[basivi]

I want to calculate pressure drop,

Reference pressure: 1atm

Total pressure (stable) at inlet: 20psi

Static pressure at outlet: 0pa

Fluid: water

Pressure drop: area average total pressure at inlet - area average total pressure at outlet.

Is this the right approach? any suggestions or corrections?

[ghorrocks]

Have you read the CFX documentation on choosing boundary conditions? It has some good tips on which combinations of boundary condition work well.

[Gert-Jan]

a massflow average would be better than an area average.

[urosgrivc]

What you are setting up is not ok...

You have specified a pressure drop as a boundary condition (inlet 20psi outlet 0pa)
this is the answer (you must not set the answer to your problem as a boundary condition, because where is the point then?)

If you want to get the pressure drop as a result from the simulation:
you would have to specify either Inlet or Outlet pressure and mass flow (or velocity which is the same thing)
Now you would be able to get pressure drop as a result

What you have done by setting inlet and outlet pressure (you have fixed the pressure drop) from this simulation result would be mass flow or any of the flow velocities

[Gert-Jan]

I do not agree. I think the setup is ok. Total pressure includes the dynamic pressure component which is unknown from the start since the velocity is yet unknown.

So, it depends on definition of pressure drop. You cannot take the difference between total pressure on the inlet and static pressure on the outlet.
It is either difference in total pressure or difference in static pressure.
But from a bernoulli point of view it is best to take the difference in total pressure.

The total pressure on the oulet is not known yet. It will be the outcome of your simulation. So I think your setup is ok. However, as mentioned earlier, I would take the mass flow average instead as area average.

[basivi]

Originally Posted by ghorrocks

Have you read the CFX documentation on choosing boundary conditions? It has some good tips on which combinations of boundary condition work well.

Yes, also I am confused, maybe because I am reading a lot or mixing up different scenarios I read on the forum with my case.

[basivi]

Originally Posted by Gert-Jan

a massflow average would be better than an area average.

Noted, thanks.

[basivi]

Originally Posted by Gert-Jan

I think the setup is ok. Total pressure includes the dynamic pressure component which is unknown from the start since the velocity is yet unknown.

I think the same.

How to approach the problem if I know only static pressure at inlet? and outlet is open to the atmosphere?

[urosgrivc]

In this case, I would add a large 'buffering' volume on the outlet, so the Boundary condition opening is not close to the actual 'thing (a nozzle, exhaust or whatever)' of interest, actually to simulate a part of the surrounding


This simulation would run with pressure inlet condition and opening pressure on the far-field boundary condition
the outlet, in this case, is opened to the atmosphere
The simulation is transient in this case but can be steady-state of course
in this case, Pressure drop in the muffler is obtained from the simulation as it is a part of the solution

maybe you can be more specific about your simulation as I can see we did not understand ourselves previously

[basivi]

Originally Posted by urosgrivc

In this case, I would add a large 'buffering' volume on the outlet, so the Boundary condition opening is not close to the actual 'thing (a nozzle, exhaust or whatever)' of interest, actually to simulate a part of the surrounding


This simulation would run with pressure inlet condition and opening pressure on the far-field boundary condition
the outlet, in this case, is opened to the atmosphere

maybe you can be more specific about your simulation as I can see we did not understand ourselves previously

Thanks for the reply.

1. My area of interest is to study pressure drop between inlet and outlet.

2. I am simulating UV-C water filter (no porous media inside). Based on the pressure drop data, I have to suggest changes to design.

3. I have experimental data, which are, a) Pressure (don't know whether it is static pressure or total pressure, please see the digital gauge setup) at inlet which is 20 psi, b) outlet mass flow rate 2 liters/min.

4. I finished a case without specifying massflow rate because i want to know massflow rate at outlet,

Boundary conditions:

Total pressure at inlet 20 psi, outlet static pressure 0pa

result: massflow rate at outlet: 4.4 liters/min, area average total pressure at outlet is 0.1psi.

[Opaque]

Your setup is sound since your inlet is a Total Pressure condition, i.e. a plenum upstream.

On the appropriate average to use, I would stick to areaAve ONLY because we are talking about a momentum balance, and pressure is force/area

In the case of momentum, or enthalpy transport I would definitely use massFlowAve since accounts for the total advected quantity.

an easy way to see is by integrating the transport equation over the whole domain which by the Gauss theorem becomes a surface integral, and you must balance

areaInt (mass flux * Velocity),

areaInt (wall shear)

areaInt (pressure )

and so on. You can then replace the areaInt by areaAve () * Area.

There you go. Hope it helps,

[basivi]

can anyone help me understand this,

1. Which pressure difference I have to consider? ('case 2' and 'case 3' pressure difference is close)

2. Is specifying mass flow outlet in 'case 2' as 0.03 kg/s (experimental result) correct approach?

[Gert-Jan]

Sorry to be blunt, but clearly you don't understand the real basic things of hydrodynamics. I would suggest to try to understand Bernouilli equation before performing CFD calculations.

A suggestion would be to perform multiple cases with increasing velocities on the inlet and 0 pressure on the outlet. Then use Excel to plot Total/Static/Dynamic pressures versus velocity/massflow/volumeflow.

[basivi]

Originally Posted by Gert-Jan

Sorry to be blunt, but clearly you don't understand the real basic things of hydrodynamics. I would suggest to try to understand Bernouilli equation before performing CFD calculations.

A suggestion would be to perform multiple cases with increasing velocities on the inlet and 0 pressure on the outlet. Then use Excel to plot Total/Static/Dynamic pressures versus velocity/massflow/volumeflow.

Okay Thanks.