[firestone9x]

Hello all,

Experimental set-up:
I have a basic model that consists of a rectangular duct that has a sudden contraction to a smaller rectangular channel and then a sudden expansion back to the larger rectangular duct. The flow is driven by a centrifugal blower fan at the inlet and the velocity is measured after using flow straighteners. The outlet is exposed to the atmosphere and pressure is measured before contraction and after expansion using a differential pressure transducer.
Reynolds Number in the larger duct is around 1500 to 3900 and in the smaller duct it's around 2,200 to 11,600

CFD set-up:
I have replicated the same boundary conditions in Fluent with a velocity inlet and pressure outlet. I am also using a k-w SST model with a yplus of 5 for my 3D grid and performing a steady simulation with the coupled scheme.

In Fluent I get a pressure drop 3 times lower than the experiment and I am running out of ideas as to why this is happening.
Right now I think this might have something to do with the pressure measurement since the pressure drop decreases slightly if I swap out the blower fan for a smaller one.

I would appreciate some advice.

Thanks in advance.

[LoGaL]

Reynolds number = 2000 and you are using a turbulence model. Sounds suspicious, is the flow turbulent or not?

[firestone9x]

Originally Posted by LoGaL

Reynolds number = 2000 and you are using a turbulence model. Sounds suspicious, is the flow turbulent or not?

Yes, you are definitely right. A laminar model should be used for low Re.
I should have been more specific, my apologies.

My Re range is from 2000 till 11,600. At the max Reynolds Number, the experimental pressure drop is still 1.7 times higher than CFD.

[LoGaL]

Did you run without turbulence model?

[firestone9x]

Originally Posted by LoGaL

Did you run without turbulence model?

Yes, I ran a Laminar model and the pressure was just 7 Pa less when compared to the turbulence model but still 3 times lower than experimental data.

[LoGaL]

So first thing, switch off that turbulence model, it’s really horrible to use it at such low Re. Remember that laminar model is actually bare Navier Stokes equations, which already describe the turbulence physics. So for such mild to non existent turbulence levels, you don’t need RANS.

After that, can you show me your mesh? Did you extend your inlet so as to have developed flow at the entrance of the region of interest?

Also, did you do mesh independence studies? Can you show me a plot?

[firestone9x]

Sorry for the late reply. I have switched off the turbulence models when running these simulations.

My inlet is 3.5D. You can see a picture of the mesh in the attachments labelled 'mesh-1' and 'mesh-2'.

As for the mesh independence study. Please see the attached image labelled 'mesh-independence.

[LoGaL]

Hi, if that is the finest mesh, out of which you are getting the pressure drop, then I really think it is a problem of mesh independence because it’s coarse, especially at the two ends of the small channel ( where you will have a very large velocity gradient) and even in the small channel itself

[firestone9x]

Good point, I went back to my mesh and refined the inlet and outlet ends of the small channel as you mentioned. The pressure drop didn't seem to change.

From the experiment side, I replaced the small CFM blower with one that had twice the CFM and noticed that my pressure drop readings were now 100 Pa higher. In my setup, I'm measuring the differential pressure across the small channel with two pitot tubes and this should remain the same if I swap fans. In both tests, the velocity is kept constant.

Is there something I am missing out on?

[LoGaL]

No man, you misunderstand me, the mesh you are showing is bad so I don’t expect anything good to come out of it. All those sharp aspect ratio transitions, the overall coarseness. Is the boundary layer solved? Did you check it? You should really mesh work on that.
Other than that, I don’t see what could go wrong with a laminar model, an inlet and an outlet. Which boundary conditions are you imposing? How are you obtaining the pressure drop (area average total pressure?)

[firestone9x]

Okay. I'll work on improving the mesh based on your suggestions.
I do have inflation layers with a Yplus of 1.5 to resolve the boundary layer. However, I will change my first layer thickness to see if this affects the solution.

As for BCs; I have a velocity inlet (experimental measurements with a hotwire) and a pressure outlet at 0 Pa. I used the area-weighted average of 'static pressure' at the inlet to find my pressure drop.

[LoGaL]

You should measure total pressure, non static one. Try changing that and maybe it works despite the mesh .

[firestone9x]

The difference between total and static pressure was negligible, unfortunately.
I think any further mesh refinement will not change the solution.

However, I changed my anemometer and recorded a higher velocity reading and now my CFD pressure data is close to experiments.
Now there is one pending question, which pressure readings are right since the small CFM fan is close to the CFD data but the larger one is almost twice the pressure drop of the smaller CFM fan even though the velocity is the same.

Is there a special BC that has to be implemented in CFD?

[LoGaL]

Hold on, can you explain better?

You tried two different fans pushing air in the duct. At the inlet of the duct you measured velocity with an anemometer. You also measured the pressure before and after the duct with some pressure probes.

You changed anemometer and now CFD and exp. data match for the small fan

You are saying that with the big fan CFD and exp. data do not match for the big fan.

What do you mean when you say the velocity is the same?

[firestone9x]

I measure the velocity at the inlet of the duct.
And the differential pressure is measured before and after the channel with two pitot tubes connected to a differential pressure transducer.

Now, I have two anemometers, the new one reads a higher velocity than the old one. So the higher velocity inputted in CFD will result in a higher differential pressure that matches with the experimental data for the small fan.

However, when I swap out the small fan with a big fan, the experimental differential pressure is higher than the small fan differential pressure.
When I said the same velocity I was referring to maintaining the same flow velocity at the inlet of the duct for both fans which should result in the same static pressure.

[LoGaL]

I don't get how a larger fan would give the same velocity and the same static pressure. If the duct area stays the same, I would expect either the velocity or pressure to be higher

[firestone9x]

Those were my exact thoughts.
Unless the turbulence intensity at the inlet is different due to larger and different blade geometry. But I have flow straighteners before my anemometer in all test cases.

[LoGaL]

I was wondering whether the absolute pressure value stays the same inside the duct? Not the differential one. This might make sense to me, because this larger fan has to force more mass flow in (and also provide a different pressure jump) which for the same duct means more absolute pressure. This in turn raises the density of the flow, which increases the turbulence levels.

Is the discharge pressure of the duct known? Ambient perhaps? Do you know any absolute pressure value? It is true that for low Mach flow (ie incompressible) differential pressures matters, but you need the correct density value, which in turn depends from absolute pressure value.

Basically this larger fan must change something in the inflow conditions in your exp setup, and if we don’t know what is changing, we won’t reproduce the results

[firestone9x]

I think you might be right. Since the density is increasing, the absolute pressure would increase and therefore I will need to calculate a gauge pressure in addition to the velocity value at the inlet.
However, I'm surprised that the flow would be compressible at such low velocities but then again the larger fan is forcing a lot of air through a small channel.

Yes, the discharge pressure is measured to be atmospheric.

I would need to get an absolute pressure sensor to get those values and then repeat the simulations.

[LoGaL]

If your velocity does not change with the larger fan, there has to be higher pressure or I can’t see how you could pass more air 🥲.