[medaouarwalid]

Hi, when performing a transiant simulation , should i do the same length time that i needed in experimentation. For example if it took me 1 hour to mesures all velocities in different points. Should the time of the simulation be 1 hour ? And if the mesurement in exerimental was not in a constant time step ( for example 10 seconds for a mesure and 15s for the next mesure) because the nature device of mesurement (you need until the numbers are stable on the screen ) does this have an effect ?

Sent from my F1f using CFD Online Forum mobile app

[BlnPhoenix]

It took one hour to measure all different points in the apparatus. But did you check if the value was changing over time at the same spot? So, did you check after 5 mins, 30 mins, 1hr the same spot? If so, is the value constant over time? If the answer is yes, my answer would be (assuming LES):

It is ok to simulate 5 mins. and check afterwards.

[medaouarwalid]

Originally Posted by BlnPhoenix

It took one hour to measure all different points in the apparatus. But did you check if the value was changing over time at the same spot? So, did you check after 5 mins, 30 mins, 1hr the same spot? If so, is the value constant over time? If the answer is yes, my answer would be (assuming LES):

It is ok to simulate 5 mins. and check afterwards.

For the velocity yes it was pretty much the same values . But for the temperature no it rises because the ambien temperature of the room rises, thats why i used the dimensionless temperature (Ti-T ambient / T max-T ambien). So either i perform an hour of simulation or i just do a dynamic study and i exclude the temperature ?

Sent from my F1f using CFD Online Forum mobile app

[BlnPhoenix]

Originally Posted by medaouarwalid

For the velocity yes it was pretty much the same values . But for the temperature no it rises because the ambien temperature of the room rises, thats why i used the dimensionless temperature (Ti-T ambient / T max-T ambien). So either i perform an hour of simulation or i just do a dynamic study and i exclude the temperature ?

[/URL]

You can also compare the temps after 5 mins. or whatever your first measured time is. Should be ok.

[FMDenaro]

While comparing a transient simulation with experimental measurements, the main problem is in setting the same initial condition otherwise you LES will produce only a numerical transient.

[BlnPhoenix]

Originally Posted by FMDenaro

While comparing a transient simulation with experimental measurements, the main problem is in setting the same initial condition otherwise you LES will produce only a numerical transient.

This is true. But i guess finding good initial conditions for this case startup of hairdryer, or what it exactly is i don't know, can be tricky. I guess it depends also on the flow history before the inlet into the computational domain.

[FMDenaro]

Right. And if it is not possible to match the initial condition, at least close to the nozzles, the only meaningful result is when the LES solution forgets the initial condition. But that does not match the transient measurements...

[medaouarwalid]

Originally Posted by BlnPhoenix

You can also compare the temps after 5 mins. or whatever your first measured time is. Should be ok.

I dont think so, because numer of mesurements in 5 minutes

Originally Posted by BlnPhoenix

You can also compare the temps after 5 mins. or whatever your first measured time is. Should be ok.

Yes, but the number of mesurements that i did for 5 minutes is not enough to do a study of the thermal homoginization that i need. So if i will not simulate the temperature i will be only interrested by the velocity wich is not changing with time, i am afraid it is like if i am doing an Les for a steady flow !!

Sent from my F1f using CFD Online Forum mobile app

[medaouarwalid]

Originally Posted by FMDenaro

Right. And if it is not possible to match the initial condition, at least close to the nozzles, the only meaningful result is when the LES solution forgets the initial condition. But that does not match the transient measurements...

