# Pressure Drop Computed is Too Small

cwl6750084
Member

in Fluids

Hello,

I am simulating high pressure (~3.5 MPa) vapour flow in a straight pipe of 12 m in Fluent. The known mass flow rate is 3 kg/s. The simulation was setup and however, the resulting pressure drop from inlet to outlet is less than 500 Pa. This pressure drop across the pipe seems way too small and incorrect. I wonder if anyone can shed some ideas on what could have been wrong. I checked the settings of the model and could not find any mistakes (as far as I can tell). Thanks.

## Comments

What material properties and boundary conditions are you using? How well resolved is the mesh?

For liquid water, I used polynomials curve fits based on the steam table. For water vapour, the density was assumed ideal gas, other properties were polynomial curve fits from steam table data. The boundary conditions are pressure inlet and pressure outlet with temperature being set at the saturation temperature of the corresponding pressure.

We did a mesh-independent study by making the mesh twice and four times as dense, the end flow parameters distributions are the same.

Thanks.

Are you adding water or steam at the inlet? Which multiphase model?

The VOF model with 99.5% volume fraction for steam at the inlet.

By the way, the turbulence model was the k-epsilon model with enhanced wall treatment.

If I switch to the standard wall function, the pressure drop is much higher. Does this imply the choice of wall function was incorrect?

Vof model is wrong. Either mixture or Eulerian should be used. If no stratification you might even use DPM. Are you expecting mass transfer?

Also if fou assume single phase of vapor does hagen poieusille pressure drop estimation match?

Are you getting the right mass flux? What do you know at inlet?

Flow is probably turbulent at some point down stream. I thought hagen poieusille pressure drop estimation match assumes laminar flows. Yes, the inlet fluid is 99.9% by vol steam but we expect a little of it be condensed.

The computed mass flow rate is correct and we are give the inlet pressure and temperature.

For VOF the inlet boundary needs to be 100% one phase or the other. Move the conditions to be slightly above saturation and see if that helps. For the outlet you may need a "drain" boundary to let the water out.

But for condensation type modelling you want to listen to @DrAmine

VOF model is not correct! If you do not expect any mass transfer and no stratification of droplet you might even use DPM Model.

Thanks your advises. Let me try it with the mixture model. The inlet is about 99.5% by volume of steam and it is expected ~95% by volume at the outlet of the pipe.

What does it mean by a "drain" boundary?

With VOF some boundaries have all of one (or another) phase enter or leave the domain. It's sometimes then necessary to add a "drain" to get small amounts of the "other" phase out of the domain. As you're looking at a tiny fraction of second phase the DPM model is possibly better suited to this; Eulerian or Mixture may be another option.