illogical result !!
 

hello every one, this is a nozzle called ''lobed nozzle'', it has a circular shape at the inlet and a corrugated shape at the exit, in my case, the area of the inlet is 314 mm² . the area of the exit is 213 mm² .
experimentally, the velocity at the center of the inlet area was 7.5 m/s and when i mesured the velocity at the center of the exit it was 4.5 !!!
numérically it was an other thing , when i set inlet velocity at 7.5 it gave me 10 m/s at the exit which i think is a logical result if we consider the continuity equation. now i don't know what to believe because i repeated the experimental many times and i get the same result each time. There is something wrong here but i didnt find it
noting that i used the ''SST K-omega'' model and i set the the walls of the nozzle as '' no slip WALL'' in BC
https://img15.hostingpics.net/pics/125822xxxxxx.png

What about the density? Are you injecting a gas?

Hot Air from hair dryer connected to the nozzle inlet

Ok, so density can change between inlet section and outlet section, and all we know is that mflux=dens*A*vel=const. Therefore it is possible that experimental velocity is correct (:D!). Talking about your simulation: have you double checked the gas properties you're using in the model? Are you using ideal gas or what? Are the wall boundaries adiabatic, fixed T, etc.? What is the distance between inlet and outlet of the nozzle?

I didnt check gas properties, i am assuming that the fluid is incompressible because the velocity is not that high to concidere change in density , also for the walls i used the default setting , the distance between inlet and outlet is 90 mm

Ok, so now you have a list of things to check at least. ;)

I don't know which program you're using, so I suppose that your "default" settings for wall are consistent with adiabatic walls.

Another question: is the nozzle "representative" of a small hair dryer in your intentions? If yes, then the "inlet" section is filled with cold air while hot air flows through the outlet section, or I am missing something?

First, the program i am using is ansys fluent and i cheked only option ''no slip" in wall BC.
second i am studying the effect of the geometrie of that nozzle on the augmentation of mixing the blowing air with the ambiant air, so the hair dryer is tool to give me hot hair , the outlet of the blow dryer is equal to the inlet of the nozzle. Also, i want to say that i mesure the inlet velocity afther that i joined the nozzle inlet to the blow dryer exit .

I went back to the lab and i did other mesurements. This time i mesured the central velocity not only in the inlet and outlet of the nozzle but also in different points of the centerline of the nozzle , here the new results:
- the velocity was 7.5 m/s only in the point of the grid of the exit of the blower ( see image 3 blower +nozzle ) ,
- when i go down a little bit from there , the velocity decreases until 3.15 and stay like this in the cylindre shape of the nozzle until it reaches the corrugated shape of the nozzle
- then it begins to increase until it reaches 4.6 m/s at the exit of the nozzle !!! Any explications please https://img4.hostingpics.net/pics/57...0607170610.jpg

Now it makes sense to me:

1- the velocity you measured at the center of the nozzle inlet section is not representative of average inlet flow, because it is influenced by the grid and other stuff you have in the blower near its outlet section. I really think the velocity distribution is all but uniform in the nozzle inlet section.

2- going down along the centerline of the nozzle, the disuniformities you have tends to fade out and a more uniform flow is achieved, therefore the 3.15 m/s you mesured on the centerline "could" be considered representative of the mean flow though a nozzle section

3- the velocity you measured on the outlet section of the nozzle is 4.6 m/s in the centerline, I suppose. Here again I don't expect a very uniform velocity distribution on the outlet section, because of the particular geometry, but the continuity equation tells us that we're very close to theory:

3.15 * 314 / 213 = 4.64 m/s

and you have measured 4.6 m/s... It makes sense.

Btw: how are you measuring the local velocity? You have also to consider the influence you have on the flowfield.

The setting of the numerical parameters at the inlet is very important... doing RANS you should prescribe a statistically averaged velocity profile. Consider also the requirement of the turbulence model varaibles at the inlet.
What is the geometry before of the inlet of the nozzle?

