Airflow don't go on straight

joseitor · February 11, 2016, 06:16

Hello fellas!
My problem is the next one: I'm simulating a airflow that go through a nozzle and then leave it by open outlet. I was taking measures in different cases and there weren't problems, but now I want know velocities of airflow in different distances from my nozzle, but when I try it further away than 25 cm the airflow diverge and the measure is almost 0.
Can somebody tell me what might be wrong? I have already tried creating a regular mesh in the way of fluid and with some different models of turbulence.

Default Domain:
Air at 25ºC
Reference Pressure= 1 atm
Turbulence model: SST

Inlet:
Total Pressure= 3.5 bar

Opening:
relative pressure=0

I applied Symmetry in two faces (i'm working with a quarter of nozzle) and Opening in the another faces.

This is what happens:

ghorrocks · February 11, 2016, 06:34

1) Your simulation does not look converged yet. Run it to tighter convergence - and check the imbalances as well.
2) You have used quarter symmetry but this flow may well have large scale flow fluctuations which you cannot use symmetry for (or steady state either).
3) RANS turbulence models have known difficulties in modelling free shear layers like this. Look it up in the literature if you want more details.

joseitor · February 12, 2016, 11:24

First of all, thanks you so much for you early answer.

I have tried with a better convergence (RMS: 10-5) but results go on being the same.
In addition, I have tried without symmetry too, and the same, the behaviour is the same

Have somebody an idea else?

Thanks!

turbo · February 12, 2016, 12:49

Where is your nozzle exit?
Where did you see a zero velocity? (I see continuous flow streams)

joseitor · February 12, 2016, 13:04

Inlet is in the left and exit of nozzle where you can see that the geometry of nozzle ends.

After where streamlines stop to be straight, if I measure the velocity there (with a small circular plane with the same diameter than the nozzle), the measure is almost zero; obviously because the airflow go up, left, right..but no straight any more.

ghorrocks · February 13, 2016, 06:13

Check your imbalances as well. Residuals are not always enough to confirm convergence.

Did you read my comment #3 in my previous post - you have a fundamental problem here which you are going to have a hard time to overcome

In other words I expect most 2 equation RANS turbulence models to generate excessive turbulent dissipation in a free shear flow like this, which will result in the jet dissipating too quickly and just disappearing. And this is exactly what you are seeing

joseitor · February 14, 2016, 04:04

This were the imbalances.

Are right? Even I made the simulation with get 10e-5 residual and behaviour was the same (but I have the results in another computer).

If they are right, what are the way to follow? What could I do to try to solve it?

Sorry for so many questions but I am quite new in Ansys.
Thanks you so much everyone!

ghorrocks · February 14, 2016, 04:54

If the results with convergence of 1e-4 and 1e-5 are essentially the same then convergence tolerance is unlikely to be affecting things.

I am suggesting that you are seeing a fundamental flaw in 2-equation RANS turbulence modelling. A RSM will probably be better, or a LES model better still. Note that for LES you cannot use symmetry and must use a transient model.

Have you done a literature search on this topic?

joseitor · February 15, 2016, 07:19

Finally I got solve the problem using LES model. Now fluid flow go straight and I can take measures.

Thanks so much everyone!

ghorrocks · February 16, 2016, 00:35

It is good to hear you are ready to proceed. I presume then you have done the normal checks required of a LES model - you checked the modelled turbulence spectrum reaches steady state, you have checked the turbulence spectrum the model gives you is correct, you have checked your mesh size is correct for the turbulence length scale you are modelling, you have chosen a suitable sub-grid model etc etc. LES models are much more complex than RANS models and require far more user knowledge for them to be done correctly.

Also - have you looked at what the jet breakup length for this type of flow should be? Jets decay into turbulence a distance away from the nozzle. Do you know what this length should be for your flow?

