[Carles_SM]

Dear experts,

I have a 3D Fluent CFD model of an air ejector (also know as Venturi pump or vacuum ejector) and currently trying to correlate to measured values:
at primary inlet: volume flow rate and pressure at primary inlet, P1 and Q1 in the attached picture
at secondary inlet: volume flow rate (Q2)
Air_ejector.jpg

CFD settings:
boundary conditions
pressure-inlet at primary inlet
pressure-inlet (P=0) at secondary inlet
pressure-inlet at outlet (air volume far out of the ejector)

; flow solve model
/define/models/viscous kw-sst y
/define/models/energy y n n n y
/define/materials/change-create air air y ideal-gas n n n n n n
;solve settings
/solve/set p-v-coupling 24 ; 24=Coupled; 20=SIMPLE; 21=SIMPLEC


results correlate fairly well for Q2=f(P1) (CFD: blue line)Q2vsP1.jpg
but hitting an asymptotic behavior for Q1 (CFD: blue line) Q2vsQ1.jpg

When looking at density distribution, I see clearly that at primary inlet it is increasing.
The fact that the fluid walls are adiabatic may be the reason? If so, does it mean that I should go through the conjugated heat transfer path?

Any hints are deeply appreciated.
Thank you for your time,
Carles

[LuckyTran]

It's not a heat transfer problem so don't bother. It's not a turbulence model problem either.

The blue curve from CFD makes sense but the experimental results do not. At some point you choke the driving fluid and it becomes the moving fluid and wont get any more flow rate. Is this comparison actually apples to apples or has the data been rescaled in some way that doesn't respect compressibility effects? You can imagine that at very very high pressures the Q1 will become negative. The experimental curves do not show any of these tendencies.


Another thing is you have run thousands of steady cases at various conditions in order to get these flow curves or is this some sort of transient analysis?

[Carles_SM]

Originally Posted by LuckyTran

Is this comparison actually apples to apples or has the data been rescaled in some way that doesn't respect compressibility effects?

This is the very first though I had (isn't it a natural reflex from the simulation guy to doubt about the measures he got?).
To my knowledge (I will double check with the measurement team) it is raw data obtained from flow sensors
for Q1: SFAM-62-5000L-TG12-2SV-M12 (Festo)
I am not really familiar with this sensors...looking at the data sheet it is specified that the measuring principle is thermal.
And from some readings, it seems that this kind of flow measuring principle gives mass flow and not volumetric flow....So may be the sensor uses a predefined density value to go from mass to volumetric flow. I will double check with Festo.

Originally Posted by LuckyTran

Another thing is you have run thousands of steady cases at various conditions in order to get these flow curves or is this some sort of transient analysis?

Not thousands but almost 20 steady cases at various P1 values

Finally, another doubt:
First steady case runs with P1=0.05bar
it converges at the 84th iteration.
Then I change P1 to 0.10bar and it converges at the 85th iteration....does it mean that my convergence criteria (by default) are not tight enough?
iteration.jpg

[LuckyTran]

Steady CFD does not converge in 80 iterations, ever. Just run it longer, regardless of what the residuals say. It would have been very helpful if you started the discussion with "my result haven't converged yet"

What you have is a thermal flow sensor. What it does is, it heats up the fluid (air?) and uses V^2/R to determine the input power. Depending on the particular make it either uses 1) the formula Q=mdot*cp*deltaT to back calculate the mass flow rate, generally super inaccurate or 2) uses a heat transfer correlation to back-calculate the Reynolds number and massflow rate. Accuracy will be whatever it is and you should be relatively okay as long as you understand what the reading means and you don't dunk the sensor in liquid metal before you use it.

I said the CFD makes sense because it follows the higher-order trend that I expect over decades but my words mean nothing when there is no scale. Assuming that you do have decade over decades of data for CFD and experiments (unlikely), you should not see the flowrate stay linear forever.

None of these matter if your results aren't converged yet.


Probably the best thing you can do is create a monitor of the volumetric flowrate (since that is the parameter you are interested in) and plot that vs iteration and use this to judge convergence and not some stupid residual using default criteria.