CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

3D DES simulation of turbulent jet

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 10, 2017, 12:46
Default 3D DES simulation of turbulent jet
  #1
New Member
 
Join Date: May 2015
Posts: 22
Rep Power: 6
Kostas_K is on a distinguished road
Hello all,

Im a beginner in Fluent and CFD so please bear with me.

Im trying to run a DES simulation for a 3d turbulent jet. I want to visualize the velocities (x,y,z), vorticities (x,y,z) etc.

I am trying to simulate a duct (0.35mx0.35mx0.25m). The duct is seperated by a wall which has a sharp-edged rectangular orifice configuration(70 mm x 7 mm). My inlet is 0.1 m before the wall that has the orifice and my outlet 0.15m after the wall. My mesh consists of tetrahedrons everywhere exccept where i used inflation. There are 1.6 million elements total.

Given data was ony the Reynolds number at the orifice (Re=23000 or Re hydrolic diamaterer=42000). It is calculated that the velocity at the orifice is v2=50m/s and so the velocity at the inlet has to be v1=0.133m/s. Also the simulation is done as incompressible.

In Fluent my inputs are:
Pressure-based solver
Transient
Energy off
Delayed Detached Eddy Simulation (DES) with the Spalart-Allmaras model

Boundary Conditions:
for walls i used default options
for outlet i used default options
for interior i used default options
for inlet i used mass-flow inlet
-mass flow rate = 0.19958 kg/s
-z component of flow direction = 0.133m/s
-turbulence specification method = turbulent viscosity ratio
-turbulence viscosity ratio=10

SIMPLE scheme was selected.
Gradient: Least square cell based
Pressure: Second Order
Momentum: Second Order Upwind
Modified Turbulent viscosity: Second Order Upwind
Transient Formulation: Bounded Second Order Implicit

Under-Relaxation factors were left default except for:
pressure: from 0.3 (default) --> 0.4
momentum: from 0.7(default) --> 0.8

All Residuals were changed to 1e-05

Using Standard Initialization, the solution was initialized as zeros (0) everywhere

For time step i choose Dt=5e-04 and max iterations/time step= 10

I use solution animations to check the results while running the simulation and the results are very close to what was expected...but the residuals are not willing to go down and converge

Do you have any changes to propose for all the above settings ?
Did i make a mistake somewhere ?

Sorry for the long thread.

Any help will be greatly appreciated

Thank you.
Kostas
Attached Images
File Type: jpg 3d view.jpg (18.5 KB, 22 views)
File Type: jpg xy plane.jpg (20.3 KB, 24 views)
File Type: jpg yz plane.jpg (22.5 KB, 25 views)
File Type: jpg mesh.jpg (154.1 KB, 27 views)
Kostas_K is offline   Reply With Quote

Old   April 11, 2017, 02:43
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,572
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Do you mean residuals are stuck at high values or are they decreasing but not enough to meet your convergence criteria? If it's the 1st, then it hints at a problem with the setup. If it's the 2nd...

I think it is because you are using SIMPLE which needs many iterations to converge (because the urf's are not 1). You can verify this by increasing the number iterations per time-step to a really high number like 50 or 100 (just to check). Just do it for a few time-steps to test. You can change it back later. Also have you tried a smaller time-step?

Since you don't have coupling with any other equations, I highly recommend PISO. The disadvantage is you'll need small time-steps. The advantage is, you can get away with as few as 2 iteration per time-step. You should be able to take a bunch of smaller time-steps faster.

SIMPLE is great when you are also solving a lot of other equations, because coupling between equations is what slows convergence. If you're only solving continutiy & momentum, it's probaby the P-V coupling that's limiting.

You could also give the COUPLED solver a whack, but it has urf's and so it's behaves more like SIMPLE. But definitely do the check using SIMPLE with 100 iterations to make sure.

Btw I highly recommend you always use the bounded central differencing whenever possible (momentum especially). But maybe it's not available for DES.
LuckyTran is offline   Reply With Quote

Old   April 11, 2017, 02:48
Default
  #3
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,291
Rep Power: 36
-mAx- will become famous soon enough
If you are a beginner, I would:
*run a steady state case first
*set all under-relaxation parameters to default settings
*set all numerical schema to default
*set turbulent model to default (k-eps?)

I would modify some parameters if you get bad results or poor convergence

What is for you the default BC for outlet?

I would also extend your domain , inlet and outlet are to close to the restriction
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 11, 2017, 08:41
Default
  #4
New Member
 
Join Date: May 2015
Posts: 22
Rep Power: 6
Kostas_K is on a distinguished road
Hello LuckyTran,
Thank you for your answer

When the simulation begins the residuals decrease. After a few hundreds iterations they stop decreasing or they decrease with a very slow rate. The residuals of x,y,z velocities and nut oscilate between 1e-04 and 1e-06. Only continuity stays between 1e-02 and 1e-03.

For my mesh i used body of influence to create the fine areas. I put 2mm for the element sizes as an input so i calculated the timestep like this:
Dx/v=Dt => 0.002/50=0.00004=4e-05.
But I also tried to run a simulation with 2e-05 which is half of the above. But i couldn't get a good result. Maybe because the solution advances very slow and I didn't let it run for more than a coyple days.

I will try what you said about simple and piso scheme and let you know.
Kostas_K is offline   Reply With Quote

Old   April 11, 2017, 09:13
Default
  #5
New Member
 
Join Date: May 2015
Posts: 22
Rep Power: 6
Kostas_K is on a distinguished road
Hello Max,
Thank you for your answer

*I have already tried running a steady state simulation. And then when the residuals were flat (not converged) i changed the solution to transient and used the steady state values an initials.
*Also i had the urf's at their default values. Only in the last case that i posted about had i changed them.
* The schemes were also default
*I can not use the k-e model because i want to visualize vorticity and the k-e doesn't show it. Only with LES or DES could i see the vorticity. And the LES is more demanding than the DES

Also i used to have a bigger domain but it reached about 4-5 million elements and my computer wasn't able to solve it. So i was forced to make it smaller.