The géométrie before the inlet of the nozzle is in the figure number 1 of the photo in the comments. A conical géométrie with a grid at exit

Ok, so i will take the velocity inlet as 3.15 m/s, also To mesure velocity i am using The TSI VELOCICALC® Multi-Function Ventilation Meter 9565-
Thank you for helping me ,m. Cordially

Well, maybe you could do a try in adding this cone in the simulation.. I don't know how the grid can influence the inflow in the nozzle, in general a grid is used to make the flow more homogeneous...
If you use the incompressible formulation you can prescribe either the velocity or the pressure, what measurement about the pressure do you have?

I didnt mesure the pressure because i am doing a dynamic study and i am interessting just in velocity, should i do mesurements of the pressure also ?

The key is that if you use RANS, you should measure a statistically averaged profile at the inlet (at least a sufficient number of points)... Are you able to do such a measure on the plane at the inlet?

Well the mesurements tool (
The TSI VELOCICALC® Multi-Function Ventilation Meter 9565-) has a probe wich dont allow me to do much mesurements at that plane ( i think you mean the grid) , maybe at the center and near to the nozzle walls thats all

would be more simple to do the measure in the cone plane before the nozzle??

the cone is a small blow dryer i cant take off the grid of the exit

you can try to add the full cone in the simulation and prescribe a turbulent profile at the inlet of the cone...

I dident understand what do you mean by prescribe a turbulent profile at the inlet of the cone , can you please explain more.

I mean that you can try (and have luck) to suppose that a fully develeped turbulent profile (for a pipe) exists and prescribe it if you have some velocity measurement. The cone will allow to let the flow develop towards the nozzle.

I have no other idea than "try and test" ...

I dont have any mesurements of the velocity in the inlet of the cone ( blow dryer) .

Looking at the photo and thinking of a typical hair dryer, I think there are lot of things inside the blower that could create wakes in the flowfield. Therefore, I think that even if you include part of the end cone of the blower in your computational domain, you won't be able to impose a statistically representative quantity for velocity, pressure and turbulent quantities, on the "new" inlet boundary of your simulation.

Considering this, I would suggest to reduce your computational domain: the nozzle you're investigating has a cylindrical shape in the initial part and it seems that a steady flowfield is achieved in it, as long as your measurements are concerned (some diameter after the hair dryer-nozzle junction the exp. velocity is not chaning anymore). I suggest you to cut your computational domain and put the new inlet boundary in the same position where you experimentally observe that the flow velocity within the nozzle is not changin anymore, and then impose the same velocity on the computational boundary (3.15 m/s). I would assume that the wakes have disappeared/dissipated on the new inlet section, at least the bigger.

I agree that an experimental pressure would certainly help to better impose the boundary conditions on your computational domain. You have however to assume turbulent quantities on your inlet boundary, as prof. MFDenaro already wrote, and the best thing you can do to start is assume a fully developed turbulent profile. To verify the impact of this assumption on your CFD3D results, you can re-run your simulation with different inlet turbulent quantities and check how much the results will change (e.g. change turbulence intensity, etc. etc.).

You can also do another thing: add a cylindrical pipe between the blower and the nozzle. The longer the cylindrical pipe the better it is theoretically, but some diameter length will be enough. Then you can measure the velocity profile in the junction between the nozzle and the cylindrical pipe, this way avoiding the wakes coming from the blower. You can measure the velocity in the centerline and near the walls easily there and you don't have any close grid upstream influencing your measurements... If the pipe is long enough, you will have a fully developed turbulent profile in it so you should be able to set turbulent quantities easily in your model (and you don't have to reduce your computational domain).

What it is not clear to me (I don't have enough experience in experimental devices) is if this velocity measurement is accurate or not. For turbulent flow it would requires a very accurate device. And the measures must be statistically averaged to be congruent to the RANS simulation...

Thank you for your suggestions, i did listened to it by using the velocity 3.15m/s at the i let wich was almost constant in the cylindre shape of the nozzle, now the new problem is when the jet exits the nozzle the numerical axial velocity at the exit was almost the same like the experimental data ... Fine, after that it keeps going up for few axial stations then it decays , where in the experimental mesurements there is no going up, the velocity decays the moment it exits the nozzle. Could you help me finding why ?