-Maxim- · February 18, 2016, 06:12

just a quick note on the imbalances in case other people read this thread and don't switch to LES: As ghorrocks already assumed, your imbalances are still too high (over 3%). The goal is at least to go under 1%.

joseitor · February 18, 2016, 18:14

Quote:

Originally Posted by ghorrocks

It is good to hear you are ready to proceed. I presume then you have done the normal checks required of a LES model - you checked the modelled turbulence spectrum reaches steady state, you have checked the turbulence spectrum the model gives you is correct, you have checked your mesh size is correct for the turbulence length scale you are modelling, you have chosen a suitable sub-grid model etc etc. LES models are much more complex than RANS models and require far more user knowledge for them to be done correctly.

Also - have you looked at what the jet breakup length for this type of flow should be? Jets decay into turbulence a distance away from the nozzle. Do you know what this length should be for your flow?

I have not checked all those things ( no more than in the previous simulations where check toi RMS models), I didn't know about that, but my results still are not good at all. I will go on trying some options and I will tell you as it finish.

Quote:

Originally Posted by -Maxim-

just a quick note on the imbalances in other people read that and don't switch to LES: As ghorrocks already assumed, your imbalances are still too high (over 3%). The goal is at least to go under 1%.

Then I run more time the simulation and obtained imbalances below 3% and results was the same, but thanks for the information. It's good to know it.

Thanks guys!

ghorrocks · February 18, 2016, 18:21

The most important thing is to understand what should be happening in this flow: Turbulent jet break up is a standard CFD test case and there are many CFD analyses of it. Here is one good example: http://www.sciencedirect.com/science...01932213001985

The important thing to note is that turbulent jets do break up some distance away from the start of the jet. Do you know how far the jet you are modelling should go before breaking up? If not then you better do some literature review and find out.

joseitor · February 23, 2016, 10:43

I took some measures in a experiment and at least more farther than 1m from the outlet of my nozzle i obtained velocities around 20m\s

ghorrocks · February 23, 2016, 17:55

And what velocity does your model give at the same location?

February 11, 2016, 06:16	Airflow don't go on straight	#1
joseitor New Member Jose Rodriguez Join Date: Jan 2016 Posts: 13 Rep Power: 10	Hello fellas! My problem is the next one: I'm simulating a airflow that go through a nozzle and then leave it by open outlet. I was taking measures in different cases and there weren't problems, but now I want know velocities of airflow in different distances from my nozzle, but when I try it further away than 25 cm the airflow diverge and the measure is almost 0. Can somebody tell me what might be wrong? I have already tried creating a regular mesh in the way of fluid and with some different models of turbulence. Default Domain: Air at 25ºC Reference Pressure= 1 atm Turbulence model: SST Inlet: Total Pressure= 3.5 bar Opening: relative pressure=0 I applied Symmetry in two faces (i'm working with a quarter of nozzle) and Opening in the another faces. This is what happens:

February 18, 2016, 06:12		#11
-Maxim- Senior Member Maxim Join Date: Aug 2015 Location: Germany Posts: 413 Rep Power: 13	just a quick note on the imbalances in case other people read this thread and don't switch to LES: As ghorrocks already assumed, your imbalances are still too high (over 3%). The goal is at least to go under 1%. Last edited by -Maxim-; February 19, 2016 at 03:01. Reason: missing word

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Heat Transfer from airflow to concrete	Mary2788	FLUENT	1	June 22, 2011 11:43
Actuator disk model	audrich	FLUENT	0	September 21, 2009 08:06
Where's the singularity/mesh flaw?	audrich	FLUENT	3	August 4, 2009 02:07
Simulation of pump with Straight blades	veera	CFX	4	January 12, 2006 01:52
modelling airflow through an inlet restrictor on a four stroke engine	mike ede	Main CFD Forum	0	October 8, 1999 10:06

February 11, 2016, 06:34		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	1) Your simulation does not look converged yet. Run it to tighter convergence - and check the imbalances as well. 2) You have used quarter symmetry but this flow may well have large scale flow fluctuations which you cannot use symmetry for (or steady state either). 3) RANS turbulence models have known difficulties in modelling free shear layers like this. Look it up in the literature if you want more details.