An other problem about initial conditions is that it depends also of the mesurement device, because it is not like a PIV or whatever else wich gives instantanous mesure, the device i use has a probe wich capture the velocity then displays it on the screen, you will see the velocity rises until it became stable and at that time you can pike the value. For example if i put the probe at the exit of the nozzle, befor i turn on the hairdryers the velocity on the screen is zero m/s, when the air reaches the probe it doesnt display the true value at that fraction second but i have to wait for the velocity to rise from zero until the stable value. So i cant know the exact time to concider it as initial condition

Sent from my F1f using CFD Online Forum mobile app

[FMDenaro]

Originally Posted by medaouarwalid

An other problem about initial conditions is that it depends also of the mesurement device, because it is not like a PIV or whatever else wich gives instantanous mesure, the device i use has a probe wich capture the velocity then displays it on the screen, you will see the velocity rises until it became stable and at that time you can pike the value. For example if i put the probe at the exit of the nozzle, befor i turn on the hairdryers the velocity on the screen is zero m/s, when the air reaches the probe it doesnt display the true value at that fraction second but i have to wait for the velocity to rise from zero until the stable value. So i cant know the exact time to concider it as initial condition

Sent from my F1f using CFD Online Forum mobile app

I suggest to take some measurements in the room but with all nozzles turned out. See in several position of the room the velocities to understand if you have a convective motion as base flow. You could try to replicate first a simulation (without nozzles) of the room base fow and use it as initial condition.
Conversely, if you measure an almost zero velocity field you could set an initial condition corresponding to the rest with superimposed a small random fluctuations.
Furthermore, the boundary conditions for the temperature should consider the correct heat flux leaving the room from the walls. Otherwise, if you set all adiabatic conditions, the heat flow from the nozzle produces an increasing in the internal energy that can drive to a numerical instability.
You need to model you problem at the best you can.

[medaouarwalid]

Originally Posted by FMDenaro

I suggest to take some measurements in the room but with all nozzles turned out. See in several position of the room the velocities to understand if you have a convective motion as base flow. You could try to replicate first a simulation (without nozzles) of the room base fow and use it as initial condition.
Conversely, if you measure an almost zero velocity field you could set an initial condition corresponding to the rest with superimposed a small random fluctuations.
Furthermore, the boundary conditions for the temperature should consider the correct heat flux leaving the room from the walls. Otherwise, if you set all adiabatic conditions, the heat flow from the nozzle produces an increasing in the internal energy that can drive to a numerical instability.
You need to model you problem at the best you can.

Of course I took mesurements in the room before turning on the blowers, velocities were zero in all places were i mesured, i was working in a room of 3*2.5*2.5 m³ with all door closed. For the temperature i am realy thinking of either exluding it's study at least for now or talking to my professor to use URANS instead of LES because of the cost in time of calculation, with a time step arround 10^-5 i will never succed with the available computer ( 12 processors and 16g of RAM) to do a simulation of a a long periode. Pr Denaro if you remember i launched the calculation 2 days ago, and it is now about 1 second of simulation !! Knowing that i didnt generate a very fine mesh ( 500000 element) + i am using NITA and FSM

Sent from my F1f using CFD Online Forum mobile app

[Blanco]

Originally Posted by medaouarwalid

Of course I took mesurements in the room before turning on the blowers, velocities were zero in all places were i mesured, i was working in a room of 3*2.5*2.5 m³ with all door closed. For the temperature i am realy thinking of either exluding it's study at least for now or talking to my professor to use URANS instead of LES because of the cost in time of calculation, with a time step arround 10^-5 i will never succed with the available computer ( 12 processors and 16g of RAM) to do a simulation of a a long periode. Pr Denaro if you remember i launched the calculation 2 days ago, and it is now about 1 second of simulation !! Knowing that i didnt a very fine mesh ( 500,000 element) + uqing NITA and FSM

Sent from my F1f using CFD Online Forum mobile app

Considering you available hardware, the time-period you'd like to simulate and the uncertanities arisen in different posts concerning initial conditions, etc. etc... I strongly suggest to switch to a less-precise URANS simulation. This will bring you to a solution (which will be for sure less precise...but still realistic hopefully) in the short-term and you can obtain some useful insight on what you're investigating. Btw, what are you trying to reproduce exactly?

[medaouarwalid]

Originally Posted by Blanco

Considering you available hardware, the time-period you'd like to simulate and the uncertanities arisen in different posts concerning initial conditions, etc. etc... I strongly suggest to switch to a less-precise URANS simulation. This will bring you to a solution (which will be for sure less precise...but still realistic hopefully) in the short-term and you can obtain some useful insight on what you're investigating. Btw, what are you trying to reproduce exactly?