The default BC for the outlet is
type - Pressure outlet
at momentum tab
gauge pressure (pascal) - 0 constant
backflow direction specification method - normal to boundary
turbulence specifiction method - turbulent viscosity ratio
backflow turbulent viscosity ratio - 10 constant
Kostas_K is offline   Reply With Quote

Old   April 11, 2017, 11:25
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,572
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by Kostas_K View Post
The residuals of x,y,z velocities and nut oscilate between 1e-04 and 1e-06. Only continuity stays between 1e-02 and 1e-03.
This behavior is pretty normal. 1) You have your mesh which limits convergence. 2) Large time-steps also makes you lose some temporal bandwidth and also makes it harder to converge because you enter a time-step with error. 3) Over many time-steps, the error also accumulates but hopefully reaches some limit so that your sim doesn't diverge.

Quote:
Originally Posted by Kostas_K View Post
For my mesh i used body of influence to create the fine areas. I put 2mm for the element sizes as an input so i calculated the timestep like this:
Dx/v=Dt => 0.002/50=0.00004=4e-05.
So your courant number is 1 or so? Btw you should also check this with like a volume maximum monitor and/or some contours. Just visually inspect to make sure.

Honestly I think your simulation is fine and you only need to do some sanity checks. Make some point monitors at interesting points (like where you expect the shear layer) and check that the x-velocity, y-velocity, z-velocity, & pressure are converged to #.### decimals at every time step. You can also probe the vorticity since that's what you're interested in. Rather than worry about how much residuals are dropping, you should start post-processing and check whether the result makes any sense. I.e. verify that you have the expected turbulence.
LuckyTran is offline   Reply With Quote

Old   April 13, 2017, 14:33
Default
  #7
New Member
 
Join Date: May 2015
Posts: 22
Rep Power: 6
Kostas_K is on a distinguished road
No my courant number is not 1. It would be if i hab used for a time step 4e-05 but i used 5e-04. Because it would take too much time otherwise.
Also i just started testing what you said for PISO because for 2 days now i have been running another simulation.
I started with DES model and steady solution to get a initial value for my case (i know that DES model is only meant for transient solution). After 1600 iterations when the residuals were flat (not converged) i changed the solution to transient and used the steady state values an initials. The results in comparison with the experiment for z velocity and z vorticity can be seen in the pictures. The only problem are the residuals. Can i say that my solution is converged ?
Attached Images
File Type: jpg computational.jpg (87.1 KB, 22 views)
File Type: jpg residuals.jpg (52.9 KB, 17 views)
File Type: jpg experimental.jpg (57.7 KB, 17 views)
Kostas_K is offline   Reply With Quote

Old   April 13, 2017, 15:08
Default
  #8
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,572
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
If you want to know if your solution is converged, then look at the solution, not residuals! Look at velocities, etc. Make a plot of velocity vs iter.

Also you need to verify that your DES is actually DES. I am worried that because you did not apply any perturbations (i.e using init-instantaneous-velocity or something equivalent) that you do not have a turbulent flow. Check the spectrum and verify that it is indeed turbulent and not laminar.

Quote:
Originally Posted by Kostas_K View Post
No my courant number is not 1. It would be if i hab used for a time step 4e-05 but i used 5e-04. Because it would take too much time otherwise.
It is not wrong to do so, but I hope you are aware of the implications of using a very large time-step in DES/LES. Your temporal bandwidth is now extremely limited.
LuckyTran is offline   Reply With Quote

Old   April 14, 2017, 08:34
Default
  #9
New Member
 
Join Date: May 2015
Posts: 22
Rep Power: 6
Kostas_K is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
Also you need to verify that your DES is actually DES. I am worried that because you did not apply any perturbations (i.e using init-instantaneous-velocity or something equivalent) that you do not have a turbulent flow. Check the spectrum and verify that it is indeed turbulent and not laminar.
How exactly can i verify that i have a turbulent flow ?
Also if i do have a laminar flow how can i apply some pertrubations using ansys in order to make it turbulent and get the right solution ?
Kostas_K is offline   Reply With Quote

Old   April 14, 2017, 10:19
Default
  #10
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,572
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by Kostas_K View Post
How exactly can i verify that i have a turbulent flow ?
Also if i do have a laminar flow how can i apply some pertrubations using ansys in order to make it turbulent and get the right solution ?
Check out Paolo's blog. He has some cute scripts you can use. If you had started with a RANS as an initial condition though, you could have just typed in solve/initialize/ init-instantaneous-vel

https://www.cfd-online.com/Forums/blogs/sbaffini/

How to check... Well how do you verify that any flow is turbulent? I.e. forget that you are doing CFD but you are just an observer or experimentalist. If I set up this problem in a lab, how do you verify that it is indeed turbulent?

Well one way is to get the spectrum of the the turbulent kinetic energy and show that it is broadband and looks like a typical turbulent spectrum.
LuckyTran is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Jet fan and Tunnel simulation ahlo7 CFX 9 November 13, 2019 05:54
Water jet simulation harry123 STAR-CCM+ 9 April 19, 2016 05:30
LES of Turbulent Jet knuckles OpenFOAM Running, Solving & CFD 1 March 31, 2016 20:33
Impinging Jet simulation with rhoSimpleFoam dappe OpenFOAM Running, Solving & CFD 7 December 1, 2015 04:42
Unsteady RANS simulation of Jet in crossflow harshad88 FLUENT 0 June 2, 2013 14:29


All times are GMT -4. The time now is 15:09.