February 12, 2016, 11:24		#3
joseitor New Member Jose Rodriguez Join Date: Jan 2016 Posts: 13 Rep Power: 10	First of all, thanks you so much for you early answer. I have tried with a better convergence (RMS: 10-5) but results go on being the same. In addition, I have tried without symmetry too, and the same, the behaviour is the same Have somebody an idea else? Thanks!

February 12, 2016, 12:49		#4
turbo Senior Member Join Date: Jun 2009 Posts: 174 Rep Power: 17	Where is your nozzle exit? Where did you see a zero velocity? (I see continuous flow streams)

February 12, 2016, 13:04		#5
joseitor New Member Jose Rodriguez Join Date: Jan 2016 Posts: 13 Rep Power: 10	Inlet is in the left and exit of nozzle where you can see that the geometry of nozzle ends. After where streamlines stop to be straight, if I measure the velocity there (with a small circular plane with the same diameter than the nozzle), the measure is almost zero; obviously because the airflow go up, left, right..but no straight any more.

February 13, 2016, 06:13		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	Check your imbalances as well. Residuals are not always enough to confirm convergence. Did you read my comment #3 in my previous post - you have a fundamental problem here which you are going to have a hard time to overcome In other words I expect most 2 equation RANS turbulence models to generate excessive turbulent dissipation in a free shear flow like this, which will result in the jet dissipating too quickly and just disappearing. And this is exactly what you are seeing

February 14, 2016, 04:04		#7
joseitor New Member Jose Rodriguez Join Date: Jan 2016 Posts: 13 Rep Power: 10	This were the imbalances. Are right? Even I made the simulation with get 10e-5 residual and behaviour was the same (but I have the results in another computer). If they are right, what are the way to follow? What could I do to try to solve it? Sorry for so many questions but I am quite new in Ansys. Thanks you so much everyone!

February 14, 2016, 04:54		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	If the results with convergence of 1e-4 and 1e-5 are essentially the same then convergence tolerance is unlikely to be affecting things. I am suggesting that you are seeing a fundamental flaw in 2-equation RANS turbulence modelling. A RSM will probably be better, or a LES model better still. Note that for LES you cannot use symmetry and must use a transient model. Have you done a literature search on this topic?

February 15, 2016, 07:19		#9
joseitor New Member Jose Rodriguez Join Date: Jan 2016 Posts: 13 Rep Power: 10	Finally I got solve the problem using LES model. Now fluid flow go straight and I can take measures. Thanks so much everyone!

February 16, 2016, 00:35		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	It is good to hear you are ready to proceed. I presume then you have done the normal checks required of a LES model - you checked the modelled turbulence spectrum reaches steady state, you have checked the turbulence spectrum the model gives you is correct, you have checked your mesh size is correct for the turbulence length scale you are modelling, you have chosen a suitable sub-grid model etc etc. LES models are much more complex than RANS models and require far more user knowledge for them to be done correctly. Also - have you looked at what the jet breakup length for this type of flow should be? Jets decay into turbulence a distance away from the nozzle. Do you know what this length should be for your flow?

February 18, 2016, 18:21		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	The most important thing is to understand what should be happening in this flow: Turbulent jet break up is a standard CFD test case and there are many CFD analyses of it. Here is one good example: http://www.sciencedirect.com/science...01932213001985 The important thing to note is that turbulent jets do break up some distance away from the start of the jet. Do you know how far the jet you are modelling should go before breaking up? If not then you better do some literature review and find out.

February 23, 2016, 10:43		#14
joseitor New Member Jose Rodriguez Join Date: Jan 2016 Posts: 13 Rep Power: 10	I took some measures in a experiment and at least more farther than 1m from the outlet of my nozzle i obtained velocities around 20m\s

February 23, 2016, 17:55		#15
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	And what velocity does your model give at the same location?