Ok i will give an abstract . Multiple jet configuration is the one in which two or more numbers of jets discharged from the same exit plane and separated by a finite distance. For thermal homoginization It was shown that it is more efficient to have multiple small jets instead of a single big jet for the same momentum flux at the nozzle exit. There is different kinds of multiple jets accodring to the shape of the nozzles (swirling jets, circular ...) I am trying to simulate a kind of multiple jet to study the interaction between the jets and the effect of this interaction on the thermal homoginezation to sort an optimal configuration that can be used in a cooling or heating systems. From the literature, the values of interest was velocity , volumetric flow rate and temperature. After doing experimentations on one configuration i want to find a numerical model which will be close to mesurements for the goal of use it to compare that configuration with other configurations after changing some parameters ( changing the the disposition of the jets, the number ....).

Sent from my F1f using CFD Online Forum mobile app

[FMDenaro]

Originally Posted by medaouarwalid

Of course I took mesurements in the room before turning on the blowers, velocities were zero in all places were i mesured, i was working in a room of 3*2.5*2.5 m³ with all door closed. For the temperature i am realy thinking of either exluding it's study at least for now or talking to my professor to use URANS instead of LES because of the cost in time of calculation, with a time step arround 10^-5 i will never succed with the available computer ( 12 processors and 16g of RAM) to do a simulation of a a long periode. Pr Denaro if you remember i launched the calculation 2 days ago, and it is now about 1 second of simulation !! Knowing that i didnt generate a very fine mesh ( 500,000 element) + i am using NITA and FSM

Sent from my F1f using CFD Online Forum mobile app

The run seems too slow for this grid size...

[medaouarwalid]

Originally Posted by FMDenaro

The run seems too slow for this grid size...

time step is 10^-5 so i need 100 000 time step to have 1 seconde of simulation , if the time step increments every 1 seconde ( which is not the case) , it takes 27 hours to complete the simulation , so it is logical somehow

[BlnPhoenix]

Originally Posted by medaouarwalid

time step is 10^-5 so i need 100 000 time step to have 1 seconde of simulation , if the time step increments every 1 seconde ( which is not the case) , it takes 27 hours to complete the simulation , so it is logical somehow

Try the RANS approach first and compare your velocity value from the experiment with the CFD solution. It will give you some idea about accuracy. Afterwards you decide what further you can do to improve.

[Blanco]

Originally Posted by medaouarwalid

Ok i will give an abstract . Multiple jet configuration is ....).

If you're going to simulate multiple jets entering into a quiescent room then I would definitely start with a RANS. It will give you something usable in the short term and you can also use the RANS results to eventually do a LES simulation later (i.e. you can initilize the flowfield with the RANS results with some perturbation, this will speed-up the "flush out" of initial conditions in the LES sim)

[medaouarwalid]

Originally Posted by Blanco

If you're going to simulate multiple jets entering into a quiescent room then I would definitely start with a RANS. It will give you something usable in the short term and you can also use the RANS results to eventually do a LES simulation later (i.e. you can initilize the flowfield with the RANS results with some perturbation, this will speed-up the "flush out" of initial conditions in the LES sim)

Okay i will do a Rans simulation afterthat i will contact you. Thank you all

Sent from my F1f using CFD Online Forum mobile app

[medaouarwalid]

hi , after your suggestions i did 3 seconds of simulation using unsteady realizable K-epsilone , always with that low numbers of elements mesh ( refinement only in close to the nozzles) and a time step of 0.001 seconde just to have an idea. residuals was 10^-4 for continuity ; 10^-6 for k and epsilon ; 10^-6 for x,y,z velocities and 10^-8 for energy. For the radial velocity, the results was good even with that low mesh ( figure) but for the axial velocity not so good (as you see). now what do i have to do ? should i refine the mesh and use the results as initial conditions for LES or only count on Urans if it gives me better results .

[FMDenaro]

I would first refine the grid to check if the solution changes