Pressure drop vs Flow rate curve

[sigurd.naess]

Hi!

I have a geometry of the void volume of a subsea stab and receptacle that I want to compute  Pressure drop vs Flow rate curve for

I have set up 5 scenarios where I vary the inlet condition (volume flow rate) and keep the outlet at Total Pressure = 0. The results are plotted in excel

The calculated pressure drop is a lot less than measured data I have

Any thoughts on what I should do?

The center circle and 5 extrusion are the stab flow volume, the surrounding vlume is the receptacle cavity

[frederic.gaillard.7]

Hello @sigurd.naess , 

Meshing, boundary layer and turbulence model have an impact on the pressure drop. 

1. Can you share your CFZ file through a compressed folder 

2. What turbulence model are you using ? 

3. Gravity and hydrostatic pressure might be important if your looking for accurate prediction
Fred

[sigurd.naess]

1. Can you share your CFZ file through a compressed folder 

See attached (hope I got it right)

2. What turbulence model are you using ? 

Default values

3. Gravity and hydrostatic pressure might be important if your looking for accurate prediction

I do not think gravity and hydrostatic pressure is relevant for this case. The stab measures approx. 40cm long with a diameter of approx. 66mm, the receptacle outlet has a diameter of 73mm.

The test data I compare with was done on land with a hose connected to the stab

Thank you for taking a look 🙂 

Regards 
Sigurd

[frederic.gaillard.7]

Hi, 

I can not open rar file, can you compress it with zip file ? 
Using k-epsilon for pressure drop prediction is a good to start, but like you just experiment, it generally underestimate this aspect. Try to swith with a SST Komega model with 10 boundary layer to adequately capture the drag cause by the wall. Y+ will be an important parameter of your analysis check out this link for more detail or this link for a deeper understanding of the near wall treatement. 

For meshing, aim for at least 4-5 element thought the thickness of your system. 

Fred

[sigurd.naess]

Added ZIP file

[frederic.gaillard.7]

Any particular reason why you consider your fluid compressible ? 

[sigurd.naess]

no, before this analysis i did an identical one with incompressible fluid. I then tested with compressible fluid with little difference between the two...

[frederic.gaillard.7]

Hello @sigurd.naess , 

Before diving into the turbulence modeling world your CAD geometry is not designed correctly for a CFD analysis. 

Your outlet has to be longer. Right now you have recirculation throught your 0 pressure boundary condition (your mass conservation principle is violated). Your flow throught your outlet must be unidirectional. In the picture below it's clearly not the case.

Recirculation Behavior

To avoid this, make your outlet longer (generally speaking a good practice is  : length = 10*outlet_diameter)

Once you will correct this aspect we are going to dive into CFD specific modelization

THX 
Fred

[sigurd.naess]

Thanks for all your feed back, much appriciated 😄 

I will update my 3D model and read up on the turbulence model you suggested

Regards 

Sigurd