is a compressible, so the extension outlet can't be made to simple the case. The information shows as below,
"The exit of the vessel will be the inlet of a compressor"

[QUOTE=Guava Wang;356776]Hi LuckyTran

Your point? It's still not meaningful to apply a velocity boundary condition when it should be a pressure boundary